Bonded Contact Usage

cmcnamara

Hi,

I am working on a project in graduate school on the design of a solar panel. I would like to model the frame and glass subject to a wind pressure. I have modeled the frame and the glass as separate CAD models that I have imported as .STP. I have a bonded contact BC on all four edges of the plate glass which are slaves coupled to their respective master surfaces in the aluminum frame. Unfortunately when I attempt to solve I get multiple crashes concerning improper constraint for many nodes. Is there something I am missing on the usage of this boundary condition?

Sergio

Can you share the model? Maybe I could take a look and see what happens.

Regards

Victor

Thanks Sergio - it's always helpful to see the model.

I suspect in this case that there may be other constraints on the same nodes. A limitation of bonded contact in Mecway is that you can't put any other constraints on the slave nodes, and if there are other constraints on the master nodes, they should typically be in all 3 directions.

If you must have constraints there, a workaround is to extrude a thin layer of elements from one surface and use the bonded contact on the new outer surface. Then you can constrain the original nodes which are just next to it. You could use Mesh tools -> Extrude for this but then you'll have to redo it every time you regenerate the mesh.

If the constraints are frictionless support, or only normal to their surfaces, a much simpler workaround is to use elastic support instead, and specify an arbitrary high stiffness.

cmcnamara

Hi guys,

Thank you for the support. I have attached the model for your viewing. I think that the case may be that there are loads applied to front surface of the glass which the side nodes would also be constrained by the bonded contact. I am not sure yet and have not re-run the model following changes to this. I will re-run and update you. Great, inexpensive program by the way!

VMH

Can you also provide the .step files? Thanks

Victor

Thanks for the file Eric. It's none of what I said in my last post. There are two problems causing this error:

1) The nodes on each corner of the GLASS part are slaves of two sets of bonded contact, which isn't allowed.
2) The 4th bonded contact is a duplicate of the 1st.

Problem 1) isn't very easy to solve. I did it by deleting all the corner elements of GLASS. There are so small, they probably don't have a significant effect on the solution. But you'll have to delete them again each time you regenerate the mesh. If you can bevel the corners in your CAD model or put split face edges near them that would be ideal.

Another potential issue is the very high aspect ratios of some elements in the frame. Expect poor accuracy of stress in these regions, and possibly too much stiffness.

VMH

I went ahead and took dimensions of your model and recreated it. The holes are not correct but good enough for demonstration purposes. Like Victor mentioned, you need to chamber or bevel the glass edges so the bonded surface don't share nodes. You can also get a better meshes by tweeting Mecway meshing options so you don't have too much elements at sharp corners and have a more uniform meshes to get better aspect ratios. Local meshing can also be added at local areas you need more elements. Note that the meshes I used can be refined further to get better results and check previous results for convergence. Just a note, for glass type material (brittle), von Mises stresses would not be ideal (good for ductile materials like steel).

Creating model, exporting, importing, meshing, etc. are shown on the video (download and view) in the following link:

https://www.dropbox.com/s/z3ygfx6t7jqnhpk/frame.mp4?dl=0

Victor

Thanks for another excellent comprehensive video VMH. It seems to finish quite abruptly in the middle of setting meshing parameters. Maybe that's just my internet connection. But it still captures pretty much the whole process.

VMH

Thanks, if you view it on the web browser than it has a 15min limit on dropbox webpage and the quality is not great. There should be a download tab that you can download the video (HD quality). The run time is about 26min (I purposely made a few trial and error just to show tweeting of the meshing parameters so the video is a little longer than I would like it).

VMH

I realized that my model didn't have the similar height as the reference model so I went back to edit the created geometry and redo FEA.

Video link (download to view):
https://www.dropbox.com/s/qo6nwxrvxf4a9l6/frame revisit.mp4?dl=0

cmcnamara

Apologies for being absent from the thread for so long, its finals week

Thank so for the guidance, I'm going to take a look through the videos and see if I can replicate the same scenario that you have VMH. I'll also take a shot at beveling on the CAD model to see if I can streamline the process some more for my mesh independence studies.

Also thank you for the pointer on the von Mises stress, I had planned on using the principles due to the brittle material but it is nice to have confirmation.

Again thank you so much, I'll report back with my attempts later this week!

VMH

Uploaded to YouTube:
1st:
2nd: