[Spinnetti]

I'm struggling to not get chatter on a long piece I'm trying to machine. Its made from 1.25 x .5 x 9" 6061 rectangle, and is machined on all sides. I'm using two vises and holding it fully on both ends, and cutting a taper over the full length where its deepest at the ends and shallow in the middle. I'm getting hit or miss results with a lot of chatter. I've tried deep cuts, shallow ones, fast and slow (using G-wizard, plus experimenting).... Any ideas on how better to fixture it?

[txcncman]

Use oversize stock on the thickness (1.5"?) and mill as needed then flip and mill off excess using toe clamps or special soft jaws extra long with the part profile milled into them.

[neilw20]

Through the center hole bolt a large chunk of steel on the back, and machine the front.
Pause and put the chunk on the front now.
or EMBED it in a great big chunk of ice, might work.

[SCzEngrgGroup]

What you've got there is pretty much a tuning fork, and chatter is inevitable. You need to figure out a way to support the middle MUCH better. You could make a fixture to support the back while you machine the front and vice-versa. Or put a bolt through the middle, and a block underneath, so you can clamp the middle to the table for support. Even 1" thick stock will vibrate a lot once you go beyond a couple of inches of overhang.

Regards,
Ray L.

[Steve Seebold]

You could eliminate the chatter if you used the right feed and speed and the correct cutter.

Discribe your cutters to us. It might not be the part that is chattering. It could be the cutter. If a cutter is too sharp and/or too long, it will sing like a canary.
Another way is to machine one side complete, then clean up that side and pack it with clay.

There is some stuff you can get from McMaster. I'm not sure what the actual name it, it's some kind of clay, but the industry name is bear shyt (the y is really an i). If you call them and ask for it, most of their people will know exactly what you're talking about.

The part I see does not look that difficult to machine.

[mrquacker]

Bear ****? Really?

[LRF]

We called it Whale **** and bear describes it to. I looked in McMaster and can't find it, its been awhile since I even had a thought about it.

On the part, there is a center hole with 2 intersecting holes, are they tapped? If yes then fit a rod into the hole and use set screws to clamp to it. Now clamp the other end in a v block and then clamp dont the V block. Do one side then the other.
The tuning fork analogy is probably your issue which then gets the cutter vibrating, the deeper you go the worst it gets.
Anyway just my opinion.

[nitewatchman]

Duct Seal.

[MichaelHenry]

Would it makes sense to rotate the part 90° and mill one side with a 3D toolpath? That way you could the vises closer (or use long soft jaws) together to support more of the work. That might take a lot longer and need some clean up if surface finish is important.

Mike

[dertsap]

get a small rubber strip for under the part , and make yourself some small screw jacks to place snug along the bottom of the part and out of the way of the cutter (not too tight or you will shift the part) . Put an m0 before you do a finish cut , then add your jacks . This will help by absorbing the vibration as well as support the unsupported area . the rubber probably isn't necessary but may or may not help , every situation is different . I'd also try conventional milling


.

[Spinnetti]

Thanks for all the tips and ideas. I think the jack idea might be the most feasible. I can't bolt through the holes because the cutter passes over them. The cross holes are only #50, so don't want to damage those, though I suppose I could finish tapping those and put a 1/2" steel bar through and another holder... hmm.

Interesting thing is, sometimes the cut is great, most of the time not. What I was doing is profiling the edges 90 degrees to this cut first which removes a lot of mass (but cut great at 5100rpm and 20ipm, .2doc full slot), so I'm going to try doing this cut first which leaves a lot more stock in place, then cut the other profiles. If that doesn't do it, I'll add jacks. I also just ordered some better cutters. I was using a HSS 1/2" cutter of standard length, but ordered coated high helix aluminum cutters and will try 3/8 instead. I was using "conservative" setting (one off minimum) in gwizard. I tried .2doc at a time, and full depth with shallow cuts etc..

PS, was going to do 3d toolpaths originally, but don't have the software for it... using HSMexpress which is 2d. Hmmm.. just tried "trace" which seems to do it, but would I use a ball end cutter for that or would a flat one work?

[SCzEngrgGroup]

A smaller cutter will make things worse, not better, as it will be MUCH more flexible. You want to use the largest diameter you can. A variable helix endmill will also help fight chatter, as it doesn't induce as much vibration at a single frequency.

Regards,
Ray L.

[TXFred]

You cut away a lot of material underneath your part in a previous op. Next time, leave that material in place, and mill the profile of the part. The excess material can be held in vise jaws, and the part won't want to chatter.

