Bend - Curved surface

[Lukin]

Hello everyone,

I would need advice on how to make bent flanges on the enclosed part.

The bends should look like the attached picture. The requirement is that the sheet is round and not bent into pieces.

While searching, I came across the fact that the SW is not able to make bends on a curved surface.

Unfortunately, I do similar things quite often and this is quite limiting.

Any ideas or tricks?

Thank you all for any advice, ideas or tricks.

 

[Lukin]

I will add that then after SW I want calculated unfolded pattern.

 

[HaroldL]

Your image looks like a Contour Flange part in section. It's not clear what is the end design supposed to look like. Where on the Lofted SM part are the flanges created?

 

[Lukin]

Your image looks like a Contour Flange part in section. It's not clear what is the end design supposed to look like. Where on the Lofted SM part are the flanges created?

When you download the attached model, bends are created in that cut-out area of the component. In other words, if you imagine that you would cut the downloaded model roughly in the middle and the cutting plane would be parallel to the XY plane, a shape would be created as in the attached picture.

 

[HaroldL]

Would it be anything like this:



These flanges were added by using Part Modeling tools to extrude a sketch along the edge of the cutout to the end face of the cutout. I created a Precision Section view then Projected to Sketch the edges of the cutout. After Locking a sketch line for the thickness I sketched the rest of the flange profile then did the Extrude Boss.

I did have to modify your cut sketch a bit to get a straight edges. As you open the model and examine the sketch you will see the mods I made.

You will not be able to flatten these flanges so it is best to create them in a Configuration. You will need to create a second configuration for the flat pattern and add the developed flat for the two flanges to it.

 

[Lukin]

Thank you for your work and for your time. You understood it and did exactly as it should be.

I have two questions:

1. How do you get from standard sheet metal module to common modeling (for example, extrusion type)? I can switch from a normal part to sheet metal, but on the contrary I don't see the possibility.

2. What did you mean by that configuration?

Is it necessary to first make an exploded pattern of two flanges, then the main component and connect this manually (draw in 2D)? SW just can't do it automatically at this moment?

Thanks again.

 

[HaroldL]

1. Make sure you have the Part Modeling tab turned on in Sheet Metal. While you are in the sketch you can select the Part tab from the ribbon then select the Extrude Boss tool to create the flange.




2. You can add configurations by right clicking on the Configurations label in the Design Explorer. You can then name the new config and make it active so you can work on it.



In the Flat config you can add the material for the flanges as sheet metal Tabs. Just be sure to calculate the flat development for them. Here's a model with configs added for examples. I just applied some guess work to the two Tabs I added for the flanges in the flat config.

Double click on the config that you want to see or work on to make it active.