Midplane mesh with gaps - how to solve this?

[tasnad.peter_pureco]

Dear All,

I would like to ask you for your kind help! I have to validate the design of a rectangular tank. The tank material is of steel, the load is hydrostatic pressure (2.3m height of water). The tank has steel frames for reinforcement.

The analysis type is “Static Stress with Linear Material Models”. Because the steel thickness is very low comparing with the total size of the tank, I have to use midplane mesh type. My problem is that my frames and the tank are different parts. So after meshing there are gaps between the tank and the frames. I tried to set the contacts of the surfaces manually, but on the result page the frames are overlooked. According to the Simulation Mechanical help with this kind of analysis type it is not allowed to be gaps between meshed surfaces in case of bond contact type.

If I combine the assembly into one part there will be no gaps, so I can run the simulation that considers the frames. However, it would be great to skip this extra step.

Thank you for your help guyz!!

Best wishes,

T.

[John_Holtz]

Hi T.

The best solution would be if the software would generate the contact between midplane meshes in linear static stress -- which it does not. But I see that it is a popular request on the Ideas list. Please add your vote to Midplane meshing contact.

All of the other options require some amount of work by the user. Here they are in no particular order:

1. Run the analysis using nonlinear. The nonlinear analysis type (either MES or Static Stress) has a special type of surface contact known as "tied contact". It will bond the surfaces together even when there is a gap between surfaces and the meshes do not match. You can set the shell element's "Element Definition" to be small displacement to make the nonlinear analysis ignore large deformation effects and give a result more like linear stress. This option may be the easiest to setup, but convergence in a nonlinear analysis is a potential issue to deal with. (Try performing 1 time step instead of multiple time steps.)
2.  Draw contact elements. There is a command that will draw lines between two sets of nodes: "Draw > Design > Contact Elements". You could use this to create beam elements to simulate the weld connection between the edge of the stiffener and the sidewall of the tank. The beam elements would be somewhat random length and orientation depending on how close the mesh on the stiffeners and sidewall were to matching. (There is an option to limit the length of the lines created, so contact between the entire tank and all of the stiffeners could be designated, and the command would only generate lines for the "closest pair of nodes".)
3. Mesh selected surfaces. Instead of generating plate elements at the midplane of the thickness, in some cases it may be acceptable to generate the plate elements at one of the surfaces of the solid. (This would work if the parts are large compared to the thickenss.) For example, mesh the "outside" of the tank and the "outside" of the stiffener. Since these surfaces are in contact, the parts will be bonded. you can select "one side" of the CAD solid model to mesh, and define the mesh to be plate. (In Simulation Mechanical, you would select surfaces that you do not want to mesh, right-click, and choose "CAD Mesh Options > Suppress for Meshing", and set the "Mesh > Mesh > 3D Mesh Options" to "Plate/shell".)
4. Make a surface model in CAD. Many CAD applications can create a surface model, either by creating a surface at the midplane of a part, or by offsetting a surface. After generating the surfaces, the new parts could be moved to bring the midplanes into contact.

The first three options are shown in the attached images.

[John_Holtz]

Hi @tasnad.peter_pureco,

A separate post on the forum a few days ago (Midplane mesh with gaps - welded contact is not working) highlighted a feature that I was not aware of, and it would also work for your modeling. If you have the Nastran solver ("Analysis > Analysis > Run Simulation > With Nastran" from within Simulation Mechanical), then you can use the Nastran contact type of "offset weld" to connect the two midplane-meshed parts together! The offset weld is similar to the tied contact that I described, but the offset weld is available in linear static stress.

Let us know if you have any questions.

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[John_Holtz]

Hi @tasnadipeter

I wanted to follow up with you to see how your modeling is going. Do you have any other questions?