Cutter comp restriction

[So not a Guru]

I need to restrict our cutter comp to a linear move. Our Mazaks do not allow cutter comp to be set on a circular interpolation move (G41 or G42 on these machines). Does anyone know how I can create this restriction in our post? This is our Cutter comp section of the post:

 

pccdia          #Cutter Compensation
      #Force Dxx#   
      if prv_cc_pos$ <> cc_pos$ & cc_pos$, prv_tloffno$ = c9k
      sccomp
      if cc_pos$, tloffno$
      !cc_pos$

 

Zeke

[htm01]

that's set in control def

[Myth Project]

that's set in control def

htm01, the box isn't checked on my system and it will still place cutter comp cancel on arc movements...  

[So not a Guru]

htm01, the box isn't checked on my system and it will still place cutter comp cancel on arc movements...  

Same here, I had already looked to see if this could be set in control def, but my box is unchecked & my post still outputs comp on G2s & G3s.

[htm01]

I don't know then, I have never run into a machine that will do cc on arcs

[Myth Project]

So not a Guru,

 

What kind of feature are you having trouble with?  Mine is usually on a helix bore, it'll cancel on the arc exit.

[So not a Guru]

So not a Guru,

 

What kind of feature are you having trouble with?  Mine is usually on a helix bore, it'll cancel on the arc exit.

I have trouble with helix bores & 2D contours.

[Myth Project]

On the helix bores, if you have a perpendicular entry checked it won't have an issue with the start of the cutter comp.  The only way I know to fix it at the end is hand edit.  Or, you could use a ramp contour in place of the helix bore and as long as your lead in lead out isn't too big you won't have an issue. Same should prove true for 2D contours.  As long as you have ample space for the lead in and lead out, you shouldn't have it placing cutter comp values on arcs.

[So not a Guru]

I fixed this by removing pccdia, from my pcirout section.

[ahaslam]

One quick thought about this, If you remove the pccdia command from your arc move wont that remove your cc entirely, and doesn't that make the whole thing meaning less?

 

I only ask because I am having the same issue and tried to delete my cc from the arc line and then force cc in the next line but it never came.

[jlw™]

I program for nothing but mazaks, 3 to 6 axis.

 

Don't mess with your post, handle this in the tool path. For helix bore, do perpendicular entry.

 

For 2d contours do perpendicular and you can still put a radius on it and it will work. Make sure your lead in is enough to absorb cc on and off.

[ahaslam]

Okay then, I will keep that in mind, thank you.

[gcode]

On the helix bores, if you have a perpendicular entry checked it won't have an issue with the start of the cutter comp.  The only way I know to fix it at the end is hand edit.  Or, you could use a ramp contour in place of the helix bore and as long as your lead in lead out isn't too big you won't have an issue. Same should prove true for 2D contours.  As long as you have ample space for the lead in and lead out, you shouldn't have it placing cutter comp values on arcs.

helix cutter comp setting

start at center

change arc on from 180 degrees to 90 degrees

 

you'll get at straight line from the center followed by an arc into the cut

[jlw™]

That's exactly how I do it.

 

Start at center and arc on set to 90 also works.

[gcode]

That's exactly how I do it.

 

Start at center and arc on set to 90 also works.

tablet key pad fail

I posted 0, I meant to post 90

[jlw™]

Also, threadmill will work, just trick the tool. Had to do that in visualmill all the time, works in mcam too but the helix bore and contour ramp work in mcam so no need.

[civiceg]

 

 

I have trouble with helix bores & 2D contours.

 

Trick I learned on here for using 2d contour. 

 

(hole diameter-endmill diameter)/2 x .4142= both length and radius

use a 135 degree entry angle and select tangent

 

Puts the tool in the center of the hole and has a nice straight lead in/out for cc before arcing onto the chain. 

[civiceg]

I have been using more of the point toolpaths because of the start at center ease. But if I am interpolating a bore or oval with a minimal difference between endmill size and feature, the above method is my go to for finishing.