arc output in post

[Bill]

We have a brand new POS Hurco which is replacing the older POS Hurco.

 

Anyhow, they same the same post I have will work on this one, but I was writing a quick contour test program on an arc. In the cont defs I have it set to output quadrants arcs in XY and filter in the program parameters to an arc.

 

The post has quadrants and seems like it should work BUT the code comes out point to point. No G2 or G3 anywhere.

 

Am I missing something?

 

Thanks for any help

[Slepydremr]

are you using arc check?

code:

---

arccheck    : 1     #Check for small arcs, convert to linear

atol : .01 #Angularity tolerance for arccheck = 2

ltol : .002 #Length tolerance for arccheck = 1

---

if so, what are your tolerances set at?

[Bill]

Let me check on that.

[Bill]

I do not see that in the post at all.

[Bill]

I am getting a G17 call out in my gcode. But that's in between countless points.

[Nathan G. Baldwin]

Bill,

If yer using Mcam X, check your control def under "arc" and look for the break options. the questions sleepy's referring to above were replaced in X posts by the control def options.

 

HTH.

[Bill]

Ok Nathan. Will check there.

 

Thanks guys BRB

[Slepydremr]

Oops, My bad.. I guess you did say in your control def up above... for some reason id didn't click that you're using X. Sorry for the bad info. I haven't gone to X yet, still waiting for MR1.

[Bill]

I have looked through the control def and I can find that anywhere.

 

Under the arc page in Cont Defs I have break options.

 

Support arcs XY, XZ, YZ

arc center type all set to absolute

break at quadrants

Arc error check = length of arc

= parallel axis motion on quadrant

=end point check (round endpoint-break on failure

 

I left a message at my reseller for some help but no reply yet.

[Nathan G. Baldwin]

Bill,

which post and machine def are you using?

[Post dept]

Billh,

 

Something is linearizing the arcs. It's either your post or Mastercam. Check the nci file, are they linear moves or arc moves? Another way to check is to check the value of the variable linarc. If it's 1 then the post is linearizing the arcs.

 

Also, check to make sure your toolpath has the arc filter turned on.

 

Brett

[Nathan G. Baldwin]

Right on brett! I was racking my brain trying to find the concversion to arcs.

 

Bill,

You'll be looking for linarc$, should be in the pinit section of the post.

[Bill]

Will check on that now. Left early yesterday.

 

Thanks for the suggestion guys.

[Bill]

linarc$=1

 

That's what it says.

[Bill]

It worked. Changed it to =0

 

Nathan and Brett thank you.

[Nathan G. Baldwin]

Woo Hoo!

[CarbonCAD]

I get this error. What is up with the 10201?

 

CONTROL DEFINITION - - Post variable 'arccheck$' was re-initialized from 1. to 10201.

 

This is what is in the post:

arccheck$ : 1 #Check for small arcs, convert to linear

[Robert Bernobic from CNC Software]

The Arc page in control def sets the value of arccheck$. The message is telling you that your post is trying to set a different value. The CD options will blow away the value in your post, so Mastercam is warning you. Go to the Arc page in your CD and make sure the options are set correctly.

 

HTH,

Robert