Re: [Emc-users] Threading on a mill with fourth axis
Andy, I've never seen such a grinding wheel around here. Can you please tell me about who is supplying these, and for which purpose? Peter Am 22.03.2013 17:18, schrieb andy pugh: On 22 March 2013 15:56, Gene Heskett ghesk...@wdtv.com wrote: I have been threatening to make me one of those disks and buy an oz of diamond dust in oil. I have never seen such a tool sharpener in the catalogs since. http://www.frets.com/HomeShopTech/Projects/HandCrankGrinder/handcrankgrinder.html -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Very cool Igor... even better than a skate boarding dog... ! ;-) This needs to go into the Wiki.. Dave On 3/21/2013 7:39 PM, Igor Chudov wrote: Here's a VIDEO of this working. Not the most fun video like a skateboarding dog, but it shows the nature of the process. http://www.youtube.com/watch?v=JMENnIJrl9Y On Thu, Mar 21, 2013 at 5:41 PM, Igor Chudovichu...@gmail.com wrote: I am not sure how I can put the code in Wiki. I am releasing the following code under the GNU Public License: (Makes a thread on a round part rotated in my fourth axis) (Uses a 60 degree end mill) Othread_on_fourth_axis sub #x0 = #1 (X0, left side) #x1 = #2 (X1, right side) #y= #3 (Y, middle of the top edge of the round) #z0 = #4 (Z, top of the edge of the round) #safez= #5 (Safe Z for rapids) #zstep= #6 (Z Step, positive) #spr = #7 (Step Per Revolution, Also determines Total Depth) #depth= #8 (Depth of thread, positive, determined automatically if 0 based on 60 degree thread.) #diameter = #9 (Diameter of the round, needed for calculations of feed rate) #frate= #10 (feed rate based on surface speed) #left_handed = #11 (Set to 1 if left handed) #rpm = [#frate/3.1415/#diameter] #horizontal_feedrate = [#rpm*#spr] #vertical_feedrate= [#frate/5] #total_angle = [ 360 * [#x1-#x0]/#spr ] (Set negative total angle if left handed thread) Oif if [#left_handed NE 0] #total_angle = [-#total_angle] Oif endif Oif if [#depth EQ 0] #depth = [#spr*1.73205/2] (depth = spr * sqrt 3 / 2 ) Oif endif Owithdraw call [#safez] G0 A0 (go to 0 degree) G0 X[#x0] Y[#y] Z[#safez] ( Start drilling down to Z0, I could rapid, ) ( but slow is safer, will not break end mill ) G1 Z[#z0] F[#vertical_feedrate] #direction = 1 (1 is right, 2 is left) #z = #z0 Oloop while [ 1 ] #z = [#z - #zstep] Oif if [#z LT [#z0 - #depth] ] #z = [#z0 - #depth] Oif endif G1 Z[#z] F[#vertical_feedrate] (Depending on direction, we go to X1 on the right and turn total_angle,) (or go to X0 on the left and go back to ZERO angle) Oif if [#direction EQ 1 ] #direction = 0 G1 X[#x1] A[#total_angle] F[#horizontal_feedrate] Oif else #direction = 1 G1 X[#x0] A0 F[#horizontal_feedrate] Oif endif Oif if [ #z LE [#z0 - #depth] ] Oloop break Oif endif Oloop endwhile Owithdraw call [#safez] G0 X[#x1] G0 A0 (go to 0 degree) Othread_on_fourth_axis endsub M2 On Thu, Mar 21, 2013 at 10:46 AM, Gene Heskettghesk...@wdtv.com wrote: On Thursday 21 March 2013 11:44:24 Igor Chudov did opine: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Thanks to all! That ought to be put in the wiki, Igor. Can you? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page:http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml For courage mounteth with occasion. -- William Shakespeare, King John I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list
Re: [Emc-users] Threading on a mill with fourth axis
On Fri, Mar 22, 2013 at 2:34 AM, Igor Chudov ichu...@gmail.com wrote: Yes, I would love to find a suitably shaped end mill for ACME threads. end mill...n This is the way I do acme https://www.youtube.com/watch?v=Jbp8SJ9RxqI Dave Caroline -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Hi, regarding the ACME end mill: I would love to find a suitably shaped end mill for ACME threads. From time to time I order custom made or modified solid carbide end mills from a local company [1] equipped with the latest technologies in CNC grinding. These special mills are surprisingly cheap, grinding the shaft down to a specified diameter costs about 5 to 10 EUR, an end mill with a custom designed profile (the last one was a cone with ball end about 50 mm long, 6 mm diameter) was about 50 EUR. cu Flo [1] http://www.wedco.at/ -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Friday 22 March 2013 11:22:16 jeremy youngs did opine: forgive me but im recalling the cnc mill vs lathe discussion of about a week ago and im