Okuma Cadet OSP5020L programming arc

I’m new to lathe programming. I am trying to program a pretty simple radius on a 1.0x.625 diameter spacer. The radius is 1.6” and starts .1 in from face and ends .1 was back of part.

I have searched YouTube and googled, but I don’t find anything that seems to be relevant to this control. There is a lot of talk programming with the Radius method. But as I have read you have more control with I and K.



I’m not understanding how to figure the math for G2/G3’s, and using I and K.

I tried to copy what my cam software spits out and only use the G2 line. It almost works as expected trying to drop that line into my lap cycle. But it comes up and goes back for the .1 off the back of the face and it’s undersize .005 as shown in the image below.



I told my cam software to output G42 but do not calculate tool compensation.

Below is the complete post from the cam software, but I was only using the G2 line.


The turning segment of code in my program within the lap cycle shown below

Again, I’m a complete noob with programming at the control on a lathe. And I’ve never uploaded a post into my lathe from any cam software. I’ve been trying to learn how to program by hand. But I lack experience.

Thank you for any help I appreciate it.

I and K are the distance and direction from the start of your arc to the center of your arc.
In your example the K(Z component) is .4 to the left of your starting Z of -.1312.
The I (X component) is 1.5492 above your starting X of .625.

Neither one of these values matches your print, but it's close and can cut an arc with the data provided.
The ending X of the arc you programmed is .620. Then you feed back to Z-1.031 up to x.625 and back to Z-1.125.
That's why you have a step. It's doing what is programmed.

The correct code would be:
G1 Z-.135
G2 Z-.927 I1.5495 K-.365
G1 Z-1.125

Or you could forget about comping in the computer, use tool tip 8 and program directly from the print:
G42 G1 Z-.1
G2 Z-.9 I1.5495 K-.4
G1 Z-1.125

I’m not sure what you mean tool tip 8. Are you referring to Tool Code, or Form Code for that tool in Tool Data?

I tried your code this is what simulation produces. It’s showing an undercut when it should just go straight back.

I don't know why it would be undercutting like that, I'd have to see the code.
I guess it would be the form code on the data page. I have OSP U10L control so I'm not familiar with yours.

Here is what I got, and the code for the turning.

Try getting rid of the last X.625 and Z-1.125 lines. That might fix the undercut. The tool tip should be on the offset page. Mine has X offset, Z offset, TNR for X, TNR for Z and Tool Tip No.

That tool data page is just for the graphics.

Try using the interactive grapgic function IGF on the machine to program

clayton said:

Here is what I got, and the code for the turning.

Click to expand...

This is on a new okuma but should work for u

That NO114 line is what u r lookin for must be written just like that

Drew@acms said:

That NO114 line is what u r lookin for must be written just like that

Click to expand...

Just this morning I finally wrapped my head around it. And this is what I have now. To me it seems correct, and the part measures correct. I am using cutter comp, shows when I face up the part, do a small chamfer and go back to start the arc.

Why is your code just slightly different?

Not for sure it may b a parameter i used the igf function

Drew@acms said:

Not for sure it may b a parameter i used the igf function

Click to expand...

Ahh! I haven’t used IGF yet. That seems like a whole other learning curve. However everyone says you don’t need cam software for complex geometry when using IGF. I don’t know if that’s 100% true or not. But it won’t hurt that I understand the fundamentals of G Code and the cycles as I learn them in the Okuma. Then I can step into IGF.

I really appreciate everyone’s help with this. Between reading through documentation and seeing the examples you all have posted helped the light bulb go off.

Again thank you!