Re: [Emc-users] Feeds and speeds

[andrew beck]

I found the aliexpress and Amazon endmills are just the budget ones.  I pay
the same price for Chinese cutters that are so much better.  You need to go
to a factory I found..  Aliexpress sellers are actually putting a premium
on things as hard as that is to believe.

And you don't have to use high rpm.  Just hack with them like you normally
do.

Only now rpm doesn't matter so much The cutter doesn't care.  It's more
what the machine can handle

On Wed, Feb 19, 2020, 7:26 PM John Dammeyer  wrote:

> Amazon.ca has a set of 5 carbide 6mm for $34.29 Cdn.  I imagine that $6.85
> each isn't too high a price?
>
> https://www.amazon.ca/4-Flute-Tungsten-Carbide-Milling-Diameter/dp/B07B9PRNWC/ref=sr_1_8?keywords=carbide+end+mill+1%2F4&qid=1582092811&sr=8-8
> John
>
>
> > -Original Message-
> > From: andrew beck [mailto:andrewbeck0...@gmail.com]
> > Sent: February-18-20 9:50 PM
> > To: Enhanced Machine Controller (EMC)
> > Subject: Re: [Emc-users] Feeds and speeds
> >
> > You guys all probably know this but I'll say it anyway..  You should
> start
> > using carbide endmills.  I run a tooling company here in New Zealand
> > selling to the local machine shops.  Carbide is awesome.  Anyway I have a
> > couple of Chinese suppliers I buy my stuff from and a Taiwanese supplier
> > for higher quality stuff.  Shout out if you want to find some suppliers
> and
> > I'll connect you up.
> >
> > On Wed, Feb 19, 2020, 5:12 PM Jon Elson  wrote:
> >
> > > On 02/18/2020 08:45 PM, John Dammeyer wrote:
> > > > I've got Mecsoft AlibreCAM generating the tool paths for this in the
> > > attached photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4"
> HSS
> > > end mill.  I'm trying to figure out, using Machinists tool box, exactly
> > > what feeds and speeds could be used for milling the slot.
> > > >
> > > > I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per
> flute
> > > the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of
> > > tool diameter for depth per pass so 0.025"
> > > >
> > > > Is that too conservative or likely to break something?  Doing it
> > > manually I'd do it by feel but once it's automatic it's harder to
> decide
> > > SFM and chip load.
> > > >
> > > Those numbers sound mostly OK to me.  But, I LONG AGO gave
> > > up plain HSS, the tool life was just awful.
> > > I learned on a box of P&W Stellite tools and got spoiled.
> > > When I finally wore them out, I started using
> > > M42 and M57 cutters, which have at least 3X the tool life.
> > > I'm showing 60-80 SFPM so that would be more
> > > like 900-1000 RPM, but coolant would be required.  And, I
> > > usually plunge about 1/2 the cutter diameter
> > > per pass.  It all depends on the stiffness of your machine
> > > how much of a cut it can handle.
> > >
> > > Jon
> > >
> > >
> > > ___
> > > Emc-users mailing list
> > > Emc-users@lists.sourceforge.net
> > > https://lists.sourceforge.net/lists/listinfo/emc-users
> > >
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Feeds and speeds

[John Dammeyer]

The attached photo shows the general idea of what I'm trying to build.  
Although the slots could probably have been easily cut with the unbent HRS held 
at an angle with a manual mill, the CNC adds the ability to make it fancy.

I'll clamp a test piece into the vice and give it a try.

John


> -Original Message-
> From: dave engvall [mailto:dengv...@charter.net]
> Sent: February-18-20 11:00 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] Feeds and speeds
> 
> Hi all,
> 
> By hot roll I assume you mean something like A36. Alloy comp not
> controlled just mechanical. It tends to be low alloy scrap plus 4140.
> 
> Using a� TiAlN coated 1/4 carbide I can� use 2200 rpm and 11 ipm, doc
> 0.05, any more and it screams at me. This is basically slotting, on a
> side cut same rpm,� and feed, .7 doc for radial of only .025.� Makes for
> a lot of passes. This� is on a Cinci contourmaster 1963 vintage,
> converted to servos. Going deeper and slower doesn't seem to help. Since
> TiAlN likes to run hot I machine dry. It is not unusual for small jobs
> to run for a couple of hours.
> 
> On a machining site someone recommended ... increase the feed until you
> break a mill, then back off 10%. Pretty aggressive.
> 
> Rumor has it that AlCrN coated carbide� with flood coolant lasts a long
> time; and that was in a production environment. If ... (when) I get my
> big machine up I'll give more serious stuff a go.
> 
> I do a lot of A36 because it is cheap and OK for experimental work but
> CR machines like a dream by comparison. HTH
> 
> Dave
> 
> 
> On 2/18/20 10:09 PM, John Dammeyer wrote:
> 
> > Thanks everyone.  The trouble with the machinist workshop program and
> some of the others is they are targeted at production speeds.  I'm not even
> sure about the alloy of Hot Rolled Steel which is what will be used here.
> >
> > The part is designed to hook around the ears of a pipe crucible so accuracy
> isn�t that big a deal and at the moment, HSS is all I have.  With manual
> machining, as Wallace said, you can turn the hand wheels and get a feel for
> what it should do.And yes the machine is pretty rigid.
> http://www.autoartisans.com/milton.htm  This picture was when it first
> arrived.
> >
> > I do have a coolant pump but have yet to use it.  Not sure what kind of
> coolant to use.   A large part of my machining has been aluminium castings.
> I've not yet set up mist coolant.  Any suggestions for what type of coolant to
> use for a machine that is only used occasionally?
> >
> > All things considered the CNC conversion is the easy part.  My heart is
> always in my throat a bit when first start running a CNC program.  That's the
> really hard part.
> >
> > John
> >
> >
> >> -Original Message-
> >> From: Stuart Stevenson [mailto:stus...@gmail.com]
> >> Sent: February-18-20 7:04 PM
> >> To: Enhanced Machine Controller (EMC)
> >> Subject: Re: [Emc-users] Feeds and speeds
> >>
> >> John,
> >>
> >> Do you have flood coolant or mist coolant?
> >>
> >> I would be inclined to try the cut full depth if you have flood or mist
> >> coolant. 1/4 inch is on the borderline of having the strength necessary to
> >> make a full depth cut.  I would think 5.5ipm might be a little aggressive
> >> but I would leave it programmed at that feed and speed and turn the
> >> feedrate to about 20% to start the cut. After you get into the cut I would
> >> move the feedrate up about 10% to see, hear and feel how mill is cutting.
> I
> >> would keep moving the feed up until I saw, heard or felt the mill working
> >> too hard. I would then start turning the speed up a little at a time to see
> >> how the mill responds.
> >> I think 30sfm might be a little slow but you can adjust the speed after
> >> entering the cut.
> >> If you can adjust the feed and speed to make the full cut sound good and
> >> you have another part to run I would change your program to enter the
> cut
> >> as you did the first time but the add lines to make it more aggressive
> >> after you have entered the cut.
> >> If you are leaving a little material to clean up the you can drastically
> >> increase the speed and feed after you turn around at the end of the slot.
> >> Is the slot you are cutting wide enough to allow at least .010 thou. for a
> >> finish pass and maybe a spring pass.
> >> I would make the finish pass and spring pass in a conventional cut rather
> >> than a climb cut.
> >> Stuart
> >>
> >>
> >> On Tue, Feb 18, 2020 at 8:47 PM John Dammeyer
> 
> >> wrote:
> >>
> >>> I've got Mecsoft AlibreCAM generating the tool paths for this in the
> >>> attached photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS
> >>> end mill.  I'm trying to figure out, using Machinists tool box, exactly
> >>> what feeds and speeds could be used for milling the slot.
> >>>
> >>> I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute
> >>> the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10%
> of
> >>> tool d

Re: [Emc-users] Feeds and speeds

[dave engvall]

Hi all,

By hot roll I assume you mean something like A36. Alloy comp not 
controlled just mechanical. It tends to be low alloy scrap plus 4140.


Using a  TiAlN coated 1/4 carbide I can  use 2200 rpm and 11 ipm, doc 
0.05, any more and it screams at me. This is basically slotting, on a 
side cut same rpm,  and feed, .7 doc for radial of only .025.  Makes for 
a lot of passes. This  is on a Cinci contourmaster 1963 vintage, 
converted to servos. Going deeper and slower doesn't seem to help. Since 
TiAlN likes to run hot I machine dry. It is not unusual for small jobs 
to run for a couple of hours.


On a machining site someone recommended ... increase the feed until you 
break a mill, then back off 10%. Pretty aggressive.


Rumor has it that AlCrN coated carbide  with flood coolant lasts a long 
time; and that was in a production environment. If ... (when) I get my 
big machine up I'll give more serious stuff a go.


I do a lot of A36 because it is cheap and OK for experimental work but 
CR machines like a dream by comparison. HTH


Dave


On 2/18/20 10:09 PM, John Dammeyer wrote:


Thanks everyone.  The trouble with the machinist workshop program and some of 
the others is they are targeted at production speeds.  I'm not even sure about 
the alloy of Hot Rolled Steel which is what will be used here.

The part is designed to hook around the ears of a pipe crucible so accuracy 
isn’t that big a deal and at the moment, HSS is all I have.  With manual 
machining, as Wallace said, you can turn the hand wheels and get a feel for 
what it should do.And yes the machine is pretty rigid.  
http://www.autoartisans.com/milton.htm  This picture was when it first arrived.

I do have a coolant pump but have yet to use it.  Not sure what kind of coolant 
to use.   A large part of my machining has been aluminium castings.  I've not 
yet set up mist coolant.  Any suggestions for what type of coolant to use for a 
machine that is only used occasionally?

All things considered the CNC conversion is the easy part.  My heart is always 
in my throat a bit when first start running a CNC program.  That's the really 
hard part.

John



-Original Message-
From: Stuart Stevenson [mailto:stus...@gmail.com]
Sent: February-18-20 7:04 PM
To: Enhanced Machine Controller (EMC)
Subject: Re: [Emc-users] Feeds and speeds

John,

Do you have flood coolant or mist coolant?

