Jump to content


- - - - -

NPT Thread Milling


  • Please log in to reply
12 replies to this topic

#1 ducati

ducati

    Member

  • Members
  • PipPip
  • 115 posts
  • Location:Deep South

Posted 04 October 2011 - 10:41 AM

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

#2 Horton@who.com

Horton@who.com

    Curmudgeon at large

  • Members
  • PipPipPip
  • 1,855 posts
  • Location:Moving on

Posted 04 October 2011 - 10:52 AM

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

#3 jeff

jeff

    Advanced Member

  • Members
  • PipPipPip
  • 6,569 posts

Posted 04 October 2011 - 11:08 AM

drill
threadmill with npt threadmill

what's this tapered hole nonsense? Posted Image

#4 ablucra

ablucra

    Member

  • Members
  • PipPip
  • 161 posts
  • Location:Newington,CT

Posted 04 October 2011 - 11:24 AM

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.

#5 Goldorak

Goldorak

    I Live. I Ride. I am Jeep.

  • Members
  • PipPipPip
  • 1,619 posts
  • Location:Quebec Canada

Posted 04 October 2011 - 11:56 AM

View Postablucra, on 04 October 2011 - 11:24 AM, said:

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

#6 Horton@who.com

Horton@who.com

    Curmudgeon at large

  • Members
  • PipPipPip
  • 1,855 posts
  • Location:Moving on

Posted 04 October 2011 - 12:40 PM

View PostGoldorak, on 04 October 2011 - 11:56 AM, said:

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

#7 Mic6

Mic6

    Advanced Member

  • Members
  • PipPipPip
  • 3,235 posts
  • Location:Sunnyvale, Ca

Posted 04 October 2011 - 01:01 PM

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

#8 Odin

Odin

    Member

  • Members
  • PipPip
  • 217 posts
  • Location:Indiana

Posted 04 October 2011 - 01:16 PM

View Postjeff, on 04 October 2011 - 11:08 AM, said:

drillthreadmill with npt threadmillwhat's this tapered hole nonsense? Posted Image


View PostMic6, on 04 October 2011 - 01:01 PM, said:

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.

#9 ducati

ducati

    Member

  • Members
  • PipPip
  • 115 posts
  • Location:Deep South

Posted 05 October 2011 - 10:29 AM

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!!

#10 ducati

ducati

    Member

  • Members
  • PipPip
  • 115 posts
  • Location:Deep South

Posted 05 October 2011 - 10:31 AM

View Postducati, on 05 October 2011 - 10:29 AM, said:

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.



#11 Horton@who.com

Horton@who.com

    Curmudgeon at large

  • Members
  • PipPipPip
  • 1,855 posts
  • Location:Moving on

Posted 05 October 2011 - 10:35 AM

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

Good Luck :)

#12 SBerg

SBerg

    Member

  • Members
  • PipPip
  • 55 posts
  • Location:Camas, Wa

Posted 05 October 2011 - 10:43 AM

http://www.threadmillsusa.com/NPT.htm

#13 McLaren

McLaren

    Member

  • Members
  • PipPip
  • 275 posts

Posted 05 October 2011 - 10:44 AM

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.

Attached Files