Need Help!- MX3 G code

[chipcrazy]

hello everybody,I have a question about how can you change the way mastercam generate the g code for circular motion G2 And G3 I have been getting the code broken in two sections of 180 degree and thou there is nothing wrong with the final result, in this case is my boss who just does not like it that way since he is the one who actually does the set up I need to learn how to change this

G41 D3 X-.0262
G3 X.0262 R.0262
X-.0262 R.0262
G1 G40 X0.

to only one line for the 360 arc

G1 Z-.1667 F5.
G41 D3 X-.0262
G3 X.-0262 R.0262
G1 G40 X0.
Z-.3333

thank you for your help.

[Superman]

We agree that ther is nothing wrong with this code

G41 D3 X-.0262
G3 X.0262 R.0262
X-.0262 R.0262
G1 G40 X0.

on some machines, this code is wrong
full arcs require I J output ( sometimes a R- for arcs larger than 180 deg. )

G1 Z-.1667 F5.
G41 D3 X-.0262
G3 X.-0262 R.0262 ( I.0262 J0. )
G1 G40 X0.

It is in your interest to find out if your machine is capable of doing full arcs at a higher feedrate, breaking it into 2 segments helps to create a more quality job. Having multiple points on a toolpath, the machine will check its positioning before going on to the next block of code.

Let him know, that if it looks a neater code, is not neccessarily correct code
before changing, have him prove that the machine will hold it's accuracy


To allow full arcs, open your Machine Definition file and, under "arcs", turn ON " Allow Full Arcs"

[Mike Mattera]

Somehow telling the boss to "prove" the benefit may not be the best thing to do if this guy wants to keep his job. The boss says do it. I don't think it's going to make any difference in the machining. Most likely he's concerned about smaller programs that are easier to edit at the machine.

To Change it... Go To....
Settings - Control Def.
Select "Arc" from the left side.
In the dialog on the right, under "Arc Breaks - XY Plane" check....
Allow 360 degree arcs and set Arc Break Point to "Dont Break Arcs".

I wouldn't bother to change it for YZ and ZX arcs. It's probably pretty rare that you ever do them.

That should fix you up.

Mike Mattera

[Superman]

Originally Posted by Mike Mattera Somehow telling the boss to "prove" the benefit may not be the best thing to do if this guy wants to keep his job. The boss says do it.

Defining arcs with IJK as opposed to R is a contentious issue.
In this and other forums

Using IJK will give only (1) solution to a radius
Now, using R there can be (2) solutions, some machines have shown that position checking is not maintained thru the entire cut, features tend to be rounded

Yes, R is easier to read, alter and so on, but if you want accuracy IJK is the only way to go.

I have surfaced parts using both, and the IJK outputs leave the other for dead in respect of quality

As I said, let him physically and scientifically "PROVE" that R output will maintain quality on his machine. Do a test, interpolate 2 circles side by side-fast, (1) using R and the other IJ-and break circle into (2). Also do a surfacing test say a wave form ( 1" rads pitched 1" apart, fillet 3/4" and machine with a 1/2" ball ).