What's new
What's new

Thread Milling Issue

Masczek

Plastic
Joined
Nov 20, 2023
I'm thread milling various ID threads (1/2x28 to 13/16x16) and the all have the same problem. When I'm testing the thread fit, the test parts will screw in 2-4 full rotations and then the threads get tight until you can't thread the test part on any further. This is with all threads I'm machining. I've checked the run out on my tools, I'm doing multiple spring passes, and I've check and verified the minor diameter, thread pitch in the program is fine, everything checks out okay. I'm running out of ideas, hoping some of you might shed some light on it. I've got only one thread mill I'm doing these jobs with, so I don't know for sure if it's the thread mill or not. I've also checked my programing to see if it's threading some sort of tapper, everything looks normal (using Fusion 360.)

Let me know if there is anything else I can try. Thanks!
 
Make sure your comp is set to "wear" in the passes tab. You'll most likely need to comp negative at your machine to remove more material.
 
Last edited:
I've got only one thread mill I'm doing these jobs with, so I don't know for sure if it's the thread mill or not.
This may be your issue. The thread pitches you mentioned are from 28 down to 16. A single-point thread mill can only cover a few sizes due to the flat area at the tip that cuts the root or minor diameter of your parts. If you're using too blunt of a cutter or too sharp of a cutter, the pitch diameter won't be in the proper location on the part. Also: Metric thread form is round at the root while SAE is flat at the root. The kind of cutter you're using will affect all of this.

To get a 100% correct form, you probably need a purpose-ground cutter for each pitch. Second choice would be a single-point for that particular pitch and standard (SAE or Metric).
 
Both blind and through holes, threads have the same problem.

I've tried both modeled and un-modeled threads, same issue regardless.

I'll give "wear" a try, but it doesn't make sense that I was cutting threads just fine until recently. Maybe the thread mill is wearing out?

I've had this thread mill for awhile now, but I'd be surprised if it's already wore out, I wouldn't have guessed I would have used up the thread mill by now. I haven't cut that many threads yet, or so I thought.
 
This may be your issue. The thread pitches you mentioned are from 28 down to 16. A single-point thread mill can only cover a few sizes due to the flat area at the tip that cuts the root or minor diameter of your parts. If you're using too blunt of a cutter or too sharp of a cutter, the pitch diameter won't be in the proper location on the part. Also: Metric thread form is round at the root while SAE is flat at the root. The kind of cutter you're using will affect all of this.

To get a 100% correct form, you probably need a purpose-ground cutter for each pitch. Second choice would be a single-point for that particular pitch and standard (SAE or Metric).

Great point! You might "Shank Out" the cutter before you can get a good thread on that 16 pitch.
 
Both blind and through holes, threads have the same problem.

I've tried both modeled and un-modeled threads, same issue regardless.

I'll give "wear" a try, but it doesn't make sense that I was cutting threads just fine until recently. Maybe the thread mill is wearing out?

I've had this thread mill for awhile now, but I'd be surprised if it's already wore out, I wouldn't have guessed I would have used up the thread mill by now. I haven't cut that many threads yet, or so I thought.

Yeah, thats the purpose of wear comp.

if the tool has a finer point in the root of the thread they will wear out faster than if it has a radius or small flat but like Donkey said, the same single point threadmill might not cover both pitches properly.
 
When I've had that kind of fit, it's usually been a pitch error. If you can, measure the pitch on both the part you're making, and the mating part you're fitting to, and see if there's a difference.

It's also possible that you have some taper; a multi-form threadmill will deflect a bit more with more forms engaged, making the thread a bit smaller at the bottom. More skim passes can rectify this.
 
This problem is with 16 TPI, 24 TPI, 28 TPI and so on. It happens regardless of the threads I'm cutting. I guess I don't understand that I can be the tool if it's cutting the first 3rd of the threads just fine and the last 2 thirds too tight. Tool pressure should be the same from top to bottom should it not? Besides, if I thread mill top to bottom or bottom to top it still cuts a "tapered" thread.
 
