Smoothing finish passes

[Dan_AKA_ROY]

Hello, all. Being new to the CNC industry, I do things using intuitive common sense. Are there better ways to accomplish the same task at hand? Undoubtibly, there must certainly be!

Here's my next task. The bosses want the surface finish on our molds to be "smooth as a baby's bottom" - the least amount of handwork to be required and in the fastest time possible.

We have a 3 axis router with a 3.5HP spindle. Router bits can cut deeper and faster when housed in a more powerful spindle, as most of you in this forum already know. Typically, router spindle horsepowers range from 10-20 HP, 15 HP being quite enough to blast through aluminum with an attitude. But our spindle is a puny 3.5HP.

When roughing, I gotta go with very slow speeds. Finishes can go faster, but not as much as I'd like. Here's what I do to obtain that really smooth surface finish. I run the finish passes at .05 stepover at a slower feed. After the finish passes are done, I set the stepover to .005 and rerun the finish passes at a much higher feed - like around 200-400 ipm. This technique works well, but is there a better way? Tolerance settings? Filtering settings? Cutting methods- which are limited in surface toolpaths? Is stepover the only way to obtain smooth as silk finishes?

[Trevor Bailey]

Sometimes I will leave at least a few thousands for the final pass and I will change direction of the cut path.

[Dan_AKA_ROY]

Hi Trever. Thanks for the tip. Cut direction? As in the 'direction' button in the 'surface parameters' tab? This will change the direction of cut, resulting in a smoother finish? [if so, I learn something new from this wonderful forum everyday!] Could you clarify for me that this direction button would yield a smoother finish? Forgive my ignorance, and thanks for your help.

[Trevor Bailey]

Direction is like a lead in/out for surfacing toolpaths or you can control how much above the actual part you want to start feeding, etc...

 

The direction change depends on what toolpath you are using. WHich one are you using for your last two passes?

[Dan_AKA_ROY]

I'm utilizing four different finish toolpaths, each pass run separately. A finish parallel, finish steep parallel, finish shallow, and a finish flowline. Is this overkill? I'm wondering if the finish shallow cut is necessary?

[Trevor Bailey]

You maay need all of them. It all depends on your geometry. Since you are using so many to finish with, changing the cut direction is not needed. However, for your knowledge, look on the 3rd tab of the surfacing toolpath for something like "machining angle". ( More specifically - see parallel toolpath )

 

You may also want to check out the finish-project-BLEND toolpath. It is pretty nice. It would be better if you could keep a constant scallop height, but who's dreaming .

[Dan_AKA_ROY]

I'm machining a surfaced part with a contoured slope. Project blend toolpath sounds interesting. I'll have to experiment with that toolpath. Oh, and the machining angle parameter -I'll have to see how that affect the finish, as well.

[Rick Damiani]

You might also want to look at Finsih|Scalop, Finish|Leftover, and Finish|Pencil.

 

Finish Scalop spirals around the part while adjusting the stepover to maintain a constant scalop height.

 

Finish Leftover lets you use a larger mill for most of the part, coming back with a smaller mill (or several smaller mills, as appropriate) to pick up leftover material.

 

Finish Pencil will take a mill and run it along surface intersections.

[Dan_AKA_ROY]

Thanks for the valuable maching tips, Trever and Rick! I've never tried finish scallops before. I'll have to look into it. Rick, your description of finish leftover passes has given me an idea on how to speed up machining.

The books I've read and online help descibe HOW TO run these toolpaths; however, I need ideas about 'the applications' of these toolpaths. Ultimately experience will further my development. When I have a specific problem at hand, the aid of this forum is an invaluable resource! I'm tinkering with the finish project blend toolpath. I use it for engraving purposes, but now realize I can do a lot more with it.

[Trevor Bailey]

Try this:

 

1) Surface-rough-pocket - Rough out cavity

2) surface finish parallel - one direction

3) Surface finish parallel - change direction

4) Surface finish scallop - final machining depending on smallest corners, you may need to use a couple of Rick's suggestions.

 

Good Luck

[Chris Rizzo]

Hey Dan,

 

Which books have you found motst helpful for surface toolpaths? We are in need of some good info here.

thanks

[Trevor Bailey]

cmr, check out MC Handbook V2.

[Dan_AKA_ROY]

Hey,cmr. I'm purchasing the MC Handbook vol. II today, in fact. It is highly recommended by the good folks here in the forum. I like the Mill Training Tutorial book by In House Solutions which can be purchased on this website. Master the Coons surfacing technique. Powerful stuff.