NPT thread milling

[Tim Johnson]

I am milling a 3/4 npt hole. the numbers look good but the path is programmed in 180 degree arcs. Is this good enough for a npt thread? I've manually programmed them in 45 degree arcs.

[Mgrenier]

Hello Tim,

 

We did quite a few 3/4 NPT holes with thread milling. I programmed 90° arcs and it worked like a charm. I would say that 180° arcs are too big but the 45° arcs will do the trick.

 

Hope that helps,

[Tim Johnson]

marting,

 

How do you break the toolpaths into 90 degree arcs? I tried to break my geometry circle into 4 arcs, but the toolpath still came out as 180 degree arcs. I am also circle milling several paths and would like to keep them as full circle blocks.

[Toolfab]

You shouldn't have to break the geo. What post are you using? I just select the hole that I want to threadmill, go thru the stuff in MC, don't forget the 1.7889 deg taper angle, and my post outputs in 90 deg's. 180 is tooooo much, IMO.

 

[Tim Johnson]

I'm using MPFAN.pst. I have the MPmaster.pst, but have not set it up yet. Will MPmaster.pst fix this? If so, I will have a good excuse to work on it.

[Toolfab]

Tim, can you post some code so I can see it?

[Tim Johnson]

Paul,

 

Here it is:

 

%

O0000

(PROGRAM NAME - 617-856)

(DATE=DD-MM-YY - 14-04-04 TIME=HH:MM - 09:07)

N100G20

N102G00G17G40G49G80G90

(.790 DIA 14 NPT PITCH THREAD MILL TOOL - 44 DIA. OFF. - 144 LEN. - 44 DIA. - .79)

N104G00G90G54X1.47Y-.7A0.S5803M03

N106G43H44Z1.5M08

N108Z1.35

N110G01Z.55F100.

N112X1.5085F17.41

N114G41D144X1.47Y-.7588

N116G03X1.5788Y-.7Z.5679I.0385J.0588

N118X1.3601Z.6036I-.1093J0.

N120X1.581Z.6393I.1104J0.

N122X1.47Y-.639Z.6571I-.0722J0.

N124G01G40X1.5087Y-.7

N126X1.47

N128Z1.1214F100.

N130X1.5101F17.41

N132G41D144X1.47Y-.7766

N134G03X1.5966Y-.7Z1.1393I.0401J.0766

N136X1.3423Z1.175I-.1271J0.

N138X1.5988Z1.2107I.1282J0.

N140X1.47Y-.6212Z1.2286I-.0885J0.

N142G01G40X1.5103Y-.7

N144X1.47

N146Z1.35F250.

N148G00Z1.5

N150M05

N152G91G28Z0.M09

N154G28X0.Y0.A0.

N156M30

%

 

This is after I broke the geometry into four arcs.

(The same as a full circle)

[Toolfab]

Search for this in your post.

 

code:

---

 helix_arc   : 1    

---

Set it to 1 and you shoudl get code like this...

 

 

code:

---

 %

O0000

(PROGRAM NAME - ABRASIVESNC)

(DATE=DD-MM-YY - 05-04-04 TIME=HH:MM - 09:52)

N100G20

N102G0G17G40G49G80G90

(TOOL - 1 DIA. OFF. - 1 LEN. - 1 DIA. - .37)

N104T1M6

N106G0G90G54X0.Y0.A0.S1237M3

N108G43H1Z.25

N110Z.1

N112G1Z-.5F50.

N114Y-.0083F7.5

N116G3X.0183Y0.Z-.4861I.0073J.0083

N118X-.0192Z-.4583I-.0188J0.

N120X.0201Z-.4306I.0196J0.

N122X0.Y.0101Z-.4167I-.0125J0.

N124G1Y0.

N126Z.1F50.

N128G0Z.25

N130M5

N132G91G28Z0.

N134G28X0.Y0.A0.

N136M30

%

---

HTH

[Tim Johnson]

Paul,

 

I made the change from :2 to :1. no change.

 

Hey, I just noticed the your path is also 180 degree arcs.

[Toolfab]

code:

---

N116G3X.0183Y0.Z-.4861I.0073J.0083

N118X-.0192Z-.4583I-.0188J0.

N120X.0201Z-.4306I.0196J0.

N122X0.Y.0101Z-.4167I-.0125J0.

---

4 quadrants. This is the code that I use for my threadmilling. I have never had a problem.

 

you need to set your active teeth to what is actualy on your thread mill. So if its an 18 pitch, and its 6 flute, set your active teeth to 108. I know I get weird code if I dont do that.

 

::still thinking of why that didnt help you::

[Tim Johnson]

code:

 

N116G3X.0183Y0.Z-.4861I.0073J.0083

N118X-.0192Z-.4583I-.0188J0.

N120X.0201Z-.4306I.0196J0.

N122X0.Y.0101Z-.4167I-.0125J0.

 

Paul,

If the code broke into quadrants, you would get:

 

N118X0,Y,Z-,I-,J0

N120X-,Y0,Z-,I0.,J-

N122X0,Y-,Z-,I,J0.

N124X,Y0,Z-,J,I0. (WITHOUT CALCULATING)

 

But if that code works for you, then it will also work for me.

 

 

Thanks Paul.