thinking both of these operations can be done in a cnc lathe with a 3 dollar hand ground hss tool. im not knocking what you have accomplished as its good work inddeed:) im just sayin :) I think that was a little more than a week ago, but the only time I tried to hand grind a single tooth, I took it back to the mill with the thread half cut and resharpened it to the proper angles using my A axis to set the angles. I can get a far sharper edge using a dremel diamond disk than I can hand grind on a 120 grit wheel on my bench grinder. I do not turn it with the dremel though as its minimum speed is still too fast, overheating the diamond and dulling it prematurely. The 2500 revs my mill can muster works much better. When I was a bench tech at OceanoGraphic Engineering in 1959, I saw our machinist pull an small electric motor powered thing out of his tool cupboard, that had a 1/4 post sticking up out of its frame along side a brass disk the motor turned at about 200 rpm, and a tool holder that looked like a block of swiss cheese with many 1/4 holes through it at marked angles. He wet the top of that brass disk with a small drop of diamond dust in oil added enough oil to coat the disk smeared it around for an even coat. Fixing a dull 1/4 hss tool in the holder, he then spent about 30 seconds on each face of the tool by dropping it over the post so it was held at the right angle swept it over the face of the spinning wheel. Took about a minute. Tested it on his arm to see if it cut hair, which it did. He took it back to the huge Clausing we had bought to make cases for the cameras used it for about an hour making the cuts in the end of two bronze cases about 7 in diameter where the Navy supplied quartz windows were to be fitted. They were going on the Trieste for its dive into the marianes trench in Feb '60. Or 61, I forget, but wikipedia has the details anyway. I have been threatening to make me one of those disks and buy an oz of diamond dust in oil. I have never seen such a tool sharpener in the catalogs since. Do any of the other old timers here have, or know where one similar could be purchased today? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml Alimony is the curse of the writing classes. -- Norman Mailer I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On 22 March 2013 15:56, Gene Heskett ghesk...@wdtv.com wrote: I have been threatening to make me one of those disks and buy an oz of diamond dust in oil. I have never seen such a tool sharpener in the catalogs since. http://www.frets.com/HomeShopTech/Projects/HandCrankGrinder/handcrankgrinder.html -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Dave Caroline wrote: On Fri, Mar 22, 2013 at 2:34 AM, Igor Chudov ichu...@gmail.com wrote: Yes, I would love to find a suitably shaped end mill for ACME threads. end mill...n This is the way I do acme https://www.youtube.com/watch?v=Jbp8SJ9RxqI And that's the PROPER way to do it. Jon -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Fri, Mar 22, 2013 at 5:13 PM, Jon Elson el...@pico-systems.com wrote: Dave Caroline wrote: On Fri, Mar 22, 2013 at 2:34 AM, Igor Chudov ichu...@gmail.com wrote: Yes, I would love to find a suitably shaped end mill for ACME threads. end mill...n This is the way I do acme https://www.youtube.com/watch?v=Jbp8SJ9RxqI And that's the PROPER way to do it. Thanks :) I forgot to mention the homebrew threading with an insert on the mill tooling Top left picture http://www.archivist.info/cnc/stage6/ It is an abuse of a carbide insert due to the intermittent cut but does allow me a well formed thread I set the top of the insert above the centerline to make sure I had clearance as it is on a rotary tool. Dave Caroline Jon -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Friday 22 March 2013 16:24:17 andy pugh did opine: On 22 March 2013 15:56, Gene Heskett ghesk...@wdtv.com wrote: I have been threatening to make me one of those disks and buy an oz of diamond dust in oil. I have never seen such a tool sharpener in the catalogs since. http://www.frets.com/HomeShopTech/Projects/HandCrankGrinder/handcrankgri nder.html That isn't exactly what I'm looking for, but the whole siote is a wealth of info, so its bookmarked FFR. Thanks Andy. Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml In 1962, you could buy a pair of SHARKSKIN SLACKS, with a Continental Belt, for $10.99!! I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Thanks to all! On Wed, Mar 20, 2013 at 11:55 PM, Chris Morley chrisinnana...