Connections of SHELL/SOLID elements

[Sampetai_Koen]

I have designed and assembled some solid parts in Autocad Inventor and then imported them as a single .step file in Ansys WB in order to conduct Modal Analysis to this structure. However, I needed to use plate/shell elements to some of those parts, as their length is much larger than their thickness (>20 aspect ratio). I did so by using the midsurface in Ansys Designer Modeler, which created a surface of a specific thickness, let's say 3mm. Then, I tried to make sure the connections were correct, and I used MPC formulation along with Projected, Uncoupled U to ROT Constraint Type, as I saw in some videos from Ansys page in YouTube. However, when using the Contact tool I get the orange Color Legend, and indeed there is a very big Gap and Penetration between the part (almost 1.3 mm max). I am confused regarding how I should handle the surfaces and their contacts with the solid parts. Should I create a top and bottom mid-surface to make sure Ansys undestands the connections? Should I try to take care of the gap and penetration by changing the Formulation? Should I use the surface Extend as I have seen in some videos? Apart from that, I would like to know if I am able to do model updating through Inventor and update the geometry directly in Ansys WB, as well as how should I do the meshing convergense study (should I keep changing the element size to converge as much as possible to the desired ones?). Thanks in advance!

[peteroznewman]

It would be helpful if you include some images of your midsurface and solid bodies and show the gap.

Generally, when midsurfacing a thin-wall solid body of a Tee intersection of a plate with a rib perpendicular to the plate surface, there will be a gap and you do want to extend the surfaces.

Try SpaceClaim instead of DesignModeler, you may find it easier to use.

Review this chapter to see how to connect shell and solid elements when the faces are touching. https://innovationspace.ansys.com/courses/courses/fea-for-large-telescope-truss/lessons/physics-setup-lesson-5-10/topic/2-solid-surface-to-shell-surface/

When a straight edge of the shell touches the face of the solid elements it is important to select the edge for the contact and the face of the solid for the target and use a Pinball Radius to allow the bonded contact to find nodes on either side of the shell edge to support the rotation of the shell about the straight edge.

[Sampetai_Koen]

 

Unfortunately I cannot post any pictures. However, it basically is a thin cylinder with two wings that are NOT connected to the cylinder (there is an offset between them). Instead brackets are both connected to the wings and the cylinder, above and below the wing. They are normally connected to the cylinder by inside brackets, which I have designed, but instead of bolts, I have used the bonded contact/connection. As I said both the cylinder and the wings are considered thin surfaces according to the aspect ratio, that is the reason I want to use plate elements on them. Is there a chance that I have to create two surfaces using the midsurface tool (both in the wings and the cylinder), one interior to connect with the inside brackets and one exterior to connect wi the outside brackets in the case of the cylinder, and respectively one to connect the upper brackets with the top surface of the wing and one to connect the bottom brackets with the bottom surface of the wings?

 

[Dennis Chen]

Hi Sampetai, it's pretty unclear exactly what your problem is from your text in your messages so if I may suggest something:   try creating the simplest possible form of the problem by using dummy shapes (cylinder, square, rectangle, etc) to see if you can recreate the issues you are seeing.

A few things to think about regardless of how you look at the problem (simple first principle representation with dummy shape or your real life project):

1) shell element nodes have 6 DOF while solids have 3, if you use MPC contact, you do not tie the RDOF together.   this isn't necessarily a problem but it can be.  this is also why penalty based formulation is better for this (augmented lagrange or pure penalty)

2) look at shell element offset, and usually it's a good idea to turn it on and adjust your pinball radius accordingly

3) check yoru shell element normal direction in the contact setting as well, as this also affects contact tool results

4) contact tool initial status gives you a very good idea of how the contact behaves at the start of your analysis,  you can also post process this to see how this behavior changes as you progress through the time steps in your analysis

The key is to not get so focused on your actual problem, but try to create the simplest possible form of the problem, find a solution there (it takes way less time this way) and then implement the fix in your real model.