Lazarusman

Tapping Speeds and Feeds

Recommended Posts

I don't know if this topic has already been covered. I did a search, and didn't find anything. What I'm looking for is some information on spindle speed, and threads per inch for rigid tapping. My mastercam software keeps putting in insanely high spindle speeds. and aggressive threads per inch values in my programs, and I keep breaking taps. Any help would be appreciated.

Thanks

Share this post


Link to post
Share on other sites

What sizes?

Generally run our taps at 2k+ RPM when rigid tapping...it's never gets there though

Share this post


Link to post
Share on other sites

depends on machine and size of tap. feed is dependent on speed and threads per inch

also the quality and type of tap (spiral point, spiral flute, etc)

on our haas it was recommended under 300rpm

Share this post


Link to post
Share on other sites

I'm running a 7 or 8 year old Akira-Seki vertical mill, with taps made by Kennametal... 1/4-20, 3/8-16. Broke them both right off. I ran them at 196rpm, with 14. threads per inch. My machine uses an E value for TPI...which is new to me. I'd love to find some resource material for spindle speed, and TPI, to cross reference my programs. The speeds and feeds that MasterCAM is putting out, for the taps at least, seem quite high.

Thanks again for y'all's imput.

Share this post


Link to post
Share on other sites
51 minutes ago, Lazarusman said:

I'm running a 7 or 8 year old Akira-Seki vertical mill, with taps made by Kennametal... 1/4-20, 3/8-16. Broke them both right off. I ran them at 196rpm, with 14. threads per inch. My machine uses an E value for TPI...which is new to me. I'd love to find some resource material for spindle speed, and TPI, to cross reference my programs. The speeds and feeds that MasterCAM is putting out, for the taps at least, seem quite high.

Thanks again for y'all's imput.

thats the problem, 1/4-20 is 20 threads per inch = 200 rpm 10 ipm,  3/8-16 = 160 rpm 10 ipm

also are you sure you have rigid tapping?

  • Like 1

Share this post


Link to post
Share on other sites

Find out if the machine can use pitch....then the feed is      1/no. of threads

1/4-20 would be .050 on the feed

3/8-16 would be .0625 on the feed

Then just set a speed

Share this post


Link to post
Share on other sites

As a starting point, I adjust (all sizes of taps) the rpm to achieve a 20-30 ipm feedrate.

Kinda slow but it has never failed  me.

Share this post


Link to post
Share on other sites

We don't do mad quantities just big expensive parts mostly.

I try to have my guys keep a constant 5ipm on all taps, the RPM is easily confirmed by the operator (multiplying it by 2) 

We used to use 10ipm but noticed most "send backs" were cut in half.

1/2-13 @  5ipm = 65rpm x 2 = 130  

1/2-20 @  5ipm = 100rpm x 2 = 20

3/8-16 @ 5ipm = 80rpm x 2 = 160

If a tap gets broken it won't be from a speed feed issue. I know it may sound slow but in the end way faster than burning out a broken tap.

  • Like 2

Share this post


Link to post
Share on other sites

Like with any cutting operation you got to find first:

               what material are you cutting

               what is your tap made of

               is it a cutting tap or a form tap?

 For aluminum with a HSS cut tap I do about 50sfm or for tool steel I would use 5-8sfm. With these sfm find your RPM.  I don't know if your machine needs inches per minute or inches per revolution. The sample below is for ipm.

For 1/4-20  tapping aluminum (50*3.82)/.250=764 this is your RPM then divide by tpi to find you ipm 764/20=38.2     so your rpm is S764 and your feed is F38.2 

In any case if you need the feed for ipr format is just a simple operation 1/20=.050 so your rpm would be S764 and feed F.050  

There are too many variables to expect mastercam to give you the right feed and speed all the time. Just find the correct SFM for the tool you are going to use and for whatever material you will be cutting.

 

 

 

Share this post


Link to post
Share on other sites

We rarely do production runs of more than a few parts, when we do I use threadmills.

The formula I use is:

RPM = TPI x 10 & IPM = 10

So 1/4-20 = 20 RPM & 10 IPM, 3/8-16 = 160 RPM & 10 IPM, 1/2-13 = 130 RPM & 10 IPM etc.

Except on hardened steels and exotics, this has rarely failed me.

Share this post


Link to post
Share on other sites

I'm typically making prototype parts, so I don't always need aggressive cuts, but I always go for 1/TPI feed at RPM 400 G95 G98. It's a safe, slow speed good for most materials including stainless, but might not be good for exotics like niobium.

 

Share this post


Link to post
Share on other sites

My taps for most steels are 50-100 sfpm

 

Share this post


Link to post
Share on other sites

I never understood why G95 isnt the standard for tapping.. It doesnt matter what the spindle speed is . Your feed rate is always the pitch.. For example a 1/2-13 I would usually just default to 1000 rpm and F .0769 (1/13 for the TPI) 

It is much easier when looking through a program to verify the feed rate is correct 

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

  • Recently Browsing   0 members

    No registered users viewing this page.

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