Creasing/cross-breaking sheetmetal parts? 1

[rossob]

Hi all,

Wondering if it were at all possible to crease/cross-break a sheetmetal part, as per attached image, in NX9?

I can create a flat plate and draw a line/s. Using the bend command allows me to bend one side only. Attempting to bend the second line results in the plate being split, as follows:

At this stage, my work-around is purely to add some lines on the drawing view as an instruction to crease at those locations. Has anyone had any success in doing this a different way, or have any best practices they would like to share? Thanks in advance.

Regards,
Ross

 

[KhimaniMohiki]

I think you'll have to do it in Solid Modelling rather than sheetmetal with the flat pattern being purely the projection of the perimeter.

Khimani Mohiki
Design Engineer - PENSO Consulting Ltd

 

[rossob]

Hi Khimani,
I have managed to find a few ways of doing this.

The first is to create your sheetmetal part, then add a sketch to define the required crease/s. This sketch can then be added to the model reference set, so it shows up in a parent assembly, and then also added as additional curves to the flat pattern. This doesn't look great in a modelling context as you see sketch curves.

The second is a bit more long-winded, but looks much better.
1. Create the sheetmetal part, and add a sketch to define the required crease/s. Add some planes along those crease lines.

2. Extract the body and ensure "fix at current timestamp" is checked.
3. Divide the face using the newly created planes

4. Create a flat pattern, using the required face of the extracted body as the Upward face
5. Add the edges created by the Divide face feature as additional curves
6. Create drawing view/s, ensure that smooth edges is turned on. Callouts to the crease lines will need to be manually added

Ross
NX9.0.3.4
TC V10.1.2.2