I would be inclined to try the cut full depth if you have flood or mist
coolant. 1/4 inch is on the borderline of having the strength necessary to
make a full depth cut.  I would think 5.5ipm might be a little aggressive
but I would leave it programmed at that feed and speed and turn the
feedrate to about 20% to start the cut. After you get into the cut I would
move the feedrate up about 10% to see, hear and feel how mill is cutting. I
would keep moving the feed up until I saw, heard or felt the mill working
too hard. I would then start turning the speed up a little at a time to see
how the mill responds.
I think 30sfm might be a little slow but you can adjust the speed after
entering the cut.
If you can adjust the feed and speed to make the full cut sound good and
you have another part to run I would change your program to enter the cut
as you did the first time but the add lines to make it more aggressive
after you have entered the cut.
If you are leaving a little material to clean up the you can drastically
increase the speed and feed after you turn around at the end of the slot.
Is the slot you are cutting wide enough to allow at least .010 thou. for a
finish pass and maybe a spring pass.
I would make the finish pass and spring pass in a conventional cut rather
than a climb cut.
Stuart


On Tue, Feb 18, 2020 at 8:47 PM John Dammeyer 
wrote:


I've got Mecsoft AlibreCAM generating the tool paths for this in the
attached photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS
end mill.  I'm trying to figure out, using Machinists tool box, exactly
what feeds and speeds could be used for milling the slot.

I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute
the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of
tool diameter for depth per pass so 0.025"

Is that too conservative or likely to break something?  Doing it manually
I'd do it by feel but once it's automatic it's harder to decide SFM and
chip load.



Thanks
John


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



--
Addressee is the intended audience.
If you are not the addressee then my consent is not given for you to read
this email furthermore it is my wish you would close this without saving or
reading, and cease and desist from saving or opening my private
correspondence.
Thank you for honoring my wish.

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lis

Re: [Emc-users] Open source CNC architecture

[Rafael Skodlar]

On 2020-02-17 04:49, Les Newell wrote:


  One issue jumps to mind that is different.  The tiny shop I have 
doesn't have room for a Keyboard, Mouse and Display by the lathe.  I 
currently have a nice work triangle set up for the lathe toolbench and 
tool cabinet.  It would require a lot of work to change that at a cost 
of space lost somewhere else.


Monitor on the wall behind the lathe? Support arm bolted to the wall for 
the keyboard? If you wanted these things you'd make room. As you don't 
want them you won't make the room. I'm not saying that's a bad thing. We 
just have different requirements.



And that's really, from my perspective all I am talking about.   If 
have to add an external intelligence of some sort to do faster 
stepping or PWM then the sky's the limit on what is added because that 
3GHz 1GB PC isn't fast enough to do what can be done with a small 32 
bit ARM if the dedicated $250 CNC boxes from China are to be believed.


Go for it. If you design the board the LinuxCNC developers would be very 
willing to help you integrate it with LinuxCNC. Of course you'll have to 
be able to produce it at a price that makes it attractive to buyers.


This is not "start from scratch" situation! We don't live in a vacuum! 
SBCs are popping up all over the place:

http://linuxgizmos.com/category/boards/

One sysadmin motto I learned long time ago: "Be a lazy sysadmin. Do 
whatever it takes to simplify or minimize your tasks. Just don't tell to 
your boss or you'll get even more work to do" ;-)




If you can do it for the right price and if it has the I/O capability I 
need I'll buy one for my next machine. The display stuff is of no 
interest to me but keypads are always handy. I use modbus for my keypads 
at the moment.


First thing to look for is what others are doing using with embedded 
systems. Most COTS manufacturers support their products for 5 or even 10 
years. And there are alternative HW sources. That should be good for CNC 
also.


I guess what I am suggesting is that it's time for LinuxCNC to be 
broken apart and a standardized interface for Ethernet control be 
developed.  Once that could talk to dumb FPGA devices like the 7i92H 
or to full blown standalone CNC controllers that can act as simple 
DRO/Power Feed or even simple G-Code like the 3D printers.  Or be 
connected to the much more powerful LinuxCNC to add, in addition to 
G-Code the fancy tool changing apparatus along with robotic cells that 
load and unload the parts.


You are completely missing the point. You don't need to 'break apart' 
LinuxCNC. It is designed from the ground up to be modular. The 


'break apart' is architectural change just like it happened to so many 
GNU-Linux services or programs. Robotics is one of the closest functions 
to CNC. Some robots depend on RT kernel but do not have or need GUI on 
top of it.


Medical robotics is the most critical example of a device that needs to 
work as planned and programmed. What do they use to write programs or 
configure the OS? According to one job posting, INTUITIVE SURGICAL uses 
something like:

https://www.openembedded.org/wiki/Main_Page
https://www.yoctoproject.org/

Yocto Project works on any architecture. "...You are not locked down to 
any one supplier as Yocto Project is both open source and supports many 
architectures" except freaky old parallel port!


"...More and more, these types of devices are prototyped (and sometimes 
implemented) with easily available consumer hardware devices such as the 
Raspberry Pi or the BeagleBone, or MinnowBoard"


trajectory planner is just another module. Want to run an external box 
with it's own TP and I/O? No problem. Write a module to replace it that 
talks to your TP and you're off to the races. If you have the knowledge 
to write your own 6 axis TP on an external board, writing the HAL module 
to talk to it will be a piece of cake.


Les


examples of embedded system customization:
https://wiki.st.com/stm32mpu/wiki/OpenEmbedded
http://wiki.openmoko.org/wiki/OpenEmbedded

To naysayers; there's gold in those hills: 
https://www.crunchbase.com/hub/hardware-companies#section-recent-activities


One more comment on application distribution. It's based on my 
experience from few years ago where "cloud service" was designed on 
Centos distribution. Programs, libraries, and configuration files were 
packed as RPMs and installed as such. I proposed much simpler and more 
flexible packaging, tar files as in Slackware. The advantage would be in 
architecture where more than one version of service could be installed 
in parallel without interfering with another one.


Active service would be a link 'from the top directory'. Switching from 
one version to another one would be simple:

- service  stop,
- relink top directory,
- service  start.

What we were doing was order pizza, stop services, install RPMs on top 
of old ones, start services. That process took about 3 hours on all 
servers in the evenings when the network tr

Re: [Emc-users] Feeds and speeds

[John Dammeyer]

Amazon.ca has a set of 5 carbide 6mm for $34.29 Cdn.  I imagine that $6.85 each 
isn't too high a price?
https://www.amazon.ca/4-Flute-Tungsten-Carbide-Milling-Diameter/dp/B07B9PRNWC/ref=sr_1_8?keywords=carbide+end+mill+1%2F4&qid=1582092811&sr=8-8
John


> -Original Message-
> From: andrew beck [mailto:andrewbeck0...@gmail.com]
> Sent: February-18-20 9:50 PM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Feeds and speeds
> 
> You guys all probably know this but I'll say it anyway..  You should start
> using carbide endmills.  I run a tooling company here in New Zealand
> selling to the local machine shops.  Carbide is awesome.  Anyway I have a
> couple of Chinese suppliers I buy my stuff from and a Taiwanese supplier
> for higher quality stuff.  Shout out if you want to find some suppliers and
> I'll connect you up.
> 
> On Wed, Feb 19, 2020, 5:12 PM Jon Elson  wrote:
> 
> > On 02/18/2020 08:45 PM, John Dammeyer wrote:
> > > I've got Mecsoft AlibreCAM generating the tool paths for this in the
> > attached photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS
> > end mill.  I'm trying to figure out, using Machinists tool box, exactly
> > what feeds and speeds could be used for milling the slot.
> > >
> > > I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute
> > the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of
> > tool diameter for depth per pass so 0.025"
> > >
> > > Is that too conservative or likely to break something?  Doing it
> > manually I'd do it by feel but once it's automatic it's harder to decide
> > SFM and chip load.
> > >
> > Those numbers sound mostly OK to me.  But, I LONG AGO gave
> > up plain HSS, the tool life was just awful.
> > I learned on a box of P&W Stellite tools and got spoiled.
> > When I finally wore them out, I started using
> > M42 and M57 cutters, which have at least 3X the tool life.
> > I'm showing 60-80 SFPM so that would be more
> > like 900-1000 RPM, but coolant would be required.  And, I
> > usually plunge about 1/2 the cutter diameter
> > per pass.  It all depends on the stiffness of your machine
> > how much of a cut it can handle.
> >
> > Jon
> >
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
> >
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Feeds and speeds

[John Dammeyer]

Thanks everyone.  The trouble with the machinist workshop program and some of 
the others is they are targeted at production speeds.  I'm not even sure about 
the alloy of Hot Rolled Steel which is what will be used here.

The part is designed to hook around the ears of a pipe crucible so accuracy 
isn’t that big a deal and at the moment, HSS is all I have.  With manual 
machining, as Wallace said, you can turn the hand wheels and get a feel for 
what it should do.And yes the machine is pretty rigid.  
http://www.autoartisans.com/milton.htm  This picture was when it first arrived.

I do have a coolant pump but have yet to use it.  Not sure what kind of coolant 
to use.   A large part of my machining has been aluminium castings.  I've not 
yet set up mist coolant.  Any suggestions for what type of coolant to use for a 
machine that is only used occasionally?

All things considered the CNC conversion is the easy part.  My heart is always 
in my throat a bit when first start running a CNC program.  That's the really 
hard part.  

