How can I convert a 3d face into a flat pattern?

[Anonymous]

I got an ipt which was created in a weird way (revolve, shell, spline, etc.), and am thus unable to easily convert the parts into flat patterns. I need to convert each little section into a flat pattern of its own. I am able to select the face i want converted into flat pattern. From here, am I able to do anything to easily convert it into a sheet metal and then a flat pattern? Maybe a 3D sketch of some sort? Appreciate it!

[DRoam]

Hi levi97. You should be able to follow these steps to get your flat patterns:

1. Start the "Thicken/Offset" command from "3D model" tab --> "Modify" panel
2. Select a face that you want to use to make one of your flat patterns
3. Select the "New solid" button (). (You may have to toggle between "Solid" and "Surface" on the "Output" options to get New Solid to be selectable, it's kind of buggy sometimes)
4. Look at the green-lined preview, and make sure it's going the direction INTO your part (as if you're re-creating it--which you are). If it's not, change the direction with the buttons withthe orange rectangle and black arrow.
5. Give it the proper thickness
6. Click "OK"
7. Do this for each part that you want a flat pattern for. Make sure and select "New solid" each time.
8. In your Browser tree, click the first new solid you created (it should be the second one). Hold down "Shift" and select the last one, to select all of your new solids.
9. Go to "Manage" tab --> "Layout" panel and click "Make Components"
10. Choose a name and location for the new assembly which will contain all of your new "Sheet metal" parts.
11. Click "Next". Use the default settings and click "OK"
12. Save the new assembly.
13. You now have an assembly containing one individual Part for each piece you need. You can now open each one, convert it to Sheet Metal, and it should function as a proper sheet metal part for which which you can create a flat pattern.

Let me know if that works for your or if you have any questions.

[Anonymous]

Hi Droam, thanks!!! 

I was able to get way further than I did on my own. I isolated each part on it's own, however when I click to convert into a flat pattern, it doesnt do it. It simply dissplays the bent piece while showing that it is folded

[JDMather]

Can you start over from scratch and create the parts in the proper way?

[DRoam]

A couple of things to check:

1. Once you've pushed your geometry into a part, after you click "Convert to Sheet Metal", when Inventor asks you to pick a Base Face, make sure you pick one of the big faces that you want to become flat.
2. Once you've converted to  Sheet Metal part, make sure your Sheet Metal's defined Thickness is exactly the same as the thickness of your geometry.

Since you've already converted your parts, I would find the button that says "Sheet Metal Defaults", click the drop-down that says "Setup", and click "Convert to Standard Part". Then convert it back to sheet metal and follow the above guidelines. Let me know if that fixes your issue. If it doesn't, feel free to attach one or more of your parts and I can take a look.

[DRoam]

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@Anonymous wrote:

Can you start over from scratch and create the parts in the proper way?

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JDMather's suggestion is definitely a good one to follow if you have the time.

Depending on how it was constructed, you may be able to mostly use the original Part but use multi-body techniques to make each piece a separate body to begin with. That's more robust than grabbing faces and offsetting them as I described.

That's all assuming that by "the proper way" JD meant using multi-body modeling [EDIT: and sheet metal tools]. That's how I would do it anyway.