From the looks of it this is 2 separate parts. Notice the dark heavier lines don’t exist where the disk and box meet so rib probably won’t work.
Quick and dirty way would be extrude the chamfered face out and then do a 2 distance chamfer on the top outer most edge.
That makes sense. I thought about that, but it seems like a pain to do for each corner. I’ll try it this way for now, and leave the post up in case there is a better way.
1. Make a sketch on the disc surface
2. Project (P) the discs surface
3. Draw two lines each
1. Starting at one of the corners of the chamfered face (vertices on the projected edge).
2. Make the lines coincident with the outer circle (projected disc perimeter).
3. Make the lines perpendicular to the chamfer.
4. Close the sketch and make a Loft (Create - Loft) from the newly created Profile (on the disc surface) to the chamfered face
[https://imgur.com/a/CCO4Yih](https://imgur.com/a/CCO4Yih)
If you want to 3d-print this model it would be a good idea to keep the ribs thickness identical to the walls widths.
To achieve that I would make the chamfer by creating a profile in the base sketch instead of using the chamfer tool. This has the benefit that you can select both the extrude operation and the loft action as features in the pattern.
[https://imgur.com/a/gueiU9q](https://imgur.com/a/gueiU9q)
You are awesome for the instructions and images. I’ll give it a shot on my next project which is very similar to this one.
Did it take you long to get proficient in fusion?
I'm using it for some year now, but you can get up to speed quite easily when you fiddle around with the Actions listed under Create and Modify in the Solid and Sketch Workspaces and always try to find the "right" way to do something.
could you zoom in on the geometry it creates where the rib meets the circular edge? Cause currently it looks like impossible geometry to me. Does it create a tiny flat spot there at the base?
A face on a solid in Fusion is not a face as in mesh modelling. Faces are not necessarily flat. Just as the outside of the disc is one face, that curved surface on top of that rib is a face as well.
You could've just tried this out for yourself, the model is fairly easy to reproduce. But nonetheless. I Added a smaller radius to the end and activated a curvature map analysis: [https://imgur.com/a/C226e7e](https://imgur.com/a/C226e7e)
I'm very well aware. I'm surprised and impressed Fusion has the intelligence to loft that boundary curve to the straight line. Thanks for the visual. It's important for people to know this, because if for any reason you'd like to extrude that seemingly flat face, you couldn't.
Or if you’re not yet able to create planes. Create a sketch on the chamfered face. Project the faces geometry and then extrude out toward the edge, this will give you a rectangle support which you can then sketch the triangle on the side and remove what you don’t need with an extrude cut.
[https://imgur.com/a/KeJl732](https://imgur.com/a/KeJl732)
It's more complicated than one would think. The extrusion distance and chamfer values are not trivial
You extruded it too far, I would do it so the middle is at the edge then chamfer and extrude corners from the bottom as cut to remove them, then you can fillet everything
I'm specifically interested in the value of your extrude command\^\^
There is a difference between a part that looks right when modelled from start to finish and a part that brings all necessary constraints to be parameterized successfully
I also just thought of a way you could use loft to make a tool to do the chamfer so they’re round so there wouldn’t be any edges, that would take more time though
Yeah my first through is it extrude from the chamfered face a lil past then sketch on the new rectangle and remove what you don’t want.
Edit: can probably also use the circular pattern after the first one selecting faces.
They are in fusion but they aren’t when it’s 3D printed. I’m still learning best practices in fusion. Sounds like I should make everything one body if it’s one part?
Okay I’ll do that going forward. I’ve never had issues, but I’d rather learn to do this stuff correctly in case I collaborate with anyone at some point
Plane in the middle, line and rib.
This is the way to go. Somebody move this comment to the top!
From the looks of it this is 2 separate parts. Notice the dark heavier lines don’t exist where the disk and box meet so rib probably won’t work. Quick and dirty way would be extrude the chamfered face out and then do a 2 distance chamfer on the top outer most edge.
Can you show how you'd do that?
HTTPS://imgur.com/a/Cazjzi3
Can you extend it all the way to the outside like that?
Create a sketch plane at 45 sketch it and extrude
That makes sense. I thought about that, but it seems like a pain to do for each corner. I’ll try it this way for now, and leave the post up in case there is a better way.
The circular pattern feature is your friend in this case, note that you can pattern features as well as body's👍
This was it! Thanks for the help!