@hotmail.comwrote: From: bodge...@gmail.com Date: Wed, 20 Mar 2013 10:17:24 + To: emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Threading on a mill with fourth axis On 20 March 2013 10:14, andy pugh bodge...@gmail.com wrote: G10 L2 P1 A0 Actually, I got that wrong. G10 L20: http://www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L20 -- If you use P0 then you don't have to worry what G5x your in. Chris M -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Thursday 21 March 2013 11:44:24 Igor Chudov did opine: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Thanks to all! That ought to be put in the wiki, Igor. Can you? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml For courage mounteth with occasion. -- William Shakespeare, King John I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
I am not sure how I can put the code in Wiki. I am releasing the following code under the GNU Public License: (Makes a thread on a round part rotated in my fourth axis) (Uses a 60 degree end mill) Othread_on_fourth_axis sub #x0 = #1 (X0, left side) #x1 = #2 (X1, right side) #y = #3 (Y, middle of the top edge of the round) #z0 = #4 (Z, top of the edge of the round) #safez = #5 (Safe Z for rapids) #zstep = #6 (Z Step, positive) #spr = #7 (Step Per Revolution, Also determines Total Depth) #depth = #8 (Depth of thread, positive, determined automatically if 0 based on 60 degree thread.) #diameter= #9 (Diameter of the round, needed for calculations of feed rate) #frate = #10 (feed rate based on surface speed) #left_handed = #11 (Set to 1 if left handed) #rpm = [#frate/3.1415/#diameter] #horizontal_feedrate = [#rpm*#spr] #vertical_feedrate = [#frate/5] #total_angle = [ 360 * [#x1-#x0]/#spr ] (Set negative total angle if left handed thread) Oif if [#left_handed NE 0] #total_angle = [-#total_angle] Oif endif Oif if [#depth EQ 0] #depth = [#spr*1.73205/2] (depth = spr * sqrt 3 / 2 ) Oif endif Owithdraw call [#safez] G0 A0 (go to 0 degree) G0 X[#x0] Y[#y] Z[#safez] ( Start drilling down to Z0, I could rapid, ) ( but slow is safer, will not break end mill ) G1 Z[#z0] F[#vertical_feedrate] #direction = 1 (1 is right, 2 is left) #z = #z0 Oloop while [ 1 ] #z = [#z - #zstep] Oif if [#z LT [#z0 - #depth] ] #z = [#z0 - #depth] Oif endif G1 Z[#z] F[#vertical_feedrate] (Depending on direction, we go to X1 on the right and turn total_angle,) (or go to X0 on the left and go back to ZERO angle) Oif if [#direction EQ 1 ] #direction = 0 G1 X[#x1] A[#total_angle] F[#horizontal_feedrate] Oif else #direction = 1 G1 X[#x0] A0 F[#horizontal_feedrate] Oif endif Oif if [ #z LE [#z0 - #depth] ] Oloop break Oif endif Oloop endwhile Owithdraw call [#safez] G0 X[#x1] G0 A0 (go to 0 degree) Othread_on_fourth_axis endsub M2 On Thu, Mar 21, 2013 at 10:46 AM, Gene Heskett ghesk...@wdtv.com wrote: On Thursday 21 March 2013 11:44:24 Igor Chudov did opine: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Thanks to all! That ought to be put in the wiki, Igor. Can you? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml For courage mounteth with occasion. -- William Shakespeare, King John I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Here's a VIDEO of this working. Not the most fun video like a skateboarding dog, but it shows the nature of the process. http://www.youtube.com/watch?v=JMENnIJrl9Y On Thu, Mar 21, 2013 at 5:41 PM, Igor Chudov ichu...@gmail.com wrote: I am not sure how I can put the code in Wiki. I am releasing the following code under the GNU Public License: (Makes a thread on a round part rotated in my fourth axis) (Uses a 60 degree end mill) Othread_on_fourth_axis sub #x0 = #1 (X0, left side) #x1 = #2 (X1, right side) #y = #3 (Y, middle of the top edge of the round) #z0 = #4 (Z, top of the edge of the round) #safez = #5 (Safe Z for rapids) #zstep = #6 (Z Step, positive) #spr = #7 (Step Per Revolution, Also determines Total Depth) #depth = #8 (Depth of thread, positive, determined automatically if 0 based on 60 degree thread.) #diameter= #9 (Diameter of the round, needed for calculations of feed rate) #frate = #10 (feed rate based on surface speed) #left_handed = #11 (Set to 1 if left handed) #rpm = [#frate/3.1415/#diameter] #horizontal_feedrate = [#rpm*#spr] #vertical_feedrate = [#frate/5] #total_angle = [ 360 * [#x1-#x0]/#spr ] (Set negative total angle if left handed thread) Oif if [#left_handed