Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: TT350 on March 29, 2008, 12:55:45 AM
-
This is some weird stuff guys, After this was cut I checked my X/Y position and found that my X was out over an inch.
This sould been a round hole. I was cutting this on my Tormach.
Take a look at the code and see if any thing is wrong.
Chris
-
What did you use to create the code and the drawing?
The code is very long for such a simple job.
Graham.
-
Visual mill 5.0
-
I cut a part about 6 mouths ago where it cut an arc and the arc was made up of lots of little flats.
I called the guys at VM and they told my where to make changes so VM would cut the arcs smooth with out the segments.
With this selection made VM outputs the I&J’s for hole pocketing.
-
Normally you would output without any options ticked, then you should get a single line of code for each move down in Z.
E.g.
G03 I-.25 Z-.05
G03 I-.25 Z-.10
Etc.
Graham.
-
The hole is 1.0 why is the I-.25?
Chris
-
is it skipping steps in one axis in the G00's? If you turn off "use rapids" in the feedrate dialog in VM it'll do G01's at the selected feedrate instead. Have you checked your motor tuning to make sure it can still run at top speed in that axis?
-
Yes it is skipping steps.
After it cut what you see in the board I checked the X Y zero
and the X was way out, over an inch.
Chris
-
I don't think there's any G00's in the Hole pockting code.
-
Is the X DRO out as well or is it just the axis?
-
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.
-
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?
-
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?
-
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.
-
Guys I don't know what I'd do with out !!!!
-
Here ya go
-
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?
-
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.
-
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?
-
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?
-
leave "output arcs as linear motions" UNCHECKED then the circular part of the hole will be smooth - it's just the spiral lead-in that'll end up as line segments - but with CV on Mach will interpolate a smooth curve anyway. VM wants to make a spiral move with an R3 with a Q, if you take the Q out you'll just get an arc (not a spiral) which is almost certainly not what VM wants the toolpath to look like.
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?
-
I deleted the Q from the post with no luck, it cut the hole the same.
I left the liner motions unchecked and put check marks in the other 2
and it cut a nice hole.
Thanks to all that responded to help me resolve this.
Chris