OKUMA OSP5020M CUTTER COMP HELP

Please forgive my ignorance, but we are still trying to get the most out of our Okuma MC4VAE with the OSP5020. We haven't had to use the cutter comp until now. I understand the Fanuc cutter comp system but the Okuma is of course different. From what I have gathered using the "Control" compensation option in Mastercam X7 that we have to put the tool radius into the D# at the control. Does the "Wear" compensation option from Mastercam work the same way or would you put the amount needed to shrink the endmill (-.002 for example)? What would be the best way to control the comp at the machine, Control or Wear when using Mastercam. No one in the shop has used OSP controls before, we are a bunch of Fanuc junkies. :)

Quote:

---

Originally Posted by KENNY D

Please forgive my ignorance, but we are still trying to get the most out of our Okuma MC4VAE with the OSP5020. We haven't had to use the cutter comp until now. I understand the Fanuc cutter comp system but the Okuma is of course different. From what I have gathered using the "Control" compensation option in Mastercam X7 that we have to put the tool radius into the D# at the control. Does the "Wear" compensation option from Mastercam work the same way or would you put the amount needed to shrink the endmill (-.002 for example)? What would be the best way to control the comp at the machine, Control or Wear when using Mastercam. No one in the shop has used OSP controls before, we are a bunch of Fanuc junkies. :)

---

Forgiven

Okuma & Fanuc is very similar in the way comp is written
I think you will find Okuma quite comfortable to work with ( in time), & find it is easy to jump from one to the other
- bad thing with the 4VA I worked with, was that it couldn't do a 3 axis move on arcs ( ie. ramp out a hole )

I'll start with the machine
- each offset table # holds 2 numbers, being the H & D fields

Tool length (H) is called up like the Fanuc's G43....but Okuma use G56 in it's place,

The D call-up is the same process as the Fanuc, it is a radial distance. And MUST start / finish with a linear move on the G41/42 & the G40 lines
- normal practice is to use the same offset numbers as the tool number ( I may be stating the obvious, but you never know who may need extra guidance )
- a larger number input will make the tool stay further away from the programmed path
- a smaller number will make the tool profile closer to the programmed path, -ive numbers can make the tool profile on the other side of the path.

Now Mastercam
- there is 4 common methods for compensation
1/ -"In Control" = where the D# is the cutter radius in the control, toolpath output from Mastercam is the profile line that you chained, lead in/out lines & arcs MUST be larger than the tool radius
2/ - "In Computer" = tool centreline path is output, tool used must be as programmed, NO comp codes in NC file for adjustment of the cutting path
3/ - "Wear" = tool centreline path is output, if tool used is same as programmed, then D# is set to zero, +ive number will make tool cut further away from selected chain, -ive number will make tool cut into part area,lead in/out must have linear move greater than the starting offset you place in the D# field, arc & sweep as per your preference......I usually adjust so that tool doesn't descend onto material
4/ - "OFF" = for making tool stay on top of a selected chain ( ie to follow a line drawn for centre of a slot to rough out) ,,,,,& with lead in/out turned off for engraving letters / text etc. No comp codes are output to the NC file

I found that the "Reverse Wear" not suitable for general machining, I think it reverses the +ive / -ive number concept of "wear" compensation, very confusing, so I don't use it at all.

Great, this explains a lot of what we were experiencing with our experimenting. We went with the "in Control" and figured out we had to input the tool radius in the "D" input. I appreciate your response and this info helps greatly.