Re: [Emc-users] G28 behaviour
In 1979 the Dynamic Machinery Sales Chicago class for a Miyano 7BC lathe with Fanuc 5T control taught me to use G91 G28 X0 Z0 at the end of every program to make sure the machine reference was always accurate. I can't tell you how many times I watched the reference lights come on in the next six years - a bunch. Regards Stuart On Fri, Jun 25, 2021, 6:06 PM John Dammeyer wrote: > Yeah I wondered about that. I initially tried it with positive and with > it at machine zero still moved up 2" and then back down again. Totally > contrary to logical since my machine zero is furthest from the tool and any > motion towards the tool should be negative? > > Thanks > John > > > > -Original Message- > > From: Feral Engineer [mailto:theferalengin...@gmail.com] > > Sent: June-25-21 3:35 PM > > To: Enhanced Machine Controller (EMC) > > Subject: Re: [Emc-users] G28 behaviour > > > > That's exactly the behavior that g28 follows on industrial controls. Try > > g28z2. (positive) and it'll move up without having to switch to > incremental > > > > Phil T. > > The Feral Engineer > > > > Check out my LinuxCNC tutorials, machine builds and other antics at > > www.youtube.com/c/theferalengineer > > > > Help support my channel efforts and coffee addiction: > > www.patreon.com/theferalengineer > > > > On Fri, Jun 25, 2021, 6:28 PM John Dammeyer > wrote: > > > > > In effect the G91 incremental with a Z0 just cancels out the initial > move > > > to the Z position. > > > > > > I did try it on the mill as > > > G28 Z-2 > > > > > > All that really happens is the machine sounds like it stumbles as it > heads > > > toward Z0 stopping briefly at Z-2. > > > > > > Very strange. > > > John > > > > > > > > > > -Original Message- > > > > From: Todd Zuercher [mailto:to...@pgrahamdunn.com] > > > > Sent: June-25-21 10:17 AM > > > > To: Enhanced Machine Controller (EMC) > > > > Subject: Re: [Emc-users] G28 behaviour > > > > > > > > I'm pretty sure all of our Fanuc machines use G91 for incremental G28 > > > commands and not U V W. (maybe some older Fanuc controls > > > > or controls specialized for some manufacturers or maybe just > T-series, I > > > only have worked with Ms.) > > > > > > > > But as to why the intermediate command, I have no idea, It's just how > > > Fanuc's G28 has always been. > > > > > > > > Todd Zuercher > > > > P. Graham Dunn Inc. > > > > 630 Henry Street? > > > > Dalton, Ohio 44618 > > > > Phone:? (330)828-2105ext. 2031 > > > > > > > > -Original Message- > > > > From: John Dammeyer > > > > Sent: Friday, June 25, 2021 1:06 PM > > > > To: 'Enhanced Machine Controller (EMC)' < > emc-users@lists.sourceforge.net > > > > > > > > Subject: Re: [Emc-users] G28 behaviour > > > > > > > > [EXTERNAL EMAIL] Be sure links are safe. > > > > > > > > Thanks for the explanation but I'm still curious why the intermediate > > > point. > > > > > > > > I suppose if I had a tool changer at the machine 0,0,0 position (or > > > close to that) and my A axis sitting on the left of the work I'd want > > > > to move to a position that allows a clear path directly to the tool > > > changer. > > > > > > > > But, why a special code for this? If I need Z to be at a specific > > > machine position doesn't a > > > > G53 G0 Z10 > > > > G53 G0 Z0 > > > > do the same thing? Granted two lines but one doesn't have to look > up > > > what a G28 does... > > > > > > > > > -Original Message- > > > > > From: Feral Engineer [mailto:theferalengin...@gmail.com] > > > > > Sent: June-25-21 9:51 AM > > > > > To: Enhanced Machine Controller (EMC) > > > > > Subject: Re: [Emc-users] G28 behaviour > > > > > > > > > > G28 is a return to reference using an intermediate point > > > > > > > > > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > > > > > reference zero (machine zero in most cases). By using g91 g28 z0, > you > > > > > specify that the intermediate point is your current position and > the > > > > > machine will reference return from there.
