Please Help, surface finish contour trouble.

[DDLES]

Please Help.

Mastercam will not machine the center of a drive surface. I'm using surface finish contour but I can't get mastercam to machine the center of the drive surfaces.

Any help would be greatly appreciated.

[Superman]

Surface Finish Contour may be the wrong strategy to actually finish that form.
This operation works well for "hogging" the material away from the part but still leaves a lot of uncut areas. You may be better to try a different operation that keeps the tool in contact with you part longer and not "waste time" finishing areas that would need more finishing later.

IMO, try Surface Finish Flowline on the "hump" or cut it when in the left view with a 2D contour using the side of the endmill

[Matt Berube]

You need to use Surface Finish Contour (with "remove cuts from shallow areas" selected) and then also make a "Surface Finish Shallow" operation to clean up the shallow areas.

There is also an option in Surface Finish Contour to "add cuts to shallow areas" but it doesn't usually get everything you need... The first method I described is the way to go.

A few more details about this strategy here... (post #30 on page 3) http://www.cnczone.com/forums/showth...t=88105&page=3

[DDLES]

Thanks for all the help. I couldn’t have done it without you guys.

I tried both of the methods suggested and ended up going to the Surface Finish Parallel, which is just about the same as Surface Finish Flowline but you have more options and Check Surfaces and Containment Chains. And I ended up needed the containment to get a good surface finish.

Thanks again for the help.

[ObrienDave]

What you really need to understand is what different toolpath functions actually do.

Without getting into the differences between the Rough and Finish details, basically, Contour slices the geometry in the XY plane with constant depths in Z.
This results in large steps when the surfaces approach being parallel to the XZ plane.

Parallel, on the other hand, slices geometry parallel to the Z axis at any rotated angle.
This results in large steps when the surfaces approach being parallel to the rotational angle you are using to create the cut.

Flowline is best used for a single surface.
Before anyone flames me, yes, I know flowline will do multiple surfaces.
But, my experience is the resulting toolpath is based on which direction the surface was created.
Kind of difficult to control which direction it cuts if the surfaces are not consistant.

There are other methods that would have worked nicely for what you are trying to cut.

I've said it before, and I'll say it again.
You take 50 different programmers, and you will get 50 different ways to do the same thing.