topic Re: Creating threads on inner face in Fusion Support Forum

Creating threads on inner face

taranparshotam_nz — Sun, 24 Mar 2024 03:21:44 GMT

Hi there,

I have been working on a project that requires for me to create an inner thread inside my design to connect two parts. However, Fusion won't let me select the inside face when the thread function is open.

It recognises the inside part as a face:

But it won't let me select it for a thread:

Can anyone help me or provide an alternative way to connect the two pieces?

Re: Creating threads on inner face

MRWakefield — Sun, 24 Mar 2024 11:27:38 GMT

Could you attach your model here so we can take a look?

Re: Creating threads on inner face

taranparshotam_nz — Mon, 25 Mar 2024 07:05:25 GMT

I am creating an arcade type button. Attached is the f3d file.

Re: Creating threads on inner face

HughesTooling — Mon, 25 Mar 2024 08:38:02 GMT

The problem is you used a form so the face is not part of a cylinder. You can see if you select the edge it only reports the length not it diameter. The form you created looks pretty simple and could easily be done as a revolve in the solid workspace.

As a bodge to fix the problem you can create a sketch with 2 circles and extrude a true cylindrical face to use for your thread. See attached file. Another problem with using a form is I could not easily measure the diameters of the part so I added a M36x1 thread as a guess.

Re: Creating threads on inner face

HughesTooling — Mon, 25 Mar 2024 09:02:11 GMT

Here's your revolve done as a sketch, another advantage is now you can add exact sizes. Not sure what thread you want, the ID seems to be around 37mm using your form and a guide?

One tip, avoid using copy\paste for bodies because it can lose it's reference body and there is no way to fix or reselect a new body if this happens. You'll note on the right click menu there's no edit option on a copy paste!

Attached is a new version using a solid revolve. The timeline's a bit of a mess, not sure why you moved parts to a new component. Better to create parts in their own component from the start. Best practice is to keep geometry as simple a possible so I used lines and arcs in the sketch rather than a spline. The attached file has a M38x1.5 thread, just edit to whatever you need.