Question Regarding Thread Milling

[Italiano83]

So I'm pretty new to thread milling, but I believe I have my program correct and I have still been breaking thread mills. The scenario is like this: 304 SS Material, Internal Thread, 9/16-18 Thread Size, Thread Mill Multi-Tooth Solid Carbide

Now before the tool breaks, which happens every few parts the thread comes out PERFECT. The reason I believe the tool may be the problem and not the program is that the tool needs to stickout a bit more than I would like to reach the area to be threaded. I have a feeling a solid carbide tool is the problem. I believe the tool pressure exerted on the brittle carbide tool is the issue. I'm thinking of switching to a hardened steel holder with removable carbide inserts to overcome this issue.

Has anyone had similar problems? I just feel a solid carbide ID thread mill is not ideal for this type of operation with forces along X-Axis of the tool.

Any comments regarding this would be helpful. Thanks, -Jon

 

[DMF_TomB]

So I'm pretty new to thread milling, but I believe I have my program correct and I have still been breaking thread mills. The scenario is like this: 304 SS Material, Internal Thread, 9/16-18 Thread Size, Thread Mill Multi-Tooth Solid Carbide

Now before the tool breaks, which happens every few parts the thread comes out PERFECT. The reason I believe the tool may be the problem and not the program is that the tool needs to stickout a bit more than I would like to reach the area to be threaded. I have a feeling a solid carbide tool is the problem. I believe the tool pressure exerted on the brittle carbide tool is the issue. I'm thinking of switching to a hardened steel holder with removable carbide inserts to overcome this issue.

Has anyone had similar problems? I just feel a solid carbide ID thread mill is not ideal for this type of operation with forces along X-Axis of the tool.

Any comments regarding this would be helpful. Thanks, -Jon

.
i often adjust tool diameter comp and rough out the threads.
.
then put tool dia comp back to normal to finish the threads. often hard to do threads all at once

 

[Finegrain]

Program multiple passes. Threadmills tend to have a high engagement since the cutter size is close to the hole size -- get in, get out, don't dwell in the cut. Also make sure you're blasting the chips out of the hole, as any recutting will likely lead to a little kaboom.

Regards.

Mike

 

[Bobw]

I can guarantee the fact that its a carbide tool is not the problem.. Actually 99% chance that
its not the problem..

If breaking endmills (threadmill), the first place to look is too much feed..

How are you programming it? If you are programming centerline, the actual chipload is going
to be approximately 5X what your programmed feed is.

What are your speeds and feeds??

 

[DMF_TomB]

if you got a slot to make 1" deep and 1" wide do you mill it in one pass or take multiple passes ??
.
thread milling not much different. if not programmed to take enough multiple passes i just adjust tool comp and rough it out first then put tool comp back to normal and rerun it

 

[Italiano83]

I can guarantee the fact that its a carbide tool is not the problem.. Actually 99% chance that
its not the problem..

If breaking endmills (threadmill), the first place to look is too much feed..

How are you programming it? If you are programming centerline, the actual chipload is going
to be approximately 5X what your programmed feed is.

What are your speeds and feeds??

1700RPM
Entry 6 in/min
cutting at 150 in/min in circular interp mode

 

[doug925]

1700RPM
Entry 6 in/min
cutting at 150 in/min in circular interp mode

1) How many cuts to full thread depth?
If you are trying to get it in 1 pass, that IS the problem. You will need at least 2 passes (maybe even a 3rd) to cut the thread reliably.

2) Double check your feedrate. Like Bob said, linear feedrate is MUCH different than interpolated feed.


Doug.

 

[athack]

We use Allied Machine and Engineering thread mills and their free software to generate the code. Works great everytime and have neve broke a thread mill. Ussually has multiple cuts, 50% then 85% then the rest.

 

[Bobw]

.088" per rev.... There is your problem.

 

[G00 Proto]

All in one pass... at 150 in/min. That's pretty aggressive for a multi tooth cutter, especially with that course of a thread (deep threads). Not to mention the fact that you may be having control issues. Depending on your post and cam setup, there maybe a lot of code to make that simple threaded hole and you machine may be starving for data and stuttering.

I would take it in two passes, or slow it down by 50% and see if that cures it. I should mention that I prefer single tooth threadmills. They are definitely slower, but I seem to have fewer problems such as these and they are much cheaper and more versatile.

 

[Larry Dickman]

150 ipm? I hope that's a typo

Where are your tools breaking?

 

[sinha]

If you are programming centerline, the actual chipload is going
to be approximately 5X what your programmed feed is.

