toolpath in backplot are arcs, but after post, the nc file are small lines.

[koves]

hello, eveyone one. I need help about post setting or tolerence setting.

 

I created a small test file, the nci toolpath shows that my toolpath are many arcs plus some lines, but after the post, the nc file becomes many lines. I can see this from the G1 X..Y...

 

Do we have a way to tell the post, to post according to the NCI toolpath? I mean don't break NCI arcs to small lines when posting nci toolpath.

 

Many thanks!

[crazy^millman]

What version of Mastercam? If V9 this could be post related? If X then it could be control Def related so know the version will allow someone to help you easier.

 

HTH

[MotorCityMinion]

2d, 3d, surfaces? More info please. Try using the filter for 2d, 3d contours. Same with surfaces. Start with 2:1/.001 tt.

[iowajim62]

Look in your control def, linerize arcs might be the culprit.

[koves]

I am using mastercam x4 version.

when doing surface finish contour and surface finish blend (or some other 3D surface, not test yet).

 

I did dis-tick the option :Present arcs as line segments at the Refine Toolpath. And my NC file do have some of the G2,G3,plus many G1. The only problem is, the post break some of the arcs to small segments, but not all of the arcs. And what I want is no breaking of my arcs.

 

The reason I want my NCI as same as my NC is to control my NC file size and other benifits.

 

Please help me if you can, many think.

[kennebec]

Hello Koves

 

Check your post for Break arc on Quadrants and allow 360 deg arcs.

 

Also I have experienced cutting a contour with fillet size very close to cutter rad (1/2Ø e mill cut a .255R)I turned comp in control on and that was ok until the machinist went to a smaller tool now the tool dives into my .255r and I too have G1 not G2 or 3 and the only way I can see this is in backplot with (Simulate Cutter Comp Off)

[koves]

Hi, Kennebec

 

I tried every combination of the arc setting at the control definition, but it still not work.

 

I believe it is the tolerence setting or somewhere else to make the post break the arcs automaticly. But I don't know where.

[kennebec]

Hello koves

 

Look in your actual pst file for somthing like this it is in General output settings.

 

breakarcs$ : 2 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

arcoutput$ : 1 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

skp_lead_flgs$ : 1 #Do NOT use v9 style contour flags

arctype$ : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

do_full_arc$ : 0 #Allow full circle output? 0=no, 1=yes

helix_arc$ : 2 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

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

 

CAREFULLY TRY ALTERNATE COMBINATIONS

I am NOT a post guy, and others my disagree with my suggestion, PLEASE proceed with caution post changes can have ADVERSE effects.

[koves]

hello, Kennebec

 

I tried your suggestion, but it didn't work.

So I emailed mastercam technical support team and they replied me that my tolerence in CD was too low. After enhanced it, it works as what I want.

Problem fixed, but it cost me more than two days strugging without any clue. I am wondering are there any Mastercam software team guys used to answer the question at this forum?

 

Thank you, Kennebec