G93 for Rotary LinuxCNC Post Processor

This forum is for requests and queries about machine tool support for Vectric Products
Post Reply
rjshust
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder

G93 for Rotary LinuxCNC Post Processor

Post by rjshust »

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 currently run my gcode through a free product called “Rapid Rotary” (there is a nice youtube video showing the issue, and showing the software). This software does a good job converting the code to work with the G93 command, and if I cannot get the PP to work, I will still be ok. I would much prefer elimination that step, and having more control using the vectric PP.

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.

gregk
Vectric Staff
Posts: 94
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: G93 for Rotary LinuxCNC Post Processor

Post by gregk »

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:
  • 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]"
I hope that helps. In any case if you decide to modify the post processor make sure that you've make a copy of the original file and be sure to inspect and verify generated g-code to ensure that it works the way you would expect, before sending it to the machine. Performing an air cut my also be a good idea.

Greg K

rjshust
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder

Re: G93 for Rotary LinuxCNC Post Processor

Post by rjshust »

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

rjshust
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder

Re: G93 for Rotary LinuxCNC Post Processor

Post by rjshust »

I am getting error:

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 35 times

gregk
Vectric Staff
Posts: 94
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: G93 for Rotary LinuxCNC Post Processor

Post by gregk »

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:
  • 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:
LinuxCNC_Wrap_Y2A_inch test.pp
(5.52 KiB) Downloaded 54 times
Greg K

rjshust
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder

Re: G93 for Rotary LinuxCNC Post Processor

Post by rjshust »

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 that other program was generating.

User avatar
Mogal
Vectric Craftsman
Posts: 206
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

Post by Mogal »

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!
Attachments
Spindle G93 - 2.txt
(331.08 KiB) Downloaded 4 times
Mogal-UCCNC_inch - Rotary.pp.txt
(5.77 KiB) Downloaded 6 times

4DThinker
Vectric Wizard
Posts: 1327
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

Post by 4DThinker »

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

Post Reply