Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Unexpected toolpath result from Threadmill Operation - Pitch Diameter Offset

Message 1 of 8
426 Views, 7 Replies

Unexpected toolpath result from Threadmill Operation - Pitch Diameter Offset

I have programmed for several parts where I have used the threadmilling operation with some single tooth threadmills and it performed as expected in simulation and on the machine. When it comes to the pitch diameter parameter, I am working with models drawn to the minor diameter so it has always worked for me to subtract the tapdrill/minor diameter from the major diameter of the thread I want to mill with only minimal radius comp adjustments at the machine needed when it is actually run for the first time.


Now I have a part that I am using single tooth threadmills for a few threads and they are simulating fine as described above, but I also have a 20 tooth 20TPI threadmill that appears to be giving me bad simulation results. I am trying to mill a 1-20 UNEF-2B thread. The model feature is drawn to a Ø0.9515 inch minor, so I used a pitch diameter offset value of 0.0485 inches to get to the Ø1 inch major. When simulated, the thread appeared to be cutting too deep (see attached image below) since the modeled chamfer at the top is Ø1.0115 inches at its max. When I set the pitch diameter offset to 0 it looks closer to the correct size, but I don't understand why it is working differently with this particular threadmill. Is this a bug?


When it comes to sharing this file, it is a customer supplied model, so I am not comfortable publicly sharing it on this post.


This is an image of what the simulation looks like with 0.0485 inch pitch diameter offset. Notice how it is cutting beyond the top chamfer max diameter which is Ø1.0115 inches.

Zero pitch diameter offset.PNG

Labels (2)
Message 2 of 8

Okay, can you send the file privately? seth dot madore at autodesk dot com

I've seen this before. Are you using Control or Wear Comp? What does the posted code look like, and what post processor are you using?

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 3 of 8

Sure. I can PM it to you shortly.


To briefly answer your questions:

  • using wear comp.
  • haasumc-750.cps that I made some edits to a while back


N25 G53 G0 Z2.5
N30 G53 G0 X-29.5
N35 T14 M6
(.371 X 1.00 3 FLT 20TPI CARBIDE THREADMILL - HX3/8.371-I20UNFTM)
N40 S3400 M3
N45 G54
N50 M8
N55 G53 G0 Z2.5
N60 G0 B90. C0.
N65 G254
N70 G0 X0.75 Y0.
N75 G43 Z2.3 H14
N80 G0 Z0.8511
N85 G1 Z0.7711 F3.6
N90 G41 X0.9965 Y-0.1113 D14
N95 G3 X1.1078 Y0. Z0.775 I0. J0.1113
N100 X0.3922 Z0.8 I-0.3578 J0. F12.
N105 X1.1078 Z0.825 I0.3578 J0.
N110 X0.9965 Y0.1113 Z0.8289 I-0.1113 J0.
N115 G1 G40 X0.75 Y0.
N120 G0 Z2.3


  • VS the toolpath moves from the operation: toolpath.PNG


Message 4 of 8

It is good that you noticed this in simulation. The bug is introduced when your "Number of teeth" x "Thread Pitch" is equal to your Flute and Shoulder Length. You can either define your tool as a 19 tooth, or give it a 1.025 Flute and Shoulder length


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 5 of 8

I likely never would have found out what was doing this myself. Thanks for your help @seth.madore!

Message 6 of 8

I've logged this as CAM-22915

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 7 of 8
in reply to: seth.madore

I had an issue like this where it wouldn't cut to the correct depth.  After advice I had to alter the settings until it cut to where I wanted.


The actual issue as far as I am aware hasn't been resolved within Fusion yet.

Message 8 of 8
in reply to: danpayneuk

I am now having the opposite issue as the OP, where it is cutting small instead of cutting big.  I have a 0.495" diameter 20 tooth thread mill for cutting a 3/4"x16tpi thread.  I had it so that the pitch (0.0625") times the teeth matched the flute length since that is how the tool physically is, so I changed the tooth number to 19 to get a mismatch, but the code hasn't changed when post processed.  My model is set to a minor diameter of 0.689" and I've got a pitch diameter offset of 0.0654" (I'm accounting for the flat on the thread form) but it is *barely* taking a scratch cut on the very last pass.


Simulation shows it working perfectly.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Technology Administrators

Autodesk Design & Make Report