topic Re: Cutting up a single sheetmetal into multiple in Inventor Forum

Cutting up a single sheetmetal into multiple

B_Bevelander — Wed, 17 Jan 2018 15:04:04 GMT

So im working on a box that I've turned into a sheetmetal, but it being a single flat pattern makes it impossible to bend it all.

Is there a way to cut up this single flat pattern into multiple so they can actually be properly folded and assembled?

Attached I've added the part im working on.

Re: Cutting up a single sheetmetal into multiple

mdavis22569 — Wed, 17 Jan 2018 15:17:10 GMT

So you want to make this into how many pieces

Also, what version of Inventor? Have you considered making a multi-body sheetmetal part?

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2016/ENU/Inventor-WhatsNew/files/GUID-B0691F9D-46AF-40CB-93D5-977658927A83-htm.html

Re: Cutting up a single sheetmetal into multiple

NigelHay — Wed, 17 Jan 2018 15:27:16 GMT

It also looks like the flat pattern is too big to cut from a single sheet.

Re: Cutting up a single sheetmetal into multiple

Thomas_Savage — Wed, 17 Jan 2018 16:11:01 GMT

Hello,

You will need to make this in 2 parts.

Using Multi body like @mdavis22569 said.

I have create 2 solid bodies from your 1.

I did this by Cutting a radius (You could use rip as well).

Then Thicken offset a surface.

Then Delete face. And select the parts of the model i did not want, and wanted to make in to another part.

Then Thicken offset, using Thickness.

Then using the bend command to add bends to the sheets.

I will attach a screencast for you. It is just now working at the moment.

You can place the cut (rip), that creates the other solid body anywhere you want. I just placed it there.

Hope this helps?

Thomas.

Re: Cutting up a single sheetmetal into multiple

Thomas_Savage — Wed, 17 Jan 2018 16:23:45 GMT

Hello @B_Bevelander

I have finally got my screencast to upload!

This is how i created 2 solids from 1. So you can flat pattern them both.

It is best to model these as 2 separate parts. Instead of 1, and doing this. So when you create a new Face, select that as a new solid. Then place flanges on it.

But this still works fine.

Hope this helps,

Thomas.

Re: Cutting up a single sheetmetal into multiple

B_Bevelander — Thu, 18 Jan 2018 08:56:24 GMT

Would it also be possible to just copy the part and have 2-3 parts total with different cut faces? and then thicken that?

Re: Cutting up a single sheetmetal into multiple

Thomas_Savage — Thu, 18 Jan 2018 09:21:16 GMT

Hello,

Do you mean create 2-3 parts, then on each part the cuts (rip) is in different places on each part?

So you end up with different flat patterns in each part?

You could do that if you do.

Thomas.

Re: Cutting up a single sheetmetal into multiple

B_Bevelander — Thu, 18 Jan 2018 11:11:11 GMT

Trying to copy the part leaves me with surfaces I can't seem to thicken ..

Need to try a different approach, As what i did, was make a part and turn it into sheetmetal, instead I want the start with a sheetmetal right away and then add flanges to get this similar size, any tutorials out there that explain in depth how all the features of sheetmetal work?

Re: Cutting up a single sheetmetal into multiple

Thomas_Savage — Thu, 18 Jan 2018 11:21:19 GMT

Hello,

Can you not Save copy as. Then Change where the cuts (rip) is?

Could you show me where you want your cuts (rip) on the different parts?

On YouTube you will find loads of tutorials that explain Sheet Metal in Inventor.

You need to look at Multi Body Sheet metal also. I have attached a link below.

https://www.youtube.com/watch?v=M3npmmadpO0

Thomas.

Re: Cutting up a single sheetmetal into multiple

B_Bevelander — Thu, 18 Jan 2018 11:25:29 GMT

Thanks for the help, I'll look into things and see whats the best approach for this and future projects.

Re: Cutting up a single sheetmetal into multiple

Thomas_Savage — Thu, 18 Jan 2018 11:31:19 GMT

You're welcome

Thomas.

Re: Cutting up a single sheetmetal into multiple

Anonymous — Fri, 19 Jan 2018 01:19:35 GMT

Another way and it has worked well for me.

Create the shape as a solid, create a new sheet metal part and derive the solid parts in as a surface.

Create a sketch on each surface required, project geometry of each line bounding the surface.

Once you have a closed sketch, create face, repeat on adjacent faces, if the face you are creating has multiple options for bend you will have to pick the line where you want the bend.

once you have all the faces that can be bent from one pc of sheet metal repeat for another part.

All editing for shape is done on the solid part

Resulting parts are then put together in an assembly using origin.

See attached examples, put all 3 in same folder done in Inventor 2016

Face test is the solid part, you may have to point to it for pt 1 and pt 2 to work