[Zygoat]

not sure if this is the right section, if not mods feel free to move me.

i am having trouble with some thread milling. i cut the threads (external( the program runs fine, the machine cuts fine, the threads are beautiful. the only problem is that the off the shelf nut does not fit. lets just say for example i am cutting 1 3/8 unf 2a.

i am using a treadmill just like this one
http://cdn.mscdirect.com/global/imag...4023293-23.jpg

the tool is set up correctly and appropriate for the threads i am trying to cut.

i am pretty sure i am just missing something when i program the cut. i am using mastercam. and running on a haas vf3

i set the tool path to cut a dia. of 1.2739 and i cut the od of the thread to 1.370. is there something i am missing? i can get the threads to fit perfectly, but i ususaly have to end up taking around another .030 off of the cut dia. 1.2739 down to something like 1.2439. at which point the off the shelf nut fits beautifully, but i should not have to do this. it seems like i am missing something. hopefully someone can point it out to me. my guess is that is has something to do with the fact that the thread form is supposed to be square on the inside, and the cutter i am using is pointed. so perhaps i have to cut deeper by the distance of the square thread form to the point of my cutter?

thanks in advance for any help

[Superman]

You seem to be doing things correctly.......at least it's not undersize

Threads are controlled by the pitch diameter, are you setting the cutter using a pitch mic. ??
- what cutter you use to create the thread form is fairly critical, where the tool that you have selected may be "multi-functional" to suit many different threads ( small root rad on vee )

What may be an issue is the radius on the cutter being smaller than specified for that thread form
- thus, your tool description in Mastercam should be a smaller OD ( allowing for a larger root radius on the Vee )

[Zygoat]

first off, thanks for your response.

i think i know what you are talking about, but is there any chance you could link to a picture about the radius? i am a visual person and just want to be on the same page.

i think this is what you are talking about.

http://upload.wikimedia.org/wikipedi...nsions.svg.png

i am currently setting the cutting dia. to Dmin in this picture.

and i think you are talking about the radius shown for clearance right there as well? this is my suspicion as well, however the tool i have has a sharp point (no radius on the vee( so i believe that i need to set it to cut Dmin - H/4 in this picture. what do you guys think?

[mountaindew]

Looking at above info it looks correct using stock constants for thread depths
for external threads 0.61343
for internal threads 0.54127
Using the above numbers a thread pitch of 1/12 = .08333 x 0,61343=0.05109
0.05105 x 2 sides of diameter = 0.10219
1.375- 0.10219= 1.2728
Im currently learning this math myself and figured I would post a break down
md

[Kingjamez]

As stated above, the single point thread mills have a sharp V where UN threads need a radius. I made a youtube video a while back showing the math and how to make the required adjustments to get a good thread the first time.

https://www.youtube.com/watch?v=rRzCDZt8ZsY

-Jim

[Superman]

first off, thanks for your response.

i think i know what you are talking about, but is there any chance you could link to a picture about the radius? i am a visual person and just want to be on the same page.

i think this is what you are talking about.

http://upload.wikimedia.org/wikipedi...nsions.svg.png

i am currently setting the cutting dia. to Dmin in this picture.

and i think you are talking about the radius shown for clearance right there as well? this is my suspicion as well, however the tool i have has a sharp point (no radius on the vee( so i believe that i need to set it to cut Dmin - H/4 in this picture. what do you guys think?

You are on the right track.
these threadmill tools are generally made to make an internal thread, so they usually create a root radius to suit a wide range of thread forms for internal threads.
- but as per your pic, the root rad of an internal thread is a lot smaller (H/8), when compared to an external thread (H/4)......2x the size
---- remember that this area of a thread gives it the strength. So making an external thread with a small rad will reduce it's strength.

Plus when using a CAM system in this manner, you would have to allow the tool to have an "overcut" value.....being the difference of the 2 root radius values
- you would have to draw it on CAD to see what value may have to be input.