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:

Triple Square Modified 10° thread


Recommended Posts

I'm got a part o make that called out a

 

Triple Square Modified 10° right hand thread

Pitch = .750

Lead = 2.250

 

Its basically a triple lead ID thread with a major diameter of 27.188" 

The form is 3/8" wide flat bottomed with 10° angled walls

 

What I'm not getting is the 2.25" Lead.. what does that mean?

 

We don't do much threading around here

I'll have a choice between a Fanuc controlled VTL or a high Okuma 5X  mill turn

 

Either way, Its going to be interesting

 

Link to comment
Share on other sites

2.25 / 3 = .75

 

If you ask me, most people use the term pitch when they should be using lead.

 

The lead is 2.25... that is what you program for a single lead... that doesn't change for this thread either... you will still program that in 3 different positions... all .75 apart... that gets you the triple lead thread.

  • Like 1
Link to comment
Share on other sites

 

You don't necessarily have to shift your start point for a multi-start thread.

Sometimes clearances will not allow for this.

You can use "Q" to shift the start angle.

This works with canned threading & long code threading. (G32)

So for a triple start thread you would use:

G32 ............Q0.

G32 ............Q120.

G32 ............Q240.

 

or;

 

G76X_Z_I_K_D_F_A_P_Q_;

I : Difference of radiuses at threads

K : Height of thread crest (radius)

D : Depth of the first cut (radius)

A : Angle of the tool tip (angle of ridges)

P : Method of cutting

Q: Shift angle of thread cutting start angle

 

Depending on your control, you may not be able to use decimal points for the "Q" value.

Q120. could need to be Q120000 or similar.

  • Like 3
Link to comment
Share on other sites

Tom, we do a lot of multiple start threads. But ours are for medical, ie: bone screws.

The 2.250 is usually the total lead of .750 pitch * 3 starts.

I tend to stay away from the G76 canned cycles, as you lose control compared to G32.

Link to comment
Share on other sites

I'm thinking about milling these on our Okuma VTM

Get a form cutter built, kick the head to the correct angle

and run a helix tool path

The ID is 27" so there is plenty of room

This part has dozens of mill features and they are all timed to the

threads. I'm concerned about maintaining that timing if I turn the threads

If I mill them, that's not an issue as long as I orient my drive chains correctly

Link to comment
Share on other sites

I have had timing to feature requirements before too.

I used to cut a custom thread on a 10' dia with a 4.0" lead. on a 5 meter VTL with double start threads.

Yes, 10 foot Dia.,(rock crusher parts).

Anyway, I would scribe the O.D. With stock still on, calculate my "Q" (angular) shift & go.

My requirements for this particular thread were to be within .001" every 90 degrees.

I'm just letting you know that you can thread this very accurately & faster than milling.

HTH

  • Like 2
Link to comment
Share on other sites

Another question is gaging the thread.

How do you even measure something like this??

We have tooling $$$ to build a gage, but how do you gage the gage

three "wire" method using Romer arm at the machine?

-or just romer arm against a good model. I would want to do a dry run on a gauge/blank before cutting a real part. Would be nice to test fit gauge on existing mating part, as a sanity check.

 

I see you're still doing the easy stuff. :blushing: Better you then me.

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...