3D Milling Surface Finish Problem

[TurboME]

I'm doing some 3D surfacing on 1018 steel and am getting a bad surface finish. See attached picture. I understand there will be step over marks but I'm not happy with the pitting.

I'm doing a rough cut with a 1/2" end mill, .4" step over, .01" surface offset.

The finish cut is with a 1/2" 2 flute carbide ball mill, 15.4 ipm, 2567 rpm.

Any recommendations? Should I lower the step over on the rough cut?

[jkeyser14]

What's the stepover you have the ball end mill set for?

[JPMach]

What type of holder is the finish mill in, setscrew or collet? I would try making the finish pass all one direction instead of zigzag. I usually get a torn finish like that when 3-d milling when the tool is not climb milling. You get a nice line one direction but then on the way back it goes to hell.

Also what is the stepover fo the finish mill? Is it solid carbide? For the .010" skin you have left you must remember that when a ball mill cuts only that deep the actual cutting diameter is very small. There for the RPM can go quite a bit higher.

Out of curiosity, what is the part you are cutting? It almost looks like a anvil horn.

JP

[TurboME]

Thanks for the tips, I'll try a one direction cut next time.

The step over on the finish is .0275" (.0005 scallop height)

The tool is being held in a collet holder and is solid carbide.

The part is a die for flaring steel tubing on a press.

I used the speeds and feeds recommended by the tool manufacturer for a DOC of .1" (.2xD) and .25 WOC (.5xD).

Is there a good formula or guideline to adjust the speed and feed for a lighter cut?

[RICHARD ZASTROW]

TurboME.
You might try contacting A.S. Thomas Inc. I worked with them on milling gummy stainless steel turbine blades. They had designed and patented an indexable carbide insert tool that had geometry built in to act almost like a wiper. 63-32 Rms finish & no tears or rips in the surface. They are in MA. www.asthomas.com

[ViperTX]

Seems to me that you're trying to cut a taper and the result that you're getting seems acceptable.....just think about what the profile of the end mill looks like......you need to look at another scheme for cutting the taper....I would think a lathe would give you a much better finish.

[Joey]

The problem with ball nose cutters is twofold.
The cutting edge geometry at the bottom of ball does not give much room for swarf clearance and more importantly the speed of rotation is virtually zero at the bottom of ball. In effect you`re pushing the material rather than cutting it.

Wherever possible its far better to either tip the head over or clamp the job at an angle to cut further up the flute of the ball nose.
Either way you`ll have to datum the job through use of a tooling ball mounted on the job. But this extra setup time far outweighs trying to hand finish the part.

[RICHARD ZASTROW]

Joey, The cutter mentioned in #5 eliminates that problem, it is not a ball end mill. Also, you might Google "sturz milling" and "P-6". It might give you a different idea.

[jason.davis05]

What machine and software are you using?

The two 1/2 cutters your using will do just fine, you just need to change the step over, step down, rpm, and feed. You may also need to look at how your getting the chip out of the cut, but from the look of your part that shouldn't be a big problem.

[todd71]

Doesn't look that bad. Most 3d stuff will require some "hand finishing" to blend away the step overs if your looking to get smooth surface. Hand finishing is an "art" that is under appreciated in most shops.

[jason.davis05]

Originally Posted by todd71 Most 3d stuff will require some "hand finishing" to blend away the step overs if your looking to get smooth surface.

Wrong answer!! 3D can be cut to require NO hand finishing.

It all depends on the CAM software, cutter used, and machine. The required RMS will also affect the ability to finish the part at the machine, but I have successfully cut to 6 RMS on my V56 Makino and I cut to 10 RMS on a regular basis. Handwork is an “art” but also a necessary evil, we will never fully get rid of it but the need is for it is reducing every year.

I don’t mean to bash anyone, but just because it isn’t done in your shop doesn’t mean it can’t be done.

[blowmebigtime]

I agree with jason's previous post,, we polish and hand fit NOTHING when making our plastic injection molds, unless of course they need a diamond finish on a show surface. The accuracy and finish off of todays high speed milling machines is remarkable. Looking at the picture the first thing that comes to mind is that the conventional move your making is killing your finish,, I would only climb mill even if you have more rapid and lifts, tool life will be much longer,, finish will be much greater and size will be more accurate.. also more rpm's. This is a picture I personally programmed and cut from start to finish on a high speed 5 axis machine,, it is a core for an engine cover mold which required NO hand fitting of the shutoffs and NO polishing.