ducati

NPT Thread Milling

13 posts in this topic

I need advice on milling some 2 1/2 - 8 TPI female NPT threads in Plexiglass Full Depth.

 

This will be my first time so be kind

The project:

20 each 2 1/2 NPT female holes in Plexiglass.

Options to consider?

 

Bore hole. Mill taper profile with endmill, then thread with single point tool? Will it follow tapered profile?

 

Bore hole, thread with Tapered Thread mill?

Each part will have about 10 plus hours into the process when it comes time to cut the threads so......

 

Suggestions please

 

Thanks

Share this post


Link to post
Share on other sites

Me, personally, I would do a pocket, then contour (with bullmill) with tapered wall option checked and input 1.783 for the angle and then use a tapered threadmill (because we already have them :) ) with the same 1.783 angle in the threadmill op

 

If you use an endmill w/.09 rad and step down around .01 per pass it will be smooth enough for threads

 

HTH

Share this post


Link to post
Share on other sites

drill

threadmill with npt threadmill

 

what's this tapered hole nonsense? tongue.gif

Share this post


Link to post
Share on other sites

If the part can handle the added force a straight hole with tapered mill will work fine. If the thread is in a boss with little wall

thickness then I would taper mill the hole and use a single point thread mill.

Share this post


Link to post
Share on other sites

If the part can handle the added force a straight hole with tapered mill will work fine. If the thread is in a boss with little wall

thickness then I would taper mill the hole and use a single point thread mill.

 

x2

 

the cutting force can crack the part very easily

Share this post


Link to post
Share on other sites

x2

 

the cutting force can crack the part very easily

 

Yes it will....plexiglass is a b!tch to drill, that's why I suggested pocket, or even a helix bore would work good too

Share this post


Link to post
Share on other sites

Mill Hole>Chamfer>multipass threadmill with a fine finish pass. Are you allowed to use coolant?

Share this post


Link to post
Share on other sites

drillthreadmill with npt threadmillwhat's this tapered hole nonsense? tongue.gif

 

 

Mill Hole>Chamfer>multipass threadmill with a fine finish pass. Are you allowed to use coolant?

 

 

Mill hole then threadmill with npt thread mill 3 rough, 1 finish,1 spring pass. I do this everyday in all types of material from lexan, graphite, aluminum, and pre-hardened H13. Single point...blah. Iscar and Allied Machine and Engineering make some awesome threadmills. Solid carbide to indexable inserted style.

Use the same basic feeds and speeds as you would use with an Endmill and you will be fine.

Share this post


Link to post
Share on other sites

Thanks. Sounds like I will be purchasing several thread mills. I will need to machine some smaller NPT threads and

Some straight metric threads also. Recs on brand of thread mills? Does anyone have a link to some charts for the hole sizes

To cover standard,metric and NPT other than Machinist Handbook? I am guessing someone may have a link or a spread sheet

Done already.

As always. Thanks for your time and advice!!

Share this post


Link to post
Share on other sites

Thanks. Sounds like I will be purchasing several thread mills. I will need to machine some smaller NPT threads and

Some straight metric threads also. Recs on brand of thread mills? Does anyone have a link to some charts for the hole sizes

To cover standard,metric and NPT other than Machinist Handbook? I am guessing someone may have a link or a spread sheet

Done already.

As always. Thanks for your time and advice!!

Yes I can use coolant or WD40.

 

Share this post


Link to post
Share on other sites

Scientific Cutting Tools has some info on their site and sell threadmills also

 

Good Luck :)

Share this post


Link to post
Share on other sites

Vardex threadmills rock.

Here's a xls spreadsheet I made for programming. It gives the gage line major diameter that you should program to, the depth to get 2 extra turns past the wrench makeup length (like 5 turns past the gage length), and the drill diameter.

 

Just need to change the extension back to .xls

 

EDIT;

Brain fart. Accidentally put Iscar instead of Vardex. Iscar actually sucks.

NPT THREADMILL DEPTH.txt

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