Tapping 0-80 in 303 Free machining SS

[mike561h]

We have been tapping by hand or with a tapmatic 0-80 threads.  I'm drilling the hole .052 so they don't break.

I'm going to just start tapping on the machine if i can get them not o break.  Only going .150 DP. I know if guys who use RPM of 1000 for Titanium

for 6-32 4-40 etc..  We are using standard taps nothing fancy. Any recs on speeds and feeds  303 free machining. these are a bitch to remove after they snap.

Thanks,

mike

[Leon82]

I would try to find a form tap.

 

We are tapping a m1 thread in fee machining invar which machines similar to stainless.

It is an emuge form tap and was 70 bucks each but its worth it. 

I peck tap at 2mm peck I believe. I can get the EDP number tomorrow if you wish. They should have an inch selection.

 

[mike561h]

1 minute ago, Leon82 said:

I would try to find a form tap.

 

We are tapping a m1 thread in fee machining invar which machines similar to stainless.

It is an emuge form tap and was 70 bucks each but its worth it. 

I peck tap at 2mm peck I believe. I can get the EDP number tomorrow if you wish. They should have an inch selection.

 

Would you say that $70 tap will last.  How deep are you going. what speeds and feeds.  

[Leon82]

It has never broken. I think I changed it once over the entire time we have been using it only because the piece of material is $1000+.

I go at least 4 mm deep but probably more at 500 rpm. I can give the exact number when I'm at work tomorrow.

[Matthew Hajicek - Singularity]

Or go the safe rout and threadmill them.

[mike561h]

mastercam calculates 27.85 feed and 2228 rpm at 35 SFM.  

[mike561h]

6 minutes ago, Matthew Hajicek™ - Conventus said:

Or go the safe rout and threadmill them.

Thread mill a .052 hole  thats really cool

[Matthew Hajicek - Singularity]

3 minutes ago, mike561h said:

Thread mill a .052 hole  thats really cool

Harvey has 00

http://www.harveytool.com/prod/Thread-Milling-Cutters/Holemaking---Threading/Browse-Our-Products_271/Thread-Milling-Cutters---Single-Form_157.aspx

 

[mike561h]

7 minutes ago, mike561h said:

mastercam calculates 27.85 feed and 2228 rpm at 35 SFM.  

509 rpm 6.36 feed at 8 sfm  what are you cats using....

[mkd]

+1 for OSG coated form tap, especially if it is a regular job.

 I just finished a Ti job with 2mm threads. i threadmilled one pattern just to hit a specific depth. Took forever.

[Leon82]

12 minutes ago, mike561h said:

509 rpm 6.36 feed at 8 sfm  what are you cats using....

I'm a snail tapper. 1000 rpm is most likely perfectly fine

[mike561h]

just ran 11 holes to .150 deep at 500 rpm 6.3 feed and it looks good.

[metalmansteve]

We use TiCN coated roll tap OSG 1400100108 on 49% nickel parts all the time.  $14.20 from Western Tool.  It never occurred to me to peck tap a form tap but maybe that works.  We go 1500 rpms.  Drill #54.  We can do a thousand holes (or more) per tap...typically about .100 deep.

 

[RaiderX]

you prob. already know but watch your drills that stuff will work harden and you will be banging your head on the table wondering why your taps are not working?

sorry been there done that. lol

[nickbe10]

300 series is pretty low grade compared to say 15-5 (real free machining), I would be more worried about impurities than anything else with a tap that small, so roll tap might help you out here.

[mike561h]

4 hours ago, metalmansteve said:

We use TiCN coated roll tap OSG 1400100108 on 49% nickel parts all the time.  $14.20 from Western Tool.  It never occurred to me to peck tap a form tap but maybe that works.  We go 1500 rpms.  Drill #54.  We can do a thousand holes (or more) per tap...typically about .100 deep.

 

I told the guys here to order a couple. 1000 holes sounds good to me...

thanks,