Restrictor Machining

[FryGuy]

I know ive seen teams with aluminum restrictors but i can't machine one with any type of presicion. Ive done one out of machinable wax already, but when i switched to aluminum i got a horrible surface finish. The boring bar seems to be vibrating quite a bit but i cant shorten the length of it at all or i won't be able to reach the throat of the restrictor with it. Anyone have any suggestions or tricks for maching the restrictor?

[FryGuy]

I know ive seen teams with aluminum restrictors but i can't machine one with any type of presicion. Ive done one out of machinable wax already, but when i switched to aluminum i got a horrible surface finish. The boring bar seems to be vibrating quite a bit but i cant shorten the length of it at all or i won't be able to reach the throat of the restrictor with it. Anyone have any suggestions or tricks for maching the restrictor?

[repeatoffender]

get someone else to do it?

[drivetrainUW-Platt]

We have run aluminum ones in the past...from what I have heard, it took forever to make, very small cuts to keep deflection of the boring bar to a minimum.
You would almost have to have it cnc'd unless you dont care about the profile and have a few days to sit at a lathe.

[FryGuy]

Well i am cncing it, but i still have the problem with vibration and deflection in the boring bar. We have made aluminum ones in the past but they were all two piece with a flange so the boring bar length and deflection wasnt much of an issue. I am trying to make this one one piece.

[drivetrainUW-Platt]

ours were 1 piece but I know they had to make a few sets to get it as close to the desired restrictor dia at the throat.

[billywight]

http://img443.imageshack.us/img443/8246/nochatterku7.jpg

Make a reinforced boring bar. This cut is about 6.5 inches deep with no chatter at all. The boring bar only has about .030" clearance throughout the cut - you need to model up the restrictor and the boring bar to get it as stiff as possible. Adding some rubber o-rings helps out as well, and of course get your speeds and feeds right.

[Jersey Tom]

Try using a carbide boring bar. Use the absolute thickest one you can, make sure your insert is sharp, etc. Run light DOCs, try running really low RPMs (200-300).

[VFR750R]

It might sound half-assed, but get close with tooling and then use sand paper on the lathe to get your last few thou. Surface finish comes out great and as long as you keep checking your throat you can get very close to size.

[FryGuy]

That reinforced bar looks like it would work pretty well. I assume you made the taper before going boring all the way through. I was running rubber bands on it to try to dampen some of the vibration out but it didnt help much. Did you drill holes through the boring bar then to mount that sleeve? I'll have to talk that one through with the shop boss before i try that one.

[billywight]

I stepped into the part before making the finish passes. I took off about .050" in diameter per pass and ran at about 1200RPM. Can't remember the feed off the top of my head, but it was pretty quick.

It's a 5/8" boring bar with a carbide insert. The bar has some areas ground out for clearance and the reinforcement is a piece of 1.5" diameter stainless that was lying around the shop. It's reamed to the OD of the boring bar. The boring bar is held in place by set screws (no holed were drilled in the boring bar).

[Dave_Dal]

This issue is a classic workpiece/tool stiffnes problem. If you really want to get your feeds and speeds right you have to calculate the oriented transfer function of the tool (because it is the part that is flexing) and use the results to find your resonant frequency. From there you can calculate the speeds to stay away from in order to reduce the chance of hitting resonance and calculate the depths of cut to limit chatter.

Also, don't forget that taking very small depths of cut can be counter productive because of the tool stiffness. There is a limit to how fine you can cut before you essentially start wasting your time. This is called boring copy error, if you wanted to look it up.

And finally, does anyone use a CNC mill with a ball nose end mill to machine their restrictors? That should be stiffer and produce satisfactory surface finishes. However, you would most likely have to make the restrictor in two parts unless you are very careful with your tooling setup.

[Chris Allbee]

for simplicity's sake i would try to follow jersey tom's advice. Like others have mentioned there is a limit to how light a depth of cut you can take so keep that in mind, but slowing down the RPMs REALLY make a difference. We machined aluminum antiroll bars last year to a final diameter of a little less than 1/2 inch and about 12 inches long. Nasty chatter was a problem at any RPM above 150. Don't be afraid to slow it down and be patient with it. this should help you get a pretty good finish and you can always hone it in with fine sand paper.

[Bill Kunst]

Like Mike fom P-ville said, we ended up taking two tries at it because the first one was so bad. The person machining it didn't bother to try different feeds/speeds despite the resonance that was shaking campus foundations. It seems to do more damage to surface finish (1/8" gouges spiraling through the body of the restrictor) then simple chatter.
Bill

[rjwoods77]

There is published feeds and speeds for this kind of stuff. I would spend a little more time on your tooling,setup and education instead of just going straight for the cut. I can program conversational and get cam software to write code but i havent the foggiest on speeds and feeds. That is a mixture of science and art. I would ask a real machinist of tooling supplier before just flying off and making something.

[Bill Kunst]

The feeds and speeds are going to be dynamic, especially on the cone shaps or any other profile where the diameter is changing, as the sfm will change throughout if the rpm is left the same. This is the very difficult part of this and why you cannot just set a generic rate for any aspect of it. Sort of tricky, and that is why a good machinist makes big money. I am sure there are guys who have so much experience that they could do it first try just by listening to the machine and playing with the dials as it goes.