topic Re: Convert a hollow solid part to sheet metal flat pattern(s) in Inventor Forum

Convert a hollow solid part to sheet metal flat pattern(s)

Anonymous — Sat, 18 Apr 2015 19:03:00 GMT

Hi all,

I'm designing a simple fuel tank to be constructed out of stainless steel sheet metal. This is a custom fit part with some odd angles, so it was easiest to model a solid with the proper outer dimensions rather than try to make a series of sketches in a sheet metal part. I've used the "Thicken/Offset" with the "intersect" mode to turn the solid into a hollow shell with a 1/16" thickness, but I have no idea how to get this into a sheet metal pattern.

It's a rather large surface to simply unfold into a single pattern, so I was hoping to create two or three flat patterns from the solid that way each pattern would actually fit under our laser cutter. I figure this might be the first step, but whether (and how) to do this with the "split" command or something like the "rip" command in the sheet metal interface escapes me.

Anyway, I'm using Inventor Professional 2014 and the .ipt is attached.

Re: Convert a hollow solid part to sheet metal flat pattern(s)

mdavis22569 — Sat, 18 Apr 2015 19:24:49 GMT

I like rip but that keeps it a s one part still ......split lets "split" them up

Re: Convert a hollow solid part to sheet metal flat pattern(s)

admaiora — Sat, 18 Apr 2015 21:03:03 GMT

Check it out tboettn:

http://forums.autodesk.com/t5/inventor-general-discussion/creating-sheet-metal-around-solid-part/m-p/5548271/highlight/true#M540068

Re: Convert a hollow solid part to sheet metal flat pattern(s)

JDMather — Sat, 18 Apr 2015 21:27:50 GMT

You have done an astonishing amount of extra work for a very simple part.

Re: Convert a hollow solid part to sheet metal flat pattern(s)

Anonymous — Sat, 18 Apr 2015 21:51:07 GMT

The video in the link helps, but it doesn't get around the problem of needing multiple flat patterns. Additionally, the "Bend" tool fails to run on many of the edges that change width due to the "v" shape along the bottom of my design (it can not find the second face for some reason).

Re: Convert a hollow solid part to sheet metal flat pattern(s)

Anonymous — Sat, 18 Apr 2015 22:09:34 GMT

Thanks, I guess.

I only have a little experience with Inventor, and no formal training. I'm a college student, and they only trained us with NX. A lot of the skills carry over, but it's not like my one semester of CAD lessons is enough to make anyone a master.

The design is for my Formula SAE team here at the college. We need a 3D model of the tank at some point or another. Since I'm not particularly familiar with the sheet metal tools and had to export 3D dimensional limits from our top-level model anyway, I just went with a big easy solid model to start with. We still didn't know how we wanted the shape to come out, or what dimensions we needed to hit our target tank capacity, so this had the advantage of being able to make quick visual edits with a readily visible volume property (it's a simple enough shape, but nobody loves three dimensional integrals of parametric functions). Another advantage was that ripping the dimensions from the top level assembly lets us position the tank model in the car with just the "ground and root" function, which save so many headaches.

That said, I'm just stumbling through the process by experimenting with the different features and would love to hear any ideas on more efficient methods.

Re: Convert a hollow solid part to sheet metal flat pattern(s)

mdavis22569 — Sat, 18 Apr 2015 22:25:06 GMT

OK, I'll go a different approach ... what would you like help with on this?

There are tons of sheet metal videos on here and youtube... the question is what can you help you with or direct you to so you can learn...

Mike

Figured It Out

Anonymous — Sat, 18 Apr 2015 23:35:19 GMT

Thanks for all the input guys,

I managed to find a suitable solution to the problem!

Originally, I used "Thicken/Offset" command to make a hollow solid of the model hoping that it would successfully convert into a sheet metal part after I adjusted the default thickness in "Sheet Metal Defaults". But the bend command refused to function with my geometry. I even tried using the "Split" command to divide the part into individual sheet first and load them into their own part files. Now, the bend command did work, but it created very poor trainsitions between faces around bends that changed widths. Namely, they would maintain the width of the first face and then suddenly jut out at a 90° angle to meet the next which creates an ugly flat pattern and a bad mating surface for welding.

In the end, I found the best method was to use the "Thicken/Offset" command to create surfaces at the exterior of my solid model, make them exportable by right-clicking and selecting "export object", then importing them to individual part files with the "Derive" function under the "Manage" tab. I could then create sketches on each face of the surface with an outline of that face (which Inventor is nice enough to do automatically). After converting the part to a sheet metal part, each outline sketch can be converted to a sheet metal face that automatically connects to adjacent faces using the rules and thickness settings in the "Sheet Metal Defaults". Thankfully, it does a MUCH better job creating bends with this method: each surface has a nice tangental curve connecting it.

This solved the issue of cutting the design into mutliple pieces and overcoming the bend command, but I still had to offset some of the edges on each piece to make room for the thickness of adjacent panels (since each piece was the exterior surface of a box extruded inward, adjacent faces generated by different surfaces would overlap). I tried sketching on the faces after converting to sheet metal, but the complex geometry around the bends prevented the "offset" sketch command from having a dimensionable offset distance. Additionally, since each edge was originally a sharp angle, and the new parts had curved bends, the mating edges wouldn't match if they were left in their current form.

Instead I went to each part that would overlap an edge, and created an exportable surface on the new interior faces again using the "Thicken/Offset" command. Then imported the surface into the part that would be overlapped. Then I could use the "Trim" function on the base surface using the imported surface as the cutting tool to perfectly match the edge to the its mating surface.

Ffter each surface was trimmed and converted to sheet metal, I could finally make the flat patterns I need.

Well that only took 6 hours.

Again, thanks for all the help!

Re: Convert a hollow solid part to sheet metal flat pattern(s)

JDMather — Sat, 18 Apr 2015 23:38:33 GMT

@Anonymous wrote:

It's a rather large surface to simply unfold into a single pattern, .....

How big do you think it is?

Re: Figured It Out

JDMather — Sun, 19 Apr 2015 00:24:36 GMT

@Anonymous wrote:

Well that only took 6 hours.

6 Hrs?

My example took 30 minutes (see attached). (and only 2 sketches)

(and my example is fully dimensioned - so editing will be a breeze)

Re: Convert a hollow solid part to sheet metal flat pattern(s)

PaulMunford — Sun, 19 Apr 2015 14:05:30 GMT

Well done for working all this out by yourself!

Here's some tips that could save a couple of steps next time.

Create your master model in a normal part file (it doesn't need to be a sheet metal part). Create a parameter that will drive thickness.

Derive this part using the 'surface' option and sheet metal template files.

You can now model your sheet metal parts using inventors sheet metal tools, and you can even drive the thickness from the master part!

Here's a couple of useful links:
https://designandmotion.net/autodesk/mfg-pages/inventor/autodesk-inventor-distributed-parameters-in-sheet-metal/

Of course, this will be much easier in 2016:
https://designandmotion.net/autodesk/mfg-pages/inventor/autodesk-inventor-2016-sheet-metal-new-features/