Fill in curved space

[nkloski]

Hi all...something hopefully simple...I have modeled a small wastebin using the sculpt command, and it has a bowed profile:

 

...and shelled it:

My question:  I want to put in three small chambers inside of the main body to hold various recycling sections.  I tried sketching the rectangle on the bottom of the bin that will serve as the housing for the three chambers to extrude up, but how do I fill in the empty spaces on the sides of the bin with solid material?

Or is it better to work from a solid model and subtract, rather than try to add to something that is already voided out via the shell command?

Thanks!

[jeff_strater]

Your method so far is good.  I would recommend the Web feature as the way to do your dividing geometry.  I have a simpler model, but the same basic idea here.  I've modeled the recangle part already (I hope I interpret this correctly), and I have sketch on the top face of this internal box, and just drew 4 angled lines from the rectangle corners.  They don't need to hit the outside of the volume (and if fact should not):

Then, invoke Web, and select these 4 lines:

type in a thickness for the web:

and click OK.  Here is what it looks like from the side, with a Glass material applied so you can see inside:

Hope this helps!

Jeff Strater (Fusion development)

[nkloski]

Thanks, Jeff!

That is a good solution, and something I will keep in mind when I want to selectively reinforce certain areas!  The intermediary step of this project will be 3D printed, so I want as many solid areas as possible because the slicer will hollow them out during slicing.  I am thinking that the best way is to "just not do it that way" and instead start by NOT shelling the object and instead cutting the main compartment out of it.

I tried "sweeping" the "web" but that really did not work at all.  I created one web with full height, and then tried to sweep a face of that web as a "new body" (which is the only option that offered me an "ok" button), but that did not turn out well....in fact I have no idea what it created, but it was not what I was looking for.  Here is the result of the sweeping of the face:

......from all named views, everything is still flat, but it looks bad, and seemed too much work.  Since I am new to design in general, this seems like one of those learning lessons where starting down the appropriate path from the beginning would save way more time than forcing the software to adapt to bad workflow?

Thanks!

[jeff_strater · Accepted solution]

Hmm...  Maybe I am not completely understanding what you want the final shape to look like.  But, you are probably right, sweep probably would not work.  Another technique that can work is to use a multi-body approach.  Model the ouside shape as a shelled body like you have above, then model the interior as a solid block that extends beyond the outer body, then use Combine to put them together.

Start with the shelled outer body:

Then, draw a sketch wherever you want the top of the filled area to be:

draw the rectangle so that it competely extends beyond the volume of the shell:

Then, extrude this rectangle into a new body (the "new body" part is critical):

Then, add whatever detail you want to the block.  In this case I just put 5 circular holes in it:

Then, you are left with two overlapping bodies.  I then used Combine, selecting the block as the target body, and the shell as the tool body.  Choose "cut" and "keep tools":

This removes the area from the block that is defined by the shell.  Now, you are left with 3 bodies (the shell, the internal volume, and the outer part of the block:

Delete or hide the outside, and you have two bodies left (the shell and the interior). Combine them again, selecting "join":

and you are left with one body that is solid on the inside areas that were part of the block.

If I still haven't captured your intent, let me know.  There are other approaches that we can try, I'm sure.  I enjoy coming up with new ways to model stuff!

Jeff

[nkloski]

That is absolutely what I wanted! That's great!

That totally works if you have something small and non-complex, but I would think that something like the sweep tool (which "almost" worked) would be the ideal.

Is not the sweep tool's intent to do things like this? The fact that it "almost" worked but gave weird artifacting lends me to believe that it should but maybe I am wrong?

Either way...thanks!!

[jeff_strater]

I probably did not understand what you were trying to do with Sweep, sorry.  I think I assumed that you were trying to use Sweep alone to fill the solid curved area, which might be difficult.  But yes, Sweep can probably be used to solve this modeling workflow as well.  One nice thing about Fusion is that there are usually lots of ways to solve a modeling problem.

Thanks!

Jeff