Re: [Emc-users] G28 behaviour
Yeah I wondered about that. I initially tried it with positive and with it at machine zero still moved up 2" and then back down again. Totally contrary to logical since my machine zero is furthest from the tool and any motion towards the tool should be negative? Thanks John > -Original Message- > From: Feral Engineer [mailto:theferalengin...@gmail.com] > Sent: June-25-21 3:35 PM > To: Enhanced Machine Controller (EMC) > Subject: Re: [Emc-users] G28 behaviour > > That's exactly the behavior that g28 follows on industrial controls. Try > g28z2. (positive) and it'll move up without having to switch to incremental > > Phil T. > The Feral Engineer > > Check out my LinuxCNC tutorials, machine builds and other antics at > www.youtube.com/c/theferalengineer > > Help support my channel efforts and coffee addiction: > www.patreon.com/theferalengineer > > On Fri, Jun 25, 2021, 6:28 PM John Dammeyer wrote: > > > In effect the G91 incremental with a Z0 just cancels out the initial move > > to the Z position. > > > > I did try it on the mill as > > G28 Z-2 > > > > All that really happens is the machine sounds like it stumbles as it heads > > toward Z0 stopping briefly at Z-2. > > > > Very strange. > > John > > > > > > > -Original Message- > > > From: Todd Zuercher [mailto:to...@pgrahamdunn.com] > > > Sent: June-25-21 10:17 AM > > > To: Enhanced Machine Controller (EMC) > > > Subject: Re: [Emc-users] G28 behaviour > > > > > > I'm pretty sure all of our Fanuc machines use G91 for incremental G28 > > commands and not U V W. (maybe some older Fanuc controls > > > or controls specialized for some manufacturers or maybe just T-series, I > > only have worked with Ms.) > > > > > > But as to why the intermediate command, I have no idea, It's just how > > Fanuc's G28 has always been. > > > > > > Todd Zuercher > > > P. Graham Dunn Inc. > > > 630 Henry Street? > > > Dalton, Ohio 44618 > > > Phone:? (330)828-2105ext. 2031 > > > > > > -Original Message- > > > From: John Dammeyer > > > Sent: Friday, June 25, 2021 1:06 PM > > > To: 'Enhanced Machine Controller (EMC)' > > > > > Subject: Re: [Emc-users] G28 behaviour > > > > > > [EXTERNAL EMAIL] Be sure links are safe. > > > > > > Thanks for the explanation but I'm still curious why the intermediate > > point. > > > > > > I suppose if I had a tool changer at the machine 0,0,0 position (or > > close to that) and my A axis sitting on the left of the work I'd want > > > to move to a position that allows a clear path directly to the tool > > changer. > > > > > > But, why a special code for this? If I need Z to be at a specific > > machine position doesn't a > > > G53 G0 Z10 > > > G53 G0 Z0 > > > do the same thing? Granted two lines but one doesn't have to look up > > what a G28 does... > > > > > > > -Original Message- > > > > From: Feral Engineer [mailto:theferalengin...@gmail.com] > > > > Sent: June-25-21 9:51 AM > > > > To: Enhanced Machine Controller (EMC) > > > > Subject: Re: [Emc-users] G28 behaviour > > > > > > > > G28 is a return to reference using an intermediate point > > > > > > > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > > > > reference zero (machine zero in most cases). By using g91 g28 z0, you > > > > specify that the intermediate point is your current position and the > > > > machine will reference return from there. You can also use values such > > > > as > > > > g90 g28 z50. To use 50mm above your workpiece origin to be your > > > > intermediate point or you can use g91 g28 z10. To move 10mm up and use > > > > that as your intermediate. > > > > > > > > Fanuc g code system a does not use g91, it uses u v w as their > > > > respective incremental axes for x y and z, which is why on a lathe > > > > you'll usually see > > > > g28 u0 w0 or something of that nature. You could use absolute values, > > > > but they come from your workpiece origin, so you'd have to say > > > > something like > > > > g28 x100 z100 to move to the absolute intermediate position above the > > > > part to not have a crash. > > > > > > > > The posted code in fusion is just ugly, no real reason to
Re: [Emc-users] G28 behaviour
That's exactly the behavior that g28 follows on industrial controls. Try g28z2. (positive) and it'll move up without having to switch to incremental Phil T. The Feral Engineer Check out my LinuxCNC tutorials, machine builds and other antics at www.youtube.com/c/theferalengineer Help support my channel efforts and coffee addiction: www.patreon.com/theferalengineer On Fri, Jun 25, 2021, 6:28 PM John Dammeyer wrote: > In effect the G91 incremental with a Z0 just cancels out the initial move > to the Z position. > > I did try it on the mill as > G28 Z-2 > > All that really happens is the machine sounds like it stumbles as it heads > toward Z0 stopping briefly at Z-2. > > Very strange. > John > > > > -Original Message- > > From: Todd Zuercher [mailto:to...