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: 

Boring/Threading Tool Retract

3 REPLIES 3
SOLVED
Reply
Message 1 of 4
randyt88rsb
177 Views, 3 Replies

Boring/Threading Tool Retract

I've attached my file, how do i get my ID boring and threading tools to not retract in x into the part?

Labels (3)
3 REPLIES 3
Message 2 of 4
a.laasW8M6T
in reply to: randyt88rsb

In both cases you had you clearance radius set as stock ID, but the part is starting from solid stock so the tool will always retract to centerline.

 

If you set to model ID with an offset then it retracts fine:

thread.png

 

Message 3 of 4
randyt88rsb
in reply to: randyt88rsb

Thank you! I have one more question and have reattached file, why is my threading bar not passing through the bore and showing collision?

Message 4 of 4
a.laasW8M6T
in reply to: randyt88rsb

Hi

 

The reason you are seeing a collision is that you are cutting a 0.1" pitch thread but you tool is only 0.04" pitch

Screenshot 2023-08-27 101506.png

If you change this to 0.1 then there is no more collision.

 

For the tool to pass through the bore you need to turn confinement on and give some value to want the tool to go past:

Screenshot 2023-08-27 101649.png

I added 0.1" past but you can make it whatever you need.

 

The frontside offset needs to be there to allow the tool to infeed in air rather than rapid into the material and also there needs to be a distance in front of the part for the tool to accelerate up to the correct threading feed from stationary.

 

The formula for this distance is 0.002 X Thread lead X RPM

so in this case 0.002x0.1x1200=0.24

 

So I made it 0.25

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

Post to forums  

Autodesk Design & Make Report