[snapman]

Hi there,

I have been an avid reader of this forum for a few months now. I have not had a need to post a question since most were already covered here but now I am at a loss.

I have been machining a part from 6061 aluminum and 360 brass. The 6061 pieces turn out pretty nice and as expected. The brass however, seems to bend or curl up a little at the ends. What could be causing this? I don't know if I can post pictures yet so I will give the details best I can:

- Minitech MiniMill 1 with Sherline spindle and high speed pully
- 3 flute carbide endmill with a...high helix for cutting non-ferrous metals
- No coolant or lubrication but I do have air blowing the chips out of the way
- Cuts are .01 deep and step over .0625.
- This is simple pocketing- with three pockets- each one a bit smaller in size.
- 10,000 rpm at 18 ipm
- The piece is tightly clamped in a fixture.
- The piece measures 1.75 x .75 x .093 with two posts extending up to .1875 on each end when finished. I start with a piece of brass 2 x .1875.
- I think I am machining the piece with the long dimensions the same direction of the grain of the metal (if that is possible, I don't even know if metal really has a grain and how to machine it)
- OneCNC Pro (amazing stuff) for CAD/CAM but I doubt that matters a bit. Unless you guys tell me to do some crazy custom coding because then it won't matter what I am using- I will be screwed!

Apologies for the lenght of this! I just would like to say that all of you have already taught me a bunch of stuff and I really appreciate this community. This is such a great forum- especially for the clueless like myself. Please have mercy on a newbie!

[Mcgyver]

Speed and feed seems high, then again I don’t know the dia of the cutter.

you will get distortion and bending when you machine off the surface of any rolled metal, the outer layer is where all the stresses are concentrated from rolling. There’s some info that will help, http://www.cnczone.com/forums/showthread.php?t=9425 except you can’s stress relieve brass without annealing it and soft brass is really soft and gummy

Brass should be pleasure to work with - most alloys I’ve used cut very nicely. two tricks, 1) only use a new cutter, once its used on steel (or AL?) its not much good for brass - that goes for end mills to files 2) brass should have a rake angle of zero. I have separate sets of drills and lathe tools for brass - all with zero rake, but there's not much you can do about the end mills. I've always just used a sharp hss end mill (in which case your cutting speed will be more like 200-300 fpm).

[snapman]

You know, I looked on here about 3 dozen different ways to find something like that post...guess it would help if I knew proper terminology...

Anyways, that helps explain a lot. I am using 1/8th inch end mills. I will keep them separated from now on- for brass and aluminum. I am going to try starting with thicker stock and shaving off the top layers to see if that helps. For prototypes this was not a big deal- just sanded the crap out of the tops and everything was fine- but it looks like we may be doing the production (with a bigger mill) and therefore I would like to get it straight to begin with. (Pun intended). Better yet I may post an RFQ on here for having it cast in zinc or something. Thanks for the response!

[DareBee]

Exactly like the other thread states it is your small thickness and amount of material machined off of 1 side.
If you could weld or press your pins in or design some ribs to run the length of the part you should be OK.
IMO the redesign is the best fix.
You could also make a straightening fixture and press them back into shape. This is ok if this is a bracket that will conform to it's own shape when istalled, but is no good at all if this is a stand alone precision part.

[cadman]

Don't know what your tool diameter is but the speed seems high and feed too slow.

I used to machine a lot of 360 brass, especially bar. We had them double disc ground and they would be straight, but after some milling and drilling they would curl like potato chips. I would just take a rubber mallet and lightly tap them into shape.

For most brass parts I would plan separate finish operations to minimize warping.

You can stress relieve brass but it will still warp slightly when machined afterwards. You can have plate flattened, which is basically clamping the plate in a fixture and heating then cooling before releasing from the fixture.