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: 

Change tapping formula?

8 REPLIES 8
SOLVED
Reply
Message 1 of 9
nocturnalwelding
190 Views, 8 Replies

Change tapping formula?

Hey everyone, 

 

I keep breaking 6/32 taps in the titan 401. 

My buddy who's a Mastercam fan boy says the fusion formula is all wrong. And wants me to use his. Is there a way I can change the formula fusion uses? Or do I need too? Here's the formula he says to use. He says 6.25ipm 200 rpm. Thank you.

1/ the pitch X the RPM.

8 REPLIES 8
Message 2 of 9

I highly doubt the Fusion formula is wrong, there is likely something else causing the problem.

 

Can you share your file here

Goto File>Export>save as .f3d

Message 3 of 9

Yeah he Definity hates fusion and thinks Mastercam is far superior. I hope i can prove him wrong lol.  He says the feed and speed is totally wrong. So thats what I need to really figure out. I included the file below. I've made this 3 times and I did get it to work one time. But i think I might of hit 5% override on my haas vf1. Thanks for the help.

Message 4 of 9

As I suspected there is nothing wrong with how Fusion calculates the feed.

 

The problem lies in how you have defined your tap.

Here is how you had it:

wrong.png

The diameter and pitch are wrong for a 6-32 tap.

 

They should be:

right.png

 

An easy way to input the correct pitch into fusion is just to type 1/TPI so in this case you would type 1/32=0.03125

 

This now outputs 200 rpm and 6.25 feed:

Screenshot 2023-09-30 155207.png

 

The pitch you had originally was 6 time greater than it should have been so there was no chance of it ever working

Message 5 of 9

Yes!!! awsome man thank you.  Thanks for explaining everything so clear, I got it from now on.  Fusion lives on undefeated. Glad it was my fault as far as my buddy goes. Thanks again take care.

Message 6 of 9

An easy way to mentally check it is use a spindle speed of 320 (10x your pitch!) so that your feed is 10ipm. 

Same with a 1/4-20 
s200 F10.


Can also do metric, Spindle 254 F7. for any 0.7mm tap. 

etc etc 

 

Please click "Accept Solution" if what I wrote solved your issue!
Message 7 of 9

Awsome thanks for the tip.👍

Message 8 of 9

I was just curious.  Should I check the use g95 for tapping box in my post? Thank you

Message 9 of 9

While it would prevent issues that caused this thread, make sure your machine allows it. Keep in mind, AFAIK g95 does respect feed and spindle overrides which can cause scrapped parts, where regular tapping cycle does not. 

We still use the default option. G95 makes more sense on lathes. 

Please click "Accept Solution" if what I wrote solved your issue!

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

Post to forums