[sundy58]

I am milling stainless for the first time on my TM-2. I need to buy some tooling and need advice.

These are the parts I'm milling.

I have turned my spindle up to 6000RPM.

I use Feature CAM and I'm working from Inventor files.

I am open to ideas on work holding and cutting methods because I need to learn!

[Geof]

I don't have any holding or cutting suggestions (yet), but I do have a comment on the design; how good is your relationship with the research people you work with?

It seems the design calls for a groove to be milled along the edge of a piece flat bar with a big notch in one piece. This is as opposed to fabricating it from three pieces of flat bar bolted together.

If you take stainless flat bar and machine it along one edge like this it is almost certain to warp; it may warp a considerable amount. This is because when the bar is rolled tensile and compressive stresses are introduced into different regions of the bar and when it is machined these stresses are relieved unevenly.

If you have a good relationship with the researchers you may be able to get them to do some experimenting by just machining along the edge of a sample of the bar to see how much it moves; or you may be able to get them to understand that if the part comes out all bent after you have machined it, it is not your fault.

[sundy58]

That is one of my concerns. I mentioned doing the three part thing but then it would 'need' to be welded.

It's going under the wing of a Twin Otter and needs to take the stress. I don't have a lot of time because the thing has to machined assembled and welded by May 19th.

I never get enough time to work out the process. I just try to apply lessons learned as I go along.

I am thinking that I would hold the bar flat and use a side mill. I guess that is as bad as anything else!

[gregben]

re: Top_Bar and Front_Back_Edge_Support (didn't look at last part)

This can easily be welded using TIG. The trick is to drill a few holes in the
outer pieces and "plug" weld. These parts obviously don't have to look pretty,
just strong and functional.

[sundy58]

Excellent suggestion.

I will try that if milling the slot doesn't work out.

Anybody know where to find carbide tipped side mills that are small enogh to do a .230 slot?

[gregben]

I'd just use a 3/16" end mill or, for a bit more strength a 5mm one.

Don't cut too meekly though; SS work hardens (but 304 isn't bad) so it is better to cut it fairly aggressively.

[sundy58]

Wouldn't you worry about the end mill wandering? I have had bad luck trying to put a long slot or groove into material with an end mill.

Just my experience which is not extensive.

[sundy58]

I'm looking at a slitting saw on Iwentool's website part # EF53-012.

I will need a good arbor also. More toys!

'made in USA' tools actually made in USA? Any good?

Who is the guy I read about who makes CAT 40 tool holders? I would love to buy from small business's.

[gregben]

No, it is almost always better to:

A) Use a smaller tool than the slot so you can climb mill all the way around.
B) Use multiple Z-level passes so you don't deflect the tool too much on any given pass.

For a slot like this I would do something like Z depth of 1/16" to 1/8" per pass.

If your machine isn't very rigid you might have to conventional mill instead of climb milling.

Other approaches to this problem include using a slitting saw and making a
series of closely-spaced drilled holes to remove the bulk of the material.

[sundy58]

I don't know how rigid a TM-2 is. Seems rigid when I lean on it! Probably much less so when milling stainless.

If I do shallow Z cuts don't I run the risk of work hardening the material?

The first pass is always climb right? If I work down to my desired Z then I can start milling the sides but until I get that first slot for clearance...

[sundy58]

Goin' to a barbecue cook off and will get back to this later.

Need to kill off the weak brain cells.

The liver is evil! It must be abused!

[gregben]

Have a good BBQ!

I took a look at your machine on the Haas web site. You definitely
can do climb milling! I didn't pay any attention to what your machine was earlier. If it was a 1950's manual Bridgeport type machine it would be a different story (unless the machine had been rebuilt).

Yes, the 304SS will work harden a bit, but the thing is to avoid very low feeds and speeds resulting in localized heating. Use plenty of coolant, and TiN coated solid carbide cutters and you should be fine.

[GaryCorlew]

I am doing some parts very similar to this, The parts I am doing in SS have a groove .625 wide and .875 deep I am doing them in one pass with a disk mill from seco tools. It only takes 4 hp. My machine is just a little bigger than yours, Its a VF11. After using one of these the first time a few days ago I would not do it any other way, Its amazing watching the chips pile up as fast as they do!!

[sundy58]

Good news for me is that our aeronautical engineers came down on the laminate three pieces instead of mill out one piece. I couldn't get the EE's to listen to me but they will listen to another engineer... sometimes!

I'm not sure we will even weld these now. AE's have some bonding process and I can't wait to see it.

Thanks for the help. I'll post some pictures along the way.

I like those disk mills. I might have to get one.

[Kool Parts]

Who is the guy I read about who makes CAT 40 tool holders? I would love to buy from small business's.

Not sure who you read about but Marti is the guy you want to get your tooling from. He makes them right there in house. Smart guy, ask him about tooling problems. He may know a way that you haven't thought of

http://www.maritool.com/