John


> -Original Message-
> From: Stuart Stevenson [mailto:stus...@gmail.com]
> Sent: February-18-20 7:04 PM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Feeds and speeds
> 
> John,
> 
> Do you have flood coolant or mist coolant?
> 
> I would be inclined to try the cut full depth if you have flood or mist
> coolant. 1/4 inch is on the borderline of having the strength necessary to
> make a full depth cut.  I would think 5.5ipm might be a little aggressive
> but I would leave it programmed at that feed and speed and turn the
> feedrate to about 20% to start the cut. After you get into the cut I would
> move the feedrate up about 10% to see, hear and feel how mill is cutting. I
> would keep moving the feed up until I saw, heard or felt the mill working
> too hard. I would then start turning the speed up a little at a time to see
> how the mill responds.
> I think 30sfm might be a little slow but you can adjust the speed after
> entering the cut.
> If you can adjust the feed and speed to make the full cut sound good and
> you have another part to run I would change your program to enter the cut
> as you did the first time but the add lines to make it more aggressive
> after you have entered the cut.
> If you are leaving a little material to clean up the you can drastically
> increase the speed and feed after you turn around at the end of the slot.
> Is the slot you are cutting wide enough to allow at least .010 thou. for a
> finish pass and maybe a spring pass.
> I would make the finish pass and spring pass in a conventional cut rather
> than a climb cut.
> Stuart
> 
> 
> On Tue, Feb 18, 2020 at 8:47 PM John Dammeyer 
> wrote:
> 
> > I've got Mecsoft AlibreCAM generating the tool paths for this in the
> > attached photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS
> > end mill.  I'm trying to figure out, using Machinists tool box, exactly
> > what feeds and speeds could be used for milling the slot.
> >
> > I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute
> > the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of
> > tool diameter for depth per pass so 0.025"
> >
> > Is that too conservative or likely to break something?  Doing it manually
> > I'd do it by feel but once it's automatic it's harder to decide SFM and
> > chip load.
> >
> >
> >
> > Thanks
> > John
> >
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
> >
> 
> 
> --
> Addressee is the intended audience.
> If you are not the addressee then my consent is not given for you to read
> this email furthermore it is my wish you would close this without saving or
> reading, and cease and desist from saving or opening my private
> correspondence.
> Thank you for honoring my wish.
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] How to get 6i25 functioning?

[Ed W]

On 19/02/2020 00:44, Peter C. Wallace wrote:

On Wed, 19 Feb 2020, Ed W wrote:
OK, well that's encouraging! Running through pncconf the pin is high 
+5v, until I click into the motor tuning when it drops to close to 0V 
(I read about 20mv)


OK, so how do I debug why I don't see any steps coming out..? Hmm. I 
am really unsure what I should be doing here...


Final state is intended to have a cheap bob with step/dir to the 
chinese cheapo clone drivers that came with the omio x6-2200. (I'm 
not welded to the bob, just had it and it has convenient connectors 
in place). There are no encoders, just a simple stepper driver and 
steppers.


I should show you the settings I have, but the machine isn't 
conveniently close at present... The settings are on whatever 
defaults pncconf gave. From memory P is set to 1000 (not sure what 
the PID settings do with a stepper?), I have no encoders and then I 
have the stepper set to 5,000 and 10,000 in the various stepper 
timing boxes.


If I click "run" or try and jog in the tuning screen then I see the 
position params appear to change. However, I wonder if the issue 
could be that something here thinks I have a servo and without an 
encoder it isn't going to move and send some steps? Should this 
screen be showing me values which look like servo config?? Have I 
made some error in previous screens?


Thanks for such a fast response - appreciated. Further ideas would be 
very gratefully received!


Ed W



Its hard to guess the issue. do you have a working LinuxCNC 
configuration?


Do the direction pins change whan you jog in different directions?

( The PID is used to manage the step generation hardware and there is 
no reason to change the default tuning )


It might be more useful to ask for assistance on the LinuxCNC forum 
where you

can post your hal/ini files



I think I can get it back to working state. I was trying to just use 
pncconf in order to keep it to the basics for now? I need to double 
check to confirm, but I think the direction pin stays low?


Are there any commands or utilities to simply strobe pins on the 6i25 
connector and read their state? This would give me some satisfaction 
that things are working. I think this is probably a 101 question, so 
please refer me to the docs, but I guess I'm hoping for something that 
will simply show me current hardware input/output states? I would like 
to pull pins low to check some of the switch inputs while I'm going


Thanks

Ed W



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Feeds and speeds

[andrew beck]

You guys all probably know this but I'll say it anyway..  You should start
using carbide endmills.  I run a tooling company here in New Zealand
selling to the local machine shops.  Carbide is awesome.  Anyway I have a
couple of Chinese suppliers I buy my stuff from and a Taiwanese supplier
for higher quality stuff.  Shout out if you want to find some suppliers and
I'll connect you up.

On Wed, Feb 19, 2020, 5:12 PM Jon Elson  wrote:

> On 02/18/2020 08:45 PM, John Dammeyer wrote:
> > I've got Mecsoft AlibreCAM generating the tool paths for this in the
> attached photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS
> end mill.  I'm trying to figure out, using Machinists tool box, exactly
> what feeds and speeds could be used for milling the slot.
> >
> > I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute
> the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of
> tool diameter for depth per pass so 0.025"
> >
> > Is that too conservative or likely to break something?  Doing it
> manually I'd do it by feel but once it's automatic it's harder to decide
> SFM and chip load.
> >
> Those numbers sound mostly OK to me.  But, I LONG AGO gave
> up plain HSS, the tool life was just awful.
> I learned on a box of P&W Stellite tools and got spoiled.
> When I finally wore them out, I started using
> M42 and M57 cutters, which have at least 3X the tool life.
> I'm showing 60-80 SFPM so that would be more
> like 900-1000 RPM, but coolant would be required.  And, I
> usually plunge about 1/2 the cutter diameter
> per pass.  It all depends on the stiffness of your machine
> how much of a cut it can handle.
>
> Jon
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Feeds and speeds

[Gene Heskett]

On Tuesday 18 February 2020 22:32:24 Marshland Engineering wrote:

> I've long gone off HSS as Carbide is so cheap from China.
>
> Starting point - 4 Flute - 1000 rpm - 100 mm min and cut in 2 passes.
> 65 m/min, 0.025 mm per tooth.
> All depends on machine rigidity.
>
> For HSS maybe 1/2,  500 rpm and 50 mm min.
>
> This is where I like my hand wheels, I can feel the cut pressure.
>
If the spindle is DC controlled so the motor currant can be monitored, I 
found that an ammeter to display motor currant to be very helpfull, 
showing me how hard it was working, and has saved me $40 in those little 
5x20 slow blow fuses since.

That teeny little bare chassis motor controller that comes in the 
smallest hf mill they were selling 20 years ago, has a very stiffly 
controlled speed, so stiffly controlled I had to rig an ammeter so I 
could see how close I was to blowing a 1.5 amp fuse.

But eventually the pass transistor in it failed. I looked up the part 
number to see what sort of a critter it was, compared that to what was 
in a dead computer psu, and the computer transistor was rated at 10x the 
currant and 2x the volts. Since those better specs implied quite a bit 
more gate capacitance to drive it, I was concerned with its much smaller 
driver, but watching it with an ir thermometer showed I needent be 
concerned. Later I took it out of the gearhead and put it in a plastic 
box with a PMDX-106 so linuxcnc could control it in both directions.

Its been there, working great for all of the last decade, until the y 
screw ignored the limit switch and unscrewed itself from the nut, and I 
cannot find the bag of oversized balls I put in those screws I got from 
Stuart almost 20 years ago. So I used the stepper kit and psu in the 
6040 after I found its motor supply was folding back to about 13 volts 
when the A axis was plugged in.  Now all the electronics in the 6040 
have been replaced. Now the 25 or 30 ipm xy moves at 200 ipm.  Same 
motors although it could use a bigger z, that water cooled spindle is 
close to too heavy as it can only make 30 going up. Teeny little motors.

> --
> Thanking you
> Wallace Weideman
> Marshland Engineering
> 704 Marshland Road
> Styx
> Christchurch
> 03 3237449
> www.marshland.co.nz
>
> On 19/02/2020 at 3:45 p.m., emc-users-requ...@lists.sourceforge.net 
wrote:
> >Send Emc-users mailing list submissions to
> > emc-users@lists.sourceforge.net
> >
> >To subscribe or unsubscribe via the World Wide Web, visit
> > https://lists.sourceforge.net/lists/listinfo/emc-users
> >or, via email, send a message with subject or body 'help' to
> > emc-users-requ...@lists.sourceforge.net
> >
> >You can reach the person managing the list at
> > emc-users-ow...@lists.sourceforge.net
> >
> >When replying, please edit your Subject line so it is more specific
> >than "Re: Contents of Emc-users digest..."
> >
> >
> >Today's Topics:
> >
> >   1. Feeds and speeds (John Dammeyer)
> >
> >
> >-
> >-
> >
> >Message: 1
> >Date: Tue, 18 Feb 2020 18:45:21 -0800
> >From: "John Dammeyer" 
> >To: "'Enhanced Machine Controller \(EMC\)'"
> > 
> >Subject: [Emc-users] Feeds and speeds
> >Message-ID: <0b0901d5e6ce$a3887c20$ea997460$@autoartisans.com>
> >Content-Type: text/plain; charset="utf-8"
> >
> >I've got Mecsoft AlibreCAM generating the tool paths for this in the
> > attached
>
> photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS end
> mill. I'm trying to figure out, using Machinists tool box, exactly
> what feeds and speeds could be used for milling the slot.
>
> >I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per
> > flute the
>
> toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of
> tool diameter for depth per pass so 0.025"
>
> >Is that too conservative or likely to break something?  Doing it
> > manually I'd
>
> do it by feel but once it's automatic it's harder to decide SFM and
> chip load.
>
> >Thanks
> >John
> >
> >
> >-- next part --
> >A non-text attachment was scrubbed...
> >Name: image001.png
> >Type: image/png
> >Size: 29705 bytes
> >Desc: not available
> >
> >--
> >
> >
> >
> >--
> >
> >Subject: Digest Footer
> >
> >___
> >Emc-users mailing list
> >Emc-users@lists.sourceforge.net
> >https://lists.sourceforge.net/lists/listinfo/emc-users
> >
> >
> >--
> >
> >End of Emc-users Digest, Vol 166, Issue 90
> >**
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first

Re: [Emc-users] RPI4 is pretty close to a decent machine

[Rafael Skodlar]

On 2020-02-18 15:23, Chris Albertson wrote:

This is a problem with many people using Linux to do something complex like
build a CNC system or using ROS to build a robot.  They are doing something
complex with Linux before they try to do simple things with Linux.


