Cutter Comp on G2/G3 Error

[RunninWideOpen]

Hello,

I'm still pretty new to mastercam.  I'm trying to use cutter comp on a slot milling operation.  There's no lead-in options in slot milling, and Mastercam keeps turning on cutter comp on a G3, which my Haas will not accept.  How do I get mastercam to turn on cutter comp on a linear move?N

2010 G1 Y-1.124
N2020 G3 X.8881 Y-1.1049 I-.0191 J0.
N2030 G41 D6 X.8691 Y-1.124 I0. J-.0191
N2040 X.8931 Y-1.148 I.024 J0.
N2050 X.9172 Y-1.124 I0. J.024

 

Haas error code is; 340 Cutter Comp Begins With G02/G03

[JParis]

Click the "Perpendicular Entry" box on the cut parameters branch

[RunninWideOpen]

As a workaround, I turned cutter comp off on Slot Milling and added some stock to leave, then I added a Contour to work as a finishing operation with cutter comp turned on.    it put the on a linear move, however cutter comp on/off wiped out the end of my slots.  The slots are suppose to be full-radius.

[RunninWideOpen]

Thank you Jparis.  That worked.  

[Leon82]

Set your default lead in for slot milling to less than 180 degrees. Same for circle Mill. And don't use high speed transitions

[Craig-B]

Plunge after first move, and retract before last move is a good option if you need comp in a tight spot. The comp on/off moves will be outside the slot.

 

[HankStarr]

Hi....In certain examples when I post a program from Mastercam, I will wind up with a line of code to turn on shaper comp that will have a G2 or G3 order on a similar line as G41 or G42. For instance. G3 G41 X0 Y0 F50. Most machine device controls will alert out when perusing such a line of code. Vericut will feel free to run this line of code without giving any blunder messages. This is utilizing the Makpro5 and Hass controls. Is there an approach to arrange vericut to give a blunder message when it incounters the present circumstance so it very well may be revised prior to running the program at the machine and having it caution out and stop?

[Leon82]

11 minutes ago, HankStarr said:

Hi....In certain examples when I post a program from Mastercam, I will wind up with a line of code to turn on shaper comp that will have a G2 or G3 order on a similar line as G41 or G42. For instance. G3 G41 X0 Y0 F50. Most machine device controls will alert out when perusing such a line of code. Vericut will feel free to run this line of code without giving any blunder messages. This is utilizing the Makpro5 and Hass controls. Is there an approach to arrange vericut to give a blunder message when it incounters the present circumstance so it very well may be revised prior to running the program at the machine and having it caution out and stop?

Mp.master checks for comp on arcs and Camplete does as well