[tenaja]

I'm looking for some advice here. I'm trying to make some 1" long BeCu pins that are 1/32" OD, with a 1/4" long x 1mm OD section near the middle... basically your typical screw machine part. The problem I'm having is the part is coming out with a slight bow to it, typically about 2-3 thou of TIR, which is unacceptable (the target is under 1 thou). I'm using a sharp cutting tool (no radius). I've double checked the tool centerline, and tried varying the cut & feed speeds. I've tried material from a couple different suppliers.

Anybody tackled a job like this and made it? Thanks!

[MikeMc]

This type of problem has always been tool center, in my experience. If you are using a formed insert (as opposed to a ground one) this could be the problem as well. This is where an Agathon grinder comes in handy. You should get the tool to razor sharp.

[PixMan]

You're dealing with internal stresses in the part. There may be some residual stress in the raw material, but it's more likely that you're introducing it in the turning operation.

I agree with MikeMc that you should be using a very upsharp edge on the cutting tool, be right on center, cut a little slow in feedrate to avoid generating heat and flood it with cutting oil to help keep it cool.

Even with those parameters in place you may get some bow. The only solution my be to do a supported turn. By this I mean turn just a short length and then bring in the sub-spindle (assuming your machine has one) to grip the part on both ends as you turn it.

[tenaja]

thanks for the tips. I've already flooded it with oil so I can hardly see the part--about 4 nozzles worth. I've already tried the centerline...moving it either direction just made it worse (software made it easy). I am already supporting it with the subspindle as soon as possible. I'm using the sharpest ground inserts I can find, and they are much sharper than I can grind, and certainly better than anything a tool grinder has been able make for me. I've got some pretty steep upsharp Iscar inserts, but the smallest radius they came with was .004"... they've got a pretty sharp edge on them, but they are formed.

So what are the best inserts you guys have used?

[PixMan]

Try a Ceratip in the PR930 grade. I apologize that I can't recall the chipbreaker designation, but they have a very upsharp edge on a DCGT 32.5x insert and go down to a .001 or .002 radius. This PVD TiCN coated insert (if you can figure out which chipbreaker I'm referring to) should solve this once and for all.

I learned to hate Iscar once I started using Ceratip, WhizCut, and especially the Utilys brands. The Utilys is also a great choice, but is ain't cheap. Call Genevieve Swiss and they can help you. More info at:

http://www.genswiss.com

In fact, if you call Genevieve Swiss and can talk to Jim (the owner), he can probably debug this problem for you easily.

[MadMax]

Could the part get bent during the final partoff operation? Are you supporting the part with the sub during the partoff?

I'm thinking that the part may be getting loaded in a way that bends it if you're supporting the far end and the parting tool pushes thru.

[HSPMInc]

What kind of material is it? And what RPM are you at? I have some little pins that are like that and the answer was lower rpm (like 3000ish i think) and a MICRO 100 tool that I ground myself for turning.

Also, does it bend it up if you just run the main side and don't pick it off with the sub? Could your sub collet/ejection pin be mucking it up? At that dia. any mismatch from front to back can mess you up.

[SwissType1]

UTILIS offers an insert with a ZERO RADIUS tool nose for problems like this. The edges are also peripherally ground producing a very sharp cutting edge. UTILIS calls is the "Multidec-TOP"

Check them out here:
http://www.genswiss.com/multideciso.htm

[tobyaxis]

I'm looking for some advice here. I'm trying to make some 1" long BeCu pins that are 1/32" OD, with a 1/4" long x 1mm OD section near the middle... basically your typical screw machine part. The problem I'm having is the part is coming out with a slight bow to it, typically about 2-3 thou of TIR, which is unacceptable (the target is under 1 thou). I'm using a sharp cutting tool (no radius). I've double checked the tool centerline, and tried varying the cut & feed speeds. I've tried material from a couple different suppliers.

Anybody tackled a job like this and made it? Thanks!

Are you using Ground Material?

Try tightening your Guide Bushing a little. Your Tooling is perfect but also increase the Positive Rake Angle. If your tip winds up wearing out too fast then put at least a .005 TNR and decrease your F&S.

What type and name brand of Swiss are you using?

[PixMan]

I tend to disagree with "Your Tooling is perfect", because it isn't working.

Why would a .005 tool nose radius work better? In my experience, the bigger the radius the more likely to increase heat and therefore bow.

[hacdlux]

applitec makes some verry keen edged tools at reasonabe prices theyre tools are mostly sharp or wiper, with a few radiuses available ive used the 762x-25front turn tools with success doing some verrry slender pins in delrin and aluminum

also have you checked the alignment of your main,gb,sub collet

[petriej]

Is your stock centerless ground. I've seen amazing differences in running wrought vs. centerless ground. I don't know much about getting BeCu ground, but we get all of our Ti alloy, CoCrMo, and Stainless centerless ground.

[EdgeCrusher]

I've had jobs with a similar problem. I was running one order once that I finished one material lot and switched to a new lot of material and it was a couple points softer on the rockwell and that material ended up being so bent we couldn't use it to make the parts. I tried every different radius tool we had .004-.03 changed feeds and speeds and nothing would help except a different lot of material.

[tobyaxis]

I tend to disagree with "Your Tooling is perfect", because it isn't working.

Why would a .005 tool nose radius work better? In my experience, the bigger the radius the more likely to increase heat and therefore bow.

A zero Radius will chip and break down faster. It is true that a small radius produces less cutting pressure (hence less heat) than a larger one but the TNR depends on what material your cutting and what dimensions your allowed in the corners if any.

[tobyaxis]

I've had jobs with a similar problem. I was running one order once that I finished one material lot and switched to a new lot of material and it was a couple points softer on the rockwell and that material ended up being so bent we couldn't use it to make the parts. I tried every different radius tool we had .004-.03 changed feeds and speeds and nothing would help except a different lot of material.

Improperly Annealed material can be a real PITA.

[DCogswell]

What kind of BeCu? It's been awhile since I've machined BeCu but, if I remember correctly CA172 is for machining and CA173 is for stamping/forming.

Free cutting turning tool will help a long way. Grind it yourself or go with Applitec. www.flptooling.com

The alignment of your Main spindle, guide bush & sub are very important. Next, you need to have the turning tool as close to the guide bush as possible. Don't use a revolving guide bush. Use a stationary one and move the guide bush assembly to within a couple of thousands away from the turning tool.

If this doesn't work, then you'll have to search for better material. Small diameter material from the mill should already be within a tight tolerance. I WOULDN"T send the material to be precision ground because the grinders may cause hard spots. And detecting those hard spots is nearly impossible.

I had a similar job where I had to turn .038" over 2.5" long with larger diameter features on both sides of the part. Our TIR was .005" and we couldn't hold it with one brand of LNC but we could with another brand of LNC.

[tenaja]

Thanks guys for the tips. I had to c'less grind it and all is well.

[tobyaxis]

Thanks guys for the tips. I had to c'less grind it and all is well.

You should never have to do this with parts made on a Swiss.
I have held +-.0001 on .06 Diameter Shafts 3.5 inches long 316L SS. Not to mention the .02 +-.0002 .08 Deep on the backside. The Swiss made short work of the Job and programming was only 15 minutes +- interruptions.

The only thing I can think of is if the machine is really old and beaten up.

[tenaja]

It was a brand new machine. I was removing too much material.

[tobyaxis]

It was a brand new machine. I was removing too much material.

Do you have Balance Turning?? This is the engagement of two turning tools at the same time. One tool roughs the other finishes.