Thread Milling not working?

[jgaertner]

Hello Forum,

2 weeks ago I posted a thread about my attempts at starting to usie thread milling in Fusion for my business. I have made three attempts and they are all off by some small margin that the parts do not fit. I am using a Lakeshore Carbide single point thread mill and am machining 6061 aluminum for "Practice". I am using the machinery's Handbook for my 24 TPI offset value but the male and female threads do not match up? I am not doing a standard bolt hole like a 1/2" x13 hole. I am trying to thread a specific diameter piece and then make a matching female thread to match.  Is there anyone else out there that has figured out what kind of fudge factor you have to use to get Fusion Thread Milling to work?  the measured ID and OD are spot on, but the parts do not fit together.  

[jgaertner]

Here is an update on my thread milling project. I machines a new ID pocket to 1.963" ID and then thread milled it using my single point thread mill 24 TPI. All came out fine. I then began "chasing" The correct size male OD blank to fit this pocket on my manual lathe after the one I machined on my CNC mill did not fit. It was way over size. The final male OD blank that I threaded and that fit the ID pocket was 1.950" in diameter or 0.013" smaller than the ID of the threaded bezel? Why is that? The depth of threads according to  TMH is 0.02255" or roughly 0.023" and 1/2 of that is roughly the amount SMALLER I had to machine my male blank before threading would work.

[Anonymous]

Thread milling can be challenging but when you'll eventually get it right it's super satisfying.

Heres a part I did yesterday, the threaded section is .375 of #8-32 thread

John Saunders' NYC CNC video on thread milling helped me out a ton, watch the video at the link and download the excel calculator they developed that will give you your pitch diameter offset.

Input that pitch diameter offset into fusion and you should be good to go.

In 6061 you're not probably going to see much tool deflection but it goes without saying to choke up as much as possible on your tool and to make sure your feeds and speeds are dialed in.

I'd also recommend a tool path tolerance of .0002 or finer

I used 1200 sfm with .0004 ipt 

At that point you should be pretty close, if it's still not threading in you could add a chamfer around the start of your hole or boss to give it a nice lead-in and then finally you could try adding some negative stock to leave but you shouldn't need to apply more than .002 or .003 negative radial stock to leave.

[jgaertner]

Thanks for your reply. I have watched John Saunder's video several times. Even he states there is some need for a fudge factor. I have had some better results making a proper chamfer and working with my own thread milling spread sheet. Still more to figure out, to get this to work. Like I said, I am not trying to thread mill standard bolts, or nits I am trying to thread mill custom instrument gauge housings so the diameter are much larger.

Jgaertner

[jgaertner · Accepted solution]

After a number of tries with different settings in the Thread Milling command screens I feel I have successfully figured out what I was doing wrong, I was using the "Depth of Int. Thd. and UN Ext. Thd." from the Machinery's Handbook when I should have been using the "Depth of UNR Ext Thd" column data. This proved out when I manually chased on the lathe, both the 16 TPI and the 24 TPI that I had done on my CNC mill, earlier that DID not fit. The additional depth of cuts measured on my DRO, coincided with the data in the other column in the book. You need this information for correctly programing the threading operations.

[Anonymous]

Ahh very nice! Glad you got it figured out, nice looking part!