Turning stainless disc with taper to knife edge, help with flatness.

I am struggling machining a part, it is a approximately 9" diameter 316 SS disc approximately 5/8" thick with a taper on one face to a knife edge, max allowed rad on sharp od is .003", the center is a threaded through hole. I need the face opposite the taper to be flat to within .002". My process so far has been to waterjet cut a blank out of 3/4" plate, face one side and bore/thread the ID, then I take it to another cnc and spin it onto a fixture with the faced side to the fixture plate to hole it for the taper machining. The fixture plate works well, I have two small blind holes drilled near the threaded hole for a pin spanner to remove the disc from the fixture plate after this op is complete. Everything looks great until this point, after removing the disc I am seeing a ton of dish near the outer edge of the disc from the plate stress relieving itself and my original faced surface is concave by about .030". I would face it after but there would be a ton of chatter and I need a 64 finish max. I thought about making another fixture with a mating female taper but I can't really think of how to hold the disc to the fixture and be able to remove it after facing as it"ll be quite tight and my spanner won't be able to access the pin holes as they're on the wrong side of the part and aren't through holes. I have attached a picture not of the actual part just a cut away of a similar design so you understand what it is I am trying to make... I have alot of these to make, not a huge panic for time frame but want to get a system dialed in, perhaps grinding the flat face after machining the taper, the OD tolerance is loose at +/- .04" and the taper face isn't critical for flatness... Thoughts?? Perhaps machining from round instead of plate would prevent some of the stresses coming out of the plate once out of the fixture?

First, definitely cut from round bar slices, second try stress relief thermal treatment if round blanks aren't good enough.

Also you may want to try a few flips during roughing, you can cut the taper to about 2/3rds distance while maintaining enough flat to stabilize as you flip back and forth, with the final pass establishing the full angled face.

If you can only have the pin spanner holes on one side (not both) you may have to use a threaded plug with a pilot that goes into a cbore on your fixture plate, then a longer cap screw secures the entirety of plug and blank to the fixture. This way you can remove the assembly without having to worry about torque through the spanner holes, or eliminate them entirely.

I will try some round stock next week, I’m hoping it stays flatter, I have tried flipping back and forth and it seems quite good until about the last .040” or so has to come off and then it starts warping. I was thinking I could maybe try a female taper fixture with a bore and two mating dowel pins then bolting to the threaded bore from the back side of the fixture plate and facing after. Really think the sharp edge needs to be supported the entire time so I don’t get vibration or it kind of catching the insert and tearing the edge.

Epic Metal said:

I will try some round stock next week, I’m hoping it stays flatter, I have tried flipping back and forth and it seems quite good until about the last .040” or so has to come off and then it starts warping. I was thinking I could maybe try a female taper fixture with a bore and two mating dowel pins then bolting to the threaded bore from the back side of the fixture plate and facing after. Really think the sharp edge needs to be supported the entire time so I don’t get vibration or it kind of catching the insert and tearing the edge.

Click to expand...

If it's good until the last passes, try using a different insert for finish cuts. What you're using may have too much of an edge prep, so "pushing" the material instead of finely slicing it. The pushing induces a stretching, and all of a sudden your part's no longer flat.

Try a sharp insert meant for Al for finish cuts - yes, you may have to replace it more often but you'll have a much lower stress in the cut while it's still sharp. That should be a major help in getting a flat part. Adjust SFM and feed to suit.

We have done similar stuff like this in the past, What I found that works best is finish the flat side, and bore threads etc
then on the side that needs the taper. use full circle alum soft jaws, make your jaws about .200 deep at the od .150 might work and finish everything to that thickness on the tapered side.
Make sure you have a way to lightly screw a clamp in the center hole after jaws are cut.

then run all you parts at the .2 thickness, then all your parts at .150 then all your parts at 100 then all your parts at 075 etc etc until you get the desired depth of .040 while blending in taper this way your only wasting 1 set of jaws. hope that made sense to you.

I would use a ccmt with very high positive(alum type insert) and a .015 rad or smaller and cuts around .010 doc.



we did some parts out of stress relieved 4340 that were .025 thick Started at .200 about 10" dia and it worked very well kept the parts flat also I was pretty amazed. the thinner the thickness gets the less jaw pressure you use.
if I were to do them again I would put a vacumm plate in the jaws with a dubling fitting at slow rpms. we did that on some plastic parts long ago and while it was a pain in the ass it worked and kept the parts flat kept the chatter down as well. you pretty much have to make everything to use vacumm however. if its a lot of parts it might be worth it to you in the long run.

double sided tape works on the jaw faces also(works very good)

I've never done this, so keep that in mind.

I might try building it the way Delw explained EXCEPT leave the OD oversized, then finish the taper to thickness. If the part is screwed through the center, it won't become a murder weapon. That last pass would be tricky to do just right. As soon as the disk is done, get it off the machine and on a surface plate, flat down.

R

Regarding the edge, I recently did some turned parts that needed to have a sharp edge. These were tubular not a disk. No matter what I was not able to "turn" the knife edge. In my case even with sharp inserts the material at the edge pushed away. What I wound up turning a little secondary bevel near the edge and getting it as close as I could in the lathe. Then I spun the part in my cutter grinder against a buffing wheel and buffed it sharp. This did a nice job. In my case the design was somewhat flexible so I could add the secondary bevel.