NE 0] #total_angle = [-#total_angle] Oif endif Oif if [#depth EQ 0] #depth = [#spr*1.73205/2] (depth = spr * sqrt 3 / 2 ) Oif endif Owithdraw call [#safez] G0 A0 (go to 0 degree) G0 X[#x0] Y[#y] Z[#safez] ( Start drilling down to Z0, I could rapid, ) ( but slow is safer, will not break end mill ) G1 Z[#z0] F[#vertical_feedrate] #direction = 1 (1 is right, 2 is left) #z = #z0 Oloop while [ 1 ] #z = [#z - #zstep] Oif if [#z LT [#z0 - #depth] ] #z = [#z0 - #depth] Oif endif G1 Z[#z] F[#vertical_feedrate] (Depending on direction, we go to X1 on the right and turn total_angle,) (or go to X0 on the left and go back to ZERO angle) Oif if [#direction EQ 1 ] #direction = 0 G1 X[#x1] A[#total_angle] F[#horizontal_feedrate] Oif else #direction = 1 G1 X[#x0] A0 F[#horizontal_feedrate] Oif endif Oif if [ #z LE [#z0 - #depth] ] Oloop break Oif endif Oloop endwhile Owithdraw call [#safez] G0 X[#x1] G0 A0 (go to 0 degree) Othread_on_fourth_axis endsub M2 On Thu, Mar 21, 2013 at 10:46 AM, Gene Heskett ghesk...@wdtv.com wrote: On Thursday 21 March 2013 11:44:24 Igor Chudov did opine: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Thanks to all! That ought to be put in the wiki, Igor. Can you? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml For courage mounteth with occasion. -- William Shakespeare, King John I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
--- On Thu, 3/21/13, Igor Chudov ichu...@gmail.com wrote: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Let's see some videos! :) -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
http://www.youtube.com/watch?v=JMENnIJrl9Y On Thu, Mar 21, 2013 at 7:42 PM, Gregg Eshelman g_ala...@yahoo.com wrote: --- On Thu, 3/21/13, Igor Chudov ichu...@gmail.com wrote: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Let's see some videos! :) -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Good work Igor! I liked the music also. What is it? +++ Anyone who believes exponential growth can go on forever in a finite world is either a madman or an economist. -Kenneth Boulding, economist “How unfortunate that the Earth’s first intelligent social animal is a tribal carnivore” -E.O. Wilson, sociobiologist From: Igor Chudov ichu...@gmail.com To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Sent: Thursday, March 21, 2013 8:26 PM Subject: Re: [Emc-users] Threading on a mill with fourth axis http://www.youtube.com/watch?v=JMENnIJrl9Y On Thu, Mar 21, 2013 at 7:42 PM, Gregg Eshelman g_ala...@yahoo.com wrote: --- On Thu, 3/21/13, Igor Chudov ichu...@gmail.com wrote: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Let's see some videos! :) -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Square thread would be just as easy. Same for Acme if the right shape end mill is available. -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Thursday 21 March 2013 22:16:19 Igor Chudov did opine: I am not sure how I can put the code in Wiki. Neither am I Igor, but there should be instructions. And it probably depends on you as your login user having perms. I haven't actually tried it either. I am releasing the following code under the GNU Public License: Thank you. (Makes a thread on a round part rotated in my fourth axis) (Uses a 60 degree end mill) Othread_on_fourth_axis sub #x0 = #1 (X0, left side) #x1 = #2 (X1, right side) #y = #3 (Y, middle of the top edge of the round) #z0 = #4 (Z, top of the edge of the round) #safez = #5 (Safe Z for rapids) #zstep = #6 (Z Step, positive) #spr = #7 (Step Per Revolution, Also determines Total Depth) #depth = #8 (Depth of thread, positive, determined automatically if 0 based on 60 degree thread.) #diameter= #9 (Diameter of the round, needed for calculations of feed rate) #frate = #10 (feed rate based on surface speed) #left_handed = #11 (Set to 1 if left handed) #rpm = [#frate/3.1415/#diameter] #horizontal_feedrate = [#rpm*#spr] #vertical_feedrate = [#frate/5] #total_angle = [ 360 * [#x1-#x0]/#spr ] (Set negative total angle if left handed thread) Oif if [#left_handed NE 0] #total_angle = [-#total_angle] Oif endif Oif if [#depth EQ 0] #depth = [#spr*1.73205/2] (depth = spr * sqrt 3 / 2 ) Oif endif Owithdraw call [#safez] G0 A0 (go to 0 degree) G0 X[#x0] Y[#y] Z[#safez] ( Start drilling down to Z0, I could rapid, ) ( but slow is safer, will not break end mill ) G1 Z[#z0] F[#vertical_feedrate] #direction = 1 (1 is right, 2 is left) #z = #z0 Oloop while [ 1 ] #z = [#z - #zstep] Oif if [#z LT [#z0 - #depth] ] #z = [#z0 - #depth] Oif endif G1 Z[#z] F[#vertical_feedrate] (Depending on direction, we go to X1 on the right and turn total_angle,) (or go to X0 on the left and go back to ZERO angle) Oif if [#direction EQ 1 ] #direction = 0 G1 X[#x1] A[#total_angle] F[#horizontal_feedrate] Oif else #direction = 1 G1 X[#x0] A0 F[#horizontal_feedrate] Oif endif Oif if [ #z LE [#z0 - #depth] ] Oloop break Oif endif Oloop endwhile Owithdraw call [#safez] G0 X[#x1] G0 A0 (go to 0 degree) Othread_on_fourth_axis endsub M2 On Thu, Mar 21, 2013 at 10:46 AM, Gene Heskett ghesk...