cutting negative angle surfaces

[terry5357]

The only way that I've been able to get MC to do undercut or cut a negative angle surgace is by using the rule cut wireframe toolpath. whats the trick to do a multi surface cut of this type.

[jeff]

Have you tried defining the tool so that it has back-taper?

Not sure if that's possible, it's just a thought.

[Fig sign]

http://www.emastercam.com/ubb/ultimatebb.p...7505;p=2#000053

[terry5357]

Isk, you are so far over my head that It don't make sense, but thanks for caring

[Steve Arteman]

Terry

what version?

[Colin Gilchrist]

Terry,

 

You need to use Surface Finish Contour and disable the "gouge checking". Then use the "Direction" button on the Surface Parameters page to get the tool into and out of your undercut area. The only other toolpath that works well in undercuts is Flowline, but you can really only drive a single surface at a time. I have gotten around this using Flowline by remodeling several adjacent surfaces as a single surface.

 

The only toolpath that will work reliably in undercuts on multiple surfaces that I have found is Surface Finish (Or surface rough) Contour. Note that there is absolutely no difference between surface finish contour and surface rough contour, they are the exact same toolpath. Because you have to disable gouge checking, I recommend using the STL compare utility to check your cut stock back to your original model.

 

HTH

 

Colin Gilchrist

The Boeing Company

MR2 and Beta test site

[Fig sign]

Sent me your model in ver9 format ,color specific color the undercuts you wanr to mill

I `l make toolpath for you

 

Sent it to

Winnie(dot)tehPooh(at)gmail(dot)com

[terry5357]

Colin,

Thank you so much. I totally understand what you are saying tried it and worked perfect. Thanks man, and once again Eforum comes through again

All smiles,

Terry

[Colin Gilchrist]

Glad I could help Terry. Doing undercuts took me days of trial and error when I learned how to do it in version 8 and 9. If you use STL compare with WCS, you can do a pretty good job of actually seeing what you are going to cut at the machine.

 

Thanks,

 

Colin Gilchrist

[normand]

Ok everybody seems to get this except for me. Any chance someone could take a look at the file "TEST negative angle" in the X3 folder on the fpt. Any tips would be greatly appreciated.

[TheePres]

Normand,

See negative angle-dan.mcx

I accomplished without turning off gouge check, Note the approach and retract directions.

I have found that even if using a dovetail cutter, define it in MC as a full radius slot cutter that seems to work for me.

[Guest CNC Apps Guy 1]

I also use Flowline Toolpath to undercut - with gouge checking turned off of course.

[Colin Gilchrist]

Flowline works great James, as long as the UV vectors of the set of surfaces are aligned. If not, Mastercam can have a problem with the tool trying to retract at the surface edge, or you get some funky motion.

 

The thing I do like about Flowline (when it works) is that you don't need a containment boundary. Bonus.