Thread Mill cutting method

[BBprecise]

Is it me or does the way MC deals with multiple depths in thread milling backwards? I've only run across this a few times in the last 15yrs, but I have a part where the ID thread is longer than my threadmill cutter. Mastercam makes 1 360º pass at the bottom then jumps up about 10 threads then makes another 360º pass to thread the hole. To me wouldn't you want to do the top pass 1st then the bottom, just like you would when doing multiple DOC's on a contour path? Either way the tool has to be relieved, but doing the bottom pass 1st means the tool has full length engagement and causes taper which requires multiple passes to straighten out. I've always moved the cuts around manually in an editor to do this and I've run my program against MC's and with my way the tool lasts longer and requires fewer passes to make the thread. Granted this is moot with a single point tool, but milling a Ø1" ID thread that's 1-5/8" deep with a single point tool would be painstakingly slow process.

 

I've sent this suggestion in to MC a few times, but apparently nobody else has (or at least not enough to make the change). If I'm missing something and I can fix this in MC than please point me in the right direction, ignore my rant and .

[RonC.]

As for the number depth cut is control by the number of active teeth

 

as for starting top or bottom of thread is control by climb or conventional cutting of thread

[djstedman]

I don't use MC for thread milling, but I have to admit the method you have outlined sure seems to make sense in some circumstance.. I think it depends on the threadmill though perhaps, since mostly if I have a threadmill with lets say 5 teeth on it.. I want full engagement on all of those 5 teeth. If your using a threadmill with lets say 15 teeth but you only want to engage 5 at a time the method you suggest would certainly make more sense.

 

And RonC, I don't think hes talking about the direction of cut.. hes talking about the order of the passes.. regardless of whether its climb or conventional motion of the tool, when the cut is broken up based on the number of teeth on the cutter he wants it to always do the passes at the top of the hole first.

[Henk]

When you start with the bottom pass, and then up there are less problems with the chips in blind holes

[GoetzInd]

Yes the benefit of starting at the bottom is less chips to deal with on a blind hole. There should definitely be an option to go top down with order of depths.

 

Mike

[Newbeeee™]

Is it me or does the way MC deals with multiple depths in thread milling backwards? I've only run across this a few times in the last 15yrs, but I have a part where the ID thread is longer than my threadmill cutter. Mastercam makes 1 360º pass at the bottom then jumps up about 10 threads then makes another 360º pass to thread the hole. To me wouldn't you want to do the top pass 1st then the bottom, just like you would when doing multiple DOC's on a contour path? Either way the tool has to be relieved, but doing the bottom pass 1st means the tool has full length engagement and causes taper which requires multiple passes to straighten out. I've always moved the cuts around manually in an editor to do this and I've run my program against MC's and with my way the tool lasts longer and requires fewer passes to make the thread. Granted this is moot with a single point tool, but milling a Ø1" ID thread that's 1-5/8" deep with a single point tool would be painstakingly slow process.

 

I've sent this suggestion in to MC a few times, but apparently nobody else has (or at least not enough to make the change). If I'm missing something and I can fix this in MC than please point me in the right direction, ignore my rant and .

Rightly or wrongly, I agree with you 100%.

Yes climb from bottom up, but if you have a thread mill say 0.4 long, and you're producing a thread that's 1" long, starting at the very bottom 1" deep is putting a lot of load on the 'top' of the thread mill, where it's relieved on the shank.

So I would have thought you would want to step down from the top, but cut from the bottom of your step down up.

So yes I agree with you, although I've probably not explained myself very well...

 

BTW - What's your enhancement request number and I'll send it in as well for what it's worth.

[Guyinthedesert]

You could always just do it with 2 ops.

[BBprecise]

Ron, I understand what you're saying and you're right I would need multiple depths because my cutter isn't long enough and it's definetly faster to do it like MC does for DOC, but if you want to climb mill you have no way to start at the top.

 

Henk, if you do multiple radial passes (as most tool manufacturers recommend) the chip problem is still there so I don't see that as being a benefit. If there's going to be a lot of chips and not much room in the bottom of the hole I rough the threads to within .002 per side then put an M0 in the prg for the operator to blow the chips out (for blind holes) then go back to finish.

 

djstedman, if my length of tool engagement is short like your example I do like you do and leave full engagement. In this particular instance I need 1-5/8" of thread with a tool that only has 1-1/2" max cutting length, that's a lot of tool pressure especially for a Ø5/8 tool.

 

Just a quirk I've noticed that I think could use some improving, I'm not in any way bashing CNC Software.

[BBprecise]

Newbeeee, don't have a number.

[BBprecise]

Guy, yeah I could do it in multiple ops (would still have some editing to do though), but it would be an easy thing to fix I would think. Then again I don't write software code, but I do know the more code you have the more difficult it is to make a change without it screwing something else up.

[GoetzInd]

Ron, I understand what you're saying and you're right I would need multiple depths because my cutter isn't long enough and it's definetly faster to do it like MC does for DOC, but if you want to climb mill you have no way to start at the top.

 

He's talking about axial depth of cuts not radial. You would be taking multiple depths of bottom up climb milling going in the negative Z direction.

