Threadmilling vs Internal Screwcutting in SAF2205

[Mick]

I'm interested in feedback or experience in threadmilling SAF2205 stainless steel.

 

We have a part that has a M36 x 2 internal thread, 60mm deep. Our Sandvik Coromant rep recommended threadmilling over internal screwcutting, and so we programmed the part using threadmilling.

 

The operator prefers internal screwcutting, and has changed to this method, for better tool control and more productivity (almost half the time)

 

Has anyone has similar experiences? I'm keen to get some feedback. Bear in mind, there was no attempt at improving the threadmilling. They just changed to internal threading.

[gary adams]

Tooling here is the key.Vargus has some new tooling that takes carbide inserts each with centre screw clamping, we used it M36 x 4 and it did it a treat in k1045, 2205 may be different. M36 x 2 shouldnt give much trouble either method.But if you are talking about coarse series threads that are two thread diameters deep, I would favour thread mill with a vargus cutter as discribed. Iscar multimaster go ok and should handle M36.

Gary

[Reko]

It really depends on the part, IMO. Is it a blind hole or a thru hole?

 

Internal thread cutting on a CNC Turning Center gets more difficult as the thread gets smaller. Problems with screw cutting can include winding chips, chatter and insert failure. Thread milling, on the other hand, generally takes longer and can suffer similar problems.

 

My opinion, in general, is that screw cutting on a CNC turning center is generally superior in both speed and finish to thread milling on a CNC machining center.

[Jayson Kramer]

Three Questions.

1) How long was it taking to thread hobb?

 

2)How is the life of your tap are you breaking any?

 

3) is the 2205 a Duplex stainless?

[Ron Branch @ Verisurf]

I would thread mill it all day long and never look back. 1.4173" is huge in the world of thread milling. 2.362 deep is on the middle range. I would look to a integrated shank type tool. You could get away with a 1.375 dia tool. Look at Advent or Carmex for a tool. I would look to the skipped tooth insert from advent and if push came to shove the multi flute single point style from Carmex.

 

next question how many holes? How much time did someone quote? Do you have to ROI this or are you willing to expect the possibly loss in quality doing it a different way? If you had to you could always run it a few .001 under size and then chase with a tap to size with a ton of cutting oil. We just did some STI's in some 10-2-3 Ti with 10" gauge lengths and we were surprised we could cut them to size with no problem. We were using a solid carbide thread mill multi-flute style not the single point style.

 

HTH

[Mick]

Thanks for all the replies.

 

The material, SAF 2205, is a duplex stainless steel. Threadmilling it supposedly took 18 minutes, whereas screwcutting it only take 8 minutes.

 

We're not doing many holes, as these are tiny batches, as in, 4 - 6 holes at a time. This thread is in the end of a shaft.

 

The hole is blind, which is why we initially went the threadmilling route. Our experience with screwcutting blind holes hasn't been favourable

[Ron Branch @ Verisurf]

How much will scrapping a part cost you? I always use the 3 for rule on scrap. If the part cost $100 then it cost you minimum of $300. If the part cost $5000 then it cost you $15000 for a scrap part. Here is my thought process. The original cost, plus the make up cost plus the time lost not put on something else. I call it for 3 for 1 rule of scrap. So yes it may take 18 minutes, but how much do you lose for scrapping one? If it is a shaft why can't you single point it with a boring bar? They make defib threading bars. You could run it to the low side if you get chatter and then finish by hand. Couple different things you could do here.

 

HTH