How to create support inside a hollow object?

[Anonymous]

I would like to know the best way to a 45degree support for my 3D printed project.

I have a hollow object needs to be printed as oriented; however, the printing fails as it gets to the top because it is literally printing vertically without support.  So I figured maybe put support at an angle around the top to help out as shown in the red marker, but I really don't know how to do it properly. So far I have imagined making another object to combine, but it is a big hassle as it the top rim is irregular

[LeonardoBN]

Hello, @Anonymous.

What slicer are you going to use? Could a slicer native support solve your overhangs?

Sorry not answering your main question, but I wanted to understand better your issue.

[Anonymous]

cura but i am trying to make a design with no support. if the interior is made with angles then it wouldn't need any support while printing

[etfrench]

Printing this upside down will give you the best print.  Here's how it would look in PrusaSlicer with the overhang threshold set to 85%.  Note: The top of this is actually flat when you think of the fillets as being on the sides 😀

Having the support on the outside also makes it much easier to clean up.

[Anonymous]

As I have said, it has to be printed in that orientation, because I am only showing a part of the project. I don't want this post as to how to print but instead how to make use of fusion 360 to best design the inner hollow part.

That object is designed with loft and shell. I don't know if there's another way around it.

[etfrench]

Here's how it looks right side up with the same settings:

If you want to create custom support, just use a .2mm offset of the inner faces. Thicken that, then cut grooves in it to reduce the contact area. 

Another technique which may work well is to rotate the piece 45 degrees. (Support threshold is set to 50% in this image.)

You can add frog pads on the corners (3 layers thick) to give it more surface area on the build plate.

[Anonymous]

Maybe I haven't explained it clearly. 

As long as an object designed by going at a less than 45 degree angle, no support will be needed. All I wanted to do is to thicken the inner top arc around the top. So on the side cut it will look more like the sketch I have just made.

[GRSnyder · Accepted solution]

@Anonymous, I'm not sure the other responses are addressing your actual question. You are willing to bridge the top, but you don't want the curved walls to have to print any flatter than 45 degrees. And you don't care about the interior shape; you're willing to add extra, permanent material to support the tops of the walls. Is that the question? Like this?

If so, this is pretty easy. Just extrude the roof downward with a 45 degree taper angle, creating a new body. Then do a Boundary Fill with that object and the original form and select the two flaps on the sides, picking Join to add them to the original form. Then Remove the extruded form.

For extra credit, you could make the extrusion a surface instead of a body. That would represent the design intent a bit more clearly: "the inside edge of 45-degree walls that would lead up to the roof". You should be able to use the same Boundary Fill process with a surface.

[Anonymous]

Yes!

That's exactly what I am looking for. But I got stuck on boundary fill and cutting the flaps that are sticking out. Would you give me a little more help please?

Thanks

[GRSnyder]

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@Anonymous wrote: Yes! That's exactly what I am looking for. But I got stuck on boundary fill and cutting the flaps that are sticking out. Would you give me a little more help please?

There's an F3D file attached above - take a look at that.

[GRSnyder]

I should say also that I'm not sure why Boundary Fill joins the flaps only to the shell in this case. The extrusion, shell, and flaps are (necessarily) contiguous, so I would have expected the Join option to produce a single, merged body. It's doing what I want, but I not what I expected. 🙂 Does anyone understand this result?

[etfrench]

Even easier is a two direction chamfer:

[GRSnyder]

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@etfrench wrote: Even easier is a two direction chamfer:

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Ha! Very clever! It looks like this approach doesn't create a constant angle with respect to the horizontal reference, though. I guess it's affected by the local curvature of the wall. 

[Anonymous]

Thank you for the replies

The chamfer doesn't work for my case because it will scale down the top which will eventually need to be open up as a lid. 

As to the extrude method, due the irregular shape on the sides, the extrusions are sticking out and I don't know how to get rid of it. When I try boundary fill, it only gives me limited parts to choose from in which I cannot exclude the corners and edges sticking out.

[Anonymous]

OH I think I did it. There was a step I missed. I needed to use shell and make that new body (45 degree extrusion) hollow before I fill the boundaries.

Thanks a lot guys