 

Mike

[RonC.]

BBprecise

 

okay I think i know what you getting at you like

to climb cut thread but instead at starting at the bottom of thread

you'd like to start at top of it like example seq. of pic below?

[BBprecise]

Ron

 

I'm not sure I understand your drawing right (probably just me being ignorant), so I attached a drawing similar to yours. I left my axis viewport on so you can see my Z axis for orientation. I want to start at 1 and thread Z+ for 1 revolution to 2 for my 1st cut. Then start at 3 and thread Z+ for 1 revolution to 4 and so on. With separate operations I could accomplish this but if I want multiple radial cuts (like threading on a lathe) I'd have to make even more operations which is time consuming. Maybe MC can implement this easily, I don't know.

 

For those that want to know my enhancement request number is D-08469.

[crazy^millman]

To get what you are after for now will probably have to old school it and draw the Helix. Break it up and then use Contour 3D and it should do it like you want.

 

Here is a sample file I what I am saying. I also attached the Threadmill file that I used to show this example with 5 days this download will be removed.

 

 

Edited:

 

Downloads removed. Email me for files.

Edited November 12, 2013 by Crazy^Millman

[BBprecise]

Millman, never thought of doing it that way. That'll get me closer to what I want than what I get now and will be less manual editing .

[jeff]

To get what you are after for now will probably have to old school it and draw the Helix. Break it up and then use Contour 3D and it should do it like you want.

 

Here is a sample file I what I am saying. I also attached the Threadmill file that I used to show this example with 5 days this download will be removed.

 

Seems like a lot of work.

Why not just write an incremental sub program by hand to get what you want?

[crazy^millman]

Make sure you use the chook arc3d to get a true Helix that will output the G3.

 

Jeff, I think you could easily make a custom drill cycle in Mastercam that would do the same thing. We sometimes think CAM is the only way, but I was doing kellering and Multi-Axis work for 10 years before I ever had a CAM system using Macros and Ratios.

[amw]

Still no way to do this properly in 2024? 

Im using a fairly big threadmill, getting a little chatter, would be nice to be able to break it into two depths. 

[JParis]

14 minutes ago, amw said:

Still no way to do this properly in 2024? 

What threadmill?   You have been able to do it for a couple decades...

Reduce your number of teeth...though I would suggest using multiple stepovers instead...

Sample file - Bottom to Top and the same tool Top to bottom

THREADMILL SAMPLE.mcam

[amw]

4 minutes ago, JParis said:

What threadmill?   You have been able to do it for a couple decades...

Reduce your number of teeth...though I would suggest using multiple stepovers instead...

We are machining 2" NPT 11.5 TPI. The tool is 5/8 diam solid carbide with 12 teeth. There is a lot of engagement with this tool, would be more efficient if I could do it in 2 depths with slightly larger stepovers. 

If I reduce the number of teeth yes it will do 2 passes, but starts with the bottom which is useless in my case. Same problem as the original poster had here over 10 years ago. 

[JParis]

Just now, amw said:

If I reduce the number of teeth yes it will do 2 passes, but starts with the bottom which is useless in my case. Same problem as the original poster had here over 10 years ago. 

Check out my sample file above

[amw]

10 minutes ago, JParis said:

Check out my sample file above

Thank you for the example, but this forces me to use conventional milling. I would prefer to use climb milling, bottom to top motion, but break it into 2 depth cuts, first one being on top. You would think this would be fairly logical way to do NPT threads.

[Chally72]

AMW, I'll pass this thread on to the product owner.

Just a note that 2025 has received a bevy of Thread milling enhancements developed in concert with tooling manufacturers. Check out the Gradual entry on the lead in/out page to reduce shock load on engagement and the expanded entry/exit controls and speed/feed overrides, among others. Spindle direction is also now considered when displaying cut direction in the Machining direction box.

Here's the full list of changes:
Mastercam 2025 – Thread Mill Updates – myMastercam

 

[bird2010]

1 hour ago, amw said:

Thank you for the example, but this forces me to use conventional milling. I would prefer to use climb milling, bottom to top motion, but break it into 2 depth cuts, first one being on top. You would think this would be fairly logical way to do NPT threads.

I don't understand English and can't understand the meaning...Is this so?

But in this case, the wear of the tool will be concentrated on the front end of the tool....

[riverhunter]

3 hours ago, Chally72 said:

AMW, I'll pass this thread on to the product owner.

Just a note that 2025 has received a bevy of Thread milling enhancements developed in concert with tooling manufacturers. Check out the Gradual entry on the lead in/out page to reduce shock load on engagement and the expanded entry/exit controls and speed/feed overrides, among others. Spindle direction is also now considered when displaying cut direction in the Machining direction box.

Here's the full list of changes:
Mastercam 2025 – Thread Mill Updates – myMastercam

 

 

This is long over due, but welcomed.  Any chance this will roll into the regular contour paths?  it would be extremely helpful to optimize feed rates in corners while maintaining the actual programmed feed rate.  I know this can be done locally, but it is a real PITA and should be handled inside MC.