geometry for thread milling

[Duece06]

when creating the circle for thread milling (external thread) should the dia be the major dia of the thread and use the over cut for the thread depth? This is the way I have a part programmed, I put in the thread depth in the over cut but it's on cutting to approx. half the depth. This makes me curious as to whether I should use a circle that is the minor dia of the thread and have no value in over cut. 

 

[jlw™]

Use a point as geo then type your thread OD in the dia. box.

[Duece06]

Cool! I couldn't figure out how to get that box to activate. As I said I had been choosing a circle, which I guess it took the dia of the circle to set the od of the thread. Thank you again!

[gcode]

you can also draw a circle to the minor diameter of the thread and select it as an entity

the threading toolpath will drive to that OD

[crazy^millman]

Both ways mentioned above the the normal way, but sometimes I will use a Helix of the thread like we did well before threadmilling was introduced as an operation. 3D contour to drive it and turn off infinite look ahead. Last thing and yes I agree completely weird you have to do this, but you have to alt-c and use the arc3d chook to get helix moves for this toolpath. Will also have to ignore the weird looking toolpath. Backplot the toolpath and you will see the weird stuff is just Mastercam freaking out. Here is an example where I don't like the threadmill operation. Reason being I want the tool to cut the threads in one pass not jump up and start a new set of cuts.

 

The other place this process is good is where you have to time the lead of the thread to a specific detail. I will use this a lot when doing Mill/Turn parts where the exact start of the thread must be between a certain angle or the pitch must intersect a certain feature.

 

HTH

 

https://www.dropbox.com/s/407fxetsvzqm6bn/5th%20Axis%20thread%20mill.mcx-9?dl=0

 

 

[BenK]

Use a point as geo then type your thread OD in the dia. box.

I got burned using a arc to drive my threadmilling operation and now I always use a point. Much simpler if you ask me. Enter the value in the toolpath and your done.

 

 

As for the original poster, is it your thread crest to root distance only cutting to half depth or the overall thread depth going half way?

[crazy^millman]

I got burned using a arc to drive my threadmilling operation and now I always use a point. Much simpler if you ask me. Enter the value in the toolpath and your done.

 

 

As for the original poster, is it your thread crest to root distance only cutting to half depth or the overall thread depth going half way?

 

Ben that is my preferred method. Sort of a checks and balances for the programmer that they are making the thread to the correct size. I have also been bitten by that ad helps me make sure I have everything like I need it. Also with not having Absolute abilities in the threadmilling cycle having the point at the bottom of the hole allows me to know that my Thread milling is to the depth I want it to be without having to do some math. Do a bunch of 5 Axis Thread milling and you found one way that works and you go from there. Hole Axis with Points and lines for your drilling and then the same for your Thread milling and you never make the mistake of picking an arc for one thing and the point for another.

[jean]

THIS IS VERY EFFECTIVE.. THANKS