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: 

Adding single form thread mill to library . . . how do I do it?

10 REPLIES 10
Reply
Message 1 of 11
longshotsystems
254 Views, 10 Replies

Adding single form thread mill to library . . . how do I do it?

As the title says. I have a Single Form threadmill from Harvey Tool, but I'm struggling with how to add it to my library so I can use it in Fusion.

 

The tool: 

https://www.harveytool.com/products/tool-details-901270-c3#moreDimensions

 

Any tips are greatly appreciated!

10 REPLIES 10
Message 2 of 11

Hi,

It looks like the thread mill creation still doesn't work properly.

The best you can get using the tool library is using settings like this

cutter.png

shaft.png

 

Another way is to create a form mill which will be an accurate model of the tool

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-366D419C-38B6-4648-A2F9-64AE6FD94FAC 

 

I've attached a file with the threadmill as a form mill

Message 3 of 11

Thank you for the help.

 

Curious if you know much about thread-milling. I have a resevior cap I'm trying to do OP 2 on. I'd like to add external threads to it, and based on the designed diameter I have it set for 2 3/8"-8 threads. The largest thread mill I have is the 1/2" single form. Using calcs for pitch offset I get an offset much deeper than the tool. 

 

I'm curious if I can use this tool to mill these threads, acknowledging they won't be as deep as you'd want for this diameter, or if it's a lost cause. 

 

I appreciate any insights. Thanks!

Message 4 of 11

No you can't cut an .125 pitch thread with that thread mill, the shank of the tool will hit the major diameter:

tread.png

 

If you make the depth shallower so the shank doesn't hit then the part will not screw into the hole.

 

you will have to get a threadmill with a larger pitch range

Message 5 of 11

Even if I'm also making the female portion of it as well and could make the thread depth the same on that piece of it? I guess if not, then what size thread-mill do I need for a 2"+? Harvey only goes up to 1". 

 

Could I increase the pitch to get better engagement with shallower threads?

Message 6 of 11

If you are making both parts then you can make it like a 2-3/8 - 12tpi and you will be able to use that threadmill

 

For larger threads i use the Iscar multimaster thread mills, but there are many brands out there that do something similar

https://www.iscar.com/eCatalog/item.aspx?cat=6492315&fnum=2498&mapp=TH&app=119&GFSTYP=M&isoD=1 

Message 7 of 11

Any advice on setting the right PTO when doing a custom thread like this then? Do I just aim for max offset the tool will allow to get the strongest engagement, and ensure i do the same on the female end? Apologies, still learning all of this :). 

Message 8 of 11

I had no idea they had indexable thread-mill inserts. Are those any good? It seems like that would be a way to cover a few bases and not be dropping $100-200 per size . . . 

Message 9 of 11

Yea they are good but they still aren't that cheap the inserts are probably like $100-200NZD and you also need a shank to screw them on. very handy for cutting a large range of threads though. that insert will cut from 3mm-4mm pitch or whatever that converts to in imperial(UN and metric share the same thread profile)

They do a smaller one too which I use a lot for cutting M18x1.5 threads

 

For UN and metric threads the PDO is normally (For an OD thread) the major - the pitch

For metric its really easy to figure out as the threads are designated by the pitch, whereas UN they are designated by TPI.

Its easy to convert though you just take the inverse to find the pitch so 1/12=0.0833333 pitch

 

so for the PDO you would enter 0.08333(you can just type 1/12 straight into the field in Fusion)

 

This may not be perfect though and depending on the threadmill you may need to adjust this to get the thread to gauge right.

 

Seeing as you are making both parts, you can threadmill the male thread first and then adjust the female thread to fit.

This wouldn't be best practice if you were making parts for a customer but if it's just a one off you can fudge it like that.

Message 10 of 11

Wouldn't .08333 be the pitch though, and not the pitch diameter offset? 

longshotsystems_0-1693715972450.png

 

Message 11 of 11

Sorry I was wrong there

It is really the difference between the major and minor diameter(2x the thread depth)

But starting at the pitch gives you a little wiggle room for adjustment so you don't over cut.

pdo.png

But in practice they will likely be different

like for My M18x1.5 example the pitch is 1.5 but I ended up with the PDO at 1.65mm(Slightly more than major-minor) to get the thread to gauge right(Thats an internal thread)

 

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

Post to forums  

Autodesk Design & Make Report