Among other things, ROS is wrongfully named Robot Operating System, when 
it's a service. Must be a tradition in naming things the wrong way. 
Cookies for example are baked in bakeries not cookeries. Therefore they 
should be called bakies!



The best approach is to fist use Linux for everyday tasks, like reading and
writing emails, watching youtube videos.  Simply use it for all your normal
tasks.Get rid of your Windows system.


It takes some courage and experimentation to use Linux for your work. 
Granted, too many silly software companies don't create their programs 
for Linux platform since 1990s when they wrote them on Unix platform in 
the first place.


This month is 26 years since I started using Linux on my home and work 
computers exclusively. Over the years I tested all kinds of 
distributions and settled on Ubuntu based Supermicro servers in my 
garage and Kubuntu for my workstation and a laptop.


Some silly recruiters ask me to send my resume in "word format". I 
respond with either simple ASCII file or PDF exported from LibreOffice 
Writer. LibreOffice set of programs is good enough for office work. 
There are other utilities and programs that make my life exciting. I use 
Kate for writing bash and Python scripts, Jupyter for testing python 
scripts, etc.


There are other great programs for taking notes, editing or viewing 
pictures, creating 3D pictures with Blender, Thunderbird for handling 
email, listening or editing music and videos, etc.


I rarely turn on large TV because I can watch TV programs on HDhomerun 
that connects over LAN to SiliconDust TV box in my garage. That's 
running in parallel to other programs for my work.


One of my favorite utilities is Virtualbox which allows me to test 
different Linux distributions (Centos for example) or other OS like BSD 
that I need for professional work. I installed LinuxCNC as a virtual 
machine to see how it looks like. RT kernel is not important in this case.


Virtualbox is available for Windows also. You can create Linux VMs for 
testing. The other way around is possible also. Yes, start using Linux 
for most if not all of your work.



It is a little like buying a harbor freight mini lathe and then your first
project is a working gas airplane engine.



Oh my, I won't be able to build a working gas engine. Little Greta told 
the World that gas engines are forbidden now anyway.


--
Rafael Skodlar


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Feeds and speeds

[Jon Elson]

On 02/18/2020 08:45 PM, John Dammeyer wrote:

I've got Mecsoft AlibreCAM generating the tool paths for this in the attached photo.  
It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS end mill.  I'm trying 
to figure out, using Machinists tool box, exactly what feeds and speeds could be used for 
milling the slot.
  
I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of tool diameter for depth per pass so 0.025"
  
Is that too conservative or likely to break something?  Doing it manually I'd do it by feel but once it's automatic it's harder to decide SFM and chip load.
  
Those numbers sound mostly OK to me.  But, I LONG AGO gave 
up plain HSS, the tool life was just awful.
I learned on a box of P&W Stellite tools and got spoiled.  
When I finally wore them out, I started using
M42 and M57 cutters, which have at least 3X the tool life.  
I'm showing 60-80 SFPM so that would be more
like 900-1000 RPM, but coolant would be required.  And, I 
usually plunge about 1/2 the cutter diameter
per pass.  It all depends on the stiffness of your machine 
how much of a cut it can handle.


Jon


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

[Emc-users] Feeds and speeds

[Marshland Engineering]

I've long gone off HSS as Carbide is so cheap from China.

Starting point - 4 Flute - 1000 rpm - 100 mm min and cut in 2 passes. 
65 m/min, 0.025 mm per tooth.  
All depends on machine rigidity.

For HSS maybe 1/2,  500 rpm and 50 mm min.

This is where I like my hand wheels, I can feel the cut pressure.  







--
Thanking you
Wallace Weideman
Marshland Engineering
704 Marshland Road
Styx
Christchurch
03 3237449
www.marshland.co.nz

On 19/02/2020 at 3:45 p.m., emc-users-requ...@lists.sourceforge.net wrote:
>Send Emc-users mailing list submissions to
>   emc-users@lists.sourceforge.net
>
>To subscribe or unsubscribe via the World Wide Web, visit
>   https://lists.sourceforge.net/lists/listinfo/emc-users
>or, via email, send a message with subject or body 'help' to
>   emc-users-requ...@lists.sourceforge.net
>
>You can reach the person managing the list at
>   emc-users-ow...@lists.sourceforge.net
>
>When replying, please edit your Subject line so it is more specific
>than "Re: Contents of Emc-users digest..."
>
>
>Today's Topics:
>
>   1. Feeds and speeds (John Dammeyer)
>
>
>--
>
>Message: 1
>Date: Tue, 18 Feb 2020 18:45:21 -0800
>From: "John Dammeyer" 
>To: "'Enhanced Machine Controller \(EMC\)'"
>   
>Subject: [Emc-users] Feeds and speeds
>Message-ID: <0b0901d5e6ce$a3887c20$ea997460$@autoartisans.com>
>Content-Type: text/plain; charset="utf-8"
>
>I've got Mecsoft AlibreCAM generating the tool paths for this in the attached
photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS end mill. 
I'm trying to figure out, using Machinists tool box, exactly what feeds and
speeds could be used for milling the slot.
> 
>I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute the
toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of tool
diameter for depth per pass so 0.025"
> 
>Is that too conservative or likely to break something?  Doing it manually I'd
do it by feel but once it's automatic it's harder to decide SFM and chip load.
> 
>
> 
>Thanks
>John
> 
> 
>-- next part --
>A non-text attachment was scrubbed...
>Name: image001.png
>Type: image/png
>Size: 29705 bytes
>Desc: not available
>
>--
>
>
>
>--
>
>Subject: Digest Footer
>
>___
>Emc-users mailing list
>Emc-users@lists.sourceforge.net
>https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>--
>
>End of Emc-users Digest, Vol 166, Issue 90
>**



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Feeds and speeds

[Stuart Stevenson]

John,

Do you have flood coolant or mist coolant?

I would be inclined to try the cut full depth if you have flood or mist
coolant. 1/4 inch is on the borderline of having the strength necessary to
make a full depth cut.  I would think 5.5ipm might be a little aggressive
but I would leave it programmed at that feed and speed and turn the
feedrate to about 20% to start the cut. After you get into the cut I would
move the feedrate up about 10% to see, hear and feel how mill is cutting. I
would keep moving the feed up until I saw, heard or felt the mill working
too hard. I would then start turning the speed up a little at a time to see
how the mill responds.
I think 30sfm might be a little slow but you can adjust the speed after
entering the cut.
If you can adjust the feed and speed to make the full cut sound good and
you have another part to run I would change your program to enter the cut
as you did the first time but the add lines to make it more aggressive
after you have entered the cut.
If you are leaving a little material to clean up the you can drastically
increase the speed and feed after you turn around at the end of the slot.
Is the slot you are cutting wide enough to allow at least .010 thou. for a
finish pass and maybe a spring pass.
I would make the finish pass and spring pass in a conventional cut rather
than a climb cut.
Stuart


On Tue, Feb 18, 2020 at 8:47 PM John Dammeyer 
wrote:

> I've got Mecsoft AlibreCAM generating the tool paths for this in the
> attached photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS
> end mill.  I'm trying to figure out, using Machinists tool box, exactly
> what feeds and speeds could be used for milling the slot.
>
> I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute
> the toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of
> tool diameter for depth per pass so 0.025"
>
> Is that too conservative or likely to break something?  Doing it manually
> I'd do it by feel but once it's automatic it's harder to decide SFM and
> chip load.
>
>
>
> Thanks
> John
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>


-- 
Addressee is the intended audience.
If you are not the addressee then my consent is not given for you to read
this email furthermore it is my wish you would close this without saving or
reading, and cease and desist from saving or opening my private
correspondence.
Thank you for honoring my wish.

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

[Emc-users] Feeds and speeds

[John Dammeyer]

I've got Mecsoft AlibreCAM generating the tool paths for this in the attached 
photo.  It's Cold Rolled steel 3/16" thick.  I'm using a 1/4" HSS end mill.  
I'm trying to figure out, using Machinists tool box, exactly what feeds and 
speeds could be used for milling the slot.
 
I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute the 
toolbox comes out with  460RPM, 5.5ipm for S460 and F5.5 and 10% of tool 
diameter for depth per pass so 0.025"
 
Is that too conservative or likely to break something?  Doing it manually I'd 
do it by feel but once it's automatic it's harder to decide SFM and chip load.
 

 
Thanks
John
 
 
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine

[Robert Murphy]

John,

I agree the Beagle bone made a very good system, well the first images
from a few years ago. I was using mine to control my mill with a custom
cape.

What turned my to Linuxcnc was just the general support infrastructure.

On 19/2/20 10:26 am, John Dammeyer wrote:

Hi Wallace,
I've been way more successful although also taken a number of stabs at it 
compared to how easy it was to get MACH2 and then MACH3 working.

Even the BeagleBone was easy because the install came with the hal and ini 
files for  the Xylotex.  So in many ways it was just like installing MACH3.  
Very turnkey.  I probably would have stayed with that config except the Xylotex 
cape was set up for NO switches.  And the enable signal internally on the board 
was the wrong polarity so ultimately that project was shelved.  Perhaps to be 
used with the lathe since limits aren't as big an issue with it.

So I went the route of the dual boot PC and I have used LinuxCNC to mill some 
parts.

Support from both forums has been good.  Given that my hardware is somewhat 
non-standard and has some odd issues, I'm finding that LinuxCNC with respect to 
ENABLE and ESTOP is a bit easier for my system.  I have to much around with the 
big red RESET button and the ONLINE button in MACH to get it to work after a 
fault.

Also all things being equal if it's a simple system with say open loop 
steppers, vfd for spindle I think MACH4 is probably worlds easier to set up and 
the Wizards would be that tipping point for the WOW factor.I was also able 
to easily add the Z probe function to my MACH3 setup on the CNC router and at 
the moment I haven't a clue where to begin on that for the mill.

If your existing mill has a BoB with the standard Parallel Port interface I'd 
suggest you find a PC with a parallel port and start simple.  ESTOP, Home/Limit 
switches and XYZ step/dir.  Don't bother about spindle speed or direction.  Use 
one of the predefined configs if possible.

