where to find info on parameters
16 Feb 2011 00:38 #7228
by Dave_Dyke
where to find info on parameters was created by Dave_Dyke
Hi emc'rs,
I have the need to change the retract distance in the G73 peck cycle, but can find no info on the subject, can anyone enlighten me.
thanks for any help.
Dave
I have the need to change the retract distance in the G73 peck cycle, but can find no info on the subject, can anyone enlighten me.
thanks for any help.
Dave
Please Log in or Create an account to join the conversation.
16 Feb 2011 08:26 #7232
by andypugh
Replied by andypugh on topic Re:where to find info on parameters
The retract bahaviour is set by G98 or G99
linuxcnc.org/docs/html/gcode_main.html#sub:G98,-G99:-Set
Generally I use G98 and then the retract is to the Z position that the tool was at prior to the canned cycle.
In fact, I pretty much always use a line like:
G98 G73 R.2 F20......
linuxcnc.org/docs/html/gcode_main.html#sub:G98,-G99:-Set
Generally I use G98 and then the retract is to the Z position that the tool was at prior to the canned cycle.
In fact, I pretty much always use a line like:
G98 G73 R.2 F20......
Please Log in or Create an account to join the conversation.
16 Feb 2011 15:03 #7239
by Dave_Dyke
Replied by Dave_Dyke on topic Re:where to find info on parameters
Sorry, I should have been more specific, what I need to change is the stand-off distance when the tool returns from the R plane (G83).
What is happening with this machine is, it flexes so much that the G73 retract distance is less than the flex, so there is no chip break.
On a haas control for instance it is setting 22 that controls this distance.
What is happening with this machine is, it flexes so much that the G73 retract distance is less than the flex, so there is no chip break.
On a haas control for instance it is setting 22 that controls this distance.
Please Log in or Create an account to join the conversation.
16 Feb 2011 15:38 #7241
by andypugh
Replied by andypugh on topic Re:where to find info on parameters
I think that G98 retract is what you need then,
Assuming material surface at Z0
G0 Z1
G98 G83 R0.1 F1 Z-1 Q0.3
Would rapid to Z=1, then rapid to Z=0.1, drill for 0.3, back out to Z = 1, rapid to Z = -0.2, drill to 0.6 etc.
If it is just chip breaking you want, then I assume (can't test right now) that the back-out is the R value?
Assuming material surface at Z0
G0 Z1
G98 G83 R0.1 F1 Z-1 Q0.3
Would rapid to Z=1, then rapid to Z=0.1, drill for 0.3, back out to Z = 1, rapid to Z = -0.2, drill to 0.6 etc.
If it is just chip breaking you want, then I assume (can't test right now) that the back-out is the R value?
Please Log in or Create an account to join the conversation.
16 Feb 2011 16:18 #7243
by Dave_Dyke
Replied by Dave_Dyke on topic Re:where to find info on parameters
Thanks for your reply Andy, I don't know that it is a G code that I am after,probably a parameter or variable.
I understand and use G99/G98
G0 Z1
G98 G83 R0.1 F1 Z-1 Q0.3
Would rapid to Z=1, then rapid to Z=0.1, drill for 0.3, back out to Z = 1, rapid to Z = -0.2, drill to 0.6 etc.
in your G code above you have the drill rapid down to Z-0.2, that is my problem, there must be clearance between the drill point and workpiece before feed motion begins, it is this clearance that I want to change, as a default it is 0.01" AFAIK
Stewart asked about this on the list a couple of years ago, but I have been unable to find it in the archive.
I understand and use G99/G98
G0 Z1
G98 G83 R0.1 F1 Z-1 Q0.3
Would rapid to Z=1, then rapid to Z=0.1, drill for 0.3, back out to Z = 1, rapid to Z = -0.2, drill to 0.6 etc.
in your G code above you have the drill rapid down to Z-0.2, that is my problem, there must be clearance between the drill point and workpiece before feed motion begins, it is this clearance that I want to change, as a default it is 0.01" AFAIK
Stewart asked about this on the list a couple of years ago, but I have been unable to find it in the archive.
Please Log in or Create an account to join the conversation.
16 Feb 2011 17:35 #7251
by andypugh
Replied by andypugh on topic Re:where to find info on parameters
Dave_Dyke wrote:
I am miles from a machine at the moment, but my impression is that it ought to use the R value as the chip-break retract in G98 mode.
<time passes>
It does actually appear to be hard-coded.
git.linuxcnc.org/gitweb?p=emc2.git;a=blo...c/interp_internal.hh
Line 42.
is used here:
git.linuxcnc.org/gitweb?p=emc2.git;a=blo...ngc/interp_cycles.cc
Line 173
If you were to edit that Line 42 in the header file and recompile EMC2, that would fix it. But that isn't a trivial or easy solution.
I am of the opinion that it should use the R value, and I might suggest that as a change to the devs.
In that example there should be clearance, as the hole is already -0.3 deep at that stage?Would rapid to Z=1, then rapid to Z=0.1, drill for 0.3, back out to Z = 1, rapid to Z = -0.2, drill to 0.6 etc.
in your G code above you have the drill rapid down to Z-0.2, that is my problem, there must be clearance between the drill point and workpiece before feed motion begins
I am miles from a machine at the moment, but my impression is that it ought to use the R value as the chip-break retract in G98 mode.
<time passes>
It does actually appear to be hard-coded.
git.linuxcnc.org/gitweb?p=emc2.git;a=blo...c/interp_internal.hh
Line 42.
is used here:
git.linuxcnc.org/gitweb?p=emc2.git;a=blo...ngc/interp_cycles.cc
Line 173
If you were to edit that Line 42 in the header file and recompile EMC2, that would fix it. But that isn't a trivial or easy solution.
I am of the opinion that it should use the R value, and I might suggest that as a change to the devs.
Please Log in or Create an account to join the conversation.
16 Feb 2011 18:12 #7255
by Dave_Dyke
Replied by Dave_Dyke on topic Re:where to find info on parameters
Thanks Andy, that's exactly what I needed to know.
I have compiled before, so I will give it a go.
I have compiled before, so I will give it a go.
Please Log in or Create an account to join the conversation.
16 Feb 2011 22:08 #7265
by Dave_Dyke
Replied by Dave_Dyke on topic Re:where to find info on parameters
Andy
Thanks again, I have it working as I wanted,
it would be really handy to be able to set the delta in the ini file though.
Dave
Thanks again, I have it working as I wanted,
it would be really handy to be able to set the delta in the ini file though.Dave
Please Log in or Create an account to join the conversation.
Time to create page: 0.084 seconds