Truncated Rectangular Pyramid in Sheetmetal???

[will.dameron]

Ok - I'm trying to make a fan shroud to put an electric fan on my Bronco. I want to cut it out of sheet metal on my CNC plasma, and then bend it up. I'm not very familiar with this kind of work, but I'll muddle through, if I can figure out this darn design...

I'll try to describe what I want, because I can't even make it far enough in fusion to upload something which will help. I'm fairly proficient at some parts of fusion, the stuff that I use more often, but not at sheet metal or these odd shapes.

What I want is this: A square of sheet metal, say 20" x 20", with a hole in it. The fan will mount to this. Next, I want to turn this into a 'pyramid', that is 3" in height. I want the wide 'base' of this pyramid to be a rectangle, say 30" x 40". That's the part I can't do. Once I get that part, I would like to add 'flaps' to 4 of the 8 edges to aid in bending/welding, and a couple of other bends for mounting flanges, which I think I can do on my own, but darned if I can make a pyramid with a rectangular 'base' and a square 'top'. Ideally said pyramid will be fully parametric, as this may take me a couple of mockups to get right - I'd love to be able to decide I want it 2.5" in height, or 45" wide, or whatever, and just change parameters to make it happen. I'm sure this is simple, but I cannot seem to get it to happen... Any help would be much appreciated!

Will

[will.dameron]

Ok, I modeled up a single component in regular 'model' space real quick. I made it random dimensions, but you can see the shape and what I'm trying to achieve, but out of sheet metal. If anyone can get this going, it would be greatly appreciated...

Note: like I posted earlier, the important parameters for me are the overall length and width of the 'base' and 'top' of the pyramid, and the 'height' of the pyramid - I don't really care what the length of the joining/mitered edges are, or the angle, which I think might make this design trickier, since that is the dimension fusion wants when you create a flange in sheet metal mode. Any way for those parameters to be made, short of doing some Pythagorean theorem?

[lichtzeichenanlage]

Perhaps this might help you (sry for the German title, I did this for the German branch of this forum. But every thing else should be English).

[TheCADWhisperer]

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@will.dameron wrote:

.... Once I get that part, I would like to add 'flaps' to 4 of the 8 edges to aid in bending/welding, and a couple of other bends for mounting flanges, which I think I can do on my own, ...

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Hollar back when you have trouble with these "flaps" that you speak of.

A couple of examples attached.

[will.dameron]

Wow - these solutions are brilliant. Very elegant, and makes use of tools I knew nothing about, namely, lofting.

I cycled back through the timeline, and was able to recreate the design myself. Then I moved onto those 'flaps'... man, this is so much harder if there are 'unknown' angles involved - Fusion really wants you to just grab an edge, make a flange, give it an angle and height. But, it won't let you 'snap' to an already known angle, plane, object, point or anything.

In the above posted examples, if you were to take one of the sides of the 'base' of the pyramid, the big rectangle, and add a 'flap' which extended 1" along the X-Z plane, how would one do that?

It's easy to grab an edge with the flange tool, and just make it, but how do you lock the new flap onto that x/z plane? You could work out the math, or use the measure tool, and just define the angle, but that's not really ideal, because if you then change any of the other parameters your angles will now be off, and that flange won't be in the x/z anymore. It's so easy to make a nice 90 degree box, but these angles are killing me. I thought I could take it from here no problem but after a couple of hours of playing around and watching youtube tutorials I'm no closer... I feel like a mouse in a maze looking for cheese. Any more help would be hugely appreciated...

Will

[TheCADWhisperer]

One example.

[will.dameron]

Very nice - but for some reason I can't quite get it to work... if I follow your exact same steps on the timeline, I must be missing a little detail or something. I can get to the lofting part - I go into Patch mode, and loft. Next do a patch on my two 'flaps'. Then a stitch to attach the flaps to the previously lofted body. Then try to fillet the body (which I assume you do because it helps it convert to sheet metal later on when 'thickening'?) where the flaps attach I get, "a blend may not be set on the boundary of a sheet body". Do you know what's causing this? Attached is a mockup that I'm trying to get to work

Will

[will.dameron]

Ugh - I figured it out after hours of trying - when you  use the trim command to make the little cutouts at the corners where the 'flaps' join the pyramid, I had made little half circles - it doesn't like that. I switched them to rectangles and it fillets just fine now. I beat my head against the wall for a while trying to figure that out.

[TheCADWhisperer]

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@will.dameron wrote:

... fillet the body (which I assume you do because it helps it convert to sheet metal later on when 'thickening'?) ...

A sheet metal part must have bends to change direction.  (And to maintain constant thickness.)  The bends must be cylindrical or conical to unfold.

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@will.dameron wrote:

... I had made little half circles - it doesn't like that. ....

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The attached example uses round bend reliefs.

Not to confuse the issue, but in the attached file I manually added the Round Reliefs.  But all I am doing manually is the same thing that can be set up in the sheet metal rules for automatic creation.  My example is that sometimes the automatic tools are restricted in such a way that can make a Design Intent difficult to achieve.  But if one understands the sheet metal rules - they can manually achieve the Design Intent even if the automatic tools don't provide an Easy Button solution.

 

At some point I will have to create an example of this using the built-in "automatic" tools.