But if you are used to being able to automatically find the X and Y edges and 
have the 0 set after subtracting half the diameter of your probe you won't find 
that in the standard distribution of  Linux and the AXIS user interface.

If things go well then by this summer I may well have an installation manual 
written that helps someone migrate from a PC WINDOWS MACH3 system to a LinuxCNC 
system.  But there's still a lot to do.

John



-Original Message-
From: Marshland Engineering [mailto:marshl...@marshland.co.nz]
Sent: February-18-20 12:18 PM
To: emc-users@lists.sourceforge.net
Subject: [Emc-users] RPI4 is pretty close to a decent machine

Les - Valuable comments, however, some facts.

I'm and BSc electrical engineer and worked as an industrial control engineer
with PLC, servos etc for a number of years.

I have 2 complete PC with Mesa servo drives, wiring, machines retrofitted
etc.
I been following LinuxCNC for a long time, even years before when it was
EMC2.

I have tried 4+ times over the years to get it all to work. I have yet to get
a one system up and running !!

I do understand that my Linux is limited and that is probably the biggest
factor.

I can buy stuff off the shelf from China and get it working, even Mach3 is
easy.

The only reason I went LinuxCNC is that I can retain the handwheels and use
servo drives.

I am going to make space in my calender this year to try again as I can see
that having it running would be a nice compliment to my SouthWestern
Indistries mill. Thread milling would be great.

PS I forgot, spent 15 years as a commercial programmer.

Cheers Wallace



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] How to get 6i25 functioning?

[Peter C. Wallace]

On Wed, 19 Feb 2020, Ed W wrote:


Date: Wed, 19 Feb 2020 00:24:55 +
From: Ed W 
Reply-To: "Enhanced Machine Controller (EMC)"

To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] How to get 6i25 functioning?

On 18/02/2020 23:23, Peter C. Wallace wrote:

On Tue, 18 Feb 2020, Ed W wrote:


Date: Tue, 18 Feb 2020 22:48:08 +
From: Ed W 
Reply-To: "Enhanced Machine Controller (EMC)"

To: emc-users@lists.sourceforge.net
Subject: [Emc-users] How to get 6i25 functioning?

Hi, new user with a 6i25 trying to get off the ground floor. I've 
loaded firmware 5abobx2, then run through pncconf. However, when I 
get to the motor tuning section for an axis I don't see any obvious 
output on the external parallel port alike connector? I'm using a 
meter (which has a basic scope type function as well), but I'm seeing 
nothing happening on pins 2/3 (configured as x axis step/dir)?


Is there some way to debug the 6i25 and confirm it's being 
assimilated correctly? Is there some utility to set/read pins so I 
can confirm it's functioning? Any thoughts on why I'm not seeing any 
output on the connector?



Background: new install on debian 9. Changed the sources to pull in 
linux-cnc 2.8. Used mesa to load firmware something like 5i25-5abobx2 
(yes, the firmware has 5i25, but the card is a 6i25). I see a 
sensible pin output when I run


/mesaflash/ --device 5i25 --readhmid

I was intending to run this with a green china BOB, mainly because it 
seems to be close to a drop in replacement for the USB thing that was 
in my OmioCNC x6 (a slightly better quality 6040 alike). However, at 
present I'm not seeing any life out of the card, so the bob isn't 
connected and I'm just probing the output connector for now.


Mesa firmware came from here (6i25 page):

http://store.mesanet.com/index.php?route=product/product&product_id=58

However, the file name says 5i25.zip is this correct?


Any other thoughts appreciated!

Ed W



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



If you are running linuxCNC, a very quick hardware check of step I/O pins
can be done by measuring the pin state with linuxCNC running and not 
running


If the stepgens are enabled in the linuxCNC config and linuxcnc is 
running,
the idle states of the 6I25 step pins will be low, if linuxcnc is not 
running,

the step pin state should be high (pulled  up to +5V with a 4.7K pullup)


Peter Wallace
Mesa Electronics



OK, well that's encouraging! Running through pncconf the pin is high 
+5v, until I click into the motor tuning when it drops to close to 0V (I 
read about 20mv)


OK, so how do I debug why I don't see any steps coming out..? Hmm. I am 
really unsure what I should be doing here...


Final state is intended to have a cheap bob with step/dir to the chinese 
cheapo clone drivers that came with the omio x6-2200. (I'm not welded to 
the bob, just had it and it has convenient connectors in place). There 
are no encoders, just a simple stepper driver and steppers.


I should show you the settings I have, but the machine isn't 
conveniently close at present... The settings are on whatever defaults 
pncconf gave. From memory P is set to 1000 (not sure what the PID 
settings do with a stepper?), I have no encoders and then I have the 
stepper set to 5,000 and 10,000 in the various stepper timing boxes.


If I click "run" or try and jog in the tuning screen then I see the 
position params appear to change. However, I wonder if the issue could 
be that something here thinks I have a servo and without an encoder it 
isn't going to move and send some steps? Should this screen be showing 
me values which look like servo config?? Have I made some error in 
previous screens?


Thanks for such a fast response - appreciated. Further ideas would be 
very gratefully received!


Ed W


Its hard to guess the issue. do you have a working LinuxCNC configuration?

Do the direction pins change whan you jog in different directions?

( The PID is used to manage the step generation hardware and there is no reason 
to change the default tuning )


It might be more useful to ask for assistance on the LinuxCNC forum where you
can post your hal/ini files





___
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.



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] How to get 6i25 functioning?

[Ed W]

On 18/02/2020 23:23, Peter C. Wallace wrote:

On Tue, 18 Feb 2020, Ed W wrote:


Date: Tue, 18 Feb 2020 22:48:08 +
From: Ed W 
Reply-To: "Enhanced Machine Controller (EMC)"
    
To: emc-users@lists.sourceforge.net
Subject: [Emc-users] How to get 6i25 functioning?

Hi, new user with a 6i25 trying to get off the ground floor. I've 
loaded firmware 5abobx2, then run through pncconf. However, when I 
get to the motor tuning section for an axis I don't see any obvious 
output on the external parallel port alike connector? I'm using a 
meter (which has a basic scope type function as well), but I'm seeing 
nothing happening on pins 2/3 (configured as x axis step/dir)?


Is there some way to debug the 6i25 and confirm it's being 
assimilated correctly? Is there some utility to set/read pins so I 
can confirm it's functioning? Any thoughts on why I'm not seeing any 
output on the connector?



Background: new install on debian 9. Changed the sources to pull in 
linux-cnc 2.8. Used mesa to load firmware something like 5i25-5abobx2 
(yes, the firmware has 5i25, but the card is a 6i25). I see a 
sensible pin output when I run


/mesaflash/ --device 5i25 --readhmid

I was intending to run this with a green china BOB, mainly because it 
seems to be close to a drop in replacement for the USB thing that was 
in my OmioCNC x6 (a slightly better quality 6040 alike). However, at 
present I'm not seeing any life out of the card, so the bob isn't 
connected and I'm just probing the output connector for now.


Mesa firmware came from here (6i25 page):

http://store.mesanet.com/index.php?route=product/product&product_id=58

However, the file name says 5i25.zip is this correct?


Any other thoughts appreciated!

Ed W



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



If you are running linuxCNC, a very quick hardware check of step I/O pins
can be done by measuring the pin state with linuxCNC running and not 
running


If the stepgens are enabled in the linuxCNC config and linuxcnc is 
running,
the idle states of the 6I25 step pins will be low, if linuxcnc is not 
running,

the step pin state should be high (pulled  up to +5V with a 4.7K pullup)


Peter Wallace
Mesa Electronics



OK, well that's encouraging! Running through pncconf the pin is high 
+5v, until I click into the motor tuning when it drops to close to 0V (I 
read about 20mv)


OK, so how do I debug why I don't see any steps coming out..? Hmm. I am 
really unsure what I should be doing here...


Final state is intended to have a cheap bob with step/dir to the chinese 
cheapo clone drivers that came with the omio x6-2200. (I'm not welded to 
the bob, just had it and it has convenient connectors in place). There 
are no encoders, just a simple stepper driver and steppers.


I should show you the settings I have, but the machine isn't 
conveniently close at present... The settings are on whatever defaults 
pncconf gave. From memory P is set to 1000 (not sure what the PID 
settings do with a stepper?), I have no encoders and then I have the 
stepper set to 5,000 and 10,000 in the various stepper timing boxes.


If I click "run" or try and jog in the tuning screen then I see the 
position params appear to change. However, I wonder if the issue could 
be that something here thinks I have a servo and without an encoder it 
isn't going to move and send some steps? Should this screen be showing 
me values which look like servo config?? Have I made some error in 
previous screens?


Thanks for such a fast response - appreciated. Further ideas would be 
very gratefully received!


Ed W




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine

[John Dammeyer]

> -Original Message-
> From: Marshland Engineering [mailto:marshl...@marshland.co.nz]
> Sent: February-18-20 3:54 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] RPI4 is pretty close to a decent machine
> 
> Just a correction, I have setup a few  stepper systems with LinuxCNC and
> step
> and direction is no problem. The problems came in when using 2KW servo
> drives
> and linear scales on the axis. I just could not get the system to respond
> correctly. From memory the StepConfig didn't seem to get the drives to work
> smoothly. My mistake but I did not know how to fix it.
> 
> I have purchased and tried a 80V 20A Servo Drive upgrade Geckodrive G320X
> DG4S-08020 DCS810 from ebay and it worked well on a small motor. I think
> having the servo tuning external to the PC is a good option. This makes the
> LinuxCNC servo installation much easier. '
> 
> Cheers Wallace.

I agree.  In this day and age with the power of embedded systems I believe the 
motors/encoders should be black boxes with a fault output of they have issues.  
The STMBL drive is one example.  The HP_UHU with Henrik Olsson's dsPIC upgrade 
for my brushed DC servos is another.  There are probably a few extras.  I've 
not run the Bergerda AC servo motor and drive long enough but once I made it 
past the teething pains with it I have been considering replacing the brushed 
DC motors with the AC servos.But all the wiring is already done I'm 
reluctant to change things at the moment.  Too many other projects.

