CAMWorks Thread Milling Question

[Pete Deal]

I have a thread to cut- I never did any thread milling before. It is m10x1.25 in 4140ph- about .5" deep. Seems to me that cutting this in one pass is too much looking at the harvey tool speeds and feeds it looks like they are saying 2 passes with about .0015 cut per tooth.

I can't seem to make CAMworks do more than one pass- I tried specifying the cut amount, final cut amount, even adding a spring pass, and still it just generates one pass- simulation only I have not run it. Can anybody suggest what I am doing wrong?

 

[Shawnrs]

I have a thread to cut- I never did any thread milling before. It is m10x1.25 in 4140ph- about .5" deep. Seems to me that cutting this in one pass is too much looking at the harvey tool speeds and feeds it looks like they are saying 2 passes with about .0015 cut per tooth.

I can't seem to make CAMworks do more than one pass- I tried specifying the cut amount, final cut amount, even adding a spring pass, and still it just generates one pass- simulation only I have not run it. Can anybody suggest what I am doing wrong?

Change your multi-point threading to single point under the thread parameter page. On your tooling page you may need to change the pitch to .049, this should give you multiple passes.

 

[AARONT]

You need to specify a previous allowance so the software knows how much material is left to remove.

Don't change a multipoint threading program to single point. This defeats the purpose of using a multipoint thread mill.

 

[rainman]

Try making your prev. allowance .024, and your cut amount something less than that. Play with the cut amount until you get what you want. Add spring passes if necessary.

 

[Pete Deal]

Thanks all! I will try the prev. allowance- which I have not done. My intent is to use a single point tool since it is only 75 shafts so it seemed sensible to use the cheaper tool that would have more future utility with other thread pitches.

Basically it is a lathe part with a tapped hole in the end and some flats on the end diameter. My idea is that since I need to put the part in the mill anyway, no live tooled lathe, I may as well thread mill the hole and avoid blind hole tapping. Is this sound thinking or am I over thinking this?

 

[Chris59]

I made up an Excel 2010 spreadsheet to help me with this. Used as reference a Scientific Cutting Tools page about programming threadmills.
Not sure the zip file worked.

 

[Chris59]

Ummm...any errors are mine. Don't blame SCT.

 

[Pete Deal]

Rainman: That was it! Prev alloance set to .024 gave me two cuts. I misunderstood how this is used.
Thanks all!

 

[rainman]

Great! I arrived at .024 by the radial difference between the minor and major. You can get more than 2 cuts if you make your cut amount to be less than half of that. For example, if you make cut amount .008, you should get 3 cuts. You can also call for a light last cut, if you like. The settings button in any contour mill operation has this same kind of options to generate multiple side passes.

 

[Dan from Oakland]

You don't mention it but I'm thinking this should be milled from the bottom of the thread to the top so you don't pack chips down the hole. Not sure if the Harvey tool stuff addresses that or not.

 

[Pete Deal]

The tool path is generated that way- bottom to top.

 

[rainman]

ID, right hand thread, climb mill = bottom to top
Change one of these parameters and it will be top to bottom.

 

[Revelstone]

I have a thread to cut- I never did any thread milling before. It is m10x1.25 in 4140ph- about .5" deep. Seems to me that cutting this in one pass is too much looking at the harvey tool speeds and feeds it looks like they are saying 2 passes with about .0015 cut per tooth.

I can't seem to make CAMworks do more than one pass- I tried specifying the cut amount, final cut amount, even adding a spring pass, and still it just generates one pass- simulation only I have not run it. Can anybody suggest what I am doing wrong?

I have NX software I make models, program and make process drawings with it. If I program a treadmill I do it by manual good old fashion math. That way I can do whatever I want how I want and I am not a slave to some software program.

 

[gregormarwick]

I have NX software I make models, program and make process drawings with it. If I program a treadmill I do it by manual good old fashion math. That way I can do whatever I want how I want and I am not a slave to some software program.

That's ridiculous.

It's threadmilling, hardly rocket science. If you can't get your cam to do it properly then you either have useless cam (you don't) or you don't know how to use it.

Don't advise people not to bother learning their cam properly just because you haven't bothered to learn yours.

 

[Pete Deal]

Once i got the parameters figured out it worked great! The threads were 10mmx1.25 in 4140ph for about 85 parts about .6" deep blind hole. I chose to use a single point cutter. Which was stupid in hind site but chose it because it was the cheapest option and I sort of figured I'd screw a few up maybe since it was my first attempt at thread milling. It also seemed like the cutter might get some additional use someday more so than a multi-tooth cutter. I got about 60 parts before I changed cutters because the tip got a little worn. So, even though it was much slower than it should have been it worked great, threads looked great.