How to offset the inner diameter of a circle?

[mallerya]

I have a model that I am trying to remix from thingiverse. There are 4 holes on the object which are 3.5mm in diameter.

On one of them, I attempted to repair the inner faces by creating a new sketch and cutting into the hole with a slightly higher diameter. After, I was going to offset the inner repaired face to return it back to it's original diameter size. However, I get an error when doing so:

"Error: The operation could not create a valid result.
Try adjusting the values or changing the input geometry."

This also happens when trying to create a thread on the existing repaired hole.

There is obviously something preventing the hole's inner face from being offseted/extruded/threaded, but I don't see it. I'm still a little new to fusion, so I am hoping someone with more experience can get back to me quickly. I am in the process of installing the screencast software so I can more easily show the issue, but I need to restart my computer in order to get it working and I have some important work open right now that I do not want to close at this moment.

I will include the model on this post for someone to take a look.

Thank you.

[jeff_strater]

models from Thingiverse are meshes.  This is the underlying source of your problem.  Mesh geometry is very imprecise.  This shape is simple enough, I would re-model this in Fusion using native solid features.  It would not take very long to do so.

Also, your design is a Direct Modeling design.  I would recommend using Parametric/history-based modeling, so you could go back and make changes later.

That said, here is one way to repair the hole - just draw a new sketch, sketch 2 circles - the inner one with the desired inner diameter, and the outer one large enough to clearly intersect with the model geometry.  Use a Join Extrude to add this material to the model

[mallerya]

Hello Jeff, and thank you for the quick response.

I do like your method very much. It seems so much faster than what I did. I will do this for the remaining 3 holes which I need to thread for the model.

Edit: When attempting your approach Fusion 360 will not show the origin point of the hole while sketching a circle. Is there a preference or feature I have to enable for it to be visible? I already enabled auto-project in the preferences->design menu.

I got one hole repaired using an (admittedly) much more complicated method via sketches. The faces are repaired, but the problem remains that Fusion will not allow me to offset the inner face of the hole.

I noticed that the model was not actually flush to the floor. I fixed this issue but the problem still remains. I also completely repaired the outer face surrounding the circle, but it still will not let me offset the inner face.

What could be causing this issue?

I will try your approach and see if it will let me use face offset. Knowing a better workflow is nice, but I understanding why I cannot do it the way I attempted will help me learn the program better as I continue forward.

Thanks again!

(I have attached a link to the updated project file)

[etfrench]

Use three point circles to convert mesh circles:

[Pradipio · Accepted solution]

Hi @mallerya,

I have checked your project, the model is solid body but created from the Mesh.

So, probably the internal property is mesh it self and it may restrict much for editing.

I did some workaround,

1. Project the sketch.
2. Then recreate new sketch with Line & Arcs.
3. Create New solid Extrude. 

Please check the attachments.

I hope this will helps to move ahead. PROJECT SKETCH

RE-CREATE SKETCHEXTRUDE SKETCH 

[mallerya]

Wow! What a great feature!

I ran into a few problems along the way with this. When project the whole body of the mesh onto a new sketch, the inner face would not be all the way filled in, and I can't identify where along the breakpoints it isn't filled.

My solution to this was to do what it looked like you did, project only the top surface, then fill in the bottom base-face later. However, this also came with another problem. The holes are still not perfect circles and I am left to repair their faces still.

Any clever solutions to this as well?

I appreciate all of your support so far. I've learned so much more from remixing this project than I have when designing simple models!

[Pradipio · Accepted solution]

Hi @mallerya,

Thanks for update, 

in this case The holes are still not perfect circles and I am left to repair their faces still.

I can suggest create the solid with out hole profile. You can add holes later, as the model is fully editable now.

I hope this will help to move ahead. 

Please accept the solution if get it done. 

ADD HOLES LATER

[mallerya]

All of the responded solutions were good approaches. The last one I think is the best because it allowed me to do what I need with the least amount of work for the scope of the project.

I discovered the technical conflict about why I was receiving an error when trying to offset the inner diameter of the circle even after repairing the faces. For some reason, the faces of the outer perimeter of the object also needed to be repaired for Fusion 360 to calculate the offset. These couldn't simply be merged either, because the arched curvature the polygons create would warp when doing so.

Because the model has many arch's along the outside with different lengths and angles, this meant that I would have to use splines liberally in order to carve out the sides and repair all the outer faces one by one. Basically, leaving me to repair the entirety of the model and not just a hole or two...

With the project-to-sketch method, it did not require significant repairing in order offset the face of the inner hole. I did have to manually repair the faces of that hole using a 3 point circle in sketch view though, and it's worth noting that when using project-to-sketch, it also did not repair the outer faces of the model after extruding upward along the Z-axis. However, the individually generated points from the projected mesh must have been high enough of a resolution for it to not to interfere with the offset of the inner hole because it seemed to work fine while using this technique.

Fusion makes tricky and complicated stuff seem easy once you understand it. The hard part is describing the issue, doing research and finding the best solution!

[jeff_strater]

here is another approach, using the Create Mesh Section and Fit Curves To Mesh Section commands.  This is exactly the purpose for which these commands exist.  I paused the recording in the middle of all the the curve fitting, as it would have been boring to watch.  Hopefully you get the idea.  I also did not use very strict distances for the Extrudes - you'd want to be more precise.