Community
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.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Offset single point thread mill question

8 REPLIES 8
Reply
Message 1 of 9
timothyhinessr
443 Views, 8 Replies

Offset single point thread mill question

I have a project that requires several M14 X 1.5 threads 1" deep in 6061.  Knowing that Fusion supports thread milling, but before familiarizing myself with it, I ordered the pictured endmill, top photo.  When I attempted to add the tool to the tool library, I found that Fusion doesn't offer that type of tool with the offset shank and single point cutter.  I don't see a way to make this tool work but wanted to check with the community before returning it and getting the kind that Fusion clearly supports, bottom photo.  Am I correct that this cutter won't work in Fusion?  Thanks,  Tim

 

 

IMG_0132.jpgIMG_0134.jpg

8 REPLIES 8
Message 2 of 9

Hi,

That's because the picture at the top is not a thread mill its a lathe boring bar, you cannot really use this tool an a rotating application.

Message 3 of 9

Ok, I've got the correct tool on the way and downloaded the tool from Harvey Tool into my tool library.  I've programmed a test setup and the simulation looks good but I have a question about how to dial in the program to get the fit I'm looking for.  From what I can discern, the way to adjust the thread depth is by adjusting the offset in the Pitch Diameter Offset field.  This would require going back to Fusion and changing the setting each time.  I've experimented a little with cutter compensation but programming a long enough linear lead in move to turn on cutter compensation results in a toolpath that cuts way too deep according to the simulation.  This is not unexpected based on the size of the cutter, .388, and the size of the hole I'm threading, .492 for an M14X1.5 thread.  I'm assuming that cutter comp would work with a hole large enough to accommodate the required linear lead in distance but haven't explored that yet.  Does anyone know if there a way to edit the g code at the machine to dial in a fit.  I'm using a Tormach 1100MX so editing at the machine is easy if I knew what was required.  Thanks,  Tim     

Message 4 of 9

If you want to adjust at the machine then you will need to use In control compensation.

Fusion automatically creates leads to center for threads so if it can activate cutter comp it will do it just fine.

 

I personally don't bother with cutter comp.

I adjust the pitch diameter until the thread gauges correctly, just reposting the code a few times as i adjust and then save it as a template.

 

Then whenever i do that thread again i just load the template and no adjustments needed

Message 5 of 9
Don.Cyr
in reply to: timothyhinessr

@timothyhinessr On the passes tab, set compensation type to wear, run the cycle at the machine using your tool diameter wear offset to dial in the size, you can then take that value from the control and go back and adjust the pitch diameter offset in Fusion using that value so it posts out the correct code before saving as a template. Typically you need to make this value larger anyways depending on the flat/radius on the thread-mill flutes. Always a good idea to keep the wear offset active in the toolpath to account for tool wear as you produce parts. 

Please click "Accept Solution" if I helped with your question or issue.
Message 6 of 9

That's what I normally do but as previously stated, the holes I'm threading are not much bigger in diameter than the tool so there isn't room for a lineal lead in long enough to activate cutter compensation.  My computer is a significant distance from my mill so I'm looking for a way to save time and steps.  

Message 7 of 9
Don.Cyr
in reply to: timothyhinessr

That's where wear offset will benefit you here, you only need small amounts in the offset to get the correct diameter so the lead-in only needs to be very short and normally only a couple thousandths added to the offset will get the result. You are only compensating for tool wear and not full tool diameter so this value at the control will be 0 initially. Your tool is Ø.388 and cutting a thread with a major of Ø.551 so there is adequate lead in to activate the wear offset. Only needs 1 trip back to the computer once the offset is dialed in.. We thread-mill tons of holes here and probably the most common is a 2-56 in 15-5PH stainless and this works for me. 

Please click "Accept Solution" if I helped with your question or issue.
Message 8 of 9

Thanks again for the input Don.  I haven't received my new cutter yet but plan to do some testing of my thread milling ops today.  I'll try what you suggest and see what happens.  It's just long been my understanding that regardless of whether I use "in control" or "wear", a linear lead-in move of slightly more than half the tool diameter is required to activate the compensation.  I'll post the results this afternoon. 

Message 9 of 9

Well this is one of those rare occasions where I'm happy to say I was wrong.  I ran two different test operations with cutter comp set to wear and using Fusion's default linear lead in settings which are fairly short.  One was just a simple contour and the other was a thread milling op.  Both operations worked correctly with no G-Code error messages.  I did get G-Code errors if I had the actual tool diameter in the tool diameter box on the controller instead of 0.0 or some other small number like 0.005.  I used In Control for cutter comp for the first couple years I had my Tormach 1100MX and always thought it was ridiculous that I couldn't use cutter compensation to dial in the diameter of a hole unless I could program a linear lead-in of at least half the diameter of the tool.  I started using cutter comp in wear about a year ago just because it seemed simpler to enter and keep track of the amount of compensation I was applying not having the actual tool diameter in the box as well.  I guess I was so sure from what I'd learned about cutter compensation to that point, that the same linear lead-in was needed regardless of of whether I was using wear or in control, that I didn't even bother to try it any other way.  The learning never stops!  Thanks again for the help!     

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

Post to forums