@pgrahamdunn.com] > > Sent: June-25-21 10:17 AM > > To: Enhanced Machine Controller (EMC) > > Subject: Re: [Emc-users] G28 behaviour > > > > I'm pretty sure all of our Fanuc machines use G91 for incremental G28 > commands and not U V W. (maybe some older Fanuc controls > > or controls specialized for some manufacturers or maybe just T-series, I > only have worked with Ms.) > > > > But as to why the intermediate command, I have no idea, It's just how > Fanuc's G28 has always been. > > > > Todd Zuercher > > P. Graham Dunn Inc. > > 630 Henry Street� > > Dalton, Ohio 44618 > > Phone:� (330)828-2105ext. 2031 > > > > -----Original Message- > > From: John Dammeyer > > Sent: Friday, June 25, 2021 1:06 PM > > To: 'Enhanced Machine Controller (EMC)' > > > Subject: Re: [Emc-users] G28 behaviour > > > > [EXTERNAL EMAIL] Be sure links are safe. > > > > Thanks for the explanation but I'm still curious why the intermediate > point. > > > > I suppose if I had a tool changer at the machine 0,0,0 position (or > close to that) and my A axis sitting on the left of the work I'd want > > to move to a position that allows a clear path directly to the tool > changer. > > > > But, why a special code for this? If I need Z to be at a specific > machine position doesn't a > > G53 G0 Z10 > > G53 G0 Z0 > > do the same thing? Granted two lines but one doesn't have to look up > what a G28 does... > > > > > -Original Message- > > > From: Feral Engineer [mailto:theferalengin...@gmail.com] > > > Sent: June-25-21 9:51 AM > > > To: Enhanced Machine Controller (EMC) > > > Subject: Re: [Emc-users] G28 behaviour > > > > > > G28 is a return to reference using an intermediate point > > > > > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > > > reference zero (machine zero in most cases). By using g91 g28 z0, you > > > specify that the intermediate point is your current position and the > > > machine will reference return from there. You can also use values such > > > as > > > g90 g28 z50. To use 50mm above your workpiece origin to be your > > > intermediate point or you can use g91 g28 z10. To move 10mm up and use > > > that as your intermediate. > > > > > > Fanuc g code system a does not use g91, it uses u v w as their > > > respective incremental axes for x y and z, which is why on a lathe > > > you'll usually see > > > g28 u0 w0 or something of that nature. You could use absolute values, > > > but they come from your workpiece origin, so you'd have to say > > > something like > > > g28 x100 z100 to move to the absolute intermediate position above the > > > part to not have a crash. > > > > > > The posted code in fusion is just ugly, no real reason to keep > > > flopping back and forth like that. Fusion posts are JavaScript, so > > > they're not terrible to modify. > > > > > > Phil T. > > > The Feral Engineer > > > > > > Check out my LinuxCNC tutorials, machine builds and other antics at > > > www.youtube.com/c/theferalengineer > > > > > > Help support my channel efforts and coffee addiction: > > > www.patreon.com/theferalengineer > > > > > > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer > wrote: > > > > > > > A friend who uses MACH3 and Fusion360 (free version) found that > > > > every G-Code file created by Fusion for the MACH environment added: > > > > > > > > G28 G91 Z0 > > > > G90 > > > > G28 G91 X0 Y0 > > > > G90 > > > > > > > > He's since figured out how to tell Fusion not to do this but loo
Re: [Emc-users] G28 behaviour
Fanuc g code system a is for lathes. Some will use system b or c but it's few and far between. Some emco lathes use system c, that much i do know. You can change g code systems via parameter on most generation fanuc controls from the last 20+ years I'd actually like to figure a way to get Linuxcnc to support system a b and c. G92 to set max spindle speed just feels so wrong to me Phil T. The Feral Engineer Check out my LinuxCNC tutorials, machine builds and other antics at www.youtube.com/c/theferalengineer Help support my channel efforts and coffee addiction: www.patreon.com/theferalengineer On Fri, Jun 25, 2021, 5:53 PM Todd Zuercher wrote: > I'm pretty sure all of our Fanuc machines use G91 for incremental G28 > commands and not U V W. (maybe some older Fanuc controls or controls > specialized for some manufacturers or maybe just T-series, I only have > worked with Ms.) > > But as to why the intermediate command, I have no idea, It's just how > Fanuc's G28 has always been. > > Todd Zuercher > P. Graham Dunn Inc. > 630 Henry Street > Dalton, Ohio 44618 > Phone: (330)828-2105ext. 2031 > > -Original Message- > From: John Dammeyer > Sent: Friday, June 25, 2021 1:06 PM > To: 'Enhanced Machine Controller (EMC)' > Subject: Re: [Emc-users] G28 behaviour > > [EXTERNAL EMAIL] Be sure links are safe. > > Thanks for the explanation but I'm still curious why the intermediate > point. > > I suppose if I had a tool changer at the machine 0,0,0 position (or close > to that) and my A axis sitting on the left of the work I'd want to move to > a position that allows a clear path directly to the tool changer. > > But, why a special code for this? If I need Z to be at a specific machine > position doesn't a > G53 G0 Z10 > G53 G0 Z0 > do the same thing? Granted two lines but one doesn't have to look up > what a G28 does... > > > -Original Message- > > From: Feral Engineer [mailto:theferalengin...