For the last op, flip the part and hold it some custom made soft jaws, and mill away the material underneath, which will now be on top. With the part held in a vise, chatter will once again be a non-issue.



Frederic

[BAMCNC.COM]

I say go with over size stock, cut your part flat, flip over and cut the excess off.

[dertsap]

I was using "conservative" setting (one off minimum) in gwizard.

I hate these calculators !
A high helix is a good choice because they can still leave a good finish when run at above average chip loads . One thing that works well on walls and the likes where chatter is an issue , is to leave a minimal amount for clean up but not too minimal so that the tool doesn't have any load (use roughly .01-.02 but lean more toward .02) , then run the finish cutter at full flute depth across with a high feed rate at lets say .01-.012/ tooth , and theres still plenty of room for more feed (just in case), generally you'll end up pushing the tool beyond what the recommended chip load would be , but this is the point of leaving a minimal amount to cut . As stated previously , I'll conventional mill when things get really ugly


.

[Spinnetti]

A smaller cutter will make things worse, not better, as it will be MUCH more flexible. You want to use the largest diameter you can. A variable helix endmill will also help fight chatter, as it doesn't induce as much vibration at a single frequency.

Regards,
Ray L.

Well, my cuts are very light... the stock is only 1.250x.5 to start with... my cheap no-name Chinese .250 HSS coated cutter just mows through it with no problem... accidently pushed it to 40ipm/full slot/.2doc) and it worked for a while There should be little deflection with carbide at the cuts I'm doing per gwhiz... A good variable helix coated 1/2" end mill is expensive too! This is just a hobby for me, so its kinda hard to shell out lots of tooling that I'll no doubt jack up as I come up to speed.... Hopefully this hobby will pay for itself in a couple years!

[Spinnetti]

I hate these calculators !
A high helix is a good choice because they can still leave a good finish when run at above average chip loads . One thing that works well on walls and the likes where chatter is an issue , is to leave a minimal amount for clean up but not too minimal so that the tool doesn't have any load (use roughly .01-.02 but lean more toward .02) , then run the finish cutter at full flute depth across with a high feed rate at lets say .01-.012/ tooth , and theres still plenty of room for more feed (just in case), generally you'll end up pushing the tool beyond what the recommended chip load would be , but this is the point of leaving a minimal amount to cut . As stated previously , I'll conventional mill when things get really ugly


.

Well, I don't know enough yet to pick my own numbers... I did exactly what you said though.... final full depth pass with .020 at 5100/20ipm if I remember right... tried lots of different finish pass speeds and feeds, down to 3000 rpm and 10ipm... sometimes it worked, some times it didn't.... seemed to depend on how well it bit in on the first lead in..... I also tried it both climb and conventional.. didn't seem to matter much.

I got the part reprogrammed trying to do "3d" with a flat cutter... we'll see what happens. My parts are mostly scrap anyway, so won't hurt to try on one of the existing ones.

Key I suppose is a better cutter and some sort of mass to stabilize it. Based on part design, the deepest cuts are at the ends anyway, and that part works fine... once it gets 1.5" or so away from the chuck, it starts singing...

[dertsap]

at 5100/20ipm if I remember right...

What I'm talking about is pushing it to .012-.02/ tooth on the finish pass , which at 5100rpm then the feed would be roughly 120 ipm for a 2 flt mill .
If the mill can't run that high of a feed then drop the rpm to accommodate .
Something that I forgot to mention is that it would be easy to add a hold down clamp over the screw jack . Add the jack and a clamp on one side then cut the other side , have an m0 , flip the clamp then do the other side . This is handy when doing a few parts but not too efficient when in production mode


.

[Spinnetti]

What I'm talking about is pushing it to .012-.02/ tooth on the finish pass , which at 5100rpm then the feed would be roughly 120 ipm for a 2 flt mill .
If the mill can't run that high of a feed then drop the rpm to accommodate .
Something that I forgot to mention is that it would be easy to add a hold down clamp over the screw jack . Add the jack and a clamp on one side then cut the other side , have an m0 , flip the clamp then do the other side . This is handy when doing a few parts but not too efficient when in production mode


.

The stuff I do is a few at a time, not production work, so a bit of overhead beats expensive fixturing.... Back to the shop to try out some of these ideas... where do I get little screw jacks?

[Steve Seebold]

How about something simple like a 123 block and an adjustable parallel.

Put the 123 block in any way it will fit, then slide the adjustable parallel in until it's snug and then put a clamp over the top of the part.

SEE? Simple.