I have a traditional CNC, and now I have recently started working with rotary CNC woodworking. My machine has X, Z, and A axis. I am currently using vcarve pro 9.5. Both my machines run on LinuxCNC.
My issue – when using rotary gcode straight out of vcarve, the rotary speeds are all over the place. Often VERY slow, but then sometimes it will suddenly go crazy fast.
I understand that as of version 9.5 vectric products now can work with G93.
I have tweaked my PP for basic changes, but I do not understand how to change the PP to work with the G93 command.
Is there already a PP out there I can tweak to work with LinuxCNC, or can someone explain how to convert my existing PP to work with G93.
G93 for Rotary LinuxCNC Post Processor
Re: G93 for Rotary LinuxCNC Post Processor
If you have a working rotary PP for your machine, enabling G93 inverse time mode should be relatively straight-forward. To enable it you need to make following modifications:
Greg K
- Add following code to enable inverse time mode in the output
Code: Select all
INVERSE_TIME_MODE = YES
- Enable inverse time mode on your controller (e.g. by adding G93 command in HEADER
- Add inverse time variable:
Code: Select all
VAR INVERSE_TIME = [FI|A| F|1.1]
- Add inverse time output for relevant moves, e.g.: by using [FI] instead of [F] in G1 moves
Code: Select all
+--------------------------------------------------- + Commands output for feed rate moves +--------------------------------------------------- begin FEED_MOVE "G1 [X] [Y] [Z] [FI]"
Greg K
Re: G93 for Rotary LinuxCNC Post Processor
Thank you so much.
I will plug this in tonight and take a look at the gcode generated. If it looks good, I will try it on the machine this weekend.
Thanks again,
Rob
I will plug this in tonight and take a look at the gcode generated. If it looks good, I will try it on the machine this weekend.
Thanks again,
Rob
Re: G93 for Rotary LinuxCNC Post Processor
I am getting error:
F1
Unknown variable name
On line 144 of file
C:\-----------------------------------
"G01 [X] [Y] [Z] [F1]"
Any ideas?
F1
Unknown variable name
On line 144 of file
C:\-----------------------------------
"G01 [X] [Y] [Z] [F1]"
Any ideas?
- Attachments
-
- LinuxCNC_Wrap_Y2A_inch test.pp
- Post P
- (5.48 KiB) Downloaded 243 times
Re: G93 for Rotary LinuxCNC Post Processor
Looks like you placed [F1]] instead of [FI]. The second character is 'I' as in 'ice'. I can see that in this font both characters look almost the same.
There a few more things that needs changing:
Please find the PP with all of the above corrections: Greg K
There a few more things that needs changing:
- In header section the postp was still issuing G94. I changed it to G93.
- I added G94 in the footer, to restore the more usual feed rate mode after toolpath is finished.
- The [F] have to be replaced with [FI] for every move, not only the FEED_MOVE. I added changed it for FIRST_FEED_MOVE as well.
Please find the PP with all of the above corrections: Greg K
Re: G93 for Rotary LinuxCNC Post Processor
Thank you.
The gcode looks good. I cannot test on the machine till the weekend, but from what I can see, it looks very similar to what other programs are generating.
The gcode looks good. I cannot test on the machine till the weekend, but from what I can see, it looks very similar to what other programs are generating.
- Mogal
- Vectric Craftsman
- Posts: 238
- Joined: Wed Oct 13, 2010 5:28 pm
- Model of CNC Machine: DIY CNC
- Location: Victoria, BC
- Contact:
Re: G93 for Rotary LinuxCNC Post Processor
A big Thank you for Greg here!
I just got a rotary axis and found out the hard way that it spins so slow!
Greg's post has helped me out tremendously!
My first (proto-type) rotary part took nearly 3 hours (with a few hiccups along the way)
The second one took a 1 hour and 14 mins! (with no hiccups)
So much quicker!
I do however get a 'gcode not supported' error. Everything works, but not sure why I get it.
A side question (observation) it seems that the rotary will spin speed changes with the function of diameter?
The closer to the center of rotation, the quicker the rotary would turn.
Thanks!
I just got a rotary axis and found out the hard way that it spins so slow!
Greg's post has helped me out tremendously!
My first (proto-type) rotary part took nearly 3 hours (with a few hiccups along the way)
The second one took a 1 hour and 14 mins! (with no hiccups)
So much quicker!
I do however get a 'gcode not supported' error. Everything works, but not sure why I get it.
A side question (observation) it seems that the rotary will spin speed changes with the function of diameter?
The closer to the center of rotation, the quicker the rotary would turn.
Thanks!
- Attachments
-
- Spindle G93 - 2.txt
- (331.08 KiB) Downloaded 210 times
-
- Mogal-UCCNC_inch - Rotary.pp.txt
- (5.77 KiB) Downloaded 206 times
-
- Vectric Wizard
- Posts: 1717
- Joined: Sun Sep 23, 2012 12:14 pm
- Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"
Re: G93 for Rotary LinuxCNC Post Processor
I run a machine using linuxCNC that had a rotary axis. The slow spin once a toolpath starts is because it general is converting X (inches/min) to A (degrees/minute) in the post processor. If the bit you have selected has a feed speed of 200ipm for example, that will equal 200 degree per minute on the rotary axis. Very slow.
My machine is hardware limited to 200ipm on X, and Y, so I usually change the feed speed for the bit I'm using on the rotary to 4000ipm or so. This gets the rotary spinning at 4000 degrees/minute (11.11 rotations/minute) but limits the Y direction moves to 200ipm. I'll use the feed speed slider in lunixCNC to slow down the CNC if any part of the cut seems/sounds too aggressive.
4D
My machine is hardware limited to 200ipm on X, and Y, so I usually change the feed speed for the bit I'm using on the rotary to 4000ipm or so. This gets the rotary spinning at 4000 degrees/minute (11.11 rotations/minute) but limits the Y direction moves to 200ipm. I'll use the feed speed slider in lunixCNC to slow down the CNC if any part of the cut seems/sounds too aggressive.
4D