CAMWorks Post Processor

Anything and everything CNC-Shark-related

Moderators: ddw, sbk, al wolford

CAMWorks Post Processor

Postby cbaldwin » Wed May 09, 2018 5:38 pm

Just bought a CNC Shark only to find that none of our CAMworks post processors work. Does anyone have any suggestions on where to find a Post for CAMworks?
cbaldwin
 
Posts: 1
Joined: Wed May 09, 2018 5:25 pm

Re: CAMWorks Post Processor

Postby Rando » Thu May 10, 2018 2:54 am

A Generic GCODE-output usually works pretty well. Some things you'll need to turn off:

  • no line numbers
  • don't use + in field values (Z+5.0 can crash the controller)
  • the controllers CAN do 3D helical interpolation
  • Do NOT use the M06 tool change commands unless you want a Pause/Continue in your process...that won't actually let you change the bit unless they're set precisely at the same height.
  • M03/M05 turn the router on and off
  • have only one M02 at the end
  • it can't handle more than one toolpath in a single file, because of the only-one M02 restriction
  • all caps in the names
  • it can do 3 digits of actual resolution (the HDs can), so I typically give it 4.
  • Comments use the # at the start.
  • The controller technically *can* handle inline comments, but I avoid them just for my own paranoia
  • I'm almost certain that the controllers CANNOT handle incremental positioning mode.
  • Inch or metric is fine
  • basic drill pecking is supported, but the newer pecking and tapping cycles are not there
  • Spindle speed commands do not control the outputs :(
  • There are no other hardware outputs, so none of the flood or other coolant controls do anything
  • remember that just because you put it in the GCODE, if you don't have the required licenses, it may not work. Think 4th axis, etc.
  • Theoretically it can do "probing" of some form, but I've seen no references as to the expected GCODE. It might be a DLL-based API that not exposed in GCODE, but who knows
  • Remember that it DOES support interpolation control (versus exact-stop mode) and you can set the tolerance

Other than that, it's a very generic post processor...and I think those are a lot of things that MAKE IT a generic one.

Most CAM systems have a post processor selection for a generic 3-axis GCODE mill.

Hope that helps

Thom


My posts are pretty heavily modified, and I've customized them for BobCAD and Vectric. Can't imagine the MasterCAM
post processors are any more complicated, given they don't do anything particularly different.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)
Rando
 
Posts: 583
Joined: Tue Jan 06, 2015 3:24 pm
Location: Hoquiam, WA


Return to CNC Shark

Who is online

Users browsing this forum: No registered users and 1 guest