Need Help!- programming Lathe operation to run on my Mill

[rms2k]

So I want to contour some round bar that I have in my spindle.
I have a 1/16"R cutter held in a vise.
I am having trouble coming up with the G-Code program for the B to C movement. It seems easy, I'm just at a loss.

I have some old software I use and I changed the post to a Lathe.
It gave me this, not even close.

G18
G00 Z-.3075 X0.
G01 F5
Z-.30761 X-.12967
G03 Z.00857 X-.58586 K.22497 I-.09821

I would like to move A to B to C
Any help would be greatly appreciated.

[neilw20]

Try this.
Everywhere,
Swap X and Z
Swap I and K
Make the G03 a G02

and make the tool stick out to the right from your vice as you had drawn it.

[rms2k]

Originally Posted by neilw20 Try this. Everywhere, Swap X and Z Swap I and K Make the G03 a G02 and make the tool stick out to the right from your vice as you had drawn it.

That's exactly what I'm looking for. I will give it a try and post back. Thanks!!!

[sinha_nsit]

Try R-method, instead of center method.

[neilw20]

Nothing wrong with center method.
Emulation worked properly.
Axis was swapped making radii wrong.

[angelw]

Originally Posted by rms2k So I want to contour some round bar that I have in my spindle. I have a 1/16"R cutter held in a vise. I am having trouble coming up with the G-Code program for the B to C movement. It seems easy, I'm just at a loss. I have some old software I use and I changed the post to a Lathe. It gave me this, not even close. G18 G00 Z-.3075 X0. G01 F5 Z-.30761 X-.12967 G03 Z.00857 X-.58586 K.22497 I-.09821 I would like to move A to B to C Any help would be greatly appreciated.

I believe the machining operation is being looked at incorrectly.

Given that the X0,Z0 of the work piece is as shown on the drawing, and making the following assumptions:
1. That if the a command of G00 X0 Z0 would place the center of the cutter radius at the same X0 Z0 point as shown on the drawing. (material removed form the spindle of course)
2. That the cutter is pointing out the right side of the vice as shown on the drawing.
Then:
A. To place the work in the spindle, relative to the tool shown at A in the drawing the command would have to be
G00 X+0.3075 Z0.0

B. To move the work from A to B the command would be
G01 X+0.3076 Z+0.1297

C. To move the work from B to C the command would be
G02 X-0.0086 Z+0.5859 I-2250 K+.0982

Note the change of coordinate sign of the above code compared to that of the program in the Original Post.

The I and K were given as the absolute center position of the radius in the Original Post program. Accordingly, the assumption is that the controls requires the I,J and Ks be designated as absolute center point and not as an incremental value.

Regards,

Bill