@wdtv.com wrote: On Thursday 21 March 2013 11:44:24 Igor Chudov did opine: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Thanks to all! That ought to be put in the wiki, Igor. Can you? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml For courage mounteth with occasion. -- William Shakespeare, King John I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml Windows: an Unrecoverable Acquisition Error! I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with
Re: [Emc-users] Threading on a mill with fourth axis
Some Russian music played on my CNC control. On Thu, Mar 21, 2013 at 8:32 PM, Greg Bernard yankeelena2...@yahoo.comwrote: Good work Igor! I liked the music also. What is it? +++ Anyone who believes exponential growth can go on forever in a finite world is either a madman or an economist. -Kenneth Boulding, economist “How unfortunate that the Earth’s first intelligent social animal is a tribal carnivore” -E.O. Wilson, sociobiologist From: Igor Chudov ichu...@gmail.com To: Enhanced Machine Controller (EMC) emc-users@lists.sourceforge.net Sent: Thursday, March 21, 2013 8:26 PM Subject: Re: [Emc-users] Threading on a mill with fourth axis http://www.youtube.com/watch?v=JMENnIJrl9Y On Thu, Mar 21, 2013 at 7:42 PM, Gregg Eshelman g_ala...@yahoo.com wrote: --- On Thu, 3/21/13, Igor Chudov ichu...@gmail.com wrote: Guys, I am extremely happy. I finally debugged my G code routine enough that it works. I can make any thread, inch, metric, right hand, left hand, whatever! It also can mill a very coarse thread in multiple passes, reversing rotation every other pass (to return to A=0, as an additional benefit). I can now make any bolt or threaded end I want! Let's see some videos! :) -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Yes, I would love to find a suitably shaped end mill for ACME threads. What I REALLY love about CNC/EMC, is that I really could not care less how much a job takes, I just start a machine, leave it running, go to my office, do something else and the job gets done. So much better than turning those manual dials! On Thu, Mar 21, 2013 at 9:14 PM, Gregg Eshelman g_ala...@yahoo.com wrote: Square thread would be just as easy. Same for Acme if the right shape end mill is available. -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Igor Chudov wrote: Yes, I would love to find a suitably shaped end mill for ACME threads. That is a tapered end mill. The only problem is finding one that has a small enough tip diameter. I think it would be listed as 14.5 degrees per side taper. I have a couple tapered end mills here, but none of them go down to a small enough diameter for typical Acme threads. Jon -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
forgive me but im recalling the cnc mill vs lathe discussion of about a week ago and im thinking both of these operations can be done in a cnc lathe with a 3 dollar hand ground hss tool. im not knocking what you have accomplished as its good work inddeed:) im just sayin :) -- jeremy youngs -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Could do ACME in three passes. First pass cut as a square thread, 2nd and 3rd passes tilt the head left or right 14.5 degrees to cut the sides. --- On Thu, 3/21/13, Igor Chudov ichu...@gmail.com wrote: Yes, I would love to find a suitably shaped end mill for ACME threads. What I REALLY love about CNC/EMC, is that I really could not care less how much a job takes, I just start a machine, leave it running, go to my office, do something else and the job gets done. So much better than turning those manual dials! On Thu, Mar 21, 2013 at 9:14 PM, Gregg Eshelman g_ala...