Can you please explain it? Wherefrom the 5X figure comes?

 

[Bobw]

Can you please explain it? Wherefrom the 5X figure comes?

We have a .450" tool cutting approximately a .570" diameter hole (thread)..
(#s chosen so they are close and easy to work with)..

Say you are feeding 10 inches per minute.. The centerline of your tool is traveling at
10 IPM, but it is only making a circle with a diameter of .120.. Approximately 0.4" of travel
(.377).. It makes that circle in 2.5 seconds... The outside of the tool cutting the .570
diameter/thread makes that circle in the same 2.5 seconds, but it is traveling 1.8". 4.5X
(5X was a pretty good guesstimate) the actual programmed feed. So your chipload is 4.5X
what you actually programmed.

Its something you need to take into consideration when milling holes. 1/2" tool in a 1" hole,
2X... 1/2" tool milling a 10" hole, its negligable. .450" tool in a 9/16 hole, it becomes a whole
lot more important. This can also bite you in the ass running small arcs in corners.

If you are running full tool diameter/radius comp, some machines are smart enough to alter the
feed, some machines aren't.

 

[Matt@RFR]

Or you could just do the math yourself. Plug this in to a spreadsheet for quick (and accurate) thread mill feedrates.

ID -- Nominal IPM * (minor dia - cutter dia) / minor dia = adjusted feedrate
OD -- Nominal IPM * (major dia + cutter dia) / major dia = adjusted feedrate

I also second the fact that this issue is not because the tool is carbide. The whole "carbide is brittle and doesn't bend" thing is taken way too literally by most. All extended reach endmills I've ever used or seen has been carbide.

 

[doug925]

Or you could just do the math yourself.
ID -- Nominal IPM * (minor dia - cutter dia) / minor dia = adjusted feedrate

This!!!
Do this ANY time you are interpolating a bore. When the bore is within 2-3x of the cutter diameter, you will need this formula.

Doug.

 

[DMF_TomB]

We have a .450" tool cutting approximately a .570" diameter hole (thread)..
(#s chosen so they are close and easy to work with)..

Say you are feeding 10 inches per minute.. The centerline of your tool is traveling at
10 IPM, but it is only making a circle with a diameter of .120.. Approximately 0.4" of travel
(.377).. It makes that circle in 2.5 seconds... The outside of the tool cutting the .570
diameter/thread makes that circle in the same 2.5 seconds, but it is traveling 1.8". 4.5X
(5X was a pretty good guesstimate) the actual programmed feed. So your chipload is 4.5X
what you actually programmed.

Its something you need to take into consideration when milling holes. 1/2" tool in a 1" hole,
2X... 1/2" tool milling a 10" hole, its negligable. .450" tool in a 9/16 hole, it becomes a whole
lot more important. This can also bite you in the ass running small arcs in corners.

If you are running full tool diameter/radius comp, some machines are smart enough to alter the
feed, some machines aren't.

tool .450 dia ?
what is tool dia comp .450 or small like wear comp of .001 ??
small I and J in gcode is a sign of wear comp and actual feed at tool circumference is faster than feed rate at center of the tool

 

[sinha]

1/2" tool in a 1" hole, 2X... 1/2" tool milling a 10" hole, its negligible.
.450" tool in a 9/16 hole, it becomes a whole lot more important.

Thanks for explaining the way Bill does!
It is not always 5X. That is what I wanted to confirm.

Edit:
I would write this formula as
Programmed feedrate = (ID - cutter dia)/ID x Cutting feedrate

 

[WABOOM]

Here's a pic of what I'm doing. Material is 316 , thread is 9/16-18

 

[Italiano83]

Here's a pic of what I'm doing. Material is 316 , thread is 9/16-18

That's an awesome place for me to start, also taking into consideration the other comments. Thank You.

 

[rcaffin]

So I'm pretty new to thread milling, but I believe I have my program correct and I have still been breaking thread mills. The scenario is like this: 304 SS Material, Internal Thread, 9/16-18 Thread Size, Thread Mill Multi-Tooth Solid Carbide

Now before the tool breaks, which happens every few parts the thread comes out PERFECT.

Just for the moment, forget all about the exact feed and spin figures. Pick up a thread mill in your fingers and give the end a poke. Hard little beggar, isn't it? And yet you are breaking it. Doesn't that suggest that the forces you are putting on it must be crazy high?

As many have said: your spin is too low, your feed is too high, your chip size is too high and you are probably not clearing the chips out of the hole. That poor thread mill! I use 3 passes, even on aluminium.

Cheers
Roger