Can't get zero to be up on Z axis
04 Dec 2014 07:57 #53667
by DaBit
Replied by DaBit on topic Can't get zero to be up on Z axis
There are more strange things going on in Cam360:
That G64 P0.2 is a large tolerance, especially since there is no futher G64 present during a finishing pass (this code is for a Toolox33 steel part, not wood), and the G53 is weird too.
On the other hand: having such powerful CAM software available at no cost for noncommercial use is great and the postprocessors can be edited. Line 571, 1213 and 1233 in the emc.cps file seems to be where the G53's are written.
%
(T1 D=6. CR=0. - ZMIN=-5.9 - FLAT END MILL)
N05 G64 P0.2
N10 G90 G94 G17 G91.1
N15 G21
N20 G53 G0 Z0.
(ADAPTIVE1)
N25 M9
N30 T1 M6
N35 S9982 M3
N37 G4 P3
N40 G54
N45 M9
..
..That G64 P0.2 is a large tolerance, especially since there is no futher G64 present during a finishing pass (this code is for a Toolox33 steel part, not wood), and the G53 is weird too.
On the other hand: having such powerful CAM software available at no cost for noncommercial use is great and the postprocessors can be edited. Line 571, 1213 and 1233 in the emc.cps file seems to be where the G53's are written.
Please Log in or Create an account to join the conversation.
11 Apr 2016 21:55 - 11 Apr 2016 21:59 #73136
by pommen
Replied by pommen on topic Can't get zero to be up on Z axis
I had the same issue today on using fusion360 cam (first time I tried it)
When going though the PP i found a function called "on section()" and it has this little bit in it, which I think is the one to change in some way. If not to make it completely ignore, then perhaps to set to a friendlier number (eg. z-5 or some-such)
I'll play around a bit with it, if noone else already have a fi, and willing to share.
Edit*
Will setting var useG28 = true; change the output to WCS Z0 ? kinda looks like it, but im not really sure what im looking at.
/Peter
When going though the PP i found a function called "on section()" and it has this little bit in it, which I think is the one to change in some way. If not to make it completely ignore, then perhaps to set to a friendlier number (eg. z-5 or some-such)
// retract to safe plane
retracted = true;
if (useG28) {
writeBlock(gFormat.format(28), gAbsIncModal.format(91), "Z" + xyzFormat.format(0)); // retract
writeBlock(gAbsIncModal.format(90));
} else {
writeBlock(gAbsIncModal.format(90), gFormat.format(53), gMotionModal.format(0), "Z" + xyzFormat.format(0)); // retract
}
zOutput.reset();
}I'll play around a bit with it, if noone else already have a fi, and willing to share.
Edit*
Will setting var useG28 = true; change the output to WCS Z0 ? kinda looks like it, but im not really sure what im looking at.
/Peter
Last edit: 11 Apr 2016 21:59 by pommen.
Please Log in or Create an account to join the conversation.
12 Apr 2016 11:27 #73153
by andypugh
It looks like it should, though I don't know where you would make that change.
You would also have to define a G28 position in LinuxCNC.
I do think that the safest thing to do is to simply set Z=0 at the top of travel.
Replied by andypugh on topic Can't get zero to be up on Z axis
Will setting var useG28 = true; change the output to WCS Z0
It looks like it should, though I don't know where you would make that change.
You would also have to define a G28 position in LinuxCNC.
I do think that the safest thing to do is to simply set Z=0 at the top of travel.
Please Log in or Create an account to join the conversation.
12 Apr 2016 17:55 #73181
by pommen
Replied by pommen on topic Can't get zero to be up on Z axis
I have my Z0 on the top, but have set soft limits to Z-1, so it was giving me a bit of frustration having to edit every file manually before running it.
I ended up with replacing the g53 Z0 command with G90 Z5 at start/ tool change and g0 15 at end. I have only tested on one part so far but it seems to do the job. Now at the start, tool change or end of the program it just raises the bit 5mm above Z0 or 15 mm and the end of the run. This is my very first attempt at looking at a PP, so I have no idea if it ends up crashing sometime in the future..but I need to start somewhere i guess =)
There are some user vars in the start of the current EMC2 post in fusion360.
I noticed that the was a post called linuxcnc as well, isn't emc2 just an older name of Linuxcnc?
I ended up with replacing the g53 Z0 command with G90 Z5 at start/ tool change and g0 15 at end. I have only tested on one part so far but it seems to do the job. Now at the start, tool change or end of the program it just raises the bit 5mm above Z0 or 15 mm and the end of the run. This is my very first attempt at looking at a PP, so I have no idea if it ends up crashing sometime in the future..but I need to start somewhere i guess =)
Will setting var useG28 = true; change the output to WCS Z0
It looks like it should, though I don't know where you would make that change.
There are some user vars in the start of the current EMC2 post in fusion360.
I noticed that the was a post called linuxcnc as well, isn't emc2 just an older name of Linuxcnc?
Please Log in or Create an account to join the conversation.
12 Apr 2016 22:01 #73198
by andypugh
Ah, in that situation you would set the home switch to be at +1 so that the highest valid position is 0.
Replied by andypugh on topic Can't get zero to be up on Z axis
I have my Z0 on the top, but have set soft limits to Z-1, so it was giving me a bit of frustration having to edit every file manually before running it.
Ah, in that situation you would set the home switch to be at +1 so that the highest valid position is 0.
Please Log in or Create an account to join the conversation.
13 Apr 2016 06:14 #73213
by pommen
Replied by pommen on topic Can't get zero to be up on Z axis
Not a bad idea at all. I think i'll do that,
Thanks Andy!Not a bad idea at all. I think i'll do that,
Thanks Andy!
Thanks Andy!Not a bad idea at all. I think i'll do that,
Thanks Andy!
Please Log in or Create an account to join the conversation.
Time to create page: 0.081 seconds