John


> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine

[Marshland Engineering]

Just a correction, I have setup a few  stepper systems with LinuxCNC and step
and direction is no problem. The problems came in when using 2KW servo drives
and linear scales on the axis. I just could not get the system to respond
correctly. From memory the StepConfig didn't seem to get the drives to work
smoothly. My mistake but I did not know how to fix it. 

I have purchased and tried a 80V 20A Servo Drive upgrade Geckodrive G320X
DG4S-08020 DCS810 from ebay and it worked well on a small motor. I think
having the servo tuning external to the PC is a good option. This makes the
LinuxCNC servo installation much easier. '

Cheers Wallace. 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine

[John Dammeyer]

Hi Wallace,
I've been way more successful although also taken a number of stabs at it 
compared to how easy it was to get MACH2 and then MACH3 working.

Even the BeagleBone was easy because the install came with the hal and ini 
files for  the Xylotex.  So in many ways it was just like installing MACH3.  
Very turnkey.  I probably would have stayed with that config except the Xylotex 
cape was set up for NO switches.  And the enable signal internally on the board 
was the wrong polarity so ultimately that project was shelved.  Perhaps to be 
used with the lathe since limits aren't as big an issue with it.

So I went the route of the dual boot PC and I have used LinuxCNC to mill some 
parts.

Support from both forums has been good.  Given that my hardware is somewhat 
non-standard and has some odd issues, I'm finding that LinuxCNC with respect to 
ENABLE and ESTOP is a bit easier for my system.  I have to much around with the 
big red RESET button and the ONLINE button in MACH to get it to work after a 
fault.

Also all things being equal if it's a simple system with say open loop 
steppers, vfd for spindle I think MACH4 is probably worlds easier to set up and 
the Wizards would be that tipping point for the WOW factor.I was also able 
to easily add the Z probe function to my MACH3 setup on the CNC router and at 
the moment I haven't a clue where to begin on that for the mill.  

If your existing mill has a BoB with the standard Parallel Port interface I'd 
suggest you find a PC with a parallel port and start simple.  ESTOP, Home/Limit 
switches and XYZ step/dir.  Don't bother about spindle speed or direction.  Use 
one of the predefined configs if possible.

But if you are used to being able to automatically find the X and Y edges and 
have the 0 set after subtracting half the diameter of your probe you won't find 
that in the standard distribution of  Linux and the AXIS user interface.  

If things go well then by this summer I may well have an installation manual 
written that helps someone migrate from a PC WINDOWS MACH3 system to a LinuxCNC 
system.  But there's still a lot to do.

John


> -Original Message-
> From: Marshland Engineering [mailto:marshl...@marshland.co.nz]
> Sent: February-18-20 12:18 PM
> To: emc-users@lists.sourceforge.net
> Subject: [Emc-users] RPI4 is pretty close to a decent machine
> 
> Les - Valuable comments, however, some facts.
> 
> I'm and BSc electrical engineer and worked as an industrial control engineer
> with PLC, servos etc for a number of years.
> 
> I have 2 complete PC with Mesa servo drives, wiring, machines retrofitted
> etc.
> I been following LinuxCNC for a long time, even years before when it was
> EMC2.
> 
> I have tried 4+ times over the years to get it all to work. I have yet to get
> a one system up and running !!
> 
> I do understand that my Linux is limited and that is probably the biggest
> factor.
> 
> I can buy stuff off the shelf from China and get it working, even Mach3 is
> easy.
> 
> The only reason I went LinuxCNC is that I can retain the handwheels and use
> servo drives.
> 
> I am going to make space in my calender this year to try again as I can see
> that having it running would be a nice compliment to my SouthWestern
> Indistries mill. Thread milling would be great.
> 
> PS I forgot, spent 15 years as a commercial programmer.
> 
> Cheers Wallace
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine

[Chris Albertson]

This is a problem with many people using Linux to do something complex like
build a CNC system or using ROS to build a robot.  They are doing something
complex with Linux before they try to do simple things with Linux.

The best approach is to fist use Linux for everyday tasks, like reading and
writing emails, watching youtube videos.  Simply use it for all your normal
tasks.Get rid of your Windows system.

It is a little like buying a harbor freight mini lathe and then your first
project is a working gas airplane engine.

On Tue, Feb 18, 2020 at 12:20 PM Marshland Engineering <
marshl...@marshland.co.nz> wrote:

> Les - Valuable comments, however, some facts.
>
> I'm and BSc electrical engineer and worked as an industrial control
> engineer
> with PLC, servos etc for a number of years.
>
> I have 2 complete PC with Mesa servo drives, wiring, machines retrofitted
> etc.
> I been following LinuxCNC for a long time, even years before when it was
> EMC2.
>
> I have tried 4+ times over the years to get it all to work. I have yet to
> get
> a one system up and running !!
>
> I do understand that my Linux is limited and that is probably the biggest
> factor.
>
> I can buy stuff off the shelf from China and get it working, even Mach3 is
> easy.
>
> The only reason I went LinuxCNC is that I can retain the handwheels and use
> servo drives.
>
> I am going to make space in my calender this year to try again as I can see
> that having it running would be a nice compliment to my SouthWestern
> Indistries mill. Thread milling would be great.
>
> PS I forgot, spent 15 years as a commercial programmer.
>
> Cheers Wallace
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>


-- 

Chris Albertson
Redondo Beach, California

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] How to get 6i25 functioning?

[Peter C. Wallace]

On Tue, 18 Feb 2020, Ed W wrote:


Date: Tue, 18 Feb 2020 22:48:08 +
From: Ed W 
Reply-To: "Enhanced Machine Controller (EMC)"

To: emc-users@lists.sourceforge.net
Subject: [Emc-users] How to get 6i25 functioning?

Hi, new user with a 6i25 trying to get off the ground floor. I've loaded 
firmware 5abobx2, then run through pncconf. However, when I get to the motor 
tuning section for an axis I don't see any obvious output on the external 
parallel port alike connector? I'm using a meter (which has a basic scope 
type function as well), but I'm seeing nothing happening on pins 2/3 
(configured as x axis step/dir)?


Is there some way to debug the 6i25 and confirm it's being assimilated 
correctly? Is there some utility to set/read pins so I can confirm it's 
functioning? Any thoughts on why I'm not seeing any output on the connector?



Background: new install on debian 9. Changed the sources to pull in linux-cnc 
2.8. Used mesa to load firmware something like 5i25-5abobx2 (yes, the 
firmware has 5i25, but the card is a 6i25). I see a sensible pin output when 
I run


/mesaflash/ --device 5i25 --readhmid

I was intending to run this with a green china BOB, mainly because it seems 
to be close to a drop in replacement for the USB thing that was in my OmioCNC 
x6 (a slightly better quality 6040 alike). However, at present I'm not seeing 
any life out of the card, so the bob isn't connected and I'm just probing the 
output connector for now.


Mesa firmware came from here (6i25 page):

http://store.mesanet.com/index.php?route=product/product&product_id=58

However, the file name says 5i25.zip is this correct?


Any other thoughts appreciated!

Ed W



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



If you are running linuxCNC, a very quick hardware check of step I/O pins
can be done by measuring the pin state with linuxCNC running and not running

If the stepgens are enabled in the linuxCNC config and linuxcnc is running,
the idle states of the 6I25 step pins will be low, if linuxcnc is not running,
the step pin state should be high (pulled  up to +5V with a 4.7K pullup)


Peter Wallace
Mesa Electronics



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

[Emc-users] How to get 6i25 functioning?

[Ed W]

Hi, new user with a 6i25 trying to get off the ground floor. I've loaded 
firmware 5abobx2, then run through pncconf. However, when I get to the 
motor tuning section for an axis I don't see any obvious output on the 
external parallel port alike connector? I'm using a meter (which has a 
basic scope type function as well), but I'm seeing nothing happening on 
pins 2/3 (configured as x axis step/dir)?


Is there some way to debug the 6i25 and confirm it's being assimilated 
correctly? Is there some utility to set/read pins so I can confirm it's 
functioning? Any thoughts on why I'm not seeing any output on the 
connector?



Background: new install on debian 9. Changed the sources to pull in 
linux-cnc 2.8. Used mesa to load firmware something like 5i25-5abobx2 
(yes, the firmware has 5i25, but the card is a 6i25). I see a sensible 
pin output when I run


/mesaflash/ --device 5i25 --readhmid

I was intending to run this with a green china BOB, mainly because it 
seems to be close to a drop in replacement for the USB thing that was in 
my OmioCNC x6 (a slightly better quality 6040 alike). However, at 
present I'm not seeing any life out of the card, so the bob isn't 
connected and I'm just probing the output connector for now.


Mesa firmware came from here (6i25 page):

http://store.mesanet.com/index.php?route=product/product&product_id=58

However, the file name says 5i25.zip is this correct?


Any other thoughts appreciated!

Ed W



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine

[Gene Heskett]

On Tuesday 18 February 2020 17:16:59 Robert Murphy wrote:

> On 19/2/20 7:17 am, Marshland Engineering wrote:
> > Les - Valuable comments, however, some facts.
> >
> > I'm and BSc electrical engineer and worked as an industrial control
> > engineer with PLC, servos etc for a number of years.
> >
> > I have 2 complete PC with Mesa servo drives, wiring, machines
> > retrofitted etc. I been following LinuxCNC for a long time, even
> > years before when it was EMC2.
> >
> > I have tried 4+ times over the years to get it all to work. I have
> > yet to get a one system up and running !!
> >
> > I do understand that my Linux is limited and that is probably the
> > biggest factor.
> >
> > I can buy stuff off the shelf from China and get it working, even
> > Mach3 is easy.
> >
> > The only reason I went LinuxCNC is that I can retain the handwheels
> > and use servo drives.
> >
> > I am going to make space in my calender this year to try again as I
> > can see that having it running would be a nice compliment to my
> > SouthWestern Indistries mill. Thread milling would be great.
> >
> > PS I forgot, spent 15 years as a commercial programmer.
> >
> > Cheers Wallace
>
> I'm a basic Builder's\Civil labourer and have had no trouble getting
> Linuxcnc up and running.
>
> Linuxcnc had really nothing to do with "Linux Skills" it's being able
> to follow instructions as per any new app you would install,
> regardless of OS.
>
> I can't get my head around Autocad, Fusion 360, is that because my
> "Windows Skills" are lacking ?
>
> Rob
>
Could be, I've had a bounty on windows crap, for 30 years, it gets nuked 
sooner rather than later here except for one win10home on a really cheap 
hp, gets used as a display for a redpitaya's smith chart antenna tuner.  
Works nice for that. Part of my retirement cash cow. :)
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] preempt-rt on the pi4b

[Gene Heskett]

On Tuesday 18 February 2020 16:47:36 Dave Matthews wrote:

> On Tue, Feb 18, 2020 at 4:23 PM Gene Heskett  
wrote:
> > Humm, yur right, so until I can fix that, add lathe-stf to the end
> > of the address bar, and that will get you a directory listing, find
> > linuxcnc4pi4b in that list and click on it.  You should be there.
>
> That did the trick.  I grabbed linuxcnc-uspace_2.9.0~pre0_armhf.deb
> while I was there.  Guessing that is what I want to install when I
> have time to play with this.
>
> Dave
>
Probably should have grabbed the Docs too, quite a bit of that has been 
updated to clarify stuff now and then.
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine

[Robert Murphy]

On 19/2/20 7:17 am, Marshland Engineering wrote:

Les - Valuable comments, however, some facts.

