3D machining strategies

[Diedesigner]

Hi all,

I have little experience in 3D machining, so I would like ask permission to tap into the knowledge base here. This is my first real attempt at 3D machining, so please forgive my many questions.

 

I am machining soft A2 tool steel for a draw die boss which will produce a shape similar to the flip-up part of a cell phone, so it has relatively shallow surfaces across most of its shape blending into steep surfaces at the edges. The piece will be hardened after milling.

 

I roughed it out with an inserted end mill using planar cuts, semi-finished it with a coated 1/2 carbide ball end mill using a parallel zig-zag tool path, and I finished it with an SGS Zcarb Tialn coated 5mm ball em, also running a parallel zig-zag tool path, at a 45 deg toolpath angle.

 

The roughing and semi-finishing ops left about .020" stock.

I ran the SGS ball end mill at 6000 rpm (which is the maximum for my machine) and 20.0" feed for the finishing passes, with the maximum step over set at .005" (slightly less than .0002" maximum scallop height). The "tolerance" was set at .001

 

The finish is not bad, but it shows a "checkerboard" pattern when you look at it against the light, and it seems to have some shallow (less than .001) grooves across the flatter portion of the surfaces. These "grooves" are in the same direction the finish passes ran.

 

-- Do you have any input as to which strategies are best for "fine-finish" finishing? How much "tolerance" should I specify? I would like to achieve as close to "mirror" finish as I can, to minimize polishing.

 

-- Would I be better off hard-milling the finish passes after heat-treat? Can you recommend how much stock to leave & speeds/feeds?

 

-- Am I on the right track, or can any of you make some suggestions which may provide superior results?

 

 

Thanks for your time with this. As always, any help is greatly appreciated.

 

Regards,

 

Chris

[Allan]

The .02" might be a little heavy for the finish cut. Crank the tolerance up. If I was shooting for a .0002" scallop I'd want the tolerance half that .0001" Parallel is not always the best cut method it depends on the geometry. I dont have any experience with hard milling, but you should be able to get the finish your after while it's soft.

 

HTH

 

Allan

[Nominal]

My 2 cents. If I understand correctly you are milling at 20ipm with a ball end mill over some sculpted surface. One thing you can look at is something we used to refer to as data starvation. If you have a zillion little short xyz-xyz moves then depending upon how large the look ahead buffer is on your control the machine may physically arrive at the last location in the buffer before it's replenished. Therefore the machine has to keep momentarily wait for the control to catch up. It may be hard to see but usually there's a bunch of noise and vibration associated with that. Depending upon the shape of the surface and all the other factors it can produce surface anomolies such as you describe. Wait that was more like 4 cents worth. :-)

[Mike Klein]

You might want to try Surface Finish, Scallop for that finish pass. Also remember there are TWO tolerance settings. ONe in Filter and one under you Finish Scallop Parameters. Usually, it's recommended that you set your finish scallop parameter to half of your filter parameter. Try setting your filter tolerance to maybe .0007 and your scallop tolerance to .0003. Adjust your Maximum stepover to give you a desireable scallop height. I run aluminum molds in this fashion and end up with a pretty decent surface that only needs a little touchup polishing. You'll end up with a big old toolpath because everything is pretty much point to point but you might minimize the faceting that you describe.

[P_Scott]

Diedesigner,

 

Welcome to the 3-D toolpath world. Almost all 3-D toolpaths, especially surfacing, will benefit from a Filter setting to reduce the size of the code by replacing all the "zillion little short xyz-xyz moves" with arcs. This also results in a smoother toolpath, producing a finer finish. A general rule of thumb for filtering is to allow the filter tolerance to be twice as large as the cut tolerance. If the cut tolerance is .001", the filter tolerance would be .002". These settings can be found in the "Total tolerance" button on the third tab of all surface operation parameters in Mcam V9. You can also do a search on this forum for Filter topics. JM2C

[Davez]

Here's my .02, I've had good luck hard milling A2, depending on the rockwell. If its going to be in the low 50 rc range, I would suggest leaving .008 - .01 for finishing, and cut it dry. Get some air on the tool if possible, and use a cutter that is made for hard milling, Hanita and Niagra have some good tools, that do great in hard materials. good luck