Re: [Emc-users] Lathe Threading
The ramps are essential for full strength as they remove the need for a safety groove Dave Caroline On 19/05/2014, Steve Blackmore st...@pilotltd.net wrote: On Sun, 18 May 2014 12:45:08 -0700, you wrote: I'm still not seeing why G76 has a entry and exit ramp. I believe the intent was to deal with Z acceleration time where the helix is not valid at the start (and I assume the end) of synchronized motion. Normally, one would start the thread off the part enough to have the Z and spindle locations synchronize in air. Absolutely. You start the thread in air so the tool is at correct feed/speed combination when it contacts the material. A good CAM program can work this distance out for you. Normally in the machine setup you tell it what the max feeds and acceleration are and you are able to enter a tolerance value so you have a little leeway. Otherwise you guess. For threads that need to start in the material rather than air, ramping may be used to ease into the thread until the helix is correct. But the way I see it, either way there will be a bit of bad helix at the start and end of the thread. Ramping-in cuts less material, so may get in the way more than plunge-and-go. Channeling before threading, so any material left will only have valid helix, seems better. I would like to know if there is any situation where ramping would be better than channeling or plunging. If the thread starts in the job, often parts are designed so there is a clearance groove in, out or both on the thread, a plunge can be made as long as the tool can accelerate to the correct feed within that groove. If that's not possible or desired a ramp in move in/out can be done, but the tool has to be at the correct feed when it hits the work - as long as the pitch of the thread doesn't alter, it's fine. Steve Blackmore -- -- Accelerate Dev Cycles with Automated Cross-Browser Testing - For FREE Instantly run your Selenium tests across 300+ browser/OS combos. Get unparalleled scalability from the best Selenium testing platform available Simple to use. Nothing to install. Get started now for free. http://p.sf.net/sfu/SauceLabs ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Accelerate Dev Cycles with Automated Cross-Browser Testing - For FREE Instantly run your Selenium tests across 300+ browser/OS combos. Get unparalleled scalability from the best Selenium testing platform available Simple to use. Nothing to install. Get started now for free. http://p.sf.net/sfu/SauceLabs ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On 19 May 2014 08:27, Dave Caroline dave.thearchiv...@gmail.com wrote: The ramps are essential for full strength as they remove the need for a safety groove You don't need a safety groove anyway with a conventional threading operation, the retract move seems consistent. I am prepared to believe that a taper-out might give a better stress concentration as the change in stiffness of the bolt is less sudden. The lead-in and -out probably see very little use, but at the same time there doesn't seem to be any penalty for them existing as an option. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Accelerate Dev Cycles with Automated Cross-Browser Testing - For FREE Instantly run your Selenium tests across 300+ browser/OS combos. Get unparalleled scalability from the best Selenium testing platform available Simple to use. Nothing to install. Get started now for free. http://p.sf.net/sfu/SauceLabs ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
The other place ramping seems to be quite important is in cutting a higbee thread. This operation follows the threading cycle with a grooving tool for the first thread, ramping out over one revolution to get rid of the sharp burr formed between a 60deg thread and a 45deg chamfer. I haven't actually made one of these higbees, but have read about them and tried to figure out how to make them. Here is one explanation: http://blog.cnccookbook.com/2012/06/16/programming-to-cut-a-higbee-thread-higbee-start-or-blunt-start-thread/ Lots of discussions on them on practicalmachinist cnc forum too. -- Ralph From: andy pugh [bodge...@gmail.com] Sent: Monday, May 19, 2014 2:06 AM To: Enhanced Machine Controller (EMC) Subject: Re: [Emc-users] Lathe Threading On 19 May 2014 08:27, Dave Caroline dave.thearchiv...@gmail.com wrote: The ramps are essential for full strength as they remove the need for a safety groove You don't need a safety groove anyway with a conventional threading operation, the retract move seems consistent. I am prepared to believe that a taper-out might give a better stress concentration as the change in stiffness of the bolt is less sudden. The lead-in and -out probably see very little use, but at the same time there doesn't seem to be any penalty for them existing as an option. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Accelerate Dev Cycles with Automated Cross-Browser Testing - For FREE Instantly run your Selenium tests across 300+ browser/OS combos. Get unparalleled scalability from the best Selenium testing platform available Simple to use. Nothing to install. Get started now for free. http://p.sf.net/sfu/SauceLabs ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Lathe Threading
I'm still not seeing why G76 has a entry and exit ramp. I believe the intent was to deal with Z acceleration time where the helix is not valid at the start (and I assume the end) of synchronized motion. Normally, one would start the thread off the part enough to have the Z and spindle locations synchronize in air. For threads that need to start in the material rather than air, ramping may be used to ease into the thread until the helix is correct. But the way I see it, either way there will be a bit of bad helix at the start and end of the thread. Ramping-in cuts less material, so may get in the way more than plunge-and-go. Channeling before threading, so any material left will only have valid helix, seems better. I would like to know if there is any situation where ramping would be better than channeling or plunging. -- Kirk Wallace -- Accelerate Dev Cycles with Automated Cross-Browser Testing - For FREE Instantly run your Selenium tests across 300+ browser/OS combos. Get unparalleled scalability from the best Selenium testing platform available Simple to use. Nothing to install. Get started now for free. http://p.sf.net/sfu/SauceLabs ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On Sun, 18 May 2014 12:45:08 -0700, you wrote: I'm still not seeing why G76 has a entry and exit ramp. I believe the intent was to deal with Z acceleration time where the helix is not valid at the start (and I assume the end) of synchronized motion. Normally, one would start the thread off the part enough to have the Z and spindle locations synchronize in air. Absolutely. You start the thread in air so the tool is at correct feed/speed combination when it contacts the material. A good CAM program can work this distance out for you. Normally in the machine setup you tell it what the max feeds and acceleration are and you are able to enter a tolerance value so you have a little leeway. Otherwise you guess. For threads that need to start in the material rather than air, ramping may be used to ease into the thread until the helix is correct. But the way I see it, either way there will be a bit of bad helix at the start and end of the thread. Ramping-in cuts less material, so may get in the way more than plunge-and-go. Channeling before threading, so any material left will only have valid helix, seems better. I would like to know if there is any situation where ramping would be better than channeling or plunging. If the thread starts in the job, often parts are designed so there is a clearance groove in, out or both on the thread, a plunge can be made as long as the tool can accelerate to the correct feed within that groove. If that's not possible or desired a ramp in move in/out can be done, but the tool has to be at the correct feed when it hits the work - as long as the pitch of the thread doesn't alter, it's fine. Steve Blackmore -- -- Accelerate Dev Cycles with Automated Cross-Browser Testing - For FREE Instantly run your Selenium tests across 300+ browser/OS combos. Get unparalleled scalability from the best Selenium testing platform available Simple to use. Nothing to install. Get started now for free. http://p.sf.net/sfu/SauceLabs ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Yes, I am supplying from an external source and have the jumper set so that the encoder is powered by the external source. I have to buy another encoder anyway for my live tooling - so I will get one and see if that fixes the problem... On Mon, Jun 11, 2012 at 6:39 PM, Dave e...@dc9.tzo.com wrote: Are you supplying the 7i33 board with a 5v power source? If so do you have the jumper on the power jumper in the right position? On 6/11/2012 7:26 PM, Brian May wrote: I believe i have it correct. (actually i hope i do not so i can avoid buying an encoder...) I have all the wires going into the correct connection on the mesa board. The A A0, B B0, Z Z0, +5v and ground Sent from my iPod On Jun 11, 2012, at 10:58 AM, John Thorntonbjt...@gmail.com wrote: Do you have it wired up as TTL? John On 6/11/2012 11:44 AM, Brian May wrote: that is the correct encoder. I just verified the part number on the encoder itself. It was working for measuring RPM with the jumper in the TTL position (Where it has been the whole time). I just moved it to the Differential position and it still measures rpm fine. But, the index is still not working for the threading... However, I am learning this as I go and not sure if I need to do something different since it is a differential line driver type encoder? Thanks for the help Brian On Sat, Jun 9, 2012 at 8:40 PM, Davee...@dc9.tzo.com wrote: Except that the encoder is not a TTL output encoder but a differential line driver model encoder: http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD TRD-N1024-RZVWD http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD%0ATRD-N1024-RZVWD Brian are you sure this is the correct part number for your encoder? Automation Direct sells a very similar encoder but with single ended TTL outputs. The jumpers on the Mesa card has to correspond to the encoder type (differential line driver or TTL) otherwise nothing will work right. Dave On 6/9/2012 3:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all
Re: [Emc-users] Lathe Threading
On 06/09/2012 12:21 PM, sam sokolik wrote: Your not still running the index through classic ladder - are you? (1ms refresh rate is going to kill your speed) On 06/09/2012 02:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace Those should be nice encoders; a step above the ones I use but these are not differential. Encoder, incremental, 50mm diameter body, 1024 pulses per revolution, 5-30 VDC, push-pull output. Maybe a higher bias would help. My typical encoder is the TRD-S2500-VD 5 v. differential and they are rock solid. Dave -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Except that the encoder is not a TTL output encoder but a differential line driver model encoder: http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD TRD-N1024-RZVWD Brian are you sure this is the correct part number for your encoder? Automation Direct sells a very similar encoder but with single ended TTL outputs. The jumpers on the Mesa card has to correspond to the encoder type (differential line driver or TTL) otherwise nothing will work right. Dave On 6/9/2012 3:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
