Creating lids above existing object

[nkloski]

I am thinking I am missing something obvious here, and hopefully it is easy to solve.

How is the best way to create a lid over an existing object?  In this example, I have a rectangular shape, and I want to create a lid that revolves around the enclosure.  I am looking for best practices on creating lids in general, that have to follow a path around an object.

Fusion file attached....thanks!

[neljoshua]

@nkloski,

I did a bit of work with this.  It is not super-precise, but it is an idea of how to do it.  A bit of tweaking could get it much nicer.

1) Make a sketch perpendicular to your original sketch with the profile you want at that new location.

2) Make a sketch approximating the path that you would like the lid to take.

3) Create a loft between the two sketches (your original sketch and the one in step 1).  Use the path sketch (step 2) as a rail.

4) Adjust the path as needed.

5) Mirror the component so that it is on all four corners of your box.

6) Combine the mirrored features into one component (not in the Screencast).

[TheCADWhisperer]

I am having great difficulty in trying to figure out your design intent.

Do you have a link to an image of a similar design?

I don't understand the purpose of three sets of offset geometry.

My usual practice would be to create outer geometry and then use the Shell command for offset faces rather than using sketch geometry.

[nkloski]

Ah...That was specific to this design....the outer shell was to be made out of acrylic, and the inner shell was to be painted a color, like the top of an Apple Magic Mouse, with different materials assigned to each to shine though.

Here is my use case:  A customer comes to me and says, "here is the envelope for some electronics, you cannot enter into that envelope...design a cool 'lid' that surrounds but does not touch the envelope.".

That is what I want to do...I don't even need to use a closed profile, if I could do this with just surfaces in Patch, that would be great, but even drawing an arc over a rectangle, I cannot figure out how to make it a completely closed lid.

[kate.raskauskas]

Hey @nkloski,

I played around in Patch a little and came up with two similar shell shapes. Is this something like what you're looking for?

I just made drawings in the Patch workspace and extruded an offset of the center rectangle, then used the Patch command with Curvature = Continuity for the tops, combined the tops with the walls, and added thickness. 

Please let me know if this helps at all!

Best,

[nkloski]

Awesome, thanks @kate.raskauskas !  

That is definitely a way to do it, but the only control you have over the top shape is that which is created by the curvature aspect of the Patch command.  I want some control aspects to this like splines/arcs, etc.  It seems like it should be easy to have something like this:

Turn into a functional lid with surface "somethings" (lofts, etc, but I just can't see how to do it)  (above file attached here as well).

I tried the surface lofts, but I was not able to get it to work, even with a control spline 😞

[TheCADWhisperer]

Download the attached file.

File>New Design from File

[nkloski]

Thanks very much @TheCADWhisperer that is a great example of using a larger extrusion, filleting down the sides to a pleasant angle, and then using that shape to do some surface patching/stitching.

Ack, I'm sorry if I am not accepting any of these answers, but I just can't!

My question is more along the lines of how to use an arbitrary shape/profile to create the lid.  In your example @TheCADWhisperer I am reliant on how fillets make a shape, for the end shape of the lid.  What if I wanted to use some weird spline curves, that a fillet could not create?  That is what I am asking.

If there was a Patch/Surface command that said "Revolve with guide rail" that would be perfect, but there isn't.

[TheCADWhisperer]

I will try to make an example tomorrow using Loft with a rail.

I will have 4 profiles (one on each side) and a rail on the bottom.

[kate.raskauskas · Accepted solution]

Hey @nkloski,

How about this?

I made two curves over the box as you did, and then I made four "quadrants" for the base. I used the Loft command in Patch, using the base quadrant and the topmost point as the two loft profiles, then selected the curves over the box as rails. Then it was just a matter of combining and thickening the mesh bodies. Is this more like what you're looking to do?

Let me know if you've come across any cool methods while experimenting 🙂

Best,

[JDMather]

I experimented with this a bit and gave up on the Loft in Fusion.

I think I would create the guide curves and then use only for reference with the Form tools.

[nkloski]

Awesome, thanks @kate.raskauskas The key here was that the quadrant sketch profile on the bottom plane is used to loft to the top point, and then I can have as many rails as I need in that quadrant to get the shape I need.  Then mirror once to get two, then mirror again to get four, then the thicken command creates one whole shell.  The great thing about this is that the shape of the arcs/splines are easily driven by user parameters to allow for easy changing....thanks!!

And thanks to @JDMather and @TheCADWhisperer for helping out on this as well!