THREAD MILLING ADVICE

[paulfell]

I have to thread mill a small external dia. (10 x 32 UNF -0.27'' deep) - I have done only limited thread milling before , I am going to mill full depth in one pass (i.e. 360 degrees with Z-.0312'' (pitch) ) should i go straight to finish size, with a couple of spring cuts or work in (i.e. multipass ) from a larger diameter, I will be ok with Mastercam side of things - its just strategy I am not sure of - any advice appreciated

[Reko]

Yes, take multiple passes.

 

You didn't mention material, but if aluminum, 2 equal rough passes and a spring cut... steel,  prolly 3 or 4 equal passes with 1 spring cut.

[Guest]

Aluminum at that size, I will cut in 1 pass everyday

[jlw™]

Yep, depends on material and what type of threadmill. If your using a "one toother" you can usually take a heavier cut than if your using a multi tooth inserted cutter. I prefer the single tooth every time.

[paulfell]

Using multi tooth on  heat treated steel - so pretty tough stuff , did full depth - 3 multipass type cuts and 2 spring cuts - done 5 so far - working really well (so far) - thanks

[BCW]

Check out Harvey tool speed and feed chart, they include stuff like recommended passes and feed calculations for internal & external threads. Should have everything you need to get started.

http://www.harveytool.com/secure/Content/Documents/SF_54200.pdf

[jeff]

Yep, depends on material and what type of threadmill. If your using a "one toother" you can usually take a heavier cut than if your using a multi tooth inserted cutter. I prefer the single tooth every time.

Yes but then you need to spiral the entire length of the thread.  Assuming you're referring to single point and not an inserted threadmill.

[crazy^millman]

Yep, depends on material and what type of threadmill. If your using a "one toother" you can usually take a heavier cut than if your using a multi tooth inserted cutter. I prefer the single tooth every time.

 

Also takes a lot longer and will not deburr the ID of the thread like the correct Multi Flute threadmill will. Better quality and faster run time it my choice every time, unless I have no choice and have to use a single tooth style threadmill.

[paulfell]

Having used multi tooth now - i think the benefits outweigh the single tooth ( that is all i had used previously)

[paulfell]

Also a good site ( re- Harveys) is http://www.guhring.com/Tech/ThreadMillCNC/CNCGenerator/ - obviously the code is not needed with Mastercam - but still an excellent tool for speeds/ feeds etc.

Using Mastercam (X8) to create code - I used a lead in/ out - I wanted to go 7mm deep - but it didnt reach this depth until the end of lead out - I wanted it to go to that depth before the lead out - is there an easy way to do this ?

[jlw™]

Vardex has some great threadmilling info too.

 

Did you use perpendicular entry? It'll go to depth then straight to center. As long as you don't change the start point you can go back in the same hole.

 

I usually program 1xpitch deeper to make sure I get depth.

[crazy^millman]

To get exact start and ends with threads it is best to use Helix with a 3D contour. Have to remember the bug in Mastercam that ignores make 3D arcs out of the contour and use the chook ARC3D for the toolpath then you are good to go. I use this when I want to take a multi-flute tool and use it for a longer thread, but not get the jumping threadmill does. Need to also remember to turn off look ahead or you will only get one pass like a threadmill operation. Have done a lot of timed threads to features and this is my go to method for controlling that. Many years wrote this stuff by hand. I had Macros for just about every machine I used until I got into Mastercam.