@gmail.com] > > Sent: June-25-21 9:51 AM > > To: Enhanced Machine Controller (EMC) > > Subject: Re: [Emc-users] G28 behaviour > > > > G28 is a return to reference using an intermediate point > > > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > > reference zero (machine zero in most cases). By using g91 g28 z0, you > > specify that the intermediate point is your current position and the > > machine will reference return from there. You can also use values such > > as > > g90 g28 z50. To use 50mm above your workpiece origin to be your > > intermediate point or you can use g91 g28 z10. To move 10mm up and use > > that as your intermediate. > > > > Fanuc g code system a does not use g91, it uses u v w as their > > respective incremental axes for x y and z, which is why on a lathe > > you'll usually see > > g28 u0 w0 or something of that nature. You could use absolute values, > > but they come from your workpiece origin, so you'd have to say > > something like > > g28 x100 z100 to move to the absolute intermediate position above the > > part to not have a crash. > > > > The posted code in fusion is just ugly, no real reason to keep > > flopping back and forth like that. Fusion posts are JavaScript, so > > they're not terrible to modify. > > > > Phil T. > > The Feral Engineer > > > > Check out my LinuxCNC tutorials, machine builds and other antics at > > www.youtube.com/c/theferalengineer > > > > Help support my channel efforts and coffee addiction: > > www.patreon.com/theferalengineer > > > > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer > wrote: > > > > > A friend who uses MACH3 and Fusion360 (free version) found that > > > every G-Code file created by Fusion for the MACH environment added: > > > > > > G28 G91 Z0 > > > G90 > > > G28 G91 X0 Y0 > > > G90 > > > > > > He's since figured out how to tell Fusion not to do this but looking > at: > > > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 > > > > > > I m curious why there are two moves involved in this G-Code. In > > > this case the G91 changes to relative so the Z0 moves exactly 0 > > > first and then to the machine coordinates Z0 position. Same with XY. > > > > > > If 5161-5166 have something other than 0 and the G91 is left out the > > > system makes some interesting moves. > > > > > > My question is why would anyone want this kind of behavior? Where > > > would a > > > G28 be used without the G91? > > > > > > Is it perhaps to move around an obstacle
Re: [Emc-users] G28 behaviour
In effect the G91 incremental with a Z0 just cancels out the initial move to the Z position. I did try it on the mill as G28 Z-2 All that really happens is the machine sounds like it stumbles as it heads toward Z0 stopping briefly at Z-2. Very strange. John > -Original Message- > From: Todd Zuercher [mailto:to...@pgrahamdunn.com] > Sent: June-25-21 10:17 AM > To: Enhanced Machine Controller (EMC) > Subject: Re: [Emc-users] G28 behaviour > > I'm pretty sure all of our Fanuc machines use G91 for incremental G28 > commands and not U V W. (maybe some older Fanuc controls > or controls specialized for some manufacturers or maybe just T-series, I only > have worked with Ms.) > > But as to why the intermediate command, I have no idea, It's just how Fanuc's > G28 has always been. > > Todd Zuercher > P. Graham Dunn Inc. > 630 Henry Street� > Dalton, Ohio 44618 > Phone:� (330)828-2105ext. 2031 > > -Original Message- > From: John Dammeyer > Sent: Friday, June 25, 2021 1:06 PM > To: 'Enhanced Machine Controller (EMC)' > Subject: Re: [Emc-users] G28 behaviour > > [EXTERNAL EMAIL] Be sure links are safe. > > Thanks for the explanation but I'm still curious why the intermediate point. > > I suppose if I had a tool changer at the machine 0,0,0 position (or close to > that) and my A axis sitting on the left of the work I'd want > to move to a position that allows a clear path directly to the tool changer. > > But, why a special code for this? If I need Z to be at a specific machine > position doesn't a > G53 G0 Z10 > G53 G0 Z0 > do the same thing? Granted two lines but one doesn't have to look up what a > G28 does... > > > -Original Message- > > From: Feral Engineer [mailto:theferalengin...@gmail.com] > > Sent: June-25-21 9:51 AM > > To: Enhanced Machine Controller (EMC) > > Subject: Re: [Emc-users] G28 behaviour > > > > G28 is a return to reference using an intermediate point > > > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > > reference zero (machine zero in most cases). By using g91 g28 z0, you > > specify that the intermediate point is your current position and the > > machine will reference return from there. You can also use values such > > as > > g90 g28 z50. To use 50mm above your workpiece origin to be your > > intermediate point or you can use g91 g28 z10. To move 10mm up and use > > that as your intermediate. > > > > Fanuc g code system a does not use g91, it uses u v w as their > > respective incremental axes for x y and z, which is why on a lathe > > you'll usually see > > g28 u0 w0 or something of that nature. You could use absolute values, > > but they come