that is the correct encoder. I just verified the part number on the encoder itself. It was working for measuring RPM with the jumper in the TTL position (Where it has been the whole time). I just moved it to the Differential position and it still measures rpm fine. But, the index is still not working for the threading... However, I am learning this as I go and not sure if I need to do something different since it is a differential line driver type encoder? Thanks for the help Brian On Sat, Jun 9, 2012 at 8:40 PM, Dave e...@dc9.tzo.com wrote: Except that the encoder is not a TTL output encoder but a differential line driver model encoder: http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD TRD-N1024-RZVWDhttp://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD%0ATRD-N1024-RZVWD Brian are you sure this is the correct part number for your encoder? Automation Direct sells a very similar encoder but with single ended TTL outputs. The jumpers on the Mesa card has to correspond to the encoder type (differential line driver or TTL) otherwise nothing will work right. Dave On 6/9/2012 3:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Do you have it wired up as TTL? John On 6/11/2012 11:44 AM, Brian May wrote: that is the correct encoder. I just verified the part number on the encoder itself. It was working for measuring RPM with the jumper in the TTL position (Where it has been the whole time). I just moved it to the Differential position and it still measures rpm fine. But, the index is still not working for the threading... However, I am learning this as I go and not sure if I need to do something different since it is a differential line driver type encoder? Thanks for the help Brian On Sat, Jun 9, 2012 at 8:40 PM, Davee...@dc9.tzo.com wrote: Except that the encoder is not a TTL output encoder but a differential line driver model encoder: http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD TRD-N1024-RZVWDhttp://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD%0ATRD-N1024-RZVWD Brian are you sure this is the correct part number for your encoder? Automation Direct sells a very similar encoder but with single ended TTL outputs. The jumpers on the Mesa card has to correspond to the encoder type (differential line driver or TTL) otherwise nothing will work right. Dave On 6/9/2012 3:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
I believe i have it correct. (actually i hope i do not so i can avoid buying an encoder...) I have all the wires going into the correct connection on the mesa board. The A A0, B B0, Z Z0, +5v and ground Sent from my iPod On Jun 11, 2012, at 10:58 AM, John Thornton bjt...@gmail.com wrote: Do you have it wired up as TTL? John On 6/11/2012 11:44 AM, Brian May wrote: that is the correct encoder. I just verified the part number on the encoder itself. It was working for measuring RPM with the jumper in the TTL position (Where it has been the whole time). I just moved it to the Differential position and it still measures rpm fine. But, the index is still not working for the threading... However, I am learning this as I go and not sure if I need to do something different since it is a differential line driver type encoder? Thanks for the help Brian On Sat, Jun 9, 2012 at 8:40 PM, Davee...@dc9.tzo.com wrote: Except that the encoder is not a TTL output encoder but a differential line driver model encoder: http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD TRD-N1024-RZVWDhttp://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD%0ATRD-N1024-RZVWD Brian are you sure this is the correct part number for your encoder? Automation Direct sells a very similar encoder but with single ended TTL outputs. The jumpers on the Mesa card has to correspond to the encoder type (differential line driver or TTL) otherwise nothing will work right. Dave On 6/9/2012 3:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed
Re: [Emc-users] Lathe Threading
Differential line driver and Differential when it comes to encoders are usually one in the same. TTL and Differential are two entirely different things. There is only one TTL/Differential jumper per encoder channel on the 7i33 board. I think AD has a 1 year warranty on those encoders. If it is still in warranty, you might want to send it back. Dave On 6/11/2012 7:26 PM, Brian May wrote: I believe i have it correct. (actually i hope i do not so i can avoid buying an encoder...) I have all the wires going into the correct connection on the mesa board. The A A0, B B0, Z Z0, +5v and ground Sent from my iPod On Jun 11, 2012, at 10:58 AM, John Thorntonbjt...@gmail.com wrote: Do you have it wired up as TTL? John On 6/11/2012 11:44 AM, Brian May wrote: that is the correct encoder. I just verified the part number on the encoder itself. It was working for measuring RPM with the jumper in the TTL position (Where it has been the whole time). I just moved it to the Differential position and it still measures rpm fine. But, the index is still not working for the threading... However, I am learning this as I go and not sure if I need to do something different since it is a differential line driver type encoder? Thanks for the help Brian On Sat, Jun 9, 2012 at 8:40 PM, Davee...@dc9.tzo.com wrote: Except that the encoder is not a TTL output encoder but a differential line driver model encoder: http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD TRD-N1024-RZVWDhttp://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD%0ATRD-N1024-RZVWD Brian are you sure this is the correct part number for your encoder? Automation Direct sells a very similar encoder but with single ended TTL outputs. The jumpers on the Mesa card has to correspond to the encoder type (differential line driver or TTL) otherwise nothing will work right. Dave On 6/9/2012 3:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed
Re: [Emc-users] Lathe Threading
Are you supplying the 7i33 board with a 5v power source? If so do you have the jumper on the power jumper in the right position? On 6/11/2012 7:26 PM, Brian May wrote: I believe i have it correct. (actually i hope i do not so i can avoid buying an encoder...) I have all the wires going into the correct connection on the mesa board. The A A0, B B0, Z Z0, +5v and ground Sent from my iPod On Jun 11, 2012, at 10:58 AM, John Thorntonbjt...@gmail.com wrote: Do you have it wired up as TTL? John On 6/11/2012 11:44 AM, Brian May wrote: that is the correct encoder. I just verified the part number on the encoder itself. It was working for measuring RPM with the jumper in the TTL position (Where it has been the whole time). I just moved it to the Differential position and it still measures rpm fine. But, the index is still not working for the threading... However, I am learning this as I go and not sure if I need to do something different since it is a differential line driver type encoder? Thanks for the help Brian On Sat, Jun 9, 2012 at 8:40 PM, Davee...@dc9.tzo.com wrote: Except that the encoder is not a TTL output encoder but a differential line driver model encoder: http://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD TRD-N1024-RZVWDhttp://www.automationdirect.com/adc/Shopping/Catalog/Sensors_-z-_Encoders/Encoders/Medium_Duty_Standard_Shaft_%28TRD-N_Series%29/TRD-N1024-RZVWD%0ATRD-N1024-RZVWD Brian are you sure this is the correct part number for your encoder? Automation Direct sells a very similar encoder but with single ended TTL outputs. The jumpers on the Mesa card has to correspond to the encoder type (differential line driver or TTL) otherwise nothing will work right. Dave On 6/9/2012 3:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263
Re: [Emc-users] Lathe Threading
I looked at the configuration CHNC and it looks the same. I followed andy's advice and found that the z-pulse is on pin 4. So I connected pin 4, (Z Pulse) to an encoder component A phase (encoder.0). Then set the encoder component to counter mode. So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. It did not, It is not counting reliably. Only at like 4RPM (turning by hand) does it count reliably.. Shouldn't the threading start when it finds the Z-pulse, even though it might be inconsistent? Or does it need it to be consistent? In other words - could I just connect a button to pretend to be the Z pulse and when I press the button it starts threading? (I tried this and it did not work...) To me it looks like I either have a cable or encoder problem. But am still confused why it would not work at all since it is getting a signal every once in a while Thanks for the help Brian On Sat, Jun 9, 2012 at 5:11 AM, John Thornton bjt...@gmail.com wrote: I have my CHNC lathe converted using 5i20 7i33 7i77 and all the wiring of the cards and my config files are here if you want to compare notes. http://gnipsel.com/shop/hardinge/hardinge.xhtml John On 6/8/2012 8:39 PM, Brian May wrote: I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Brian May www.do-precision.com -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Sounds like you need a new encoder. I've seen encoders break like that - they get intermittent. I have no idea why. Dave On 6/9/2012 1:00 PM, Brian May wrote: I looked at the configuration CHNC and it looks the same. I followed andy's advice and found that the z-pulse is on pin 4. So I connected pin 4, (Z Pulse) to an encoder component A phase (encoder.0). Then set the encoder component to counter mode. So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. It did not, It is not counting reliably. Only at like 4RPM (turning by hand) does it count reliably.. Shouldn't the threading start when it finds the Z-pulse, even though it might be inconsistent? Or does it need it to be consistent? In other words - could I just connect a button to pretend to be the Z pulse and when I press the button it starts threading? (I tried this and it did not work...) To me it looks like I either have a cable or encoder problem. But am still confused why it would not work at all since it is getting a signal every once in a while Thanks for the help Brian On Sat, Jun 9, 2012 at 5:11 AM, John Thorntonbjt...@gmail.com wrote: I have my CHNC lathe converted using 5i20 7i33 7i77 and all the wiring of the cards and my config files are here if you want to compare notes. http://gnipsel.com/shop/hardinge/hardinge.xhtml John On 6/8/2012 8:39 PM, Brian May wrote: I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 11:00:22 -0600 From: Brian May bri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading I looked at the configuration CHNC and it looks the same. I followed andy's advice and found that the z-pulse is on pin 4. So I connected pin 4, (Z Pulse) to an encoder component A phase (encoder.0). Then set the encoder component to counter mode. So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. It did not, It is not counting reliably. Only at like 4RPM (turning by hand) does it count reliably.. Can you measure the Z signal with a voltmeter and very slowly turn the shaft so find the index. It sounds like maybe the signal has marginal levels. and by measuring both High and Low Z levels you can check this (though it is tricky to find the index) Shouldn't the threading start when it finds the Z-pulse, even though it might be inconsistent? Or does it need it to be consistent? In other words - could I just connect a button to pretend to be the Z pulse and when I press the button it starts threading? (I tried this and it did not work...) To me it looks like I either have a cable or encoder problem. But am still confused why it would not work at all since it is getting a signal every once in a while Thanks for the help Brian On Sat, Jun 9, 2012 at 5:11 AM, John Thornton bjt...@gmail.com wrote: I have my CHNC lathe converted using 5i20 7i33 7i77 and all the wiring of the cards and my config files are here if you want to compare notes. http://gnipsel.com/shop/hardinge/hardinge.xhtml John On 6/8/2012 8:39 PM, Brian May wrote: I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Brian May www.do-precision.com -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users Peter Wallace Mesa Electronics (\__/) (='.'=) This is Bunny. Copy and paste bunny into your ()_() signature to help him gain world domination
Re: [Emc-users] Lathe Threading