When I've had that kind of fit, it's usually been a pitch error. If you can, measure the pitch on both the part you're making, and the mating part you're fitting to, and see if there's a difference.

It's also possible that you have some taper; a multi-form threadmill will deflect a bit more with more forms engaged, making the thread a bit smaller at the bottom. More skim passes can rectify this.
I've tried multiple skim passes, both with coolant and without, no dice. I did notice that when cutting a skim pass dry a little bit of material is being removed throughout the entire thread length, not just the bottom. So it's taking the same amount of material off for the entire thread.

I should have mentioned, I'm using a single profile thread mill:
 
Try wear if you were getting good threads before but I'm sticking to Donkey's comment. One tool won't cover that entire range of pitches properly. You MAY be able to make a functioning thread but it probably won't be a proper thread.
 
To follow up on roundness, is it possible you're getting a taper in the hole during interpolation?

Also, what are you checking these with? It's multiple thread sizes so I wouldn't think that could be the problem but stranger things have happened.

What machine?
 
You are using a "test part" instead of a thread plug gauge? Not a great idea that. Maybe the test parts are not good. How do you know if the pitch diameter is over high limit without a not go gauge? Could it be you are running the thread too tight to the test part? Then any little thing might cause an issue. Get proper gauges and open up the PD closer to high limit. You've probably already wasted enough time to pay for a few.

Will the thread gauge from the bottom side only a few threads also? If it does you likely have lead error.

Since it is a single pitch tool it seems very unlikely a dull tool is causing a tapered thread. A multi-pitch tool will easily create a tapered thread when dull.
 
You are using a "test part" instead of a thread plug gauge? Not a great idea that. Maybe the test parts are not good. How do you know if the pitch diameter is over high limit without a not go gauge? Could it be you are running the thread too tight to the test part? Then any little thing might cause an issue. Get proper gauges and open up the PD closer to high limit. You've probably already wasted enough time to pay for a few.

Will the thread gauge from the bottom side only a few threads also? If it does you likely have lead error.

Since it is a single pitch tool it seems very unlikely a dull tool is causing a tapered thread. A multi-pitch tool will easily create a tapered thread when dull.
THIS, I couldn't agree more. I need to start investing in the proper tools, it's a never ending list...

The test parts are provided by the customer. I found out this evening that the test part is 49/64x16, while the threads I machined are 13/16x16, which was also on the model provided by the customer. So that answers most of my question, 49/64x16 won't thread into 13/16x16 lol.

That being said, I'm still a little stumped on why the 5/8x24 and 1/2x28 threads have the problem I described above. However, I've got a handful of things to try tomorrow now that I have the proper thread dimensions.
 
I'm thread milling various ID threads (1/2x28 to 13/16x16) and the all have the same problem. When I'm testing the thread fit, the test parts will screw in 2-4 full rotations and then the threads get tight until you can't thread the test part on any further. This is with all threads I'm machining. I've checked the run out on my tools, I'm doing multiple spring passes, and I've check and verified the minor diameter, thread pitch in the program is fine, everything checks out okay. I'm running out of ideas, hoping some of you might shed some light on it. I've got only one thread mill I'm doing these jobs with, so I don't know for sure if it's the thread mill or not. I've also checked my programing to see if it's threading some sort of tapper, everything looks normal (using Fusion 360.)

Let me know if there is anything else I can try. Thanks!
Sounds like a pitch error, does it get gradually tighter as it screws in or does it just stop?
 
Sounds like a pitch error, does it get gradually tighter as it screws in or does it just stop?
Gradually tighter. I though it could be a pitch error in the programming, but everything checks out okay. I've got someone that's going to lend me a similar new thread mill, so I'll try that and see how it comes out.
 
I didn't see where you mentioned what material your cutting.
Also looking at the tool your using, it has a 1/4" shank. Might want to try something slightly bigger.
 








 
Back
Top