# Solid model to shell model

• 74 Views
• Last Post 30 January 2019
• Topic Is Solved
dimgi posted this 28 January 2019

Hi all,

I am trying to run a structural simulation of a model from shell elements. I had the solid model and the procedure that I followed to succeed it was to create surfaces from the faces. Also, I chose middle in the offset type and I defined the thickness of the shells as the solid thickness/.

Do you think that the way that I followed is correct ?

sathya posted this 28 January 2019

Hi, You haven't shown the complete model.So it is incorrect to say that the setup is fine. But seeing from the model tree, you have four surface body in the part body. If it is a closed geometry you could have used Boolean to stitch the geometry. If you could show the applied force magnitude and corresponding reaction forces, only then we can say whether it is correct or not.

dimgi posted this 28 January 2019

Hello, the magnitude of the force is 1000 N. In the picture below you can see the model

sathya posted this 29 January 2019

Hi,

It should be fine if the resultant magnitude is also 1000N.

If needed you can run the setup with Body operation > Sew to make it as single part single body.

dimgi posted this 29 January 2019

Hi, I have another question. If the offset type is middle should I define the actual thickness of the shell or the thickness divided by two? Many thanks

jj77 posted this 29 January 2019

You define the thickness of the shell (not half).

dimgi posted this 29 January 2019

Hi again, I am having a problem possibly due to contact issues. How should I well defined the contact of surface bodies ?

jj77 posted this 29 January 2019

Can you post/attach your model so we can have a look.

jj77 posted this 29 January 2019

Thanks, but my virus system blocks this. Can you please use the Attach button next to your post.

dimgi posted this 29 January 2019

I think that I uploaded it.

jj77 posted this 29 January 2019

I would make all parts a multi body part, then no need to define a contact (the contact is not working as it is). Assuming the gap/penetration is not too large (seems to be typically about 0.05 m as seen from the contact tool)

Insert a contact tool and you will see it is far open.

You can close it by adjusting the pinball region under the bonded contact settings (say make it 0.05 m), and that works. have in mind though that parts are far away still, so you might need to bring them closer in order not to get this warning (closed contact but large gap).

Also I would define the contacts manually, by selecting connected edges (not faces). You can show and hide bodies to pick the correct ones.

dimgi posted this 29 January 2019

Yes, but if I do it like this then the mesh that is generated is not well defined because areas are overlapping

jj77 posted this 29 January 2019

Adjust it then so it is not overlapping or have too large gap. Or define the contacts manually (see image below, cont. 1,2,3,4,..) edge by edge so you know what is going on (finally check the initial contact with the contact tool).

dimgi posted this 30 January 2019

Hello and thank you for the reply. That seems to be the solution. I have defined two contact regions what are the other two ?

jj77 posted this 30 January 2019

I think I had, one for the left tube with the middle plate edge, one of the right tube with the middle plate edge, one for the right tube with the bottom stiffener (their edges), and one for the middle plate with the bottom stiffener (their common edges). Not sure if the last two are needed since the mesh might be compatible there.

In any case you know how this part is welded together so just connect the edges that are welded.

I would also use MPC for the bonded formulation, and then you can look at the MPCs when going to the Solution Info, and clicking on the graphics window.

dimgi posted this 30 January 2019

Many thanks

• Liked by