Weird toolpath behaviour

Hi all,

I had the most unusual thing happen when machining a component on the weekend. The last operation on this job was to run around and cut some chamfers, on one of the end profiles the cutter simply turned off the intended path and through he job!! Watching it back with both back plotting, and verification on Mastercam, all seemed normal. I've never seen this before, I changed the starting point, some small changes to the profile, still the same. It wasn't until I split the large arc into two pieces that it worked normally. This has really spooked me now, any body seen anything like this before?



This the first time I've attached a pic, so hopefully it worked. It shows the profile, as the tool reached the large arc, it ignored it and ran through to other side of profile

This sounds like a machine tool control issue. Some machines must have arc commands broken up to work properly. Others can't do arcs in certain run modes. What kind of control is driving the machine?

It's a GSK, basically a Chinese Fanuc knock off, it's had no problems in the last couple of months I've been using it, doing much more elaborate profiles than that one,

Check to see (with air cutting) if it misbehaves with circles bigger than 180° or bigger than 180° and less than 360°
(You might find that you actually do that very rarely.)

Though, it would appear you machined the profile before you chamfered it, no? What does that code look like?

I'll have to check that, I've definitely done many contours at 360 degrees, but more than 180 and less than 360? I'm not so sure. The machining before that operation did not use that profile but a combination of others. I am not that familiar with G code as I've spent 20 years on heidenhain

There are settings in Mastercam control definition that controls how arcs are generated. Like the others said, it might be an issue with full/half/partial arcs that is the problem. You can set up arcs as IJK or R, also you can say if you want to break arcs at quadrants or not, a couple other things might be in there too for you to play with...

Looks like you're right about the arcs, I was able to replicate the problem today, and splitting the arcs fixed it. I'm going to have to look through the control definition to see if I can find a solution, as it happen again today when cutting a pocket, with a circular island inside the pocket

Mike1974 said:

There are settings in Mastercam control definition that controls how arcs are generated. Like the others said, it might be an issue with full/half/partial arcs that is the problem. You can set up arcs as IJK or R, also you can say if you want to break arcs at quadrants or not, a couple other things might be in there too for you to play with...

Click to expand...

Any idea where abouts in the control definition?

MarioRicci said:

Any idea where abouts in the control definition?

Click to expand...

In the control definition, cilck on ARC on the left side

Late to the party, sorry. Sounds like you found your solution! We used to see some behaviors like yours on our old controls but would run fine on our newer machines. Our MC programmers said the paths looked fine in their simulation but the old machines would do a huge sweeping arc right through the part, lol. At the time we had Vericut which could see the weird moves because we simulated the actual nc file and were able to simulate the specific control inside of vericut which was super helpful. Sometimes the weird moves were caused by large arc segments and other times as a result of bad models from customers. Still, sometimes other post configurations can cause issues such as short segments of extremely large or small arcs which could be less than the resolution of your control. In my posts I now have upper and lower arc limits set so when the cutter path goes outside the limits it will output linear moves just to be safe.

So for us the behavior came down to:
Large nc arc segments sometimes confused older controls.
Those same large nc arcs ran fine in our newer controls.
Bad nc arc moves were sometimes executed by our old controls.
Bad nc arc moves would alarm out on our newer controls.

Mtndew said:

In the control definition, cilck on ARC on the left side

Click to expand...

Thanks again for the advice, I changed the arc setting to quadrants, and that seems to have sorted it out