I can try that, I have a C-Axis that I can engage and turn it very slowly and use the halscope to find it. On Sat, Jun 9, 2012 at 11:54 AM, Peter C. Wallace p...@mesanet.com wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 11:00:22 -0600 From: Brian May bri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading I looked at the configuration CHNC and it looks the same. I followed andy's advice and found that the z-pulse is on pin 4. So I connected pin 4, (Z Pulse) to an encoder component A phase (encoder.0). Then set the encoder component to counter mode. So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. It did not, It is not counting reliably. Only at like 4RPM (turning by hand) does it count reliably.. Can you measure the Z signal with a voltmeter and very slowly turn the shaft so find the index. It sounds like maybe the signal has marginal levels. and by measuring both High and Low Z levels you can check this (though it is tricky to find the index) Shouldn't the threading start when it finds the Z-pulse, even though it might be inconsistent? Or does it need it to be consistent? In other words - could I just connect a button to pretend to be the Z pulse and when I press the button it starts threading? (I tried this and it did not work...) To me it looks like I either have a cable or encoder problem. But am still confused why it would not work at all since it is getting a signal every once in a while Thanks for the help Brian On Sat, Jun 9, 2012 at 5:11 AM, John Thornton bjt...@gmail.com wrote: I have my CHNC lathe converted using 5i20 7i33 7i77 and all the wiring of the cards and my config files are here if you want to compare notes. http://gnipsel.com/shop/hardinge/hardinge.xhtml John On 6/8/2012 8:39 PM, Brian May wrote: I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Brian May www.do-precision.com -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users
Re: [Emc-users] Lathe Threading
Low Level is 220mv High Level 3.12 Volts On Sat, Jun 9, 2012 at 11:54 AM, Peter C. Wallace p...@mesanet.com wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 11:00:22 -0600 From: Brian May bri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading I looked at the configuration CHNC and it looks the same. I followed andy's advice and found that the z-pulse is on pin 4. So I connected pin 4, (Z Pulse) to an encoder component A phase (encoder.0). Then set the encoder component to counter mode. So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. It did not, It is not counting reliably. Only at like 4RPM (turning by hand) does it count reliably.. Can you measure the Z signal with a voltmeter and very slowly turn the shaft so find the index. It sounds like maybe the signal has marginal levels. and by measuring both High and Low Z levels you can check this (though it is tricky to find the index) Shouldn't the threading start when it finds the Z-pulse, even though it might be inconsistent? Or does it need it to be consistent? In other words - could I just connect a button to pretend to be the Z pulse and when I press the button it starts threading? (I tried this and it did not work...) To me it looks like I either have a cable or encoder problem. But am still confused why it would not work at all since it is getting a signal every once in a while Thanks for the help Brian On Sat, Jun 9, 2012 at 5:11 AM, John Thornton bjt...@gmail.com wrote: I have my CHNC lathe converted using 5i20 7i33 7i77 and all the wiring of the cards and my config files are here if you want to compare notes. http://gnipsel.com/shop/hardinge/hardinge.xhtml John On 6/8/2012 8:39 PM, Brian May wrote: I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Brian May www.do-precision.com -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https
Re: [Emc-users] Lathe Threading
On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian May bri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Your not still running the index through classic ladder - are you? (1ms refresh rate is going to kill your speed) On 06/09/2012 02:08 PM, Peter C. Wallace wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 12:21:08 -0600 From: Brian Maybri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC)emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading Low Level is 220mv High Level 3.12 Volts Well thats valid TTL so OK (as long as the 7I33 inputs are jumpered for TTL in) So the next step in tracing it is is to see if the GPIO for Z bit is visible in halmeter when you do the same test with a 1024 line encoder you will likely miss the index with HALScope on the GPIO bit above 60 RPM, so a real scope would really help in case you are losing the signal above a certain speed Peter Wallace -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On 9 June 2012 18:00, Brian May bri...@do-precision.com wrote: So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. Â I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. Â It did not, It is not counting reliably. Â Only at like 4RPM (turning by hand) does it count reliably.. Don't worry about that, it is because the GPIO pins only get updated once a millisecond by default, so you will miss lots of pulses. You can add the gpio_read and gpio_write functions to a base-thread, but I really don't think it is worth the bother. The question is, do you see the index change state? -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
I do not have anything connected to classicladder now. I can see the index (In hal scope) when jogging the axis slowly. (By slowly I mean 4RPM). Any faster, the index is not consistent. On Sat, Jun 9, 2012 at 1:48 PM, andy pugh bodge...@gmail.com wrote: On 9 June 2012 18:00, Brian May bri...@do-precision.com wrote: So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. It did not, It is not counting reliably. Only at like 4RPM (turning by hand) does it count reliably.. Don't worry about that, it is because the GPIO pins only get updated once a millisecond by default, so you will miss lots of pulses. You can add the gpio_read and gpio_write functions to a base-thread, but I really don't think it is worth the bother. The question is, do you see the index change state? -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Brian May 506.8862.9162 (Cell) 506.2293.6375 (Office) www.do-precision.com -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On Saturday, June 09, 2012 04:11:29 PM Brian May did opine: Low Level is 220mv High Level 3.12 Volts That will satisfy ttl circuitry IF its clean, no noise allowed. Generally speaking, that will not make a cmos circuity happy as the high level isn't high enough to offer very much noise immunity. I wonder what a 10k resistor from that line up to the 5 volt rail would do? On Sat, Jun 9, 2012 at 11:54 AM, Peter C. Wallace p...@mesanet.com wrote: On Sat, 9 Jun 2012, Brian May wrote: Date: Sat, 9 Jun 2012 11:00:22 -0600 From: Brian May bri...@do-precision.com Reply-To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Lathe Threading I looked at the configuration CHNC and it looks the same. I followed andy's advice and found that the z-pulse is on pin 4. So I connected pin 4, (Z Pulse) to an encoder component A phase (encoder.0). Then set the encoder component to counter mode. So now I have the encoder using the hostmot driver and also the Z Pulse being read by the encoder component. I turned the spindle on at 120RPM and expected to read the counter of the encoder component counting 2 counts every second. It did not, It is not counting reliably. Only at like 4RPM (turning by hand) does it count reliably.. Can you measure the Z signal with a voltmeter and very slowly turn the shaft so find the index. It sounds like maybe the signal has marginal levels. and by measuring both High and Low Z levels you can check this (though it is tricky to find the index) Shouldn't the threading start when it finds the Z-pulse, even though it might be inconsistent? Or does it need it to be consistent? In other words - could I just connect a button to pretend to be the Z pulse and when I press the button it starts threading? (I tried this and it did not work...) To me it looks like I either have a cable or encoder problem. But am still confused why it would not work at all since it is getting a signal every once in a while Thanks for the help Brian On Sat, Jun 9, 2012 at 5:11 AM, John Thornton bjt...@gmail.com wrote: I have my CHNC lathe converted using 5i20 7i33 7i77 and all the wiring of the cards and my config files are here if you want to compare notes. http://gnipsel.com/shop/hardinge/hardinge.xhtml John On 6/8/2012 8:39 PM, Brian May wrote: I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net
[Emc-users] Lathe Threading
I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? -- Brian May 506.8862.9162 www.do-precision.com -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
It is wired up. I don't really know how to see if it is working.. I tried connectimg it to a io port and create a latching circuit in classicladder to see if it was sending a signal. I turned the encoder by hand and it would latch the circuit every few turns. I may have had a timing issue... So i know that there is a signal... I do not see in hal a index pin for the 5i20 component. Sent from my iPod On Jun 8, 2012, at 8:04 PM, andy pugh bodge...@gmail.com wrote: On 9 June 2012 02:39, Brian May bri...@do-precision.com wrote: Am I missing something simple? Is the encoder index channel wired up and working? -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On Friday, June 08, 2012 10:21:38 PM Brian May did opine: I am having trouble setting up threading on my lathe. At this point I am thinking my spindle encoder is bad. I have the following setup in my HAL File: net spindle-revs hm2_[HOSTMOT2](BOARD).0.encoder.01.position motion.spindle-revs net spindle-vel-fb scale.0.in motion.spindle-speed-in hm2_[HOSTMOT2](BOARD).0.encoder.01.velocity net spindle-index-enable hm2_[HOSTMOT2](BOARD).0.encoder.01.index-enable motion.spindle-index-enable My Parameters are set as follows: setphm2_[HOSTMOT2](BOARD).0.encoder.01.counter-mode 1 setphm2_[HOSTMOT2](BOARD).0.encoder.01.filter 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.index-mask-invert 0 setphm2_[HOSTMOT2](BOARD).0.encoder.01.scale 1024 For everything else, the spindle has been working fine. I have been running in G96 spindle speed mode, the RPM that the encoder reads is perfect. However, when I try and do a thread, the process never starts. The machine goes to the start point and just sits there and waits. I am assuming it is waiting for an index pulse and never receives it. From what I have read in the manuals - when the index pulse is found, the motion.spindle-revs goes to zero during a threading cycle. On my machine this never happens. It just continues to count. I ran my G-code in the lathe sim and it seems to work fine. I am using a mesa 5i20 and a 7i33 daughter board. The encoder is connected to the 7i33 board. The encoder is an automation direct TRD-N1024-RZVWD. Am I missing something simple? Possibly. The interface should have an index pulse on it, could be labeled encoder.N.Z where N is the encoder enumerator if you are using more than 1. Use the halscope to search for it. If it is feeding one of the mesa boards, there should be an index pulse there, but I am not familiar enough with the 7i33 to know which pin, or even if it sends it on to someplace hal can access. To work, I would think it would have to. Have you tried to contact Peter (mesa) about this? He'll be far more knowledgeable than I can ever be. Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene love, v.: I'll let you play with my life if you'll let me play with yours. -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On 9 June 2012 03:23, Brian May bri...@diezorlich.com wrote: I do not see in hal a index pin for the 5i20 component. You won't see it as a named pin, but all the function pins are also available as gpio. So, in dmesg after booting into the config you will see a list of all the function pins, and their corresponding gpio numbers, and you can halscope the index as a gpio input. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Ok i will try that tomorrow... Sent from my iPod On Jun 8, 2012, at 8:58 PM, andy pugh bodge...@gmail.com wrote: On 9 June 2012 03:23, Brian May bri...@diezorlich.com wrote: I do not see in hal a index pin for the 5i20 component. You won't see it as a named pin, but all the function pins are also available as gpio. So, in dmesg after booting into the config you will see a list of all the function pins, and their corresponding gpio numbers, and you can halscope the index as a gpio input. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Live Security Virtual Conference Exclusive live event will cover all the ways today's security and threat landscape has changed and how IT managers can respond. Discussions will include endpoint security, mobile security and the latest in malware threats. http://www.accelacomm.com/jaw/sfrnl04242012/114/50122263/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe threading
