topic Re: Use flat pattern and folded model in assembly in Inventor Forum

Use flat pattern and folded model in assembly

hEINSTEIN — Wed, 27 Nov 2019 14:27:47 GMT

Good Day Inventors

I'm building a model for liner plates in a mill. So I'm working with a circular shape.
I have modelled all liners and built the round model of what the liners should be assembled. Using the .ipt’s (Folded model) that I have created.

No I also want to show a layout of the liners in a linear view. Is there any way I can build an assembly with the same .ipt’s but bring them into my assembly as a flat pattern?

So basically I want to use one .ipt file and use it in one model as it should be folded and in the other model use it in its flat form prior to being folded.

I’m sure I’ve seen something like this before, I just don’t see where to find the options to do this

Thank you

Re: Use flat pattern and folded model in assembly

JDMather — Wed, 27 Nov 2019 15:04:58 GMT

Can you zip and Attach example file here.

If modeled correctly - when creating the drawing you can select both finished and flat pattern views for placement on the sheet.

Re: Use flat pattern and folded model in assembly

andrewdroth — Wed, 27 Nov 2019 15:26:00 GMT

I don't think you can do that. There is no solid body associated with a flat pattern.

If you want it linked, I think you would need to make an assembly and then derive that as a sheet metal part -> do an flat pattern from that. But if you have gaps, different thicknesses, or other things going on it might not be straight forward.

Depending on how many parts you are talking about and how many holes there are, it might be worth sending the parameters to new "flat pattern" versions of each part where you remodel the part as flat.

Re: Use flat pattern and folded model in assembly

swalton — Wed, 27 Nov 2019 16:46:53 GMT

One workflow:

Make the sheetmetal part an iPart.
Add an "unfold" feature to the bottom of the model tree in the iPart Factory part.
Make two entries in the iPart table.
1. Suppress the unfold feature for the formed part.
2. Enable the unfold feature for the flat part.

Does the Inventor Nesting program help at all?

Re: Use flat pattern and folded model in assembly

andrewdroth — Wed, 27 Nov 2019 17:02:29 GMT

I forgot about unfold! I think I would just create a second derived part for the flat pattern assembly were you do an unfold. Everything stays linked.

Re: Use flat pattern and folded model in assembly

johnsonshiue — Thu, 28 Nov 2019 03:47:51 GMT

Hi! I guess you are trying to simulate the folding process of a part in an assembly. Flat pattern is actually a dependent body of the folded body. Also, its main purpose is to create the flat sheet to be folded.

You could use Unfold and Refold features to flatten the folded body in folded mode. However, Inventor part and assembly at the moment can only one geometric definition. You will need to derive or copy the files to show the part in different states.

We are aware of the deficiency. We are working on a project called Alternative Representations. If you are interested, please sign up Inventor Beta (https://bit.ly/InventorBeta), where you can try out the latest in-development build on a browser no-install needed environment. And give feedback to the project team.

Many thanks!

Re: Use flat pattern and folded model in assembly

hEINSTEIN — Thu, 28 Nov 2019 05:40:07 GMT

Hi @JDMather

Yes thank you I know about this feature, I think this is what made me think it could be done it the model aswell. Unfolding it in the drawing view won't work as I want to build a model showing the assembly of all the plates.

Thank you

Re: Use flat pattern and folded model in assembly

hEINSTEIN — Thu, 28 Nov 2019 07:10:07 GMT

Hi @johnsonshiue

I would definitely be interested to sign up, but I keep on getting back a "403 forbidden “error message. Do you know why this is happening?

And thanx for the fix to my problem, creating a derived part seems to be the easiest fix.