@yahoo.com wrote: Square thread would be just as easy. Same for Acme if the right shape end mill is available. -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Wednesday 20 March 2013 02:59:22 Igor Chudov did opine: I have a vertical mill with a fourth axis A. My buddy wants me to write a subroutine that would let me mill thread on round parts, that are held in the fourth axis, and the thread would be milled using a 60 degree chamfer end mill, rotating the part around the A axis. I have some questions about the odds and ends of this. 1. I would like to be able to say to the machine, in G code, that wherever we are on the A axis, call it zero degrees position. In other words, I want to change the coordinate system in G code for one A axis only. How do I do it. 2. Is that correct that feedrate F in a G1 statement that changes both X, as well as A, only refers to the change of X? I can live with that, I just want to know. I think the canned routine g33? might be the first place I'd check in the docs. I started to say G76, but one would have to cobble up some sort of an index pulse from the combo of A=0 + Z=0 in hal, and dummy up encoder quad signals from the step count going to the A table in order to lock the A/Z timing together on the multipass loopback g76 uses. I have one of those milling bits, but I've now cnc'd my lathe so I do all that on the lathe with the G76, at any tpi, and any diameter my spindle motor has the power to cut, perhaps an inch in diameter max. But in the mill, using that bit in the mill, the thread could be cut full depth in one pass, with the speed of the A table being the speed limit, on my 4 toy table, about 1800 degrees/minute. However, resharpening a cutoff blade to be the single tooth on the lathe is certainly a heck of a lot cheaper than resharpening such a mill, another reason my mill has only been out of the box to admire it 2 or 3 times. A very $pen$ive little milling bit. Another item to consider in writing your own routine is that the A table needs to be tilted on the X axis according to the thread pitch so the tooth arc effectively matches the threads pitch. That in turn brings in a need to drive the Y slowly in time with Z to maintain the X to part contact point at exactly along the X axis. Otherwise the thread diameter over its length will be in error according to the sine? of that X angle miss-match. That part I handle on the lathe by tilting the blade slightly in the grip of the 3 jaw on my table while driving the table to the proper angles. There are as many ways to skin this cat. :) Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml Would you care to view the ruins of my good intentions? I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On 20 Mar 2013, at 04:16, Igor Chudov wrote: I have a vertical mill with a fourth axis A. My buddy wants me to write a subroutine that would let me mill thread on round parts, that are held in the fourth axis, and the thread would be milled using a 60 degree chamfer end mill, rotating the part around the A axis. I have some questions about the odds and ends of this. 1. I would like to be able to say to the machine, in G code, that wherever we are on the A axis, call it zero degrees position. In other words, I want to change the coordinate system in G code for one A axis only. How do I do it. Gene is right: there are threading canned cycles you could use, but you still might want to reset the A to 0 when you start that. The write-it-yourself answer might depend on whether you mean you need the A value to be zero at that point inside that subroutine only, or whether it can be 0 at that point outside the subroutine as well. G92 will give you a temporary offset inside the subroutine. G92.1 cancels it So taking the controlled point to the required position then using G92 A0 should do the trick. At the end of the subroutine, use G92.1 to cancel that temporary offset. Or, working in G54 throughout, you could Home when you start Jog to where you need A to be 0 (and X0 Y0 Z0) Touch Off X, Y, Z and A in G54, making the values zero each time. (Or do the Touching Off anywhere to suit X, Y and Z Jog to the A position you need to be zero and re-home A only) Or you could use two of the offset systems G54, G55 etc So, when you start your session, Home the X, Y, Z and A axes in both G54 and G55 offsets. In your program, move to the required position in X, Y, Z and A then use G10 L20 P2 A0 G55 The G10 L20 calculates the offset required to make the current A value 0 and puts that in offset system 2 (i.e. G55) G55 switches to that offset system Because X, Y and Z are already the same in G54 and G55 X, Y