Trying to Model The Gap Between Two Controller Shell Halves

[sjarmstrongv_1]

Hello,

I have never used this forum before so please let me know if this is the right place to be posting. I am trying to design a custom controller in Fusion. So far the body split in two halves where I want it and shelled. I am having difficulties in designing the seam between the two controller halves. What I would like to do is create something similar to modern injection molded controller housings (like Xbox, PlayStation, etc.) where there is a gap and a flange designed into the seam to make sure the edge matches up and doesn't allow any light to pass through (below I have a Microsoft paint drawing of a cross-section of what I'm trying to achieve, hopefully it makes sense). I've been trying to find a way to do this over the past few days and I always run into some kind of error. So far I have tried sweeping a profile along the path where the two controller halves are separated but I always get an error saying the profile intersects itself. I have also tried splitting the face of mating surfaces and offsetting the faces to create the edge that I want but I always get an error saying the faces couldn't be rebuilt after being deleted. At this point I figured I would try posting this here and see if anyone has any experience with this type of design or sees any major flaws in my design process. At the end of the day this is just a personal project and this seam design is mostly for looks, so if this is just not possible to do I am willing to just carry on with my project without it. I have the f3d file attached below.

 

 

[davebYYPCU · Accepted solution]

I think you are trying to get too much done too quickly.

I presumed it has to be symmetrical, I went back a bit in the timeline, cut the solid body in half.

Shell by removing the inner face.

Split Body with your surface.

Made a Ruled Surface 1mm high at the inside bottom edge.  Thickened by 1mm and joined to that body.

Combine > Cut the top Body with the bottom body, and then 

Mirrored each half to a complete version.

A few things, 

Fusion tends to choke on organic shapes being manipulated with solid tools. 

Bottom lip is inside to assist with waterproofing.

Ruled Surface is vertical, so there is no draft or interference clearance, you may want to adjust things for that.  There are some sliver faces to deal with as well.

Doing half and then Mirror usually works for me without the "Can not Boolean" error / situation.

Model will be more stable with fully defined sketching.

Might help....

[sjarmstrongv_1]

Wow! That is fantastic! I knew there had to be a more simple solution to the issue, most likely due to my own lack of knowledge. I was not aware of the Ruled Surface tool. I will definitely keep that in mind for future projects. This is my first time trying to do any kind of organic shape in Fusion, or any CAD software for that matter, so I greatly appreciate the tips! (Also thanks for calling me out on not defining my sketches, it has become such a bad habit I formed since I got out of school haha)

[johnsonshiue]

Hi! If you have access to Plastic Design environment, Lip command can help create such geometry easily.

Many thanks!