Hello Guest it is January 18, 2020, 05:37:11 PM

Author Topic: Help!!!!!  (Read 7148 times)

0 Members and 1 Guest are viewing this topic.

Offline TT350

*
  •  113 113
    • View Profile
Re: Help!!!!!
« Reply #10 on: April 01, 2008, 12:52:07 PM »
It's the X that's out.

I put a edge finder on the part to see if the X was still good
and found it to be out over an inch.
Re: Help!!!!!
« Reply #11 on: April 01, 2008, 05:18:33 PM »
I just stepped through the hole pocketing in single-blk mode - you can see the toolpath move to the right (with a G03) before each arc is cut. Maybe try slowing down engage-feed in VM. Does it skip steps with aircuts or only when cutting?

Re: Help!!!!!
« Reply #12 on: April 01, 2008, 06:51:10 PM »
I think these are the problem

G03X3.2480Y1.0313I-0.1250J0.0000Q0.1250

it's that part of the path after the helical bit and before the circular cut - seems like it shouldn't look like a straight line. Any chance of a frame grab of the VM toolpath looking down at the hole?

Offline Graham Waterworth

*
  • *
  •  1,933 1,933
  • Yorkshire Dales, England
    • View Profile
Re: Help!!!!!
« Reply #13 on: April 01, 2008, 07:19:52 PM »
G03X3.2480Y1.0313I-0.1250J0.0000 Q0.1250

Mach dose not support the Q command in G03's

You need to amend the post processor to remove the Q's

Graham.
Without engineers the world stops

Offline TT350

*
  •  113 113
    • View Profile
Re: Help!!!!!
« Reply #14 on: April 01, 2008, 09:20:28 PM »
Guys I don't know what I'd do with out !!!!

Offline TT350

*
  •  113 113
    • View Profile
Re: Help!!!!!
« Reply #15 on: April 01, 2008, 09:28:38 PM »
Here ya go

Offline TT350

*
  •  113 113
    • View Profile
Re: Help!!!!!
« Reply #16 on: April 01, 2008, 10:59:43 PM »
Ok guys here's a screen shot of the VM post for spiral interpolation.
You can see the Q that it outputs.
If I select helical interpolation it will output a K

Should I delete the Q command or replace it with somting else?

Now for the helical interpolation is the K output ok or should I do somthing
with it?
« Last Edit: April 01, 2008, 11:02:25 PM by TT350 »
Re: Help!!!!!
« Reply #17 on: April 01, 2008, 11:19:02 PM »
I think you probably need to check "output spiral motions as linear segments" in the machining prefs if Mach can't interpret a G03 with a "Q" in it. It's already doing the helical part of the path as linear segments BTW. 

Offline TT350

*
  •  113 113
    • View Profile
Re: Help!!!!!
« Reply #18 on: April 01, 2008, 11:41:31 PM »
I can edit the post for the Q if needed.

When I cut a circle I wont it to be smooth without the little flats,
so witch one do I leave unchecked?
Re: Help!!!!!
« Reply #19 on: April 02, 2008, 03:01:16 AM »
I don't know if this is useful or not, but in the last control system I had it would make crazy spirals and loops whenever I tried to cut a interpolated hole like what I see you are doing.  I found an option in the old control setup (not Mach 3) to select Fanuc or Bridgeport style arcs when processing G-Codes.  I was using MasterCAM's default post-processor, so in the machine control I selected Fanuc arcs.  Is this related to the Q parameter?
--Scott