Andy Thanks very much for the info on setup for lathe threading, and for the link to a lot more info on the subject. I got the setup going within a few minutes after reading your proposals. The only extra thing I did was to put the input pin from my one-pulse-per- rev sensor on both the phase-A and phase-Z pins of the encoder. And now the G33 and G76 codes work. I use position-interpolation. I will fit a proper encoder on the spindle later. I am very impressed by the software and the people behind it. Thanks for the great support as well. It is quite a pleasant experience for me after having battled with other popular and cheap software for many years (of frustration). I hope I can contribute some day to this community. Regards Rudy __ Information from ESET Smart Security, version of virus signature database 4872 (20100216) __ The message was checked by ESET Smart Security. http://www.eset.com -- SOLARIS 10 is the OS for Data Centers - provides features such as DTrace, Predictive Self Healing and Award Winning ZFS. Get Solaris 10 NOW http://p.sf.net/sfu/solaris-dev2dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Kirk Wallace wrote: This is what I got with 2.3.0 and the previous threading sample with 4=0.08333 at 400 RPM: http://www.wallacecompany.com/machine_shop/HNC/HALscope_2.3_threading.png Previous (2.2.8): http://www.wallacecompany.com/machine_shop/HNC/4at08-2.png 2.3.0 seems to be much better, but the HALscope is still interesting. It seems to get more unstable as the cut progresses? Well, the spindle is loaded down with the cutting effort, and may have some vibration due to that. The Z axis may be trying to follow those small fluctuations. Before, I think there was a LOT of low-pass filtering on the spindle velocity, which may have been part of the problem. Jon -- Crystal Reports #45; New Free Runtime and 30 Day Trial Check out the new simplified licensign option that enables unlimited royalty#45;free distribution of the report engine for externally facing server and web deployment. http://p.sf.net/sfu/businessobjects ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Sun, 2009-04-26 at 11:33 -0500, Jon Elson wrote: Kirk Wallace wrote: This is what I got with 2.3.0 and the previous threading sample with 4=0.08333 at 400 RPM: http://www.wallacecompany.com/machine_shop/HNC/HALscope_2.3_threading.png Previous (2.2.8): http://www.wallacecompany.com/machine_shop/HNC/4at08-2.png 2.3.0 seems to be much better, but the HALscope is still interesting. It seems to get more unstable as the cut progresses? Well, the spindle is loaded down with the cutting effort, and may have some vibration due to that. The Z axis may be trying to follow those small fluctuations. Before, I think there was a LOT of low-pass filtering on the spindle velocity, which may have been part of the problem. Jon If it makes any difference, I was cutting air, but I can imagine that there are other hardware load sources. I should do more testing on cutting real threads, but my guess is that what I have is good enough, and with some effort could get better. I certainly can use much less lead in, with higher RPM. -- Kirk Wallace http://www.wallacecompany.com/machine_shop/ http://www.wallacecompany.com/E45/index.html California, USA -- Crystal Reports #45; New Free Runtime and 30 Day Trial Check out the new simplified licensign option that enables unlimited royalty#45;free distribution of the report engine for externally facing server and web deployment. http://p.sf.net/sfu/businessobjects ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Wed, 2009-04-22 at 18:38 -0500, Chris Radek wrote: On Wed, Apr 22, 2009 at 02:04:55PM -0700, Kirk Wallace wrote: I tend to think my threading problem is due to the relay runner effect I think so too - sure looks nasty though. I bet you will have much better luck with 2.3 (this effect is why I rewrote the threading sync.) This is what I got with 2.3.0 and the previous threading sample with 4=0.08333 at 400 RPM: http://www.wallacecompany.com/machine_shop/HNC/HALscope_2.3_threading.png Previous (2.2.8): http://www.wallacecompany.com/machine_shop/HNC/4at08-2.png 2.3.0 seems to be much better, but the HALscope is still interesting. It seems to get more unstable as the cut progresses? Another note, when I loaded 2.3.0, I got a .axis_preferences file permission error while trying to start EMC2. I rooted, then changed the file owner from root to me. Then my X axis got a homing error, something like switch inactive before reversal(?). I reduced the homing rates a little, which did the trick. Now, I have new features and better threading. Thank you. -- Kirk Wallace http://www.wallacecompany.com/machine_shop/ http://www.wallacecompany.com/E45/index.html California, USA -- Crystal Reports #45; New Free Runtime and 30 Day Trial Check out the new simplified licensign option that enables unlimited royalty#45;free distribution of the report engine for externally facing server and web deployment. http://p.sf.net/sfu/businessobjects ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Mon, 2009-04-20 at 20:56 -0500, Jon Elson wrote: ... snip That is in the univpwm_load.hal file, the line I have reads : loadrt [EMCMOT]EMCMOT base_period_nsec=[EMCMOT]BASE_PERIOD servo_period_nsec=[EMCMOT]SERVO_PERIOD traj_period_nsec=[EMCMOT]SERVO_PERIOD key=[EMCMOT]SHMEM_KEY You might try that with the same conditions of your picture posted above and see if it helps. Jon I tend to think my threading problem is due to the relay runner effect, but just in case it might be helpful. I tried the above on my HNC. This didn't seem to change much. This is the before, with 4=0.08333: http://www.wallacecompany.com/machine_shop/HNC/4at08-2.png This is with TRAJ = SERVO_PERIOD and 4=0.08333: http://www.wallacecompany.com/machine_shop/HNC/traj-servo_period-1a.png If I have enough lead in, for the spindle RPM I am using, it's not a problem. -- Kirk Wallace http://www.wallacecompany.com/machine_shop/ http://www.wallacecompany.com/E45/index.html California, USA -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Wed, Apr 22, 2009 at 02:04:55PM -0700, Kirk Wallace wrote: I tend to think my threading problem is due to the relay runner effect I think so too - sure looks nasty though. I bet you will have much better luck with 2.3 (this effect is why I rewrote the threading sync.) -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Kirk Wallace wrote: I tend to think my threading problem is due to the relay runner effect, but just in case it might be helpful. I tried the above on my HNC. This didn't seem to change much. This is the before, with 4=0.08333: http://www.wallacecompany.com/machine_shop/HNC/4at08-2.png This is with TRAJ = SERVO_PERIOD and 4=0.08333: http://www.wallacecompany.com/machine_shop/HNC/traj-servo_period-1a.png If I have enough lead in, for the spindle RPM I am using, it's not a problem. That zig-zag white line is the Z velocity? Yikes, that definitely is NOT right. Do the zig-zags get smaller if you turn down the spindle RPM? Chris Radek said they had just committed a change to the spindle sync move that is supposed to help. So, you might want to try a checkout of the trunk and see if it does better. Jon -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Kirk Wallace wrote: I think in my case at least, I'm asking for impossible accelerations. When I looked at this before: http://www.wallacecompany.com/cnc_lathe/HNC/emc2/spindle_sync_surge-1b.png I decided to allow enough lead-in to have the Z settle before cutting. Well, the spindle sync doesn't really know how much lead-in you have. Richard Harris was having a problem where the Z axis just blasted at full rapid speed from beginning to end of the thread length, as I understand it. In any case, the Z axis needs some distance to accelerate, and there is no way to get around that. So, I gather that in your case, the Z feed stabilizes after some distance and you get the correct thread pitch. Is that correct? If I properly understand Mr. Harris' problem, his Z feed does NOT stabilize, but just runs ahead at full speed to the finish Z position. That would indicate the spindle encoder count is at some large value, and did not reset to zero when the index pulse ocurred. I'm still trying to understand the problem, and why I'm not seeing it here. One other thing We found this change to be MOST helpful for rigid tapping, but I believe it ALSO is very helpful in any threading operation. That was to increase the trajectory planner's dispatch rate (TRAJ_PERIOD) to equal the servo rate. That is in the univpwm_load.hal file, the line I have reads : loadrt [EMCMOT]EMCMOT base_period_nsec=[EMCMOT]BASE_PERIOD servo_period_nsec=[EMCMOT]SERVO_PERIOD traj_period_nsec=[EMCMOT]SERVO_PERIOD key=[EMCMOT]SHMEM_KEY You might try that with the same conditions of your picture posted above and see if it helps. Jon -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Mon, 2009-04-20 at 20:56 -0500, Jon Elson wrote: ... snip One other thing We found this change to be MOST helpful for rigid tapping, but I believe it ALSO is very helpful in any threading operation. That was to increase the trajectory planner's dispatch rate (TRAJ_PERIOD) to equal the servo rate. That is in the univpwm_load.hal file, the line I have reads : loadrt [EMCMOT]EMCMOT base_period_nsec=[EMCMOT]BASE_PERIOD servo_period_nsec=[EMCMOT]SERVO_PERIOD traj_period_nsec=[EMCMOT]SERVO_PERIOD key=[EMCMOT]SHMEM_KEY You might try that with the same conditions of your picture posted above and see if it helps. Jon I think that might explain the zig-zag nature of my Z position trace. I wonder if Harris' rapid is fast enough to get across the thread, where in my tests I got half way (4=0.08333) before the HNC tried to correct the rate? If I used 4=0.120 I might have gotten the same result, since decreasing 4 also reduced the effect. -- Kirk Wallace http://www.wallacecompany.com/machine_shop/ http://www.wallacecompany.com/E45/index.html California, USA -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Kirk Wallace wrote: I wonder if Harris' rapid is fast enough to get across the thread, where in my tests I got half way (4=0.08333) before the HNC tried to correct the rate? If I used 4=0.120 I might have gotten the same result, since decreasing 4 also reduced the effect. As I mentioned to Jon when I saw him at NAMES, I am almost 100% sure that Mr. Wallace and Mr. Harris are NOT dealing with the same problem. Trying to find similarities between the two sets of symptoms will just send you down the rabbit hole. I strongly suggest that you completely ignore everything about the Harris problem. I'm almost sure that Kirk's problem is the can't accelerate instantly problem that I tried to explain a couple days ago with my relay race metaphor. I'd suggest reducing the spindle speed while keeping everything else the same, and see what