I'm and BSc electrical engineer and worked as an industrial control engineer
with PLC, servos etc for a number of years.

I have 2 complete PC with Mesa servo drives, wiring, machines retrofitted etc.
I been following LinuxCNC for a long time, even years before when it was EMC2.

I have tried 4+ times over the years to get it all to work. I have yet to get
a one system up and running !!

I do understand that my Linux is limited and that is probably the biggest
factor.

I can buy stuff off the shelf from China and get it working, even Mach3 is
easy.

The only reason I went LinuxCNC is that I can retain the handwheels and use
servo drives.

I am going to make space in my calender this year to try again as I can see
that having it running would be a nice compliment to my SouthWestern
Indistries mill. Thread milling would be great.

PS I forgot, spent 15 years as a commercial programmer.

Cheers Wallace


I'm a basic Builder's\Civil labourer and have had no trouble getting
Linuxcnc up and running.

Linuxcnc had really nothing to do with "Linux Skills" it's being able to
follow instructions as per any new app you would install, regardless of OS.

I can't get my head around Autocad, Fusion 360, is that because my
"Windows Skills" are lacking ?

Rob




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] preempt-rt on the pi4b

[Dave Matthews]

On Tue, Feb 18, 2020 at 4:23 PM Gene Heskett  wrote:
>
> >
> Humm, yur right, so until I can fix that, add lathe-stf to the end of the
> address bar, and that will get you a directory listing, find
> linuxcnc4pi4b in that list and click on it.  You should be there.
>
That did the trick.  I grabbed linuxcnc-uspace_2.9.0~pre0_armhf.deb
while I was there.  Guessing that is what I want to install when I
have time to play with this.

Dave


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] preempt-rt on the pi4b

[Gene Heskett]

On Tuesday 18 February 2020 16:09:01 Dave Matthews wrote:

> On Tue, Feb 18, 2020 at 3:37 PM Gene Heskett  
wrote:
> > Assuming it already has the full raspbian 10.2 or later image on the
> > u-sd card, goto my site in the sig, find the lathe-stf link, click
> > on it, find the linuxcnc4pi4b directory and download rt-kernel.tgz. 
> > Unpack it in /, reboot, and it should show a uname -a of:
> > Linux rpi4.coyote.den 4.19.71-rt24-v7l+ #1 SMP PREEMPT RT Thu Feb 6
> > 07:09:18 EST 2020 armv7l GNU/Linux
>
> Not finding it on the url in your sig.  The word lathe appears on the
> page twice.  There is a link near them but that goes 404.
>
> Dave
>
Humm, yur right, so until I can fix that, add lathe-stf to the end of the 
address bar, and that will get you a directory listing, find 
linuxcnc4pi4b in that list and click on it.  You should be there.

>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] preempt-rt on the pi4b

[Dave Matthews]

On Tue, Feb 18, 2020 at 3:37 PM Gene Heskett  wrote:

>
> Assuming it already has the full raspbian 10.2 or later image on the u-sd
> card, goto my site in the sig, find the lathe-stf link, click on it,
> find the linuxcnc4pi4b directory and download rt-kernel.tgz.  Unpack it
> in /, reboot, and it should show a uname -a of:
> Linux rpi4.coyote.den 4.19.71-rt24-v7l+ #1 SMP PREEMPT RT Thu Feb 6
> 07:09:18 EST 2020 armv7l GNU/Linux
>
Not finding it on the url in your sig.  The word lathe appears on the
page twice.  There is a link near them but that goes 404.

Dave


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Got my new ATS-667's today, but thats a math connundrum for me.

[Gene Heskett]

On Tuesday 18 February 2020 12:05:31 Chris Albertson wrote:

> You all have missed the first and most important step.  You have to
> first adust the sensor so that it gives a 50% duty cycle square wave
> at all speeds.   With an inductive sensor and a fast-moving gear you
> might not get 50% from max speed to zero in both directions.
>
> Only after you are getting a 50% duty square wave in BOTH directions
> can you think about how to place the second sensor.   The signal from
> the second sensor needs to by 90 degrees out of phase from the first. 
>One cycle is from the leading edge of a pulse to the leading edge
> of the next pulse.If the sensor is "perfect" then the distance is
> in fact 1/2 of a tooth or 1/4 of a cycle.  (remember that a cycle
> includes both the pulse and the low "non-pulse" that follows.)
>
> If the sensor can't by adjusted for a 50% duty cycle then you can make
> a "fake" quadrature sigal that only works if you look at the leading
> edges but this would have (1) a position error when you change
> direction and (2) only half the resolution, because you only look at
> the leading edges. You really want exactly 50%   This is why optical
> encoders are so popular. Then can be near perfect.
>
The ATS-667's we were talking about, purposely have an AGC that combined 
with a built in schmidt trigger, give about a 52% square wave. If they 
are spaced correctly thats plenty good enough for the girls I go with 
considering it stays at the nominally 52% at any speed from stopped to 
several thousand revs.  Hall effects as I understand them are nanosecond 
responders. I assume they aren't balanced at 50% just to keep the 
magnetics of a nearby flourescent fixture from getting up to a noise 
trigger. It may also be because they sense the top of a tooth which is 
narrower than the gap between the teeth. Any one or a combination of 
theories, but the bottom line is that it works well with linuxcnc when  
its not tied up with a PID to amplify the quantization noise. All this 
encoder is tasked with is the cross connection to z for rigid tapping. 

>
> On Tue, Feb 18, 2020 at 1:09 AM Les Newell 
>
> wrote:
> > Hi Jon,
> >
> > Thinking about it, you're mostly right. I didn't think it through.
> > My suggested spacing assumes the teeth are square, which of course
> > they are not.
> > The actual spacing is going to depend on the sensing range of the
> > sensors and width of the tips of the teeth. 1/4 tooth spacing is
> > likely a good starting point. You aren't going to get anywhere near
> > perfect 90 degree quadrature but there isn't much you can do about
> > it.
> >
> > Les
> >
> > On 18/02/2020 05:00, Jon Elson wrote:
> > > On 02/17/2020 03:57 PM, Les Newell wrote:
> > >> They should be any multiple of the tooth spacing plus half a
> > >> tooth spacing.
> > >
> > > Nope, I made that mistake first time.  It should be "plus 1/4 of a
> > > tooth space".
> > >
> > > Jon
> > >
> > >
> > > ___
> > > Emc-users mailing list
> > > Emc-users@lists.sourceforge.net
> > > https://lists.sourceforge.net/lists/listinfo/emc-users
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Got my new ATS-667's today, but thats a math connundrum for me.

[Gene Heskett]

On Monday 17 February 2020 23:59:47 Jon Elson wrote:

> On 02/17/2020 03:20 PM, Gene Heskett wrote:
> > How far apart are they to be to output a good quadrature signal?
> >
> > Mounting them with JBKwik weld seems to be a lot less forgiving
> > because its not possible to move them a few thou to fine tune like
> > it was when using relatively flexible goop.
>
> Well, one sensor should be centered right on a tooth, and
> the other should be 1/4 of the way off
> a tooth.  The best way to check the phase alignment is to
> put a 2-channel scope on it and spin the
> spindle.  If you don't like it, then adjust and try again.
> That's how I did it.  First, I was dumb and
> put one sensor on the tooth and one on the valley.  After
> MANY minutes of confusion, I realized that
> was NOT what quadrature meant!
>
> Jon
>
I got bit by that too, which is why the slots in my bracket are wider 
than the ats-667's, but I've been busy since about 5 getting a pi4b 
kernel put up on my web page wth a eal simple installer.  And the missus 
wants lasagna for dinner, so the next 45 minutes is baby sitting the 
oven.
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

[Emc-users] preempt-rt on the pi4b

[Gene Heskett]

Greetings all;

I have finally managed hack up a script to make an installable version of 
4.19.71-rt24-v7l+ for the pi4.

Assuming it already has the full raspbian 10.2 or later image on the u-sd 
card, goto my site in the sig, find the lathe-stf link, click on it, 
find the linuxcnc4pi4b directory and download rt-kernel.tgz.  Unpack it 
in /, reboot, and it should show a uname -a of:
Linux rpi4.coyote.den 4.19.71-rt24-v7l+ #1 SMP PREEMPT RT Thu Feb 6 
07:09:18 EST 2020 armv7l GNU/Linux

Latency is in the 16 microseconds territory, and it runs my Sheldon lathe 
with all its gingerbread, and it has a bunch flawlessly with the cpu 
speed only pushed to 800 MHz. So the pi is figuratively loafing on the 
beach. :)

Have fun all you pi4 fans.

Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

[Emc-users] RPI4 is pretty close to a decent machine

[Marshland Engineering]

Les - Valuable comments, however, some facts. 

I'm and BSc electrical engineer and worked as an industrial control engineer
with PLC, servos etc for a number of years. 

