Tolerances For 3 d toolpaths

[ctyler]

We have a couple older Okuma 4va milling machines and a newer Okuma MB56. We are building blow mold cavities, so we do a lot of 3d milling. We are having a lot of tolerancing issues since going over to X7 that we did not have before in previous versions because we could suppress the refine toolpath option, which I don't believe you can do anymore. I know this option is supposed to give you a better surface finish, but we had issues where are older Okuma's would not run these programs, but if you suppressed it and use the regular tolerancing it was fine. We do not have this issue if we can finish in our MB56, but we usually cannot do that because of other projects. When running in these older machines we are running them through an Okuma DNCB off of the computer and I guess as these programs get larger it has problems reading far enough ahead. Problems we are having are cutter stopping while in a cut then going again causing gigs in the part and also tool not running close to the federate it is programmed too. Seems this option cannot be suppressed anymore I would love to get some feedback on some parameters to try or any other options that would be helpful. I am sure we are not the only ones who have had this issue and I would really like to learn to use this refine toolpath.

 

Thanks,

Clay

[Aaron Eberhard]

Clay - If the problem is too many points, try using the toolpath filter set to "minimize points." Running an arc filter is always preferred as well. That should give you a file size way smaller than the previous, unfiltered, results.

[Glenn Bouman]

Unfortunately just turning on the arc filter, sets the ratio of cut tolerance 95% to filter tolerance 5% which will not give you very effective arc filtering.

Set the Cut tolerance to 30% and you will get much better results.

 

The settings in X6 were easier for customers to understand "Short, Normal, Long/ Good Better Best"

[Peter - Avivi CNC Solutions]

We are building blow mold cavities

Glass containers? My favorite...

 

If you use Parallel Finish or similar toolpathes often, I also suggest to use arc filter strongly and not only in XY plane.

I used on XZ and YZ planes also with lot of success on this kind of moulds and older machines.

But in this case I would use I-J-K on arc moves, instead of R.

Your older Okumas has OSP5000 control?