happens. The Harris problem is almost certainly a failure of either the PPMC hardware, or the associated driver. I think it is reporting that it got an index pulse, but not clearing the count, possibly due to an obscure race condition. The ONLY way to make any progress on that front is for Mr. Harris to get a halscope trace - that will be the smoking gun that tells us what to do next. Regards, John Kasunich -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Kirk Wallace wrote: Whatever it is, it looks like I have it too. I ran the long version four times with #4=0.050 without any problems. Then before shutting down for the night, I ran one part at #4=0.08. At the start of the thread the Z would aggressively move then almost come to a stop in the middle of the pass, then surge again and nearly stop at the end of the pass. I let the thread loop go for a five or six more passes. Each pass followed the previous with a slight variation. I know I should do some HALscope captures, but I haven't used HALscope for a while so I need to plan out what I need to do. I am running 6.06 with all of the automatic updates as of today. I can get into more detail later. My lathe configuration is here: http://www.wallacecompany.com/cnc_lathe/HNC/ OK, any data is better than no data, even if it means trouble! So, we need to know EMC version, controller board version (on the EPROM at U4) and also what speed the spindle was running at. Can you run it at slightly finer pitch? I am strongly suspecting, despite what Richard Harris wrote, that this has to be a problem somewhere in EMC, as the ppmc driver and the controller board have no way to know what thread is ABOUT to be cut. Any halscope traces that show the behavior of the pins ppmc.0.encoder.0x.index-enable (the X represents whichever encoder channel has the spindle on it) or motion.spindle-index-enable and ppmc.0.encoder.0x.position or motion.spindle-revs should be quite useful. First, we have to determine if somehow the UPC board is saying it saw the index pulse, but not resetting the spindle position count. One possibility is some condition is clearing the index-enable signal from software instead of letting the encoder counter find the index. I wish I could see this problem here, then I could dig in until I find the source. Jon -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Thu, 16 Apr 2009 22:40:07 -0700, you wrote: which sets up for 20 TPI. I ran it like that first, then changed the value to .08333 to get 12 TPI. Just a thought - try changing that 0.08333 to 0.084 and see if it still misbehaves. Steve Blackmore -- -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Fri, 2009-04-17 at 11:38 -0500, Jon Elson wrote: Kirk Wallace wrote: Whatever it is, it looks like I have it too. I ran the long version four times with #4=0.050 without any problems. Then before shutting down for the night, I ran one part at #4=0.08. At the start of the thread the Z would aggressively move then almost come to a stop in the middle of the pass, then surge again and nearly stop at the end of the pass. I let the thread loop go for a five or six more passes. Each pass followed the previous with a slight variation. I know I should do some HALscope captures, but I haven't used HALscope for a while so I need to plan out what I need to do. I am running 6.06 with all of the automatic updates as of today. I can get into more detail later. My lathe configuration is here: http://www.wallacecompany.com/cnc_lathe/HNC/ OK, any data is better than no data, even if it means trouble! So, we need to know EMC version, 2.2.8 controller board version (on the EPROM at U4) USC (with UPC chip) SN:0047 Rev. 2.2 9/1/2005 and also what speed the spindle was running at. 400 RPM Can you run it at slightly finer pitch? .080 to .060 decreases the effect I am strongly suspecting, despite what Richard Harris wrote, that this has to be a problem somewhere in EMC, as the ppmc driver and the controller board have no way to know what thread is ABOUT to be cut. Any halscope traces that show the behavior of the pins ppmc.0.encoder.0x.index-enable (the X represents whichever encoder channel has the spindle on it) or motion.spindle-index-enable and ppmc.0.encoder.0x.position or motion.spindle-revs should be quite useful. HALscope screen shots: http://www.wallacecompany.com/machine_shop/HNC/4at08-1.png http://www.wallacecompany.com/machine_shop/HNC/4at08-2.png First, we have to determine if somehow the UPC board is saying it saw the index pulse, but not resetting the spindle position count. One possibility is some condition is clearing the index-enable signal from software instead of letting the encoder counter find the index. I wish I could see this problem here, then I could dig in until I find the source. Jon I think in my case at least, I'm asking for impossible accelerations. When I looked at this before: http://www.wallacecompany.com/cnc_lathe/HNC/emc2/spindle_sync_surge-1b.png I decided to allow enough lead-in to have the Z settle before cutting. -- Kirk Wallace http://www.wallacecompany.com/machine_shop/ http://www.wallacecompany.com/E45/index.html California, USA -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Wed, 2009-04-15 at 11:20 -0500, Jon Elson wrote: Kirk Wallace wrote: On Tue, 2009-04-14 at 20:57 -0500, Jon Elson wrote: ... snip problem, but I made the final fix at the 2007 EMC-Fest, and the driver fixes were in the July 2007 release of EMC2. So, I wanted to see if anyone else was seeing similar problems. Also, I don't see why the spindle sync would care what thread pitch he is cutting! That makes no sense to me at all. Jon Should I try a test on my machine? If so what would it look like? There is a test file, threading.ngc, in the /usr/share/emc/ncfiles directory. (There may be another version of this file that is MUCH shorter, about 15 lines. But, I have been working with the longer one in the /usr/share dir.) Anyway, in the longer one, about halfway down, is #4=0.05 (thread pitch) which sets up for 20 TPI. I ran it like that first, then changed the value to .08333 to get 12 TPI. You can also twiddle with the lead-in, lead-out scheme and the depth of cut. I left it with a very small increment (#2=) so I'd get a lot of passes, to see if anything went wrong. I had no failures here. I'd greatly appreciate your trying it there, just to see if there is some random problem. I cannot understand how the spindle sync would work prefectly for hundreds of parts at ~20 TPI and fail on roughly 50% (I think he said that in an earlier message) at 12 TPI. The spindle sync function has no way of knowing what the thread pitch will be! Thanks, Jon Whatever it is, it looks like I have it too. I ran the long version four times with #4=0.050 without any problems. Then before shutting down for the night, I ran one part at #4=0.08. At the start of the thread the Z would aggressively move then almost come to a stop in the middle of the pass, then surge again and nearly stop at the end of the pass. I let the thread loop go for a five or six more passes. Each pass followed the previous with a slight variation. I know I should do some HALscope captures, but I haven't used HALscope for a while so I need to plan out what I need to do. I am running 6.06 with all of the automatic updates as of today. I can get into more detail later. My lathe configuration is here: http://www.wallacecompany.com/cnc_lathe/HNC/ -- Kirk Wallace http://www.wallacecompany.com/machine_shop/ http://www.wallacecompany.com/E45/index.html California, USA -- Stay on top of everything new and different, both inside and around Java (TM) technology - register by April 22, and save $200 on the JavaOne (SM) conference, June 2-5, 2009, San Francisco. 300 plus technical and hands-on sessions. Register today. Use priority code J9JMT32. http://p.sf.net/sfu/p ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Kirk Wallace wrote: On Tue, 2009-04-14 at 20:57 -0500, Jon Elson wrote: ... snip problem, but I made the final fix at the 2007 EMC-Fest, and the driver fixes were in the July 2007 release of EMC2. So, I wanted to see if anyone else was seeing similar problems. Also, I don't see why the spindle sync would care what thread pitch he is cutting! That makes no sense to me at all. Jon Should I try a test on my machine? If so what would it look like? There is a test file, threading.ngc, in the /usr/share/emc/ncfiles directory. (There may be another version of this file that is MUCH shorter, about 15 lines. But, I have been working with the longer one in the /usr/share dir.) Anyway, in the longer one, about halfway down, is #4=0.05 (thread pitch) which sets up for 20 TPI. I ran it like that first, then changed the value to .08333 to get 12 TPI. You can also twiddle with the lead-in, lead-out scheme and the depth of cut. I left it with a very small increment (#2=) so I'd get a lot of passes, to see if anything went wrong. I had no failures here. I'd greatly appreciate your trying it there, just to see if there is some random problem. I cannot understand how the spindle sync would work prefectly for hundreds of parts at ~20 TPI and fail on roughly 50% (I think he said that in an earlier message) at 12 TPI. The spindle sync function has no way of knowing what the thread pitch will be! Thanks, Jon -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Mon, 13 Apr 2009 21:48:40 -0500, you wrote: I just ran several pieces at 12 TPI, using a program derived from the EMC sample program threading.ngc Have you tried with plain Gcode? That is a horribly complex piece of code and it's possible the error may be associated with the math involved. I think the math is trying to do constant volume cuts, but I certainly wouldn't do that on the fly. It would be easier to see where the error lies if the code was a series of lines, at least you can then narrow it to a particular move, or not, as the case might be. So, does anyone else have experience with lathe threading or rigid tapping at 12 or less TPI? I don't see why that should matter to the encoder counter reset on index function, but that is what Mr. Harris reports. I've run many 1.5 and 2mm pitch threads in testing over the last few days without any problems. My encoder count is much less though at 90 ppr and spindle speeds tried have been 500 to 1000 rpm. Steve Blackmore -- -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Steve Blackmore wrote: On Mon, 13 Apr 2009 21:48:40 -0500, you wrote: I just ran several pieces at 12 TPI, using a program derived from the EMC sample program threading.ngc Have you tried with plain Gcode? That is a horribly complex piece of code and it's possible the error may be associated with the math involved. But, It woks FINE for me! I have not yet gotten a copy of Mr. Harris' code, so have no idea how he has programmed his threading, where he IS havig this problem. I think the math is trying to do constant volume cuts, but I certainly wouldn't do that on the fly. It would be easier to see where the error lies if the code was a series of lines, at least you can then narrow it to a particular move, or not, as the case might be. So, does anyone else have experience with lathe threading or rigid tapping at 12 or less TPI? I don't see why that should matter to the encoder counter reset on index function, but that is what Mr. Harris reports. I've run many 1.5 and 2mm pitch threads in testing over the last few days without any problems. My encoder count is much less though at 90 ppr and spindle speeds tried have been 500 to 1000 rpm. What version of EMC are you using? Jon -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Tue, 14 Apr 2009 12:28:48 -0500, you wrote: Have you tried with plain Gcode? That is a horribly complex piece of code and it's possible the error may be associated with the math involved. But, It woks FINE for me! I thought YOU said One interesting quirk I did see was that the finish end of the thread was compressed to a higher TPI. What version of EMC are you using? 2.3.0 beta2 I've not seen any compression in pitch, or any other problem for that matter, and I've been deliberately trying to break it to see how robust EMC's threading is. The only thing I've not done yet is trying to thread with a faster spindle speed/higher pitch combination than the max Z velocity can handle. I would expect some sort of error message and a stop. Steve Blackmore -- -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
