Tapered Pipe Pattern to a Flat Pattern Sheet Metal

[ryan]

I am completely new to Inventor.  I have done the bottle tutorial and before that I used Inventor in HS for about 2 weeks.  I have done a couple small projects on it but nothing major.

I am trying to "unwrap" a pipe to a flat pattern for something that would be burnt out of flat sheet.

Here's what I've done so far:

- Made a 2D sketch of the profile of the pipe sidewall.

- Revolved that around the center of the pipe to create an 8" O.D. x .25" sidewall x 4" lg. pipe (this part appears exactly how I wanted it)

- I mitered each end of the pipe @ 1" to create a wedge (or a piece of pie) type-shape.  My part is now looking exactly like I need to look when complete.

- I cut a 1/16" sliver out of the pipe @ the short side of the pipe (2" lg. side after miters) to create something that could actually be "unwrapped" into a flat sheet.

This is where I run into problems:

- I select the inside face of the pipe

- Click "Create Flat Pattern"

- I get the attached error message in the photo.

I have attached a picture of the error message I am getting.  In the pic, you can also see my model (with rust finish on, looks nice) and the sliver that I have cut out at the top.

My question, what do I do from here to see the inside face of this pipe as a flat pattern capable of being burnt outo f sheet metal?

(Inventor 2013)

[JDMather]

Here is one technique

[ryan]

JDMather,

I'm not sure I follow?  Can you elaborate on what I should do next?  I see your yellow line when I "Go to Flat Pattern".  What is that and how would I create that?  I have attached my part.

Thanks.

[JDMather]

You Revolved a Rectangle as a solid body.

I revolved a line as as a surface body.

[JDMather]

I then Trimmed the surface

and then Thickened the surface by the sheet metal Thickness parameter.

You did an Extrude-Cut that results in wrong geometry for sheet metal.

Sheet metal is uniform thickness with edge sides parallel to flat sides.

[JDMather]

Similarly the Rip (Extrude3 in your part) should be done with a pie wedge shape rather than a rectangle to keep the sides parallel to the flat in the flat pattern.

[JDMather]

Here is your part made from your sketches (with a couple of changes).

Make sure you set the Sheet Metal Defaults to the intended Thickness setting.

If you had done that (you had on .12 not .125) your original part would have unfolded but is not technically correct.

[ryan]

Ok, so I revised the file to be similar to what you have and it is still not working.  Wha am I doing wrong on this one?  Could you please elaborate as I do not have much experience with Inventor?  Thanks a lot for your help, I appreciate it.

[ryan]

I only saws your first message when I posted this.  Let me try these things and see if I can get results.  Thank you.

[ryan]

Lost again...

Attached is my new file.  I don't understand what I'm doing wrong.  I followed all your steps from scratch and it will not lay out the flat pattern correctly.

[ryan]

Lost again...

Attached is my new file.  I don't understand what I'm doing wrong.  I followed all your steps from scratch and it will not lay out the flat pattern correctly.

[JDMather · Accepted solution]

If you go back to the original example I posted I did the Revolved surface 359.9° so that there was a small gap.

You did a Full revolve.

In the second example, instead of a partial revolve I did the Full revolve but then added a Rip feature to get the gap.

[ryan]

JDMather,

I was finally able to recreate this successfully!  Thanks alot for your help!  I am taking an Inventor Basics seminar offered by Autodesk in a April but am still tinkering with it now.

[JDMather]

Do this http://home.pct.edu/~jmather/skillsusa%20university.pdf

and these

http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm

I have another good link on my home computer that I'll post later.