Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Tapping Spiralock threads


JB7280
 Share

Recommended Posts

Any of you have any experience with Stanley Spiralock threads?  I'm tapping a part, 17-4PH, H1150.  Using a Guhring 8510 3.9MM drill. Using an Emuge Self-Lock Form tap.

Hole is on size, .153 and change.  Minor is on the very low side, Go gage runs in good, Hi-Limit PD does not go, but no matter what I do, the Hi-Limit Ramp gage goes in.  Tapping at 326rpm, 10.19IPM in an ER16 holder with a tapping collet.   Runout is <.0003" on the shank of the tap.

Link to comment
Share on other sites
25 minutes ago, huskermcdoogle said:

Are you using coolant or oil?  What does the thread finish look like?  I am assuming you are using a rigid tapping cycle as well?  Have you tried a snycroflex tap holder?  Is the tap showing any signs of wear or galling?

Using coolant.  I called Emuge and the gentleman I spoke to informed me that self locking threads created with an Emuge tap must be inspected with an Emuge gage.  We had a Spiralock gage.  I'm not 100% convinced that there is a difference, but we are ordering the gage.  I assumed that since they both conform to the specs of the drawing, that the gages were interchangeable.

Link to comment
Share on other sites

I would assume this to be correct, as the each brand of self locking form is likely under patent, where separate methods are patented.  They can't copy each other exactly, but the fact that it is self locking is likely not patent-able anymore.  Therefore the method of which they do it is, and therefore is different. 

Someone please correct me if my assumptions are incorrect.

Link to comment
Share on other sites
Just now, huskermcdoogle said:

I would assume this to be correct, as the each brand of self locking form is likely under patent, where separate methods are patented.  They can't copy each other exactly, but the fact that it is self locking is likely not patent-able anymore.  Therefore the method of which they do it is, and therefore is different. 

Someone please correct me if my assumptions are incorrect.

I can't speak on that, however I will follow-up when the gage arrives.  On a side note, in this material, would form or cut tapping be preferred?  8 of the holes are blind, but the drill hole is .620 deep with only .300 thread.  Would it be worth it to add a program stop to apply tapping oil and not run coolant?

Link to comment
Share on other sites
8 hours ago, JB7280 said:

I can't speak on that, however I will follow-up when the gage arrives.  On a side note, in this material, would form or cut tapping be preferred?  8 of the holes are blind, but the drill hole is .620 deep with only .300 thread.  Would it be worth it to add a program stop to apply tapping oil and not run coolant?

With Form Tapping, you are always at the mercy of the material, and relying on the tap to push a consistent amount of material out of the way. I alway prefer Cut Tapping in anything that is even semi-hard. 

Did you happen to catch that you have a Rounding Error on the Feedrate? 

At 32 TPI, and 326 RPM, Feedrate should be 10.1875.

The Post rounds to 2 decimals by default.

Please ignore my comment if you are cutting a Metric Pitch. But 326 ÷ 10.19 = 31.99215.

You could also just increase your RPM to 360, which would be a Feed of 11.25. (Rounds cleanly to 2 decimals.)

  • Like 1
Link to comment
Share on other sites
11 hours ago, Colin Gilchrist said:

With Form Tapping, you are always at the mercy of the material, and relying on the tap to push a consistent amount of material out of the way. I alway prefer Cut Tapping in anything that is even semi-hard. 

Did you happen to catch that you have a Rounding Error on the Feedrate? 

At 32 TPI, and 326 RPM, Feedrate should be 10.1875.

The Post rounds to 2 decimals by default.

Please ignore my comment if you are cutting a Metric Pitch. But 326 ÷ 10.19 = 31.99215.

You could also just increase your RPM to 360, which would be a Feed of 11.25. (Rounds cleanly to 2 decimals.)

Hm, I will change that.  Do you think that will make a noticeable improvement in the threads?  I knew it was rounded, but 2 decimals has always been enough to produce a good thread, from past experience.  

In order for MC to output 3, or 4 decimals in the future, that would be a post change?

Link to comment
Share on other sites
On 11/21/2019 at 3:37 AM, JB7280 said:

Hm, I will change that.  Do you think that will make a noticeable improvement in the threads?  I knew it was rounded, but 2 decimals has always been enough to produce a good thread, from past experience.  

In order for MC to output 3, or 4 decimals in the future, that would be a post change?

Yes, inside the 'ptap$' Post Block, you can override the Format Statement, in order to change the number of decimals for output.

The 'newfs' command can be used to change the applied FS.

The only time I don't worry about having Feed/RPM, in perfect Sync, is when I'm using some sort of spring-loaded Tap Head/Holder.

Here is a trick I use to help me calculate clean Feed/Speeds for Tapping:

Selecting the correct RPM is much easier if you consider the the 'screw' being formed over the 'unit length' of the measuring system. For 'Inch Machines', that length is precisely 1 Inch.

For a thread with  TPI of 16, we turn 16 times around over that 1" distance. Same thing for a 1/2-13 Thread, except we turn 13 times around in that same distance. 

For both those different threads, if our RPM = TPI, then our Feedrate would be F1.0 for both threads.

Consider the 'TPI' as the 'number of turns', and the Feedrate as '1.0 times the number of turns', and you're on your way to understanding the trick. 

Now, how fast do you want to tap? That will somewhat be dependent on both the cutting speed of the material, the accuracy of your machine, and the Torque Curve of your Spindle. You want to shoot for Peak Torque, regardless of the material being machined, if the tapping is difficult. Unless the peak is too fast for the material. For high-speed, low-torque spindles, there is no substitute for thread milling.

Take the feed you want to tap at (even Feed in Units per minute), and multiply it by the TPI. 

For a 1/2-13, if we want to tap at 30 IPM, we multiply 30 x 13, and get 390 RPM. Then, we look at the RPM. Is 390 right for the material and spindle? Well, if we think that is too fast,  what RPM are we targeting? If we use a feed of 20 instead, and multiply 20 x 13, we get 260 RPM. 

In your case, the magic TPI is 32. So, 32 turns for every 1 inch of distance, traveling at 1 IPM.

So, if we multiply by 10, that is 320 RPM, at 10 IPM. (You were at 326. What made you pick that number specifically? )

So, the trick is,

Add a '0' to the TPI, at 10 IPM. 

If that RPM is too low, then double or triple it, until the RPM range is right. Then do the same adjustment to the Feed. (2x, 3x, 4x, or 5x the TPI, then do the same to the 10 IPM Feed.)

For your Thread Lock Tap from Emuge, they recommend 33 Meters/Min for that Roll Tap, and in the Stainless material column, the speeds had 'footnote 2', which says "paste recommended". So likely something like Moly-D, with molybdenum in it. But not just straight coolant, unless you are pushing a high concentration. (10% at least...)

  • Like 1
Link to comment
Share on other sites
On 11/23/2019 at 12:25 AM, Colin Gilchrist said:

 

So, if we multiply by 10, that is 320 RPM, at 10 IPM. (You were at 326. What made you pick that number specifically? )

 

For your Thread Lock Tap from Emuge, they recommend 33 Meters/Min for that Roll Tap, and in the Stainless material column, the speeds had 'footnote 2', which says "paste recommended". So likely something like Moly-D, with molybdenum in it. But not just straight coolant, unless you are pushing a high concentration. (10% at least...)

Great explanation.  Thank you.   I will try 320/10, as well as a program stop to apply the Emuge tapping oil that we have on hand in the shop.  

As far as the 326rpm, I cannot find it on their site now, but if I recall correctly, Emuge recommended 14SFM, so the 326 is simply a product of that.

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...