CDC Sharp Corners

[CarbonCAD]

We have an older machine that interprets cutter comp. differently than the others and maybe someone has dealt with this before. On external corners sharper than 34 deg using g41 or g42 it will error out. On a sharp corner the centerline is projected as a sharp point instead of a radius that would keep the cutter in contact. So we put a small radius about .005" on the geometry corners to keep the cutter in contact. This is quite cumbersome on some parts. Any comments on what else could be tried?

[dolphin1]

might try roll around corners instead of sharp in cutter comp.

[CarbonCAD]

Look like it would help, but I see it can not be in control compensation type to select it. I will look into it, but we use a lot of regrinds with graphite and probably need control compensation type. Am I seeing this correctly?

[Nick Eaton]

There are i fact two different algorithms out there for calculating cutter comp:

1) "Yasnac" method

2) "Fanuc" method

 

I won't bore you with the details.

The only machine I know of which allows you to select which type to use in the control is Hass.

There may be others.

Do you use Comp. in control? Using Wear comp. might help.

You could try running comp. in computer to see if this cures it....this might suggest a fix.....

Cheers

Nick Eaton

[CarbonCAD]

Thank you. Great info about the two types. I will give your suggestions a try. They should work. I just wish there was a way that machine could be used just like the rest by changing something in the post or control def, but if that was the case it probably would have been changed and I wouldn't be asking.

[gcode]

CarbonCad,

Look on cut parameters page of 2D contour

There is a dropdown labeled

"Roll Cutter around corners"

If it is set ot None, Mastercam will output a sharp corner,

If you set is to All or Sharp, the cutter will roll around corners.

Play with this setting a little. It should

help with the problem you're having

[Rocketmachinist]

Cuttercomp Wear will help to solve this problem also. Although you do have to be careful. Under your diameter offsets in your controller the tool diameter has to be set to zero. Mastercam will compensate for the tool dia and put in a g41 g42 to compensate if needed. It's really a nice feature because Mastercam will write the code to curve around all sharp corners and you can still adjust in any direction needed. This also comes in handy when your doing internal bores because you do not need as much lead in to turn cutter comp on. The big thing I have to stress is if your going to use wear make sure everybody in your shop know your going to use it and keep all your diameters zeroed out. Otherwise you are going to get some funky parts.