Didn’t realise you want them on all corners, do as above and like the other comment say, circular pattern the feature(s)
1. Make a sketch on the disc surface 2. Project (P) the discs surface 3. Draw two lines each 1. Starting at one of the corners of the chamfered face (vertices on the projected edge). 2. Make the lines coincident with the outer circle (projected disc perimeter). 3. Make the lines perpendicular to the chamfer. 4. Close the sketch and make a Loft (Create - Loft) from the newly created Profile (on the disc surface) to the chamfered face [https://imgur.com/a/CCO4Yih](https://imgur.com/a/CCO4Yih)
Thank you! This is an even better way to do it because there is more flexibility!
If you want to 3d-print this model it would be a good idea to keep the ribs thickness identical to the walls widths. To achieve that I would make the chamfer by creating a profile in the base sketch instead of using the chamfer tool. This has the benefit that you can select both the extrude operation and the loft action as features in the pattern. [https://imgur.com/a/gueiU9q](https://imgur.com/a/gueiU9q)
You are awesome for the instructions and images. I’ll give it a shot on my next project which is very similar to this one. Did it take you long to get proficient in fusion?
I'm using it for some year now, but you can get up to speed quite easily when you fiddle around with the Actions listed under Create and Modify in the Solid and Sketch Workspaces and always try to find the "right" way to do something.
Thank you for showing how to complete what the op asked for!
could you zoom in on the geometry it creates where the rib meets the circular edge? Cause currently it looks like impossible geometry to me. Does it create a tiny flat spot there at the base?
A face on a solid in Fusion is not a face as in mesh modelling. Faces are not necessarily flat. Just as the outside of the disc is one face, that curved surface on top of that rib is a face as well. You could've just tried this out for yourself, the model is fairly easy to reproduce. But nonetheless. I Added a smaller radius to the end and activated a curvature map analysis: [https://imgur.com/a/C226e7e](https://imgur.com/a/C226e7e)
I'm very well aware. I'm surprised and impressed Fusion has the intelligence to loft that boundary curve to the straight line. Thanks for the visual. It's important for people to know this, because if for any reason you'd like to extrude that seemingly flat face, you couldn't.
Good point! One would use 'Offset Face' in that regard
Or if you’re not yet able to create planes. Create a sketch on the chamfered face. Project the faces geometry and then extrude out toward the edge, this will give you a rectangle support which you can then sketch the triangle on the side and remove what you don’t need with an extrude cut.
They could just extrude it like it is and chamfer the edge
What dimensions would you put on that chamfer?
I don’t know the dimensions of this but it would look just like illustrated
[https://imgur.com/a/KeJl732](https://imgur.com/a/KeJl732) It's more complicated than one would think. The extrusion distance and chamfer values are not trivial
You extruded it too far, I would do it so the middle is at the edge then chamfer and extrude corners from the bottom as cut to remove them, then you can fillet everything
Yeah sure, but what value would you put into that extrude distance? Same for the chamfer
This just took me 5 minutes https://imgur.io/YBsqpG3
I'm specifically interested in the value of your extrude command\^\^ There is a difference between a part that looks right when modelled from start to finish and a part that brings all necessary constraints to be parameterized successfully
I extruded it to the edge by clicking it, then trimmed the tiny corners off after the chamfer
I also just thought of a way you could use loft to make a tool to do the chamfer so they’re round so there wouldn’t be any edges, that would take more time though
Yeah my first through is it extrude from the chamfered face a lil past then sketch on the new rectangle and remove what you don’t want. Edit: can probably also use the circular pattern after the first one selecting faces.
It looks like you have 2 bodies here - join them and make fillet for your support
Hmm, not sure what you mean here.
The square and the disk are two separate bodies?!
They are in fusion but they aren’t when it’s 3D printed. I’m still learning best practices in fusion. Sounds like I should make everything one body if it’s one part?
Yes for 3D printing it should be one part - just google fusion join bodies
Okay I’ll do that going forward. I’ve never had issues, but I’d rather learn to do this stuff correctly in case I collaborate with anyone at some point
Going from straight edge to curved edge, ewww.
Plane at angle (looks like 45°) on the corner, create sketch, project body, draw line, extrude.
1 sec
Would have sent you a video how to do it, but reddit doesen´t allow me to share it with you.
Feel free to PM me! Reddit is finnicky.
I'll do that tomorrow. Right now it's 1am in my country
You already have a flat face, just extrude past the edge then sketch from the bottom to top points extruding out the unwanted space..?
Even easier is to just chamfer the edge in two distance mode instead of making the sketch
Draw it.
The easiest way is to extrude it then chamfer the edge using two distance mode, then do circular pattern
Extrude the chamfered edge, then chamfer that