Threadmill NPT

[Thoob]

Hi guys, I'm having a little issue here trying to get my mill to cut Internal NPT threads properly. To start off I want to say what I drew my geometry at. Its for a 1"-11.5 NPT The top of the hole is drawn at 1.175 and it tapers down at 1.7833 degrees. This part is no problem. The threadmill is a custom tool. I verified the diameter and it is correct when backplotting. I have the threadmill geometry set at "entity" and selected the 1.175" chain. I have .059" in the allowance overcut parameter. Run the part, its undersize. I had to adjust .039" in my compensation per side to get to the proper depth. This tells me that the tool is defined bigger than actual size and therefore cutting undersize however as mentioned, I verified that the tool is at the right diameter when backplotting. Problem with checking everything is the fact the thread is tapered. Any ideas what I'm doing wrong? Anyone who does NPT's on a mill, can you let me know how you do it? Thanks.

 

I have a zip2go available if someone wants to check it out for me.

[Matthew Hajicek - Singularity]

I do these all the time. According to my chart you should set the thread major at 1.315".

[Matthew Hajicek - Singularity]

Here's the chart that's been working for me:

 

http://www.fairburyfastener.com/xdims_pipe_threads.htm

 

Use the numbers in column 2.

[Thoob]

I have the geometry drawn at 1.175

The Major if you add the thread depth comes to 1.293.

.059 for thread depth x 2 = .118 plus 1.175 = 1.293.

I got that number from ThreadPal.

Column 2 on your chart only states what the OD is on the pipe. It doesn't give any indication of what the geometry should be drawn at, which isn't the problem anyway. I have to figure out why the thread is cutting so small.

[Robert Ouellette]

are you using the diameter of the cutter at the tip? that's the size you have to use. when I draw out my cutters that way I am within .010" of good size. I am assuming if you made a custum tool that's what you did. but you never know.

[Thoob]

Not exactly sure what you mean by tip. The cutter diameter is .854. Obviously the cutter is not perfectly sharp. If I draw it to be sharp(assuming this is what you mean), then the actual diameter of the tool would be wrong?

[Thoob]

The tool is scaled to 1" Radius. When I bring the tool in as custom, it is defined as .854"

I don't know what else I could be doing wrong. When I use the tool for a straight thread, it comes out fine.

[Matthew Hajicek - Singularity]

I do draw the custom tool profile, and use the diameter at the tip (the diameter of the thread form closest to the tip). That's the cut diameter that the cutter manufacturers specify. I've been using column 2 as the major, and we're checking the holes with gauges, and they're coming out. I never use a circle as geometry, I always use a point and specify diameter by number.

[Matthew Hajicek - Singularity]

Not exactly sure what you mean by tip. The cutter diameter is .854. Obviously the cutter is not perfectly sharp. If I draw it to be sharp(assuming this is what you mean), then the actual diameter of the tool would be wrong?

 

Are you using a tool with only one threadform? If so, use the actual diameter of that threadform. If it's more, like mine which have about a dozen arranged at the proper taper, use the diameter of the threadform closest to the tip.

[Thoob]

I still don't fully understand what you are saying. The tool is one threadform. It does a range of 12-24 TPI. I know the NPT in question is 11.5 TPI and I have adjusted the depth to compensate for it.

I double checked the tool and it is drawn to a point (my mistake from my earlier post) So from the center of the tool to the "tip" of the tool is measuring .427"

The other issue here is that I cut a straight thread shortly after I did the NPT and the offset only needed to be adjusted .006. So this tells me the tool is defined properly. I am wondering, do I have a mistake in the thread depth? What is the Single Depth for a 1"-11.5 NPT?

 

 

EDIT - I assumed it was .059. This apparently is not correct according to a few charts I looked at. Assume we use your number from Column 2 which says 1.315 and that the pipe face (md) is 1.1725 (this is correct for this 1" NPT thread), then that makes my single depth .071. If I minus .059 from that, it gives me .012 difference. This is ok however I was originally .039 out so this still leaves me with .027 of unknown. lol. This is ridiculous.

[gcode]

Draw a circle Ø1.308"

define your tool as an endmill with the diamater = to the bottom of your thread hob

It won't give you pretty eyecandy in Verify.. but it will give you good gcode

 

see the zipped mcx-6 file

1IN-NPT.zip

[Thoob]

Ok. See that is where I was different. I don't draw the MD like that. I actually drew the md and then added a number in the overcut allowance.

I did it with an endmill as you suggested vs the way I did it, and its funny the code is indeed different. Does the allowance overcut actually work different than how I think it does?

The way I drew the 2 was the 2nd side like you said, then the first side by drawing the pipe face(md) 1.175" and then putting an overcut of .0665. This technically should equal the same 1.175+.0665+.0665 = 1.308 but the code it outputs is different. See picture.