topic Re: Issue with references in sheet metal part in Inventor Forum

Issue with references in sheet metal part

bozidarJES3S — Wed, 04 Aug 2021 09:42:55 GMT

Hi,

I have made a model of double wall elbow. From a model, I have made assembly of 6 parts. On each part I have to extend edge that touch each other for 5 mm in order to bend them and joint parts in real life. When I add extension to a edge and when I change a model (for example inner diameter from 80 to 100 mm), my sketch of extension loose sketch plane, and my extrusion loose reference plane for thickness. I try to attach a film. What I am doing wrong. Which references should I choose? Or how I could do it on another way.

Please help. Thanks in advance!

Re: Issue with references in sheet metal part

cadman777 — Wed, 04 Aug 2021 13:01:15 GMT

If I understand you correctly, you have a gap in the joint and want to add a 'make-up' feature to fill it. You can prevent that by modeling differently.

The way I make 'gore elbows' is to make a layout sketch and derive it into the separate parts. Then make a simple sheetmetal cylinder and cut it at each miter with a work plane that's attached to the underlying sketch. You won't get those gaps in the joints when doing it that way.

Re: Issue with references in sheet metal part

bozidarJES3S — Wed, 04 Aug 2021 13:30:15 GMT

Actually, I do not have a gap, but at the pipes joint , they overalp each other (one pipe goes 3-5 mm into other like on a attached picture). Therefore I have to make extension of pipes to make this overlapping possible. Or, how to do that in a right way in sheet metal in order to get correct flatterned dimension with overlapping.

Thanks in advance.

Re: Issue with references in sheet metal part

cadman777 — Wed, 04 Aug 2021 13:52:35 GMT

Sorry, but if you must flatten the part in sheetmetal, I can't think of any way to do that.

Maybe someone else in here can?

Find attached 2 examples of how I make gore elbows.

If you want to make a gap, then adjust the model by using the surface method, and by offsetting work planes, and then extruding the surface between them.

Are you sure the gap isn't for welding or joining another way?

Re: Issue with references in sheet metal part

johnsonshiue — Wed, 04 Aug 2021 18:46:49 GMT

Hi! Many thanks for recording the video! I think likely it is a limitation or a bug in sheet metal. The workflow you are using is not a very robust technique. You are altering the side faces (detail faces) by adding more geometry. It inadvertently alters the bend zone. If you want to length the side faces, I suggest you use Direct Edit -> Faces -> Move in 3D Model tab. This will not alter the topology of the side faces and bend zones. The behaviors will be more consistent.

Please try it out and report your findings.

Many thanks!

Re: Issue with references in sheet metal part

cadman777 — Wed, 04 Aug 2021 19:39:12 GMT

I just watched your video.

You can do it using the simple model I provided.

Just offset a work plane from the joint per the distance you want.

Then re-cut the gore segment, and you have your overlap.

See attached...

Re: Issue with references in sheet metal part

bozidarJES3S — Thu, 05 Aug 2021 13:59:26 GMT

Hi Chris,

I've tried with derived sketch in every part as you have done in your example and it work well. I'll accept this as solution. Thank you very much!

Re: Issue with references in sheet metal part

cadman777 — Thu, 05 Aug 2021 15:26:38 GMT

Glad it worked for you!

That's how I've done most of my modeling over the years, and it's never failed me.

It's a bit more 'up front' work, but at the end of a project when the customer says 'change this and that', it's easy compared to the other ways of modeling in Inventor.