and Z values should stay the same but the A value will now be 0 The A value in the normal G54 system will be whatever it was before, because you have only changed it in G55 not G54 G54 switches back to the G54 values once you have finished. I have a question on the A axis orientation: Do you have the A axis wrapping around the X linear axis? If it is wrapped around the Z axis, it would technically be a C axis, although I guess that like myself you could be using an A axis connection swapped between either. I use A for a rotary table mounted horizontally, with the axis pointing along X (so motion is wrapped around X). I use the same rotary table mounted horizontally, pointing up the Z axis, and don't bother changing the cables or the name of the axis. Lazy; but convenient. Regards, Marcus 2. Is that correct that feedrate F in a G1 statement that changes both X, as well as A, only refers to the change of X? I can live with that, I just want to know. -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On 20 March 2013 04:16, Igor Chudov ichu...@gmail.com wrote: 1. I would like to be able to say to the machine, in G code, that wherever we are on the A axis, call it zero degrees position. G10 L2 P1 A0 2. Is that correct that feedrate F in a G1 statement that changes both X, as well as A, only refers to the change of X? I can live with that, I just want to know. Yes. You would cut the thread with G1 F10 X-2 A7200 to make a 10 tpi 2 long thread. However, F will not be the normal feedrate for a linear move, it needs to be modified by a factor of pi * D * TPI to give the right feedrate. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On 20 March 2013 10:14, andy pugh bodge...@gmail.com wrote: G10 L2 P1 A0 Actually, I got that wrong. G10 L20: http://www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L20 -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
OK, thanks guys. I wrote a really nice subroutine that can mill right or left handed threads, calculates feedrate correctly (it still remains to be tested), and can mill a thread in multiple passes. On Wed, Mar 20, 2013 at 5:17 AM, andy pugh bodge...@gmail.com wrote: On 20 March 2013 10:14, andy pugh bodge...@gmail.com wrote: G10 L2 P1 A0 Actually, I got that wrong. G10 L20: http://www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L20 -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Wednesday 20 March 2013 09:27:25 andy pugh did opine: On 20 March 2013 04:16, Igor Chudov ichu...@gmail.com wrote: 1. I would like to be able to say to the machine, in G code, that wherever we are on the A axis, call it zero degrees position. G10 L2 P1 A0 2. Is that correct that feedrate F in a G1 statement that changes both X, as well as A, only refers to the change of X? I can live with that, I just want to know. Yes. You would cut the thread with G1 F10 X-2 A7200 to make a 10 tpi 2 long thread. However, F will not be the normal feedrate for a linear move, it needs to be modified by a factor of pi * D * TPI to give the right feedrate. Humm, Early here Andy. Since it is the R that determines surface speed the A rotation gives, my natural first thought would have been PI * R * TPI. I don't doubt you are correct though. Do I need to go make a pot of coffee to get me started tight? Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml No rock so hard but that a little wave May beat admission in a thousand years. -- Tennyson I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On 20 March 2013 13:34, Gene Heskett ghesk...@wdtv.com wrote: However, F will not be the normal feedrate for a linear move, it needs to be modified by a factor of pi * D * TPI to give the right feedrate. Humm, Early here Andy. Since it is the R that determines surface speed This isn't about the surface speed, that is set by the spindle speed. This is how much longer the actual cut is than the simple linear move in X. -- atp If you can't fix it, you don't own it. http://www.ifixit.com/Manifesto -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