from your workpiece origin, so you'd have to say > > something like > > g28 x100 z100 to move to the absolute intermediate position above the > > part to not have a crash. > > > > The posted code in fusion is just ugly, no real reason to keep > > flopping back and forth like that. Fusion posts are JavaScript, so > > they're not terrible to modify. > > > > Phil T. > > The Feral Engineer > > > > Check out my LinuxCNC tutorials, machine builds and other antics at > > www.youtube.com/c/theferalengineer > > > > Help support my channel efforts and coffee addiction: > > www.patreon.com/theferalengineer > > > > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer wrote: > > > > > A friend who uses MACH3 and Fusion360 (free version) found that > > > every G-Code file created by Fusion for the MACH environment added: > > > > > > G28 G91 Z0 > > > G90 > > > G28 G91 X0 Y0 > > > G90 > > > > > > He's since figured out how to tell Fusion not to do this but looking at: > > > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 > > > > > > I m curious why there are two moves involved in this G-Code. In > > > this case the G91 changes to relative so the Z0 moves exactly 0 > > > first and then to the machine coordinates Z0 position. Same with XY. > > > > > > If 5161-5166 have something other than 0 and the G91 is left out the > > > system makes some interesting moves. > > > > > > My question is why would anyone want this kind of behavior? Where > > > would a > > > G28 be used without the G91? > > > > > > Is it perhaps to move around an obstacle before it heads for 0,0,0? > > > > > > Thanks > > > John > > > > > > > > > > > > "ELS! Nothing else work
Re: [Emc-users] G28 behaviour
I'm pretty sure all of our Fanuc machines use G91 for incremental G28 commands and not U V W. (maybe some older Fanuc controls or controls specialized for some manufacturers or maybe just T-series, I only have worked with Ms.) But as to why the intermediate command, I have no idea, It's just how Fanuc's G28 has always been. Todd Zuercher P. Graham Dunn Inc. 630 Henry Street Dalton, Ohio 44618 Phone: (330)828-2105ext. 2031 -Original Message- From: John Dammeyer Sent: Friday, June 25, 2021 1:06 PM To: 'Enhanced Machine Controller (EMC)' Subject: Re: [Emc-users] G28 behaviour [EXTERNAL EMAIL] Be sure links are safe. Thanks for the explanation but I'm still curious why the intermediate point. I suppose if I had a tool changer at the machine 0,0,0 position (or close to that) and my A axis sitting on the left of the work I'd want to move to a position that allows a clear path directly to the tool changer. But, why a special code for this? If I need Z to be at a specific machine position doesn't a G53 G0 Z10 G53 G0 Z0 do the same thing? Granted two lines but one doesn't have to look up what a G28 does... > -Original Message- > From: Feral Engineer [mailto:theferalengin...@gmail.com] > Sent: June-25-21 9:51 AM > To: Enhanced Machine Controller (EMC) > Subject: Re: [Emc-users] G28 behaviour > > G28 is a return to reference using an intermediate point > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > reference zero (machine zero in most cases). By using g91 g28 z0, you > specify that the intermediate point is your current position and the > machine will reference return from there. You can also use values such > as > g90 g28 z50. To use 50mm above your workpiece origin to be your > intermediate point or you can use g91 g28 z10. To move 10mm up and use > that as your intermediate. > > Fanuc g code system a does not use g91, it uses u v w as their > respective incremental axes for x y and z, which is why on a lathe > you'll usually see > g28 u0 w0 or something of that nature. You could use absolute values, > but they come from your workpiece origin, so you'd have to say > something like > g28 x100 z100 to move to the absolute intermediate position above the > part to not have a crash. > > The posted code in fusion is just ugly, no real reason to keep > flopping back and forth like that. Fusion posts are JavaScript, so > they're not terrible to modify. > > Phil T. > The Feral Engineer > > Check out my LinuxCNC tutorials, machine builds and other antics at > www.youtube.com/c/theferalengineer > > Help support my channel efforts and coffee addiction: > www.patreon.com/theferalengineer > > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer wrote: > > > A friend who uses MACH3 and Fusion360 (free version) found that > > every G-Code file created by Fusion for the MACH environment added: > > > > G28 G91 Z0 > > G90 > > G28 G91 X0 Y0 > > G90 > > > > He's since figured out how to tell Fusion not to do this but looking at: > > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 > > > > I m curious why there are two moves involved in this G-Code. In > > this case the G91 changes to relative so the Z0 moves exactly 0 > > first and then to the machine coordinates Z0 position. Same with XY. > > > > If 5161-5166 have something other than 0 and the G91 is left out the > > system makes some interesting moves. > > > > My question is why would anyone want this kind of behavior? Where > > would a > > G28 be used without the G91? > > > > Is it perhaps to move around an obstacle before it heads for 0,0,0? > > > > Thanks > > John > > > > > > > > "ELS! Nothing else works as well for your Lathe" > > Automation Artisans Inc. > > www dot autoartisans dot com > > > > > > ___ > > 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] G28 behaviour