Steve Blackmore wrote: On Tue, 14 Apr 2009 12:28:48 -0500, you wrote: Have you tried with plain Gcode? That is a horribly complex piece of code and it's possible the error may be associated with the math involved. But, It woks FINE for me! I thought YOU said One interesting quirk I did see was that the finish end of the thread was compressed to a higher TPI. Yes, that's right. I thought it was a minor quirk, and due to the complexity of the threading.ngc code, I didn't take the time to really figure out how the lead-out was being done. This might be something that the recent improvements in EMC take care of. What version of EMC are you using? 2.3.0 beta2 I've not seen any compression in pitch, or any other problem for that matter, and I've been deliberately trying to break it to see how robust EMC's threading is. The only thing I've not done yet is trying to thread with a faster spindle speed/higher pitch combination than the max Z velocity can handle. I would expect some sort of error message and a stop. That's the funny thing, this thread is definitely not beyond the Z axis max feed rate, as the good part of the thread proves. So, it has to be the slow-down at the end of the thread. I have to look at how this is coded to see how much distance it is allowing for the Z motion to stop at the end. I think it pulls the tool back at a 45 degree angle, but if it was hard-coded for a fine thread, then it may not be allowing enough distance for the Z to decelerate as the X pulls back. As I say, I haven't really deciphered the code. My real concern is Mr. Harris' problem with the encoder counter sometimes missing the reset on index, while it sets the bit saying that it has done so. An earlier version of the firmware/driver had this problem, but I made the final fix at the 2007 EMC-Fest, and the driver fixes were in the July 2007 release of EMC2. So, I wanted to see if anyone else was seeing similar problems. Also, I don't see why the spindle sync would care what thread pitch he is cutting! That makes no sense to me at all. Jon -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Tue, 2009-04-14 at 20:57 -0500, Jon Elson wrote: ... snip problem, but I made the final fix at the 2007 EMC-Fest, and the driver fixes were in the July 2007 release of EMC2. So, I wanted to see if anyone else was seeing similar problems. Also, I don't see why the spindle sync would care what thread pitch he is cutting! That makes no sense to me at all. Jon Should I try a test on my machine? If so what would it look like? -- Kirk Wallace http://www.wallacecompany.com/machine_shop/ http://www.wallacecompany.com/E45/index.html California, USA -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
I'm quoting a message from an EMC user to see if anyone else has seen any signs of this problem. richard harris wrote: Jon, i got a chance to run halscope today and on coarse threads 13 tpi it will occasionally not reset the encoder count, count is numerically low when it does reset 25k. I do not see this when i run fine threads 18 tpi. When the count does not reset the threading cycle will rapid the tool. I verified that I am running emc2 2.2.6, UPC SN 33 rev 2.3, US digital 500 line encoder in a shielded cable with one side of the cable grounded. What should I look for in halscope to further diagnose the problem? I just ran several pieces at 12 TPI, using a program derived from the EMC sample program threading.ngc One interesting quirk I did see was that the finish end of the thread was compressed to a higher TPI. I re-ran it at lower spindle speed and it was fine. I'm not sure how that particular program figures out how soon to pull out at the end. It shows up on the coarser threads due to the Z motion beginning to decelerate earlier, I'm guessing? Anyway, I don't know how many passes the sample program performs, it looks like about 20. So, I have run it for at least 40 passes here without ANY blips at all. How occasionally is it? Once per thousand or once in ten passes? I am NOT running 2.2.6 here, the directory says 2.2.7, but I'm sure this was compiled from CVS source on 11/29/2008. I am also using a much finer resolution encoder, it has 1728 lines, or 6912 counts/rev. That also shouldn't make any difference. What is the date code either scribed or on a printed label on the EPROM chip (U4) on the UPC? The final version for those older boards with the 5V FPGA chip was 5/2/07. But, that is the same version I am using on my minimill to test this problem. Finally, after thinking about this some, I find NO WAY the UPC board's encoder counter can POSSIBLY know what TPI thread you want to cut! That simply doesn't make sense. All it could possibly be affected by is spindle RPM, and the possibility that your encoder index pulse is somehow different at different RPM. I have certainly seen the rapid effect when the encoder fails to start from zero when the driver believes that the encoder DID see the index pulse. That is not supposed to happen with the latest UPC firmware. One last thing, coarser threads require more spindle HP, and probably more Z-axis power, too. Any possibility that more load on these motors could increase system noise? Have you run the diagnostic program in the commtest mode? If the diags show communication errors between the PC and the UPC, all bets are off! You might need to run the tests with the spindle drive on. Jon _ end of quote and my reply Anyway, I am running a different version of EMC here, compiled from CVS on 11/29/2008. Richard is apparently running an older version, 2.2.6 says it was released on 10-Aug-08, but I don't know when the code was actually locked up for that. But, it should still be recent enough to have all the changes that were important, as of about July 2007. So, does anyone else have experience with lathe threading or rigid tapping at 12 or less TPI? I don't see why that should matter to the encoder counter reset on index function, but that is what Mr. Harris reports. Jon -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Mon, Apr 13, 2009 at 09:48:40PM -0500, Jon Elson wrote: richard harris wrote: Jon, i got a chance to run halscope today and on coarse threads 13 tpi it will occasionally not reset the encoder count, count is numerically low when it does reset 25k. I do not see this when i run fine threads 18 tpi. When the count does not reset the threading cycle will rapid the tool. I would love to see plots of the behavior showing at least delta, index-enable, index, and count. -- This SF.net email is sponsored by: High Quality Requirements in a Collaborative Environment. Download a free trial of Rational Requirements Composer Now! http://p.sf.net/sfu/www-ibm-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Fri, 2009-03-20 at 23:42 -0500, Jon Elson wrote: ... snip have such a problem. Kirk Wallace is also using a UPC board on a lathe, but I don't know if he is doing a lot of threading. Maybe you should send me your threading program and I will try it here on the minimill. Is your machine natively defined in mm units or inch units? It shouldn't make a difference, but I'm pulling at straws, here. Jon Sorry Jon, I haven't done allot of threading. I have had no trouble, other than early in the conversion, I had a spindle encoder noise problem (solved with VFD filter) and finding the proper acceleration tuning to deal with lead-in oscillations. I don't recall having a runaway, other than when I had the buggy homing software version. I wonder if there is a way to have the software predict what a reasonable move would be and compare this with what the sensors indicate. In other words, for a particular command, it might be unreasonable to move above a certain rate and distance to complete the block. Or, maybe it could be user assigned: G?? (safe zone) X1 xxx Y1 xxx Z1 xxx X2 xxx Y2 xxx Z2 xxx J (any max. distance from block start) xxx ... G?? (safe zone end). - Kirk http://www.wallacecompany.com/machine_shop/ -- Apps built with the Adobe(R) Flex(R) framework and Flex Builder(TM) are powering Web 2.0 with engaging, cross-platform capabilities. Quickly and easily build your RIAs with Flex Builder, the Eclipse(TM)based development software that enables intelligent coding and step-through debugging. Download the free 60 day trial. http://p.sf.net/sfu/www-adobe-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Lathe Threading Issues
I am running Elson's servo system and EMC 2.2.6. Over the last few days I have run several hundred parts single point threading a M22x1.5 threads without a single bad thread. Yesterday I switched to cutting a M20x2.5 and suddenly on ever other part the lathe will rapid during a cut. I had a similar issues months back and upgraded EMC to 2.2.6 and the issue went away. The lathe will go to the start the thread it will do a brief pause for the index pulse and shoot off at G0 through the part. I went back to my M22 code and ran 30 parts without fail, I even reduced the spindle speed to what I am cutting the M20 at thinking I might get more noise from the VFD at the lower end of the rpm band and no effect. I also increased the number of passes on the M22 program to replicate the M20 program and no failures. Switched back to the M22 program and the second part experienced a rapid on the spring pass. Any ideas what could be the cause? Is there a way to set EMC to never attempt a threading pass that is faster than the G0 velocity? Thanks, Richard -- Apps built with the Adobe(R) Flex(R) framework and Flex Builder(TM) are powering Web 2.0 with engaging, cross-platform capabilities. Quickly and easily build your RIAs with Flex Builder, the Eclipse(TM)based development software that enables intelligent coding and step-through debugging. Download the free 60 day trial. http://p.sf.net/sfu/www-adobe-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
On Fri, Mar 20, 2009 at 03:15:41PM -0700, richard harris wrote: I am running Elson's servo system and EMC 2.2.6. Over the last few days I have run several hundred parts single point threading a M22x1.5 threads without a single bad thread. Yesterday I switched to cutting a M20x2.5 and suddenly on ever other part the lathe will rapid during a cut. I had a similar issues months back and upgraded EMC to 2.2.6 and the issue went away. The lathe will go to the start the thread it will do a brief pause for the index pulse and shoot off at G0 through the part. I went back to my M22 code and ran 30 parts without fail, I even reduced the spindle speed to what I am cutting the M20 at thinking I might get more noise from the VFD at the lower end of the rpm band and no effect. I also increased the number of passes on the M22 program to replicate the M20 program and no failures. I looked here http://wiki.linuxcnc.org/cgi-bin/emcinfo.pl?Released and do not see any relevant changes in PPMC since July 2007. This smells like an index problem. The thing that can cause it is when, due to a driver bug, the driver reports an index pulse has occurred but it doesn't reset its count. PPMC had this problem in 2007 but it is long since fixed to the best of our knowledge. MAYBE there is still one more bug lurking in this driver. Your task now is to capture the failure on halscope and do a screen grab showing what happens. You should plot ppmc.0.encoder.xxx.position, ppmc.0.encoder.xxx.count, and ppmc.0.encoder.xxx.index-enable. You should probably trigger on the index-enable. Chris -- Apps built with the Adobe(R) Flex(R) framework and Flex Builder(TM) are powering Web 2.0 with engaging, cross-platform capabilities. Quickly and easily build your RIAs with Flex Builder, the Eclipse(TM)based development software that enables intelligent coding and step-through debugging. Download the free 60 day trial. http://p.sf.net/sfu/www-adobe-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading Issues
