Author Topic: G 05  (Read 551 times)

0 Members and 1 Guest are viewing this topic.

Offline KatzYaakov

  • Active Member
  • Posts: 41
    • View Profile
G 05
« on: June 29, 2018, 02:10:05 AM »
ic that g5 not included in gcode list of mach
is there something similar ?

Offline joeaverage

  • Active Member
  • Posts: 4,520
    • View Profile
Re: G 05
« Reply #1 on: June 29, 2018, 02:50:24 AM »
Hi,
I've looked through 'CNC Programming Handbook 2nd ed' by Peter Smid, the CNC bible as it were and there is no G05.
What is it supposed to do?

There is an M05 of course, it means 'stop the spindle'. Does G05 mean the same thing?

Craig
My wife left with my best friend...
     and I miss him!

Offline KatzYaakov

  • Active Member
  • Posts: 41
    • View Profile
Re: G 05
« Reply #2 on: June 29, 2018, 02:59:19 AM »
it use to smoothing path for faster work

Offline joeaverage

  • Active Member
  • Posts: 4,520
    • View Profile
Re: G 05
« Reply #3 on: June 29, 2018, 02:59:29 AM »
Hi,
I found this in Wikipedia:

Quote
G05 P10000 High-precision contour control (HPCC) M   Uses a deep look-ahead buffer and simulation processing to provide better axis movement acceleration and deceleration during contour milling
G05.1 Q1. AI Advanced Preview Control M   Uses a deep look-ahead buffer and simulation processing to provide better axis movement acceleration and deceleration during contour milling

Is that what you had in mind?

Craig
My wife left with my best friend...
     and I miss him!

Offline joeaverage

  • Active Member
  • Posts: 4,520
    • View Profile
Re: G 05
« Reply #4 on: June 29, 2018, 03:03:38 AM »
Hi,
to my knowledge Mach4 conforms to Fanuc 21 and it has linear interpolation and circular arcs but the trajectory planner doesn't use splines
any other curve approximation algorithm.

Craig
My wife left with my best friend...
     and I miss him!

Offline KatzYaakov

  • Active Member
  • Posts: 41
    • View Profile
Re: G 05
« Reply #5 on: June 29, 2018, 04:02:12 AM »
maybe the option to work without exact stop can have similar results?

Offline smurph

  • Administrator
  • *
  • Posts: 1,051
  • "That there... that's an RV."
    • View Profile
Re: G 05
« Reply #6 on: July 10, 2018, 06:08:29 PM »
The default motion mode is determined by the general tab of the configuration dialog.  Exact Stop (G61) or Constant Velocity (G64), CV for short.  G64 is the semi-equivalent of you motion smoothing.  Most of the time, G64 (CV) is the default motion mode.  G64 it is primarily characterized by the acceleration capabilities of your machine.  The higher the accel settings/capabilities, the closer CV cuts to the true path.  There is a way to tailor the CV settings by angle.  But there isn't a way to blend with a number in a range like your G5 command. 

Steve

Offline Mauri

  • Active Member
  • Posts: 292
    • View Profile
Re: G 05
« Reply #7 on: July 10, 2018, 07:56:50 PM »
KatzYaakov,
I have used CV with great success (nothing is perfect in the CNC world).
The secret is having the correct angle Feedrate with the Blend Radius 0 to 170 degrees.
I can run a very good finish with brass using a .05mm radius TBN cutter with CV.
Example F400 Z/Y/Z CV Feedrate Maximum 150 on the angles and blend radius  (0 to 179).
You can use the Wizard mcCvTuningWizardV3-3Beta and enter your desired inputs (axis selection and tolerance).
Then go into machine.ini and reduce the larger feedrates of the small angles to a smaller constant maximum number and leave the rest.
This will the produce a good line smoothing result.
I automatically change all my angle feedrates via enties on the screen.
You can test this by doing some small lettering G-Code and running it in Mach4 with CV and the settings you set above.
On my tests I have gone down to 1mm high lettering the minimum we cut.
Depending on the speed you intend to use and the type of material you use on a job the maximum number may vary, best the do a simple lettering test or the road runnner to see how close and smooth the cutting line will be.
Regards,
Mauri