Ah. Ok. I'll try that to see what happens on my system. Sent from my Samsung S10 Original message From: Feral Engineer Date: 2021-06-25 10:36 a.m. (GMT-08:00) To: "Enhanced Machine Controller (EMC)" Subject: Re: [Emc-users] G28 behaviour So generally speaking, there are a few differences between g28 and g53. Onfanuc and mits controls, g53 is merely machine coordinate position, you canput g53 anywhere in the stroke of axis travel. G28 is reference returnposition 1, g30 is reference return 2, g30 p3 is position 3, g30 p4position 4. G30 positions are all programmable, via parameters, for whereto go. The major difference is g28 and g30 both indicate back to themachine that it has reached a "home" position, where g53 does not. If i sayg53 z0, the machine will not tool change, g91 g28 z0 will enable thereference status indicator and allow the tool change, even though it's theexact same spot.Phil T.The Feral EngineerCheck out my LinuxCNC tutorials, machine builds and other antics atwww.youtube.com/c/theferalengineerHelp support my channel efforts and coffee addiction:www.patreon.com/theferalengineerOn Fri, Jun 25, 2021, 1:09 PM John Dammeyer wrote:> Thanks for the explanation but I'm still curious why the intermediate> point.>> I suppose if I had a tool changer at the machine 0,0,0 position (or close> to that) and my A axis sitting on the left of the work I'd want to move to> a position that allows a clear path directly to the tool changer.>> But, why a special code for this? If I need Z to be at a specific machine> position doesn't a> G53 G0 Z10> G53 G0 Z0> do the same thing? Granted two lines but one doesn't have to look up> what a G28 does...>> > -Original Message-> > From: Feral Engineer [mailto:theferalengin...@gmail.com]> > Sent: June-25-21 9:51 AM> > To: Enhanced Machine Controller (EMC)> > Subject: Re: [Emc-users] G28 behaviour> >> > G28 is a return to reference using an intermediate point> >> > G90 G28 z0 would bring the tool to absolute Z0 before returning to> > reference zero (machine zero in most cases). By using g91 g28 z0, you> > specify that the intermediate point is your current position and the> > machine will reference return from there. You can also use values such as> > g90 g28 z50. To use 50mm above your workpiece origin to be your> > intermediate point or you can use g91 g28 z10. To move 10mm up and use> that> > as your intermediate.> >> > Fanuc g code system a does not use g91, it uses u v w as their respective> > incremental axes for x y and z, which is why on a lathe you'll usually> see> > g28 u0 w0 or something of that nature. You could use absolute values, but> > they come from your workpiece origin, so you'd have to say something like> > g28 x100 z100 to move to the absolute intermediate position above the> part> > to not have a crash.> >> > The posted code in fusion is just ugly, no real reason to keep flopping> > back and forth like that. Fusion posts are JavaScript, so they're not> > terrible to modify.> >> > Phil T.> > The Feral Engineer> >> > Check out my LinuxCNC tutorials, machine builds and other antics at> > www.youtube.com/c/theferalengineer> >> > Help support my channel efforts and coffee addiction:> > www.patreon.com/theferalengineer> >> > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer > wrote:> >> > > A friend who uses MACH3 and Fusion360 (free version) found that every> > > G-Code file created by Fusion for the MACH environment added:> > >> > > G28 G91 Z0> > > G90> > > G28 G91 X0 Y0> > > G90> > >> > > He's since figured out how to tell Fusion not to do this but looking> at:> > > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1> > >> > > I�m curious why there are two moves involved in this G-Code. In this> case> > > the G91 changes to relative so the Z0 moves exactly 0 first and then> to the> > > machine coordinates Z0 position. Same with XY.> > >> > > If 5161-5166 have something other than 0 and the G91 is left out the> > > system makes some interesting moves.> > >> > > My question is why would anyone want this kind of behavior? Where> would a> > > G28 be used without the G91?> > >> > > Is it perhaps to move around an obstacle before it heads for 0,0,0?> > >> > > Thanks> > > John> > >> > >> > >> > > "ELS! Nothing else works as well for your Lathe"> > > Auto
Re: [Emc-users] G28 behaviour
