Debating on Milling taper for 1/2" NPT Threadmill

S

SIM

Titanium

Joined

Feb 19, 2004

Location

Staten Island NewYork USA

• Apr 21, 2010

• #1

I'm going back and forth on way to approach job....1/2-14 NPT Threadmill. For 303 SS I was just going to drill, chamfer, run the threadmill and be done....but the next part is 316 SS...has me on the fence...should I run a tapered mill around the hole first or will I be fine just running the threadmill in.

Larger diameters I use indexables, so if I'm wrong its a 50.00 mistake. A Solid carbide threadmill is a different story. I'd rather get some insight first.

Thanks

 

Curt B

Cast Iron

Joined

Aug 16, 2007

Location

Edmonton,Alberta,Canada

• Apr 21, 2010

• #2

Just do a couple progressive cuts on diameter to avoid burying it in difficult materials.

 

Last edited: Apr 21, 2010

G

Gary E

Diamond

Joined

Jan 2, 2006

Location

Houston, TX

• Apr 21, 2010

• #3

How much does a decent quality TAP cost?
1/2 in NPT does not require that much torque and it's faster
that is unless your doing this in a little Bridgeport

 

Perry Harrington

Titanium

Joined

Oct 7, 2006

Location

Klamath Falls, Oregon

• Apr 21, 2010

• #4

Call lakeshore carbide, they know their products well and can give you this info. One reason to mill it would be if the part is delicate or not well fixtured due to other constraints.

 

S

SIM

Titanium

Joined

Feb 19, 2004

Location

Staten Island NewYork USA

• Apr 21, 2010

• #5

Roundish part...can't hold it tight enough to tap without distorting.

 

G

gregormarwick

Diamond

Joined

Feb 7, 2007

Location

Aberdeen, UK

• Apr 21, 2010

• #6

I've never had any problems starting with a straight hole in 316, even super duplex, just keep one hand on the feed override for the first part.

Only thing I'd be a bit worried about is not being able to grip it too well. Vibration or chatter will chip out the teeth on a solid carbide threadmill in short order.

If you have a few to do and are worried about it, Seco have indexables down to 3/8" for NPT.

Like curt said, taking it in a few passes might be the way to go.

 

G

Gary E

Diamond

Joined

Jan 2, 2006

Location

Houston, TX

• Apr 21, 2010

• #7

I'm old... and I have thread milled holes to produce Class 3 STRAIGHT threads...
used to only 2 axis circular and the Z linear...
NPT threaded holes are TAPERED...


let start at the bottom of the hole...
move out with a circular path and end up at the proper dia say at 12:00
Now going counter clockwise with Circular and mill 1/4 of the hole to 9:00 feeding up 1/4 of a thread pitch
but now that end point should be at a slightly larger radius ...right??

So the question is...

Do the controls you have today allow the 1/4 turn around the hole and 1/4 pitch Z move and end up at a slightly larger radius all the way around the hole??

 

SteveinAZ

Stainless

Joined

Aug 20, 2007

Location

Snowy Arizona

• Apr 21, 2010

• #8

SIM, easy-peasy. I too have 1/2" MPT in T316 on a repeating job and drill a straight hole (actually drill an 11/16" hole, and then interpolate to 0.703". After broken taps in a couple parts, I went to a thread mill and can be confident in walking away from the red button. I program it in two passes by using a second radius offset that is about 0.020" or so larger on the first pass, but use the same code other than changing the D# in the G41 line. Threads gauge perfect after a tweak or two, and then all is well.

Steve

 

G

gregormarwick

Diamond

Joined

Feb 7, 2007

Location

Aberdeen, UK

• Apr 21, 2010

• #9

Gary E said:

I'm old... and I have thread milled holes to produce Class 3 STRAIGHT threads...
used to only 2 axis circular and the Z linear...
NPT threaded holes are TAPERED...


let start at the bottom of the hole...
move out with a circular path and end up at the proper dia say at 12:00
Now going counter clockwise with Circular and mill 1/4 of the hole to 9:00 feeding up 1/4 of a thread pitch
but now that end point should be at a slightly larger radius ...right??

So the question is...

Do the controls you have today allow the 1/4 turn around the hole and 1/4 pitch Z move and end up at a slightly larger radius all the way around the hole??

Click to expand...

The common method is to split the helix up into quadrants or less and spiral outwards in x and y as you move up in z. It's theoretically not perfect but in practice is very very close. The smaller the segments the closer to true form.

 

S

SIM

Titanium

Joined

Feb 19, 2004

Location

Staten Island NewYork USA

• Apr 21, 2010

• #10

Thank you guys!

I was fairly certain about taking it in a pass or two to start with...but a couple of " Your not going to Run a Taper in that hole first" got me to thinking.

Indexable is not going to work for me on this as I prefer to have four cutting flutes....4000 pcs so every extra flute helps.


Gary E...I feel old.
My CAM program spits out the code in four quadrants, in each the diameter grows slightly to compensate for the taper as the tool rises.

First time I did an NPT threadmill I had to program long hand...pain in the butt. From there I downloaded simple software from a manufacturer which gave me the code after pluggin in the numbers. Now the Cam does it all.

 

G

gocubs68

Plastic

Joined

Jan 6, 2008

Location

Moline,IL

• Apr 22, 2010

• #11

you should be fine with drill, chamfer, threadmill like you do on your 316. That is how we threadmill all NPT (and standard) threads. Have gone up to 1-11 NPT in Hastelloy C-276 with no troubles. Good Luck.