Turning an .011 thick flange.

[BenK]

I need to turn a flange on a part that is .011 thick any ideas? The part is 3.00" dia. with a counter bore feature (2.2") with a hole in the center (1.6"dia.) the bottom face of the counter bore is the .011" thick flange. Material is hardened 4130 steel 38-42 Rc.

[K2csq7]

100, 100, GO!

 

Maybe get one face done & fill it with something (cerrolow), then turn the other side???

[BenK]

Also I need to make 30 parts.

[Del.]

I would leave it thicker on that side and stick it to a magnetic holder and wire edm off the rest of thickness. I don't see how you could turn or grind an area that thin.

[Goldorak]

program it like a thin wall in milling

 

finish it .025 step by .025 step on each side with a grooving tool to prevent warp

 

we make 2inch od by 1in id by .02 thk washer from inconel like this ant it works like a charm

[BenK]

I would leave it thicker on that side and stick it to a magnetic holder and wire edm off the rest of thickness. I don't see how you could turn or grind an area that thin.

 

 

We don't have an EDM. They want to do it all on the lathe.

[Del.]

We don't have an EDM. They want to do it all on the lathe.

 

 

Could you make like a solid plug to go into it when you face the back side off. I wonder what the purpose of such a thin section is for and how long it would hold up. Thump it with your finger and it would bend it i would think.

[K2csq7]

program it like a thin wall in milling

 

finish it .025 step by .025 step on each side with a grooving tool to prevent warp

 

we make 2inch od by 1in id by .02 thk washer from inconel like this ant it works like a charm

 

Inco is much stronger.

 

.011 in alloy steel is like .003 in Inco, IMO of course...

[Mr. M]

I've done it where you have the back side up against a shoulder or boss to do the second side down to .007 in CRS. Can you put up a picture?

[BenK]

I can't post pictures of the part, I will have to draw something up that I can show.

[BenK]

Here is the turn profile of the part.

 

 

 

 

 

[K2csq7]

Looks like your going to have to make a nice fixture to support one (finished) side of the flange, while you turn the other.

We use stuff called "Zap A Gap", (like super glue) you could use that to glue the finished side to the fixture to prevent it from lifting up on you while you finish the 2nd side.

You can get some Zap a Gap remover spray to get rid of it when machining is done.

 

:edit:

I don't think they make the remover I spoke of.

[GoetzInd]

I would do the ID side first then hold it on the id with pie jaws that went all the way to the bottom of the c'bore. Then use a insert with large corner rad. to face the other side to keep cutting pressure on the support. Done some thin parts that way but not that thin.

 

Mike

[Guest CNC Apps Guy 1]

Pinch Turn it.. (ID/OD))

[Mr. M]

I would do the ID side first then hold it on the id with pie jaws that went all the way to the bottom of the c'bore. Then use a insert with large corner rad. to face the other side to keep cutting pressure on the support.

 

Yup, this is what I've done, and for the final pass taking a .030+ pass from center out might be the ticket

[JAMMAN]

I would do the ID side first then hold it on the id with pie jaws that went all the way to the bottom of the c'bore. Then use a insert with large corner rad. to face the other side to keep cutting pressure on the support. Done some thin parts that way but not that thin.

 

Mike

 

 

Exactly what I was thinking, pie jaws are awesome. I really don't think you need a large radius tool though, you would have to make a deliberate effort to not push it against the jaws.

[chris m]

I don't see how you could turn or grind an area that thin

 

We do it all day long

 

I would suggest a collet (like a Dunham arbor, or an expanding 5C soft collet) in the ID to finish

[Larry1958]

Had a part simular to that. Used an expansion arbor (homemade out of brass). Make it the 2.2" o.d. and long enough to bottom out on c'bore face.

[BenK]

I cut the first side and the 2.2 bore is out of round by .001 (I have .0005 tolerance), I cut a setup part out of some hot rolled and the center was round within .0001. I'm wondering how much the part is going to move when I cut the other side. I'm thinking I will need to rough the part out complete then come back and finish.

[chris m]

Depends on what shape the bore is; if it is a figure eight, then roughing first will help, if it is a triangle, then roughing isn't going to do much for you. That being said, roughing first is often a smart play; you may also consider stress relieving the blanks of you have in-house heat treating capability.

[BenK]

I'm having a hard time getting this to be flat within .003 each part is coming out different.

[K2csq7]

Taper in one direction just a varying amount or completely random.... Do you have a pic/screenshot of the workholding you decided on?

[BenK]

It is random. My work holding is mandrel we made in house that holds on the ID and against the back of the .011 surface.

[Del.]

I would imagine if you can't have some type of radius in the corner of the ID bore, that is where the problem comes from. Its probably even slightly thinner there from tool pressure. Just my opinion.

[K2csq7]

How thick is the flange before your finishing op?Once the part is in your fixture and tightened up can you verify there is no distortion coming from how your holding it?

 

Del maybe onto something, if the radius on the other side varies slightly as you go around the ID, it would cause a "random" condition as you describe. How did you cut that? Did you use a dwell to ensure a consistent radius all around?