So generally speaking, there are a few differences between g28 and g53. On fanuc and mits controls, g53 is merely machine coordinate position, you can put g53 anywhere in the stroke of axis travel. G28 is reference return position 1, g30 is reference return 2, g30 p3 is position 3, g30 p4 position 4. G30 positions are all programmable, via parameters, for where to go. The major difference is g28 and g30 both indicate back to the machine that it has reached a "home" position, where g53 does not. If i say g53 z0, the machine will not tool change, g91 g28 z0 will enable the reference status indicator and allow the tool change, even though it's the exact same spot. Phil T. The Feral Engineer Check out my LinuxCNC tutorials, machine builds and other antics at www.youtube.com/c/theferalengineer Help support my channel efforts and coffee addiction: www.patreon.com/theferalengineer On Fri, Jun 25, 2021, 1:09 PM John Dammeyer wrote: > Thanks for the explanation but I'm still curious why the intermediate > point. > > I suppose if I had a tool changer at the machine 0,0,0 position (or close > to that) and my A axis sitting on the left of the work I'd want to move to > a position that allows a clear path directly to the tool changer. > > But, why a special code for this? If I need Z to be at a specific machine > position doesn't a > G53 G0 Z10 > G53 G0 Z0 > do the same thing? Granted two lines but one doesn't have to look up > what a G28 does... > > > -Original Message- > > From: Feral Engineer [mailto:theferalengin...@gmail.com] > > Sent: June-25-21 9:51 AM > > To: Enhanced Machine Controller (EMC) > > Subject: Re: [Emc-users] G28 behaviour > > > > G28 is a return to reference using an intermediate point > > > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > > reference zero (machine zero in most cases). By using g91 g28 z0, you > > specify that the intermediate point is your current position and the > > machine will reference return from there. You can also use values such as > > g90 g28 z50. To use 50mm above your workpiece origin to be your > > intermediate point or you can use g91 g28 z10. To move 10mm up and use > that > > as your intermediate. > > > > Fanuc g code system a does not use g91, it uses u v w as their respective > > incremental axes for x y and z, which is why on a lathe you'll usually > see > > g28 u0 w0 or something of that nature. You could use absolute values, but > > they come from your workpiece origin, so you'd have to say something like > > g28 x100 z100 to move to the absolute intermediate position above the > part > > to not have a crash. > > > > The posted code in fusion is just ugly, no real reason to keep flopping > > back and forth like that. Fusion posts are JavaScript, so they're not > > terrible to modify. > > > > Phil T. > > The Feral Engineer > > > > Check out my LinuxCNC tutorials, machine builds and other antics at > > www.youtube.com/c/theferalengineer > > > > Help support my channel efforts and coffee addiction: > > www.patreon.com/theferalengineer > > > > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer > wrote: > > > > > A friend who uses MACH3 and Fusion360 (free version) found that every > > > G-Code file created by Fusion for the MACH environment added: > > > > > > G28 G91 Z0 > > > G90 > > > G28 G91 X0 Y0 > > > G90 > > > > > > He's since figured out how to tell Fusion not to do this but looking > at: > > > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 > > > > > > I�m curious why there are two moves involved in this G-Code. In this > case > > > the G91 changes to relative so the Z0 moves exactly 0 first and then > to the > > > machine coordinates Z0 position. Same with XY. > > > > > > If 5161-5166 have something other than 0 and the G91 is left out the > > > system makes some interesting moves. > > > > > > My question is why would anyone want this kind of behavior? Where > would a > > > G28 be used without the G91? > > > > > > Is it perhaps to move around an obstacle before it heads for 0,0,0? > > > > > > Thanks > > > John > > > > > > > > > > > > "ELS! Nothing else works as well for your Lathe" > > > Automation Artisans Inc. > > > www dot autoartisans dot com > > > > > > > > > ___ > > > 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] G28 behaviour
Thanks for the explanation but I'm still curious why the intermediate point. I suppose if I had a tool changer at the machine 0,0,0 position (or close to that) and my A axis sitting on the left of the work I'd want to move to a position that allows a clear path directly to the tool changer. But, why a special code for this? If I need Z to be at a specific machine position doesn't a G53 G0 Z10 G53 G0 Z0 do the same thing? Granted two lines but one doesn't have to look up what a G28 does... > -Original Message- > From: Feral Engineer [mailto:theferalengin...