Rolled Plate

[zack_wallworkEKCKR]

Hi all,

I've had a look and can't see this problem anywhere else so I'm hoping someone can help.

I need a rolled plate to be welded on the outside of a vessel.

I have made it in sheet metal using a contour flange, then flattened it to cut around the bits I don't need so it is equal thickness all round. After I have done that, I have no flat sides to use as a stationary reference for when I re-fold so it is currently stuck in the flat pattern.

Does anyone know how to add one without adding or cutting bits away from the part?

Part attached for reference.

Thanks in advance!

[Frederick_Law]

Add a "flange" on one side.  Set flange length to 0.0001" later to "hide" it.

You could do the cut without unfold refold.

https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-D7D99832-BE8E-4986-9BF5-F7A986F063FA

[kacper.suchomski · Accepted solution]

Hi

Point to the re-bend command in the browser window (right-click on unfold).

[kacper.suchomski · Accepted solution]

Moreover, if the flat pattern is to be correct, the surface resulting from the cutout must be perpendicular to the face of the sheet metal.

For this purpose, you can perform an intersection operation (from the inside to the outside) or replace the hole operation with a cut tool using the "perpendicular cut" option. (I understand that you want the hole to be evenly round after bending the sheet metal.)

You can also read and reflect on my last post in this discussion to become more familiar with these tools.

https://forums.autodesk.com/t5/inventor-forum/possible-in-inventor/td-p/12401059/page/2

[zack_wallworkEKCKR]

Hi,

Thank you for your reply. When I click to re-fold, I get the attached error message, do you know why it doesn't appear on yours?

Also, the second video you sent over looks like it could be exactly what I'm looking for. Could you give me a little step by step please? I'm trying to follow the video but your page is set up a lot different to mine and I'm struggling to convert the language. What action was it you took when swiping up?

Thanks,

Zack

[kacper.suchomski]

Thicken - you can see by the icon. Inventor is hieroglyphics and pictorial writing.

[zack_wallworkEKCKR]

Hi,

Thanks for the update. I have followed your steps & I'm getting the attached error message. This seems exactly what I'm after but I'm currently unable to implement it. Any ideas?

[kacper.suchomski]

I don't know what you're doing. I can't see what and where you click.

[zack_wallworkEKCKR]

Hi,

I have clicked around & it has worked now.

Between the refold command & the thicken command, you're a life saver. 

Thank you very mmuch!

[zack_wallworkEKCKR]

Hi,

Sorry for pestering but can you talk me through the refold? It currently won't let me do it after I have thickened the part up. I have attached the screenshot & updated model for reference.

[kacper.suchomski]

Why do you have many unfold for no reason?

[zack_wallworkEKCKR]

I have been adding them on each time I have tried & failed to fold & refold.

It looks like my extrusion while flattened is the problem but I can't see how or why. 

I have deleted the first few fold/unfolds now & it has the same problem

[zack_wallworkEKCKR]

I'm so confused. I am doing exactly as you show in the screen recording but I keep getting the attached error message.

I have deleted all unnecessary fold commands but it doesn't want to play ball.

[kacper.suchomski]

What version of the program? Do you have all the updates?

[zack_wallworkEKCKR]

I'm using Inventor 2023 & it doesn't seem to need any updates.

Does the updated model I sent in the last message work as expected for you like the old one did?

[kacper.suchomski]

You should have version 2023.4.1

[zack_wallworkEKCKR]

I'm currently running 2023.2.1 & our IT department take an age to come back to us. Do you think that could be the problem? did the most recent part work as expected on your machine? 

[kacper.suchomski]

I don't know, I'm using version 2024.2.
But updates are used to fix bugs and problems, among other things.

Do it by hand. Sketch the bend line and use Bend on both sides with the appropriate radius.

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-CDC8A285-2675-4993-9C5B-225938A75018

[SBix26]

Here is one way to fix up your file (Inventor 2023 format).  Instead of making the initial contour flange much wider than necessary, I made it slightly less than necessary (on one side), leaving a small flat on the eventual extruded part.  This allows for the stationary reference to survive the extrusion process and then the Refold operation can succeed.  I then used Delete Face with Heal to remove the little flat.

I changed your Hole feature to a Cut with Cut Normal checked, which removes the need for the Thicken/Intersection feature, but that's purely optional. 

I'm curious why this part, entirely dimensioned in inches has millimeters as its length unit?  I changed it to inches.

---

Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[kacper.suchomski]

Alternatively, you can do it manually.