Cutting deep grooves in copper

[MSL]

Hi,

 I'm having hard time cutting some deep grooves in a part. The material is OFHC copper. All internal surfaces have 16 finish and profile tolerance of .001.

I do not have any problem with the finished called out, but no matter what I do, the .04 walls move. I have cut lots of copper before but I can not come up with a solution for these deep grooves. I'm trying to cut this part on our CNC lathe using custom made carbide ID grooving tool.

Please see attached picture. Anyone out there have made similar parts before? I will appreciate any help or comment.

 

 

[jeff]

What if you cut the grooves incrementally? Meaning depth cut passes for each groove until they are all at the same depth?

.02 deep on each groove

repeat until at depth.

[Matthew Hajicek - Singularity]

Yep, just like milling thin walls; you take a shallow cut on each side of each wall, then go a little deeper on them all, then a little deeper etc.

[MSL]

Here are test cuts I did.

1: Roughed all grooves left .004 per side and then finished it. (Used .100 wide ID grooving tool).

2: Roughed all grooves left .001 per side and then finished it. (Used .100 wide ID grooving tool).

3: Roughed and finished each groove. (Used .07 wide ID grooving tool).

4: Roughed and finished all grooves by stepping down .05 each time to reach the final depth. (Used .07 wide ID grooving tool).

5: Used .114 wide tool to plunged in one shot. (Tool was same size as grooves width. Used cutting oil).

6: Machined every other groove then filled out the machined grooves with Cerro- shield.

[taperlength]

I would consider roughing all grooves and then having it stress relieved before finishing.

[cnc22]

You Could try roughing and then try finishing the walls with a tool that cuts both sides at the same time. Look at Thin Bit.

[Matthew Hajicek - Singularity]

Another thought; try a super sharp cobalt steel tool.  Carbide always has a little edge radius which may be pushing.

[taperlength]

Another idea:  check your custom made tools on an optical comparator.  I have tools made before that had the wrong angles.

[MSL]

Check for clearance angles?

[taperlength]

Check for clearance angles?

Yes.  

[crazy^millman]

.001 profile on a CNC lathe in copper? I would give one in a 100 parts before you make a good one. The one way I would even think this is possible is to make supporting internal groove fixtures with .005/.010 dovetails to hold each one in place and work your way out from the inside. I would leave the ID for last and I would pack each groove with a undersized spreader to stabilize the .04 walls even if I was grinding the ID and not turning it. The tooling alone for the project would take me 80 to 100 hours to make and there would be 16 individual custom made rings cut in half after I made a split down the center the gap closed and then tapped every 10 degrees for #2-56 set screw to go in each hole. Sorry, but the material you are putting in there is not gripping the walls and you need something to grip that tall of a wall why I said use a .005 or .01 tall dovetail the #2-56 all set and done correctly should helps stabilize everything from the beginning to the end. Then you have another set like the 1st set that sit inside of each groove allowing enough room for a .001 or .002 edge break chamfer or radius if no sharp corners are required so you can then try to machine the ID. I would grind or get close and lap the ID in. Once all done remove all the hardware and pray nothing moves. Might even think about like other said do a normalize process. You have .0005 tolerance on everything and I don't know the coefficient of thermal expansion, but have to assume at every peck and every cut you are blasting the part to keep it's temperature stable and you are using a stabilizing process to keep the coolant a constant temperature.

 

Not sure who you made mad. I thought I seen some hard parts before, but that one is top 5 in my life. Goes right along with the 40 foot beams for a Robot out of 1018 engineer wanted us to hold .001 flatness and size on for the whole 40 foot. After I quoted them $100,000,000 they gave us .001 per foot.       

[Machineguy]

Done this before. Old style

Rough, heat treat, finish with .001-.003 cut pass an every groove face. Repeat till done.

It take time to do this. Feed is slow, you don't want string chips.

Heavy metal bore bar also.

 

Thin bit may work. You will need clearance on the sides of the tool so it wont rub.

We made custom tools for this job.

 

For you guys that don't know what this is I'll let the post starter say if he is allowed.

 

Its not as easy as it looks.

 

Machineguy

 

Try one 12" deep!!

[Rocketmachinist]

PHHH easy it's a death ray nozzle.

[MSL]

Hi guys,

 Thank you for the input. I made some shims to fill the grooves to support the thin walls. I will cut one groove at a time and use my shims to support the walls. I made some very big similar parts before out of Aluminum but this is a tough one. I will post out the result. This is part of deep space network.