@gmail.com] > Sent: June-25-21 9:51 AM > To: Enhanced Machine Controller (EMC) > Subject: Re: [Emc-users] G28 behaviour > > G28 is a return to reference using an intermediate point > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > reference zero (machine zero in most cases). By using g91 g28 z0, you > specify that the intermediate point is your current position and the > machine will reference return from there. You can also use values such as > g90 g28 z50. To use 50mm above your workpiece origin to be your > intermediate point or you can use g91 g28 z10. To move 10mm up and use that > as your intermediate. > > Fanuc g code system a does not use g91, it uses u v w as their respective > incremental axes for x y and z, which is why on a lathe you'll usually see > g28 u0 w0 or something of that nature. You could use absolute values, but > they come from your workpiece origin, so you'd have to say something like > g28 x100 z100 to move to the absolute intermediate position above the part > to not have a crash. > > The posted code in fusion is just ugly, no real reason to keep flopping > back and forth like that. Fusion posts are JavaScript, so they're not > terrible to modify. > > Phil T. > The Feral Engineer > > Check out my LinuxCNC tutorials, machine builds and other antics at > www.youtube.com/c/theferalengineer > > Help support my channel efforts and coffee addiction: > www.patreon.com/theferalengineer > > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer wrote: > > > A friend who uses MACH3 and Fusion360 (free version) found that every > > G-Code file created by Fusion for the MACH environment added: > > > > G28 G91 Z0 > > G90 > > G28 G91 X0 Y0 > > G90 > > > > He's since figured out how to tell Fusion not to do this but looking at: > > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 > > > > I�m curious why there are two moves involved in this G-Code. In this case > > the G91 changes to relative so the Z0 moves exactly 0 first and then to the > > machine coordinates Z0 position. Same with XY. > > > > If 5161-5166 have something other than 0 and the G91 is left out the > > system makes some interesting moves. > > > > My question is why would anyone want this kind of behavior? Where would a > > G28 be used without the G91? > > > > Is it perhaps to move around an obstacle before it heads for 0,0,0? > > > > Thanks > > John > > > > > > > > "ELS! Nothing else works as well for your Lathe" > > Automation Artisans Inc. > > www dot autoartisans dot com > > > > > > ___ > > 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] G28 behaviour
G28 is a return to reference using an intermediate point G90 G28 z0 would bring the tool to absolute Z0 before returning to reference zero (machine zero in most cases). By using g91 g28 z0, you specify that the intermediate point is your current position and the machine will reference return from there. You can also use values such as g90 g28 z50. To use 50mm above your workpiece origin to be your intermediate point or you can use g91 g28 z10. To move 10mm up and use that as your intermediate. Fanuc g code system a does not use g91, it uses u v w as their respective incremental axes for x y and z, which is why on a lathe you'll usually see g28 u0 w0 or something of that nature. You could use absolute values, but they come from your workpiece origin, so you'd have to say something like g28 x100 z100 to move to the absolute intermediate position above the part to not have a crash. The posted code in fusion is just ugly, no real reason to keep flopping back and forth like that. Fusion posts are JavaScript, so they're not terrible to modify. Phil T. The Feral Engineer Check out my LinuxCNC tutorials, machine builds and other antics at www.youtube.com/c/theferalengineer Help support my channel efforts and coffee addiction: www.patreon.com/theferalengineer On Fri, Jun 25, 2021, 12:28 PM John Dammeyer wrote: > A friend who uses MACH3 and Fusion360 (free version) found that every > G-Code file created by Fusion for the MACH environment added: > > G28 G91 Z0 > G90 > G28 G91 X0 Y0 > G90 > > He's since figured out how to tell Fusion not to do this but looking at: > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 > > I’m curious why there are two moves involved in this G-Code. In this case > the G91 changes to relative so the Z0 moves exactly 0 first and then to the > machine coordinates Z0 position. Same with XY. > > If 5161-5166 have something other than 0 and the G91 is left out the > system makes some interesting moves. > > My question is why would anyone want this kind of behavior? Where would a > G28 be used without the G91? > > Is it perhaps to move around an obstacle before it heads for 0,0,0? > > Thanks > John > > > > "ELS! Nothing else works as well for your Lathe" > Automation Artisans Inc. > www dot autoartisans dot com > > > ___ > 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] G28 behaviour
A friend who uses MACH3 and Fusion360 (free version) found that every G-Code file created by Fusion for the MACH environment added: G28 G91 Z0 G90 G28 G91 X0 Y0 G90 He's since figured out how to tell Fusion not to do this but looking at: http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 I’m curious why there are two moves involved in this G-Code. In this case the G91 changes to relative so the Z0 moves exactly 0 first and then to the machine coordinates Z0 position. Same with XY. If 5161-5166 have something other than 0 and the G91 is left out the system makes some interesting moves. My question is why would anyone want this kind of behavior? Where would a G28 be used without the G91? Is it perhaps to move around an obstacle before it heads for 0,0,0? Thanks John "ELS! Nothing else works as well for your Lathe" Automation Artisans Inc. www dot autoartisans dot com ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