I have 2 complete PC with Mesa servo drives, wiring, machines retrofitted etc.
I been following LinuxCNC for a long time, even years before when it was EMC2.

I have tried 4+ times over the years to get it all to work. I have yet to get
a one system up and running !!

I do understand that my Linux is limited and that is probably the biggest
factor.

I can buy stuff off the shelf from China and get it working, even Mach3 is
easy. 

The only reason I went LinuxCNC is that I can retain the handwheels and use
servo drives. 

I am going to make space in my calender this year to try again as I can see
that having it running would be a nice compliment to my SouthWestern
Indistries mill. Thread milling would be great. 

PS I forgot, spent 15 years as a commercial programmer. 

Cheers Wallace



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine control solution...

[Sam Sokolik]

well..  I know a lot of us have strong feelings for linuxcnc.  For me it is
seeing what it can actually do..

As (I think) Les had said.  you can run the smallest desktop machine all
the way up to a machining center with pallets and tool changer.

This is what really sold me.   We have the K&T with analog servos, 60 tool
chain and changer, pallets and all sorts of do-dads.
I bought 2 mesa cards + analog interface cards.  This gave me 90+ i/o and
10 analog/encoder counters.

Everything is controlled within linuxcnc - between the integrated ladder
and hal.  tool changes, spindle gear changes, pallet changes..  All done
within linuxcnc and all realtime..  No external plc's or anything.

sam

On Tue, Feb 18, 2020 at 11:15 AM John Dammeyer 
wrote:

> > I'm sorry, this is degenerating into a useless argument and I'm gonna
> > take a step back and leave you to it.
> >
> > Les
> >
> Thank you.  Your insights have been invaluable.
> John
> >
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine control

[dave engvall]

On 2/17/20 5:18 PM, Ed wrote:

On 2/17/20 6:20 PM, John Dammeyer wrote:

From: Sam Sokolik [mailto:samco...@gmail.com]
Because your examples are not running a full operating system...
I don't buy that.  That's like saying.  Look.  The ride is a tad 
uncomfortable but that's to be expected.  After all this is a 10 Ton 
gravel truck.  But look at what it can carry.  True it's only 
groceries today and most days but that one time it will come in so 
handy...  dear...


John

I'll buy that because it is true. Linuxcnc carries the baggage of 
being a motion controller with attached OS. If you like using a go 
between board that uses a $2 chip that sings and dances go gettum. 
Check and see the availability of that chip in a couple years.


Many CNC users don't measure machine life in weeks or months or years 
but DECADES. My first LCNC machine is still going strong after almost 
20 years, step and direction to Gecko 320's. Where will the Pi be in 
20 years or your $2 chip?


Not to knock using a Pi or whatever but to point to the fact that a PC 
running LCNC is the point to measure from and will remain so.


The $2 chip solution may a great thing esp in a headless setup as a 
facilitator but I would buy backups.



Ed.


Quote on a BP dealer site:

"Knee Mill Series I is the most popular vertical milling machine ever 
made with over 370,000 machines built over the past 70-plus years."


I suspect people that buy Griz mills, etc. start out bare and work into 
axis motor drives and maybe eventually full cnc. Part of that is cash 
flow; if you are young and have a family there simply isn't enough 
money. It gets better after the kids leave home and the dog dies. :-)


In the early 2000's manual mills could be had for hauling them off. I 
bought a Mazak V5 for $1500 ...  with a dead  control. Of course getting 
it here and shoehorned into the shop, adding new servo drives, etc is 
another story, a long story.


Speaking of motion control; we have no control over the availability of 
usable cpu's. So far we've been lucky. I like the idea of motion 
residing in a microcontroller but in terms of something surviving for 
years I think that a product based  on a popular FPGA series has the 
best chance of being viable over time. Use the FPGA only for motion and 
a general purpose computer for all the non-realtime stuff. Can I do this 
... not a chance. I do best at ideas and let the really smart people do 
the rest.


Dave









___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine control solution...

[John Dammeyer]

> I'm sorry, this is degenerating into a useless argument and I'm gonna
> take a step back and leave you to it.
> 
> Les
> 
Thank you.  Your insights have been invaluable.
John
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Got my new ATS-667's today, but thats a math connundrum for me.

[Jon Elson]

On 02/18/2020 03:06 AM, Les Newell wrote:

Hi Jon,

Thinking about it, you're mostly right. I didn't think it 
through. My suggested spacing assumes the teeth are 
square, which of course they are not.
The actual spacing is going to depend on the sensing range 
of the sensors and width of the tips of the teeth. 1/4 
tooth spacing is likely a good starting point. You aren't 
going to get anywhere near perfect 90 degree quadrature 
but there isn't much you can do about it.


The ATS667 series have two Hall sensors, and detect the 
passing of the tooth from closer to one sensor to closer to 
the other.
So, it always is supposed to switch right as the leading 
edge of the tooth passes the exact center of the sensor.
Actually, they give VERY good quadrature and quite close to 
50% pulse width, at least on my system.


Jon


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Got my new ATS-667's today, but thats a math connundrum for me.

[Chris Albertson]

You all have missed the first and most important step.  You have to first
adust the sensor so that it gives a 50% duty cycle square wave at all
speeds.   With an inductive sensor and a fast-moving gear you might not get
50% from max speed to zero in both directions.

Only after you are getting a 50% duty square wave in BOTH directions can
you think about how to place the second sensor.   The signal from the
second sensor needs to by 90 degrees out of phase from the first. One
cycle is from the leading edge of a pulse to the leading edge of the next
pulse.If the sensor is "perfect" then the distance is in fact 1/2 of a
tooth or 1/4 of a cycle.  (remember that a cycle includes both the pulse
and the low "non-pulse" that follows.)

If the sensor can't by adjusted for a 50% duty cycle then you can make a
"fake" quadrature sigal that only works if you look at the leading edges
but this would have (1) a position error when you change direction and (2)
only half the resolution, because you only look at the leading edges. You
really want exactly 50%   This is why optical encoders are so popular.
Then can be near perfect.



On Tue, Feb 18, 2020 at 1:09 AM Les Newell 
wrote:

> Hi Jon,
>
> Thinking about it, you're mostly right. I didn't think it through. My
> suggested spacing assumes the teeth are square, which of course they are
> not.
> The actual spacing is going to depend on the sensing range of the
> sensors and width of the tips of the teeth. 1/4 tooth spacing is likely
> a good starting point. You aren't going to get anywhere near perfect 90
> degree quadrature but there isn't much you can do about it.
>
> Les
>
>
> On 18/02/2020 05:00, Jon Elson wrote:
> > On 02/17/2020 03:57 PM, Les Newell wrote:
> >> They should be any multiple of the tooth spacing plus half a tooth
> >> spacing.
> >>
> > Nope, I made that mistake first time.  It should be "plus 1/4 of a
> > tooth space".
> >
> > Jon
> >
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>


-- 

Chris Albertson
Redondo Beach, California

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine control solution...

[Les Newell]

I don't buy that.  That's like saying.  Look.  The ride is a tad uncomfortable 
but that's to be expected.  After all this is a 10 Ton gravel truck.  But look 
at what it can carry.  True it's only groceries today and most days but that 
one time it will come in so handy...  dear...


I'd much rather have my 10 ton dump truck with a windscreen I can see 
out of and that can go around corners rather than your tricycle with a 
windscreen the size of a postage stamp and can't go around corners. But 
the ride is sweet...


Not to mention I very often need to haul 10 tons, not just occasionally.


I went to the Grizzly tools site.  I think I counted 38 mills.  None of them 
CNC.
You are cherry picking your results. By the same logic I can go to the 
Haas website and not find any manual machines. Therefore no-one uses 
manual machines.
For more realistic results, how about people who actually use machines 
on a regular basis? Go to any engineering job shop and take a look at 
their machines. Most will be CNC. They may have the odd manual gathering 
dust for occasional very simple on-off tasks.



CNC routers can't really operate with hand wheels so they are a different class 
of hardware
Huh? LinuxCNC runs CNC machines. By definition CNC routers are CNC 
machines.


You seem to have a fixed idea of what all users want, when in fact it's 
just what you want. Anything else doesn't count or is being done wrong. 
I'm sorry, this is degenerating into a useless argument and I'm gonna 
take a step back and leave you to it.


Les




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Got my new ATS-667's today, but thats a math connundrum for me.

[Les Newell]

Hi Jon,

Thinking about it, you're mostly right. I didn't think it through. My 
suggested spacing assumes the teeth are square, which of course they are 
not.
The actual spacing is going to depend on the sensing range of the 
sensors and width of the tips of the teeth. 1/4 tooth spacing is likely 
a good starting point. You aren't going to get anywhere near perfect 90 
degree quadrature but there isn't much you can do about it.


Les


On 18/02/2020 05:00, Jon Elson wrote:

On 02/17/2020 03:57 PM, Les Newell wrote:
They should be any multiple of the tooth spacing plus half a tooth 
spacing.


Nope, I made that mistake first time.  It should be "plus 1/4 of a 
tooth space".


Jon


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users





___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] RPI4 is pretty close to a decent machine control solution...

[Phill Carter]

> On 18 Feb 2020, at 6:51 pm, John Dammeyer  wrote:
> 
> I went to the Grizzly tools site.  I think I counted 38 mills.  None of them 
> CNC.  
> KBC tools here in Canada has, in the this month's flier, 5 milling machines 
> of various sizes and only one CNC milling machine with Acu-Rite control for 
> $41K.
> KMS tools aas 4, none of them CNC.
> Don't know how many Sherline mills are sold with or without the CNC kit.
> 
> No idea how many used Bridgeport type machines are out there starting from 
> say post war 1945 over 85 years?  I believe CNC machines are a small fraction 
> of those even if there were 10K MACH3 licenses sold.  And of those licenses 
> how many actually went to CNC routers.   I have one with a valid MACH3 
> license but it's one built from scratch.  CNC routers can't really operate 
> with hand wheels so they are a different class of hardware.
> 
> Judging by the number of $250 to $500 CNC controllers available through 
> AliExpress I'd guess the number of non-CNC machines out there is still really 
> high.
> 
Handy to know...



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users