Help on G68

[cammac]

Hello

 

There is one problem with posting G68 code. We have fadal VMC center. It is possible to use G68 in control. But:

fadal manual said that "All X and Y (or X, Z or Y,Z or X,Y, and Z) positions are required for linear moves, even if they are zero or non-motion moves"

I had try use mpfadal2.pst and mpfan.pst, which is including in Mastercam 9. But rezult was bad - there is lines with only one X or Y move.

Is this MC or post processor problem?

Can it be solved?

 

Thanks

[perfecseal mankato]

Our company used to do alot of rotation (G68)

and we had no problem with the rotation, but inserted it by editing. All our machines our fadals.

All our programming is done from the center of the part.

I would insert the G68 as follows:

 

G0 X0 Y0 E1 (program origin = center of part)

G68 R0+90. X0 Y0 ( angle & rotation point)

Z1.H1M8

 

this would then be followed by the normal program.

One problem is an arc in the G18 or G19 plane cannot be done.

As having to have all axis positions in every line

I never did this, and never had a problem.

Do not output arcs in the G18 or G19 plane.

Never did try to output the G68 in the post so I do not know if this works right or not.

In version 9sp1 I just use the transform function,

it works very well.

[Allan Brown]

You can force X and Y output on all lines by calling pfxout and pfyout in place of pxout and pyout in plinout and pcirout. Or modify pxout and pyout to force xabs and yabs output. Contact your reseller to have these changes made in the post.

[Thad]

There are a few things that the Fadal manual says that don't really have to be done. That is one of them. Just add it in manually (or modify your post) and you're all set.

 

Thad

[cammac]

Thanks for all!

 

To mancarto.

 

If you had no problem on it I hope I am too. I will try rotation very soon.

I use Mastercam v9.0 If I use transform to rotate coordinates, use method coordinate and check subprogram, post can output G68. Manualy you just need put G69.

 

To member #2

 

Your advice work fine!