Group Melee! How To Convert Imported Geometry to Sheet Metal Parts in SolidWorks Solved!

by Josh on June 18, 2009 · Comments

Hello there! If you are new here, you might want to subscribe to the RSS feed for updates on this topic.

Powered by WP Greet Box WordPress Plugin

Attack I say! Attack and plunder the riches… of … imported… geometry and… stuff. Ok, battle faces everyone, we’re on a warpath today, a warpath to create usable 3D geometric data from imported files.

It’s an interesting issue submitted by a user tired of recreating sheet metal part when he already has a 3D .IGES model, just so he can have a usable flat pattern. Normally, this is easy. You think, “Oh, a simple sheet metal bracket, just use an Insert Bend feature and grab a snack.” But what if it has features that can not be recognized in the process?

That, feature-based fans, is a whole different monster waiting to be slayed. Are you up for it? How would you suggest approaching this problem?

The Sheet Metal Beast!
Here’s the part. You’ll notice it has a very nice form feature the cuts right into the bend. How would you go about converting this imported file into a sheet metal part?

Imported SolidWorks Bracket – (Parasolid File, .X_T)

How can you flatten this imported sheet metal part?

One Solution
Here’s one solution for how to deal with imported geometry, that may seem simple, but is actually made up of unrecognizable features. The tip? simplify it.

Greg Dennis, a Design Engieer with Photo Etch, submitted this solution that removes the faces of the formed area, then turns it into converts it to sheet metal. It leaves out the form area, that you will have to re-create, but it does allow you to get the flat pattern that can then be used for CNC.

Download the imported sheet metal part solution

Thanks Greg for taking this on. If you think you have a better solution or how best to deal with imported sheet metal geometry, leave a comment or email your suggestion to josh@solidsmack.com

(1 votes, average: 5.00 out of 5)

Loading ...

Comments

Tagged as: iges file conversion, importing files, sheet metal

ckeen

I cant wait to see the response on this one.

Stephen Burke

The bottom looks as if it has been created using a form tool. Using convert to sheet metal I made a bit of progress, however the problem comes to this bottom formed section.
I tried FeatureWorks, however I didn't get very far.
It should be possible to flatten it out, however the bottom (formed) region will be very difficult to flatten.

ion

roll back, suppress, reassociate, save as bauhaus part of the first part.

ckeen

The file is coming in as IGES without a feature tree to "roll back".

Vadim

Is it even possible since it has variable thickness?

Ivan-Eden Loewen

hummmm..... hummmmm.... hummmmm... waiting... for the answer josh ;)

Josh M

yep, I'm waiting as well :) actually, there's not a good answer to this problem (except that there need to be better ways to recognize geometry for imported parts.) I'm plannign on going into this a little more in a future post.

Jeff

Thanks Josh for taking my question and submission. The thickness should be the same for both legs. It will need the form for the indent. I did ask your fellow blogger and SW Guru Matt and he suggested using Rhino. Something I know nothing about. Thanks for everyones help and contributions. I look forward to seeing how this can be done.

jmb

Grr... Can't open future version. I would like to try, but i'm still on SW'06. I imagined that as it's imported, it could have been in a parasolid form.

Josh M

I've added a parasolid version above next to the download link. Let me know if you have any problems.

Jeff

Insert into an assembly and build an unfoldable part on top of it. I have to use this method more times than not. There must be a better way?

Stephen Burke

jmb: Indeed. It could have been provided as a parasolid. If you really want to work with it, you could try uploading this file to 3d content central, let it convert it and download it as a parasolid/sw06 version (as far as I remember you could do this).

Jeff: For this part, it would be as easy to remodel the sheet metal over it. I did make some progress with Convert to Sheet Metal in SW09, but it will not convert the entire part due to the form region. It might be possible to close up the cuts around the form region and then convert to sheet metal and go from there. Either way, there is no automagic solution.

Greg D

I have come up with a partial solution using surfacing. How can I post the SW part file?

Josh M

you can email it to me josh@solidsmack.com or you can put a link to where we can download it. Interested to see what you've been able to do! Thanks Greg!

Greg D

I just sent it to you, Josh, along with my process:

I managed to use surfacing to remove the formed portion. From there I noticed that the outer radius of the bend was too small for SW to apply sheet metal features due to constant thickness problems. I used a replace face surface feature to fix that and ran the Insert Bends command to get sheet metal features. I’m not as adept at sheet metal as I’d like to be, so maybe someone who is can pick it up from here.

Josh M

Allright, all you guys following the comments. A solution has been posted in the body of this post. Thanks to Greg Dennis for having a go at this. I think the delete faces approach is about the only way you can get around that form feature. Have a look and if you come up with any ideas, let us know for sure.

matt

Smack,
This guy emailed me this part it looks like the same day that you posted here. The first problem was getting it into SW. It was originally an IGES file from Pro/E, and it had serious geometry problems. The bend faces were not concentric, which would prevent the SW tools from doing anything even if you could get by the forming tool. SW wouldn't read the file, it crashed out with this:

http://dezignstuff.com/images/error.jpg

Anyway, I used Rhino to translate to ACIS, and it worked, although it was really sloppy. It gave a 100 part assembly where each part had a single surface in it. In SW I saved that as a part and knit the surfaces, but there were a couple of very small gaps that had to be patched before it would become a solid.

On something like this I would ordinarily use some Delete Face features to remove the slots and the form, but the translation errors in the original prevented that.

Anyway, here is how I wound up solving the problem:

Http://dezignstuff.com/swparts/shtmtl.zip

That includes the repaired part (which I believe is your parasolid starting point, the artifacts of my repair are still there), features to rebuild the new sheet metal part on top of the old one, and a forming tool to make it work.

To flatten it out you have to suppress the forming tool.

Josh M

There's always a story, behind the story huh. Thanks for sharing this Matt. It goes even further to show how difficult it is to work with (or even import) geometry from other programs and use it for manufacturing. This, to me, is a relatively simple part. It's unbelievable what you had to go through to get it in a usable form. Thanks again.