i have a 4020 cadet with 5020m contoller.. i program everything through mastercam x3. ran the first part and it was a little undersized. went into the controller to do a radius compensation but when i run the program again with the compensation i get "498 cutter radius compensation, no intersecting point 300".. what gives?!!

2. There are a couple of things that would give this alarm.
and it usually happens only on lead ins from CAD generated code

-How the cutter comp is applied ( Control, Computer, Wear )
we use wear, (D comp = zero)- only allows a small amount of offset sometimes ( depends upon the contour )( a comp of -.001mm won't work but -0.05 would )
-Lead in/out --your judgement is required, try a reasonable size arc with 45° or 90° arc sweeps, if using them. 90° is a better angle ( easier to calculate )
Machine side
- open the in-position tolerance up a bit
( not sure of the actual parameter )
I think----NC Optional Parameters ( Long Word) #3--- check the operation manual

If all else fails, change the arc to a line ( don't forget to put the G2/G3 onto the next line if it also is an arc ) ( the I J or R can stay on that line as it would be ignored )

Steve

3. The Okuma cutter comp doesn't like to be lied to, since it always checks to see if a tool can fit between the current vector and the next vector. So for that reason, anytime I use comp, I tell the truth and use the actual tool radius, so for a 1/2" tool, use .25 in the comp register. Superman's method will also work, but as he states, small numbers can cause problems.

Since the control checks tool fit, you will need to be at least greater than the radius away from the start point with your approach point.

Alas we haven't been able to get Okuma to provide a parameter that will allow the tool check to be turned off, so your best bet with a CAD system is to NOT use cutter comp on your roughing tools, and let the CAD system figure out the path. Then use cutter comp on any tight finishing tools that you believe you will need to compensate. Using actual tool radius values seems to generate less errors for me.

The truth shall set you free (from errors)!

4. that's common problem with CAM (? mistakenly named as CAD here ?) software, especially with Master CAM. If You would install proper Okuma compiler.
stop at problematic line (block) number
single block mode.
green button, feederate ... untill I have error message. Then look at present coordinates and distance to travel.
Generally, it's simple.

#### Posting Permissions

We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!