Mastercam arc toolpath problems

[hesstool]

I'm sure there is an easy fix to this, but for the life of me I can't find it. I've been using OneCNC for years but I am now using MC X5.

When calculating an arc for the toolpath, MC seems to take the radius and move it to the opposite side of the toolpath start point. I first thought it was a problem in our Acramatic 2100e post, but it shows up in the HAAS and Fanuc posts as well making me think it's something in MC. Is there some absolute/incramental toggle I'm missing?

Here is a simple 2" dia. circle I just cooked up for a visual. Instead of an I,J value of I0., J0., you can see it has an I value of -1.! Why is this happening?

Here's the example in Acramatic 2100e:

;PROGRAM NAME = T;
;06-10-11 TIME =10:22;
; 1/2 BALL ENDMILL TOOL - 2 DIA. - .5;
:T2 M6
N100 G00 G90 X1. Y0. S1069 M03
N110 Z.1
N120 G01 Z-.005 F6.42
N130 G03 I-1. J0.
N140 G00 Z.1
N150 M05
N160 G28 P1
N180 G98.1 X10. Y20.
N200 M02

 

[SeymourDumore]

Unless I'm misunderstanding your question, that code looks correct.

First, it moves to X1. Y0
Then plunges down to Z-.01
Then it makes a full 1" radius circle CCW and ends up once again in X1. Y0
Then it comes out to Z.1

At the first move of G01 X1. Y0, the center of the arc is in fact -1. away, hence the I-1..
Remember, at least on the Haas and Fanuc, the I and J is incremental.
You would see an I0 J0 only if the control needs absolute arc centers.

 

[DMF_TomB]

i and j incremental

i and j incremental from arc beginning or from arc end depending on post processor used.
.
for example a Prototrak the arc is incrementally referenced from arc end
.
this is different from RS274D or RS274NGC (extremely close to Fanuc)
3 Input: the RS274/NGC Language

 

[hesstool]

Remember, at least on the Haas and Fanuc, the I and J is incremental.
You would see an I0 J0 only if the control needs absolute arc centers.

And I think that's one of my issues. The same code will run just fine on a Haas, but will not work on our Cincinnati. Anytime the machine encounters an arc it alarms out giving a warning about arc endpoints being out of tolerance.

One other thing. I can post this program to the Cincinnati Acramatic 2100e on my seat of MC and it will be bogus, yet when another user logs on and constructs and posts this, it works just fine with the arc center being at I0., J0.. Same seat of MC, same post processor, but different results...

Here is the same simple program but constructed and posted by a different user logged on to the same seat of MC:

;PROGRAM NAME = T;
;06-10-11 TIME =11:30;
; 1/2 BALL ENDMILL TOOL - 2 DIA. - .5;
:T2 M6
N10 G00 G90 X1. Y0. S1069 M03
N20 Z.1
N30 G01 Z-.05 F6.42
N40 G03 X-1. I0. J0.
N50 X1. I0. J0.
N60 G00 Z.1
N70 M05
N80 G28 P1
N100 G98.1 X10. Y20.
N120 M02

 

[superrat]

we ran into this on our old sundstrand, if you go under settings- control definition manager -arc and chose the arc center type you want, that will change the output of the i, j. the thing i'm not completely clear on is how and where it is saved? since it does not actually change the post. maybe it's associative?

hope that helps

 

[kevkess]

Break arc circles

The Cincinnati control prefers to have a circle broken into 180 segments. Use Mastercam to break arc circles and it will output two lines of code for the G03 just like you show in your second example.

 

[hesstool]

we ran into this on our old sundstrand, if you go under settings- control definition manager -arc and chose the arc center type you want, that will change the output of the i, j. the thing i'm not completely clear on is how and where it is saved? since it does not actually change the post. maybe it's associative?

hope that helps

Helps?! That was the Golden Ticket!!

A million thanks!

 

[superrat]

nice!
i've spent quite a bit of time tuning in the post/control definition to work with this sundstrand. she's a 1981 model and is finicky at best in how she likes her code. glad it worked.