how to cut out an imported step file from an engineered body

[autocadFH8KR]

I am trying to make a stand to hold an oddly-shaped component (in this case, a Looki camera).  I retrieved the step file for the camera from their downloads website and imported that into Fusion360.

Now I have created a block that will be the basis for the stand, and I have cut out the front of that base by making a sketch of the primary body (plus some wiggle room), and extruding that sketch.  Now I want to cut out the back part of that so that the camera fits cozily into the body I have created and cut.

I assume that the best approach to this, is to use the Combine (body) tool, but I cannot for the life of me get Fusion 360 to select the camera body (imported step file) as a tool in the Combine method.

The model is here: https://a360.co/3Sr1HuK

(I wanted to attach the model to this post, but Fusion360 will only save to f3z, not f3d, and this forum does not allow f3z.  Bonus points for solving that puzzle as well.)

[g-andresen]

Hi,

There is no download permission
1. Create a source that allows downloads > “allow download”
2. Zip the f3z
3. Remove the links  (chain symbol)within the design and attach as f3d

günther

[dsouzasujay]

Hi @autocadFH8KR 

Requesting to allow download or download a f3d/f3z on your local drive and attach here to the next reply

[jeff_strater]

Another command to look at is "Solid Sweep".  This command is made for exactly this kind of requirement:  Creating packaging, jigs/fixtures, or a stand from a solid body.  It allows you to "push" a solid body into another solid, that will allow for undercuts, etc.

However, the fact that you cannot select the camera body as a tool body in Combine suggests to me that the STEP file is either a surface body or maybe a mesh body.  Combine (and Solid Sweep) both require complete solid bodies.

[autocadFH8KR]

Sorry about the “no download” option.  Apparently, I have to pay a subscription fee to allow download.  Instead, I have broken the link that was holding me back, and have attached the model itself.  

[autocadFH8KR]

Instead I have attached the .f3d file in another reply.  Sorry about the first post.

[autocadFH8KR]

Hmmm… this looks promising, I will look into it.  Depending upon what’s meant by solid body (does it mean, cannot be hollow?) this may work for me.  Will know when I get the opportunity this evening.

Model is now attached in another reply in case you’re interested.

[jeff_strater]

No, Solid just means that it is a watertight body.  It can be hollow (for instance, shelled), but it cannot have any "leaks" in the geometry.  Surface bodies have a different icon (orange vs blue).

looking at your model, this is, indeed, your problem.  Body10 in the Looki model (the only one visible) is, indeed, a surface body:

And surface bodies cannot be used in Combine or Solid Sweep.  If I get a chance, I'll look at that body to see if I can figure out why it was not imported as a solid.

[jeff_strater]

I did  quick try to see if I could stitch the surface into a solid.  No luck, and the error message is not particularly helpful:

even adjusting the tolerance does not help.  I'll have the geometry team take a look at it.  

[autocadFH8KR]

Wow, thanks for the quick snd thorough response!  I look forward to more.  I am ok to pretty good with Fusion360 until I run into a problem.  Thin I become about as useful as a bowl of mud.

[jeff_strater · Accepted solution]

in the meantime, I created a workaround that, if not exactly what you need, might give you some ideas....

I created a zero offset surface from the outer side of the Looki:

Then, I deleted some extraneous faces, and patched some holes to get this:

Which I could then use as a splitting tool in Split Body to split the stand body, to get this:

Model is attached.  All the messy surface operations are in the timeline group "surface cleanup".

This is a useful technique that you can use for this kind of thing, although its usefulness is limited.  This model does not have any undercuts, which helps.

[autocadFH8KR]

Jeff, you, Sir, are a star!  Thank you so much!

I have accepted your answer - you did in fact answer the questions I asked.  I have learned much from this, and once I peruse how you accomplished this, hope I will learn more.

I owe you, Jeff.  Thank you for the contribution!