richard harris wrote: I am running Elson's servo system and EMC 2.2.6. Over the last few days I have run several hundred parts single point threading a M22x1.5 threads without a single bad thread. Yesterday I switched to cutting a M20x2.5 and suddenly on ever other part the lathe will rapid during a cut. I had a similar issues months back and upgraded EMC to 2.2.6 and the issue went away. The lathe will go to the start the thread it will do a brief pause for the index pulse and shoot off at G0 through the part. I went back to my M22 code and ran 30 parts without fail, I even reduced the spindle speed to what I am cutting the M20 at thinking I might get more noise from the VFD at the lower end of the rpm band and no effect. I also increased the number of passes on the M22 program to replicate the M20 program and no failures. Switched back to the M22 program and the second part experienced a rapid on the spring pass. Any ideas what could be the cause? Is there a way to set EMC to never attempt a threading pass that is faster than the G0 velocity? VERY strange! But, I have seen some behavior like that before. Both old revisions of software and hardware can cause it. A problem in the driver on a released version of EMC from the CNC Workshop in 2007 would go crazy like that if the spindle was allowed to run for enough time to count up 16 million encoder counts, then the CNC program was started. The 24-bit overflow was not handled properly, and the Z axis tried to Catch up to the thread which was now many feet away. My experience with this problem indicated it had nothing to do with the thread pitch, but how long, and how fast, the spindle ran between threading passes. Any version of EMC later than July 2007 or thereabouts should not have this problem in software. My log shows your UPC board has the 5/2/2007 firmware, which is the current version for that rev. level of the board. So, that should be OK, too. I'm pretty sure EMC will NOT exceed G0 velocity. But, the threading code will go up to that speed to sync up to a thread. I'm just wondering if there is any quirk in your M20 program that makes the conditions around the threading pass different than the M22 program. Are these programs descendants of the sample threading.ngc program, or were they created from scratch or by a CAM program? As Chris says, you may need to instrument the situation and then send us a screen shot of the halscope when it fouls up. I use a pretty similar setup on my minimill to do rigid tapping, and it seems to run quite reliably there. It doesn't actually need to do a spindle sync for rigid tapping, but I think it does. I also run demos doing a single-point thread on that machine, using it like a lathe, and making multiple passes. I did indeed have these problems at the 2007 NAMES show, and Chris, Jeff, John and I bashed it into submission at the 2007 CNC Workshop. Looking back at the release history, that should have gone into the complete public distro. about 2.1.7, so you shouldn't have such a problem. Kirk Wallace is also using a UPC board on a lathe, but I don't know if he is doing a lot of threading. Maybe you should send me your threading program and I will try it here on the minimill. Is your machine natively defined in mm units or inch units? It shouldn't make a difference, but I'm pulling at straws, here. Jon -- Apps built with the Adobe(R) Flex(R) framework and Flex Builder(TM) are powering Web 2.0 with engaging, cross-platform capabilities. Quickly and easily build your RIAs with Flex Builder, the Eclipse(TM)based development software that enables intelligent coding and step-through debugging. Download the free 60 day trial. http://p.sf.net/sfu/www-adobe-com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] lathe threading
On Fri, 2008-08-15 at 23:13 +0200, josep M. giili freixa wrote: i have a lathe retrofited whit servos. I tried to run it whit Mach3 but i have problems when threading. Now testing Emc2 but when configuring it whit Stepwizard all run fine except threading. Gcode stops in g76 line waithing for spindle sincro. I`m unable the get a explanation in the manuals of how arrange spindle sincro for threading in the Hal file. I have a simple 2 axis step-dir and a spindle whit 200 ppr encoder A,B,Z chanels . can anyone help-me whit the Hal file i need for this lathe. tks. Josep. For my lathe I copied Jon's (Pico Systems) config files. From those I pulled out the threading parts and modified a little. ~~~ # Set the s/w encoder scale to match the physical encoder setp encoder.N.scale [SPINDLE]INPUT_SCALE # Connect encoders to EMC2's software decoders net SpindleEncoderA parport.portnum.pin-pinnum-in encoder.N.phase-A net SpindleEncoderB parport.portnum.pin-pinnum-in encoder.N.phase-B net SpindleEncoderZ parport.portnum.pin-pinnum-in encoder.N.phase-Z # Connect the s/w encoder index to the motion controller net spindle-index-enable (continues on next line) encoder.N.index-enable motion.spindle-index-enable # Connect rev count (actually s/w encoder scaled output) # to the motion controller net spindle-pos encoder.N.position motion.spindle-revs ~~~ I think that's it. Basically you set up an encoder and scale it to the number of counts per revolution, then feed the index and the encoder counts since last index to the motion controller. At the start of each thread pass, EMC2 waits for an index. When the index triggers, the count is zero'd and then the Z axis is moved based on the spindle's count. At the end of the thread to tool is retracted, moved to the beginning and waits for another index to zero on. -- Kirk Wallace (California, USA http://www.wallacecompany.com/machine_shop/ Hardinge HNC/EMC CNC lathe, Bridgeport mill conversion, doing XY now, Zubal lathe conversion pending Craftsman AA 109 restoration Shizuoka ST-N/EMC CNC) - This SF.Net email is sponsored by the Moblin Your Move Developer's challenge Build the coolest Linux based applications with Moblin SDK win great prizes Grand prize is a trip for two to an Open Source event anywhere in the world http://moblin-contest.org/redirect.php?banner_id=100url=/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On Mon, 2007-10-08 at 21:52 -0500, Jon Elson wrote: ... snip problem? Maybe missing pulses or noise adding pulses? Thanks for any replies. It could be anything, so you have to investigate. First, put halmeter on the HAL pin ppmc.0.encoder.2.count, rotate the spindle to a known position, and read thhe halmeter value. (The above assumes you have the spindle encoder on axis 2, if it is on axis 3 use that number between encoder and count.) Now, turn the spindle exactly one turn and read again. The difference should be equal to the expected 5000 counts. Thanks Jon and Chris. I verified the encoder had 5000 pulses/revolution. I then did the above and got varying counts in the mid 4ks. Upon inspecting the encoder I found the disk had a slight wobble towards one side of the sensor. I shimmed it away from the sensor a little and I now get 5000 counts per revolution plus or minus one count on occasion. My threads now come out fine. I like these US Digital disks, but apparently, I still haven't learned the proper way to fit them to a hub. I wonder if there is a way to have EMC check encoders by comparing pulse count against the index. If index doesn't appear when the count predicts it, a warning could be issued. -- Kirk Wallace (Hardinge HNC lathe, California, USA http://www.wallacecompany.com/machine_shop/ ) - This SF.net email is sponsored by: Splunk Inc. Still grepping through log files to find problems? Stop. Now Search log events and configuration files using AJAX and a browser. Download your FREE copy of Splunk now http://get.splunk.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Kirk Wallace wrote: On Mon, 2007-10-08 at 21:52 -0500, Jon Elson wrote: ... snip problem? Maybe missing pulses or noise adding pulses? Thanks for any replies. It could be anything, so you have to investigate. First, put halmeter on the HAL pin ppmc.0.encoder.2.count, rotate the spindle to a known position, and read thhe halmeter value. (The above assumes you have the spindle encoder on axis 2, if it is on axis 3 use that number between encoder and count.) Now, turn the spindle exactly one turn and read again. The difference should be equal to the expected 5000 counts. Thanks Jon and Chris. I verified the encoder had 5000 pulses/revolution. I then did the above and got varying counts in the mid 4ks. Upon inspecting the encoder I found the disk had a slight wobble towards one side of the sensor. I shimmed it away from the sensor a little and I now get 5000 counts per revolution plus or minus one count on occasion. My threads now come out fine. I like these US Digital disks, but apparently, I still haven't learned the proper way to fit them to a hub. I got a big eBay motor that had a fancy 6-channel (ABC, plus UVW for brushless motor commutation) encoder made by Renco in it. It has a tab you pull out from the side that causes fingers to reach in from the encoder body and center it on the hub. Then you tighten the hold-down screws before pushing the tab in. This aligns the read head with the tracks on the disc. I had to realign my encoder when I got the motor. I think US Digital may have some little moded collar that serves the same purpose. But, I guess if the disc hub is running eccentric on the shaft, that won't help. I wonder if there is a way to have EMC check encoders by comparing pulse count against the index. If index doesn't appear when the count predicts it, a warning could be issued. You could pretty easily make up such a program that would command the motor to run at a slow rate but open-loop, and put the encoder counter into index-enable mode, so it counts up and resets on every index pulse. The program would check the highest number it sees every cycle, maybe reporting a histogram of the highest count registered every turn. With no belt or coupling, you could run this test for a half hour or so. I've never actually written a stand-alone HAL program, but it should be doable. Jon - This SF.net email is sponsored by: Splunk Inc. Still grepping through log files to find problems? Stop. Now Search log events and configuration files using AJAX and a browser. Download your FREE copy of Splunk now http://get.splunk.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On Wed, 2007-10-10 at 12:06 -0500, Jon Elson wrote: Kirk Wallace wrote: On Mon, 2007-10-08 at 21:52 -0500, Jon Elson wrote: ... snip ... snip count against the index. If index doesn't appear when the count predicts it, a warning could be issued. You could pretty easily make up such a program that would command the motor to run at a slow rate but open-loop, and put the encoder counter into index-enable mode, so it counts up and resets on every index pulse. The program would check the highest number it sees every cycle, maybe reporting a histogram of the highest count registered every turn. With no belt or coupling, you could run this test for a half hour or so. I've never actually written a stand-alone HAL program, but it should be doable. Jon I meant to have the process running in the background, all the time so that if you are making a part, it can detect the fault before it is finished. -- Kirk Wallace (Hardinge HNC lathe, California, USA http://www.wallacecompany.com/machine_shop/ ) - This SF.net email is sponsored by: Splunk Inc. Still grepping through log files to find problems? Stop. Now Search log events and configuration files using AJAX and a browser. Download your FREE copy of Splunk now http://get.splunk.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Lathe Threading
