ID Threads

[g-codeguy]

Originally Posted by bdyenter 150 rpm is about right. I worked for a company where they had a problem running 304 stainless castings and would chip the inserts out and scrap castings. When I got there they were trying to run at 1250 rpm. This was way to fast for stainless. 150-200 rpm max is perfect with a lay-down insert. Your tool wear will be very acceptable as well. 1.750 deep isn't that deep especially with a carbide bar. For an excellent insert try the iscar IC908 laydown series inserts with 3 corners. I run pre hardened 4140 with 12" long threads and the inserts hold up for at least 25 pc orders. I reccommend this insert for your stainless as well. So snub up your bar from your turret to 1 7/8 and chuck up on your piece as much as possible if you can. You can also set your first block of G76 cycle to G76P000060 This will not allow a finishing pass in the cycle which will sometimes reduce the chatter because you will still allow tool pressure all the way to minor or major diameter. Bryan

He has to be hanging out at least 5 times the diameter. He is using a carbide threading bar and I can tell you that is a lot for an I.D. of that size. A blind hole plus threading to within .2 of the bottom means the insert will be cutting chips. Not good.

150 RPM at that diameter is not "just about right." 100 SFM would be on the low end even for a 'soft' carbide insert such as a KC720 or BXC from Carmex. That works out to about 700 RPM. Don't know what diameter you are threading those castings at, but it should be about 2-3/16 inches at S175 using 100 SFM. We use CP500 a lot and thread 316 SS at 365 SFM (over S2500 at 14mm dia.). 99.99% of our threading is done with a laydown insert.

We currently have four 316 SS casting jobs running, all I.D. threads, ranging from S1200 for a 3/8-NPT to a 15/16-26UNF at S1450. One 15/16-26UNF job is running at S1000 because of chatter (doesn't have good support). Just finished a 1-3/16-18UN O.D. thread at S1200 in SS casting. I much prefer O.D. threads to I.D. because most of our parts are small with no place for the chips to go.

PDI-Curtis' idea of stopping every few passes isn't a bad one, but threading without any compound infeed is. His example is cutting equal amounts of material on both sides of the insert. Not only does this create more tool pressure, but the strongest chip possible. Neither is desirable in your case (especially the chip), although some load is usually needed to eliminate chatter.

Sometimes the excessively slow RPMs are the only way to avoid chatter. This is hard on an insert. Material wants to stick to the insert. The insert often chips at withdrawal or at the start (more likely) of the next cut. If it doesn't chip, the material stuck on the insert will cause the thread sides to not be nice and clean because the stuck on material will cause scoring.

This much I can tell you: Slower RPM makes chatter look worse. Higher RPM shortens the distance between the chatter marks. Usually I have to slow down until it disappears. However. I did have one O.D. thread (small diameter) that cleaned up beautifully at an RPM that was 170% faster than what the machine manufacture said the limit was for threading (120 IPM). Guess Hardinge lathes are built with a little leeway.

When I first start programming lathes, they were threading 303 SS at 500 to 700 RPM and 19 to 21 passes. This was for both 3/4-28UNF and 15/16-26UNF threads. Inserts didn't hold up well, and often had problem with chatter. I went to S1400 and 5 or 6 passes. Couldn't go faster because of the need to get close to a shoulder. No chatter. Excellent tool life. Figured the savings on just this one machine paid for my wages for the year. And this didn't take anything into account except the reduction in cycle time.

[nitemare]

just went through a similar scenario. threading 1.875"-12 i.d. in 304SS, 2.00" deep in a blind hole. ended up with a vardex 3 sided 12 pitch vtx or vkx grade - both worked well. used 2 degree modifed infeed, 10 passes at 510 rpm. after success with this method, i switched to a pull thread, naturally i just needed to get the new anvil or shim, whichever you prefer to call it, and i couldn't get much more out of it in ways of rpm or less passes...just helped with the chips not packing in the back. had the luxury of being able to drill deeper as i was doing a bar push operation.

[cncjcl]

Id threads: On the 304ss in a 14mm dia on production Id use an OSG tap in a VC10 grade. It is not recomended for ss in the book BUT Iv ran parts for weeks and weeks in 304 ,17-4 ,and 15-5. The chips flow out of the hole. the VC10 grade is the only tap iv found that works in almost any ss. Good luck

[g-codeguy]

Originally Posted by cncjcl Id threads: On the 304ss in a 14mm dia on production Id use an OSG tap in a VC10 grade. It is not recomended for ss in the book BUT Iv ran parts for weeks and weeks in 304 ,17-4 ,and 15-5. The chips flow out of the hole. the VC10 grade is the only tap iv found that works in almost any ss. Good luck

Thanks for the tip on VC10 grade. We do use some OSG taps, but I never paid any attention to the grade. Usually the purchasing agent orders the cheapest ones he can find unless instructed to order something else. The more money he can save on tools, the bigger his bonus. Course we don't get a bonus for getting the work done regardless of tooling, but hey....