On Wednesday 20 March 2013 10:48:48 andy pugh did opine: On 20 March 2013 13:34, Gene Heskett ghesk...@wdtv.com wrote: However, F will not be the normal feedrate for a linear move, it needs to be modified by a factor of pi * D * TPI to give the right feedrate. Humm, Early here Andy. Since it is the R that determines surface speed This isn't about the surface speed, that is set by the spindle speed. This is how much longer the actual cut is than the simple linear move in X. So it would be something like #_F_speed= [10 / [pi * d * tpi]] Adjust the 10 to arrive at something ones table can actually do. Mine is not a speed daemon by any means, 1800 degrees/min that needs a few shots of vactra through the brake screws hole to do that. I have a 262 oz motor on it, but it needs more because I've pulled it down pretty snug to try control its backlash. Cheap 4 grizzly table, both the bull gear and the worm are somewhat eccentric. That have a better one of course and I should bite the SS check and get it. I /knew/ I wasn't looking at it correctly, thanks Andy. Coffee under construction. :) Cheers, Gene -- There are four boxes to be used in defense of liberty: soap, ballot, jury, and ammo. Please use in that order. -Ed Howdershelt (Author) My web page: http://coyoteden.dyndns-free.com:85/gene is up! My views http://www.armchairpatriot.com/What%20Has%20America%20Become.shtml We don't have to protect the environment -- the Second Coming is at hand. -- James Watt I was taught to respect my elders, but its getting harder and harder to find any... -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
Igor Chudov wrote: I have a vertical mill with a fourth axis A. My buddy wants me to write a subroutine that would let me mill thread on round parts, that are held in the fourth axis, and the thread would be milled using a 60 degree chamfer end mill, rotating the part around the A axis. I'm a little confused by this. The A axis is traditionally parallel to the X axis, so the part rotates parallel to the table. While a 60 degree angle cutter would produce a geometrically accurate thread, it may not be the best way to machine a thread. Having the rotation axis of the cutter parallel (but offset) from the rotation of the part to be threaded produces cutter motion past the work on every part of the thread profile, while the way you seem to be describing, with the point of the cutter in the bottom of the thread groove does not. I have some questions about the odds and ends of this. 1. I would like to be able to say to the machine, in G code, that wherever we are on the A axis, call it zero degrees position. In other words, I want to change the coordinate system in G code for one A axis only. How do I do it. Just home the A axis and that will be zero. Or, touch off the A axis. 2. Is that correct that feedrate F in a G1 statement that changes both X, as well as A, only refers to the change of X? I can live with that, I just want to know. Yes, that is so. If your X is the length of the thread along the axis of rotation, then the specified feedrate will be WAY off, so you'll have to compensate for the number of turns around the diameter. I have a program for more conventional thread milling that can be downloaded from http://pico-systems.com/gcode.html (it is near the bottom of the page). Jon -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Threading on a mill with fourth axis
From: bodge...@gmail.com Date: Wed, 20 Mar 2013 10:17:24 + To: emc-users@lists.sourceforge.net Subject: Re: [Emc-users] Threading on a mill with fourth axis On 20 March 2013 10:14, andy pugh bodge...@gmail.com wrote: G10 L2 P1 A0 Actually, I got that wrong. G10 L20: http://www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G10-L20 -- If you use P0 then you don't have to worry what G5x your in. Chris M -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Threading on a mill with fourth axis
I have a vertical mill with a fourth axis A. My buddy wants me to write a subroutine that would let me mill thread on round parts, that are held in the fourth axis, and the thread would be milled using a 60 degree chamfer end mill, rotating the part around the A axis. I have some questions about the odds and ends of this. 1. I would like to be able to say to the machine, in G code, that wherever we are on the A axis, call it zero degrees position. In other words, I want to change the coordinate system in G code for one A axis only. How do I do it. 2. Is that correct that feedrate F in a G1 statement that changes both X, as well as A, only refers to the change of X? I can live with that, I just want to know. -- Everyone hates slow websites. So do we. Make your web apps faster with AppDynamics Download AppDynamics Lite for free today: http://p.sf.net/sfu/appdyn_d2d_mar ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