I did my first CNC lathe thread today. I actually got a thread which, on a first try, I didn't expect. I entered parameters for a 20 tpi thread and got something like 23 tpi. When I setup the spindle parameters in the ini file, I assumed that the encoder input scale should equal the number of pulses per revolution (1250 cpr x 4 p/cpr = 5000 ppr). --- hnc-3a.ini --- ... [SPINDLE] # Encoder INPUT_SCALE = 5000 OUTPUT_SCALE = 1 # DAC output to VFD DAC_SCALE = 320 ... --- My thinking is that INPUT_SCALE should not need to be adjusted by cut and try, so if the thread tpi is not correct, it must be an encoder problem? Maybe missing pulses or noise adding pulses? Thanks for any replies. (config files here: http://www.wallacecompany.com/cnc_lathe/HNC/emc2/ http://www.wallacecompany.com/machine_shop/ ) Kirk Wallace (Hardinge HNC lathe, California, USA) - This SF.net email is sponsored by: Splunk Inc. Still grepping through log files to find problems? Stop. Now Search log events and configuration files using AJAX and a browser. Download your FREE copy of Splunk now http://get.splunk.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
On Mon, Oct 08, 2007 at 12:31:42PM -0700, Kirk Wallace wrote: My thinking is that INPUT_SCALE should not need to be adjusted by cut and try, so if the thread tpi is not correct, it must be an encoder problem? Maybe missing pulses or noise adding pulses? Thanks for any replies. I agree, you definitely won't get it right by guess-and-check. The motion.spindle-revs pin should be revolutions (mark the chuck, turn it exactly ten revs, see if motion.spindle-revs increases by 10.0). Yours will be off, you have to just figure out why after that. It could be any number of things, including scaling and noise. If it seems ok when you turn it by hand, but is bad when you run the spindle for a while, it's surely noise. I had noise problems and knew it was fixed when I could run my spindle for 15 minutes and then line up my mark on the chuck and see motion.spindle-revs had increased an integer number of turns. I recall someone having trouble with ppmc because there is a jumper or switch that sets differential encoder mode, and he had it set wrong. This caused noise problems. 1250 seems like a strange number. Are you sure? (If that is right, your 5000 setting is correct) Congratulations on cutting your first thread though! I bet you'll be making right ones very soon. - This SF.net email is sponsored by: Splunk Inc. Still grepping through log files to find problems? Stop. Now Search log events and configuration files using AJAX and a browser. Download your FREE copy of Splunk now http://get.splunk.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Chris Radek wrote: On Mon, Oct 08, 2007 at 12:31:42PM -0700, Kirk Wallace wrote: My thinking is that INPUT_SCALE should not need to be adjusted by cut and try, so if the thread tpi is not correct, it must be an encoder problem? Maybe missing pulses or noise adding pulses? Thanks for any replies. I agree, you definitely won't get it right by guess-and-check. The motion.spindle-revs pin should be revolutions (mark the chuck, turn it exactly ten revs, see if motion.spindle-revs increases by 10.0). Yours will be off, you have to just figure out why after that. It could be any number of things, including scaling and noise. If it seems ok when you turn it by hand, but is bad when you run the spindle for a while, it's surely noise. I had noise problems and knew it was fixed when I could run my spindle for 15 minutes and then line up my mark on the chuck and see motion.spindle-revs had increased an integer number of turns. I recall someone having trouble with ppmc because there is a jumper or switch that sets differential encoder mode, and he had it set wrong. This caused noise problems. That was a real PPMC board set. Kirk has a UPC which doesn't have differential inputs on the board. (He could have an outboard differential receiver, I suppose.) 1250 seems like a strange number. Are you sure? (If that is right, your 5000 setting is correct) How about 1728? That's what I have for a spindle encoder on the mini-mill. Jon - This SF.net email is sponsored by: Splunk Inc. Still grepping through log files to find problems? Stop. Now Search log events and configuration files using AJAX and a browser. Download your FREE copy of Splunk now http://get.splunk.com/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
At 11:23 AM 6/29/2007, you wrote: trial and error. I have a project of machining a back plate for an LW dividing head, the thread is 2-1/4 10tpi. I dread test fitting the dividing head to the back plate! Roger Neal Make up a few simple rings from scrap and do a trial run or three. Then when you know it is cutting the thread size you want do the back plate. __ Andre' B. Clear Lake, Wi. - This SF.net email is sponsored by DB2 Express Download DB2 Express C - the FREE version of DB2 express and take control of your XML. No limits. Just data. Click to get it now. http://sourceforge.net/powerbar/db2/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading
Roger: The actual depth of the thread is not really important. It is the angled surfaces width that is. That is why measuring with 3 wires is the most accurate. The wires only touch the angled sides of the thread. Actually there is a formula for figuring out the best size of the wires as well. But if just comparing threads, just use an appropriate size wire-meaning you want the contact point close to the middle of the angled depth. In the machine shop I worked at we would measure the spindle nose thread with 3 wires - machine a thread gauge (same as the spindle) confirming it's size with the 3 wire method then would use that to test fit the internal thread. we would stamp the gauge and keep it safe for next time! Of course if you have something handi that fits the spindle you could use that to test fit while making the thread gauge-then you would not need to measure at all-if you are careful. It all really depends on how good a fit you need and how much time you want to spend and what you have for tools! Cheers Chris Morley From: [EMAIL PROTECTED] To: emc-users@lists.sourceforge.net Date: Fri, 29 Jun 2007 11:23:36 -0500 Subject: [Emc-users] Lathe Threading First of all, thank you developers for EMC and thank you John Kasunich for getting the m5i20 threading working. I loaded the pre 2.1.7 version and built it on my pc, the threading worked first try, I only had to change my old latch-index to index-enable and then tested it out, I now have a lathe pawn with threads! In wondering about setting up to cut threads, I thought perhaps I could set my threading tool as if it came to a shap 0 radius point and thread the full depth from that imaginary point. I drew a 60 degree point in AutoCad, drew a line through the point, then applied different radius' to the point. For a .008 radius cutting tool, there was .008 between the tool tip and the line representing point, for a .0156 radius, there was .0156 between the tool tip and point, and so on. The tool tip radius equaled the gap between the peak of the radius and the 0 radius point. So, I was wondering if I used a threading tool with a .008 radius, could I take a light test cut, measure the radius, add .008 set that as the X position of that tool, then thread to the full thread depth. This would put the imaginary 0 radius point at the full thread depth and actual point .008 out from the full thread depth. This procedure could be adapted for whatever tool tip radius you were using. If a test cut wasn't practical, you could use feeler gages to set the tool, as long as you knew the tool tip radius. Or perhaps there is an easier way I'm overlooking :-) I plan to try this out, perhaps I could learn how to measure with the 3 wire method and see how close the threads came out. My goal is to come up with a method that will give me the right thread depth with minimal trial and error. I have a project of machining a back plate for an LW dividing head, the thread is 2-1/4 10tpi. I dread test fitting the dividing head to the back plate! Roger Neal - This SF.net email is sponsored by DB2 Express Download DB2 Express C - the FREE version of DB2 express and take control of your XML. No limits. Just data. Click to get it now. http://sourceforge.net/powerbar/db2/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users _ Explore the seven wonders of the world http://search.msn.com/results.aspx?q=7+wonders+worldmkt=en-USform=QBRE- This SF.net email is sponsored by DB2 Express Download DB2 Express C - the FREE version of DB2 express and take control of your XML. No limits. Just data. Click to get it now. http://sourceforge.net/powerbar/db2/___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Lathe Threading in EMC
Hi All, Is it possible to make threads in EMC2? In the user manual it says that it is possible, but I can't figure out how to do it. Thanks, Isak. Boardwalk for $500? In 2007? Ha! Play Monopoly Here and Now (it's updated for today's economy) at Yahoo! Games. http://get.games.yahoo.com/proddesc?gamekey=monopolyherenow - This SF.net email is sponsored by DB2 Express Download DB2 Express C - the FREE version of DB2 express and take control of your XML. No limits. Just data. Click to get it now. http://sourceforge.net/powerbar/db2/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading in EMC
Thanks, I'll try the nist-lathe config. Does the index output need to be one pulse per revolution? Can it be similar to what there is in mach2 program: several pulses per rev with one pulse wider than the others. Thanks, Isak. - Original Message From: Jeff Epler [EMAIL PROTECTED] To: Isak Levinson [EMAIL PROTECTED]; Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Sent: Thursday, May 24, 2007 3:37:16 PM Subject: Re: [Emc-users] Lathe Threading in EMC Yes, it is possible. You need a spindle with encoder and index pulse output. The sample configuration nist-lathe shows the necessary HAL configuration when the encoder is connected to parport pins 11, 12, and 13. The sample ngc file threading.ngc uses a bunch of G33 (spindle synchronized motion) commands to cut a thread; the file g76.ngc uses the threading canned cycle to make a 20TPI thread. The User Manual has a descrition and diagram of the numbers that are used by the G76 threading cycle -- page 143 in the version here: http://linuxcnc.org/docs/2.1/EMC2_User_Manual.pdf Jeff - This SF.net email is sponsored by DB2 Express Download DB2 Express C - the FREE version of DB2 express and take control of your XML. No limits. Just data. Click to get it now. http://sourceforge.net/powerbar/db2/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users Ready for the edge of your seat? Check out tonight's top picks on Yahoo! TV. http://tv.yahoo.com/ - This SF.net email is sponsored by DB2 Express Download DB2 Express C - the FREE version of DB2 express and take control of your XML. No limits. Just data. Click to get it now. http://sourceforge.net/powerbar/db2/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Lathe Threading in EMC
On Thu, May 24, 2007 at 05:46:02AM -0700, Isak Levinson wrote: Does the index output need to be one pulse per revolution? Can it be similar to what there is in mach2 program: several pulses per rev with one pulse wider than the others. Right now, only a spindle with encoder and index pulse may be used. The index pulse gives one pulse per revolution, and the rest of the encoder signal (called phase-A and phase-B) ensures that emc is aware of the orientation of the spindle at all times. I think that the nist-lathe has a 1024 count per revolution encoder, which allows emc to know the angle to within about 1/3 of a degree. Jeff - This SF.net email is sponsored by DB2 Express Download DB2 Express C - the FREE version of DB2 express and take control of your XML. No limits. Just data. Click to get it now. http://sourceforge.net/powerbar/db2/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
