Metric

# 0-80 tap on 316 Stainless steel

15 posts in this topic

Hello all.

I need tap a punch of #0-80 on 316L blind holes.Please give me some speed recommendation.

I had Kennametal roll tap in hand now.

Thanks in advance.

MDT.

Share this post


Link to post
Share on other sites

use taping paste instead of coolant, the tool lige will be 100x longer

 

and be sure to hold the pre drill diameter to the tap spec a 80 TPI thread is freakin' small, just drill .005 to .007 bigger you wont get any thread in your hole

 

a 0-80 has .059 od and for a roll tap the tad drill size is .048 to .055

Share this post


Link to post
Share on other sites

That will depend largely on how quickly your machine can accelerate and decelerate. If you program for a good SFM I doubt the machine will get going that fast before getting to the bottom of the hole.

Share this post


Link to post
Share on other sites

We have Kitamura CAT30 taper with Fanuc control,I think the speed response is not the problem.

The main question is with the 0-80 TPI normally how much the SFM would be for 316L?

Thanks.

Share this post


Link to post
Share on other sites

Hello Ron,

Thank you a lot.That will give me start point to work with.By the way,are you still work with the company in Brea?

MDT.

Share this post


Link to post
Share on other sites

I would go with a threadmill.

 

If you want to tap it, use an Exo VC10 or an Emugee tap. I, myself never tried roll taps on 316.

Share this post


Link to post
Share on other sites

Hello All Bro.'s

Thanks a lot for the in put.I will let you guy know the result on Monday.

Regards.

MDT.

Share this post


Link to post
Share on other sites

Not that you want to mess with the mess but I tapped dozens (full run) of 0-80's

in A286, (much nastier than 316) @ 500 RPM, 6.25 IPM using MolyDee tapping fluid.

PITA but worked well

Share this post


Link to post
Share on other sites
also increase your ref. plane to like Z.250 to give enough time to sincronize.

 

I've never understood that logic.

 

How much Z do I need to give for enough time to synchronize out of the hole?

 

Edit: I'm showing 40sfm in my speed chart.

Share this post


Link to post
Share on other sites

I've never understood that logic.

 

How much Z do I need to give for enough time to synchronize out of the hole?

 

Edit: I'm showing 40sfm in my speed chart.

Not out of the hole but when the tap enters the hole. This doesn't really apply to newer machines, for the old klunkers it was a good idea to start the tapping operation .250 above the hole to allow the spindle to get to full RPM for entering the drilled hole. I've tapped at 2000 RPM at .050 above the hole but that was with a Brother tapping center and that's what they are made to do.

Share this post


Link to post
Share on other sites

Thanks you for all input,I finished the job today,with Kennnametal rolling tap at 400 spindle speed,all 120 holes without any problem.

Again thanks a lot for you help.

MDT.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us