Flanged sheet metal assembly help, please.

[HCb]

Hello, I've been drawing on this basic design off and on for weeks and finally gave up and came to ask for help.

 

What I'm trying to do is take a simple shape, a truncated pyramid, and design sheet metal panels which, if manufactured, would wrap around the pyramid and form a funnel or hopper or such. I model a pyramid, truncate it, and create sheet metal sides for it, no problem. I can join/constrain the panels (4 instances of one part file) without issue. However, I want to put flanges on it such that, if this thing was actually made, one panel design formed 4 times could be assembled with screws or bolts.

 

When I attempt to add the flange I have problems. First, I offset one face of the panel by the sheet metal Thickness, and thicken the other side's face by the same amount. I create a flange on the thickened side, measure the angle (which I have to tweak) and get it where the flange, with "all precision/decimal places" shown, shows to be 180 degrees. But, the first panel doesn't line up, and Inventor pitches a fit (rightfully so) about the Mates and such referencing geometry which no longer exists.

 

I have two assemblies, each with its own panel. TestAssembly2.iam shows how the panels come together before I attempt to put the flange on the part. The arrows on the panel are there so I get the part put on the same way in the assembly for each of the 4 instances of the part. TestAssembly.iam shows the part with the flange on it (and no arrow which is where I got a panel on backwards and had to change it, hence the addition of the arrow on my next attempt). I got the flange on the part okay, and got it constrained, but if you look at Side1:3, you'll see it's actually embedded in the truncated pyramid.

 

I'm using Inventor Pro 2015. I found lots of information about how to use sheet metal tools in Inventor, but have not found anything that clarified for me how to assemble sheets with a connecting flange. This shouldn't be that difficult, I wouldn't think, so I suspect that I'm doing something fundamentally wrong.

 

Thank you for your time.

 

--HC

Pyramid Solid.ipt

Side_R2.ipt

Side1.ipt

TestAssemblies.zip

[HCb]

I've made some progress. Here are the steps I went through to get this to work. I had to use some trig to get this to work which I'm pretty sure means I'm not doing something right in Inventor (thank God I remember SOD CAD and TOA from 27 years ago).

 

First, I modeled the solid pyramid (as attached previously). Then I used Inventor to tell me the angle (all precision/decimals) from one face to the adjacent face, about 107 deg:

 

 

This angle is subracted from 180 to get the FlangeAngle, about 72 (OffsetAngle). That is about 18 deg. The sheet metal Thickness divided by the Cosine of that angle gives the OffsetDistance for Thicken/Offset, about 0.0785 inches:

 

 

With the pyramid in a new Assembly, I hit Create Part and selected a Sheet Metal part template:

 

 

I then clicked on one of the faces of the triangle, then Start 2D Sketch, then clicked on the same face of the triangle, then Project Geometry and then clicked on the entire face:

 

 

After hitting Finish, I created a Face from the sketch. The next steps were fairly easy (I arbitrarily decided to put the flange on the right side of the panel): I Offset the left side of the panel to allow clearance for the bend of the flange from the adjoining piece (when all panels were put in place in the Assembly), and I Thicken(ed) the right side to allow the flange to reach beyond the adjoining panel on that side. Both Offset and Thicken commands were done using the OffsetDistance shown in the screenshots above. I then added the Flange and used the shown FlangeAngle as the angle.

 

 

In another file, to test this process, I assembled four instances of the same panel and constrained them by face and by vertex (I think that's the word; the single line along the edge of a face), and got zero warnings or errors (a first in my very many attempts to do this). I'll attach the part and assembly files.

 

I used AutoCAD to draw the joint in 2D to figure out how to measure the OffsetDistance (which is where I saw that I had this angle and that measurement and used CAD (Cosine = Adjacent / Distance) to arrive at the OffsetDistance (FYI). I'd love it if someone could tell me how I could have measured that distance with Inventor and some mouse clicks (although, now that I know how to calculate it, it's kind of moot).

 

I didn't attach the Pyramid model here because it's the same file I posted originally.

 

--HC

TestAssembly6.zip

Panel5-1.ipt

[twdant]

I hope this isn't too late, just found this forum.

 

Attached is an unfolded sheet metal pyramid with adjustable parameters for base width, top width, and height. I hope this helps.

 

-Tanner

Pyramid Funnel.ipt