Huge difference in Displacement and Mises Tension for Body vs Surface Part Analysis

Dogan_22589

Hello, 

i have a question regarding a surface vs body analysis with Altair Inspire. 2022.2.0. 

The part is basically a huge curved plate which I believe allows me to use the midsurface to create a faster FE-analysis. But as I cannot do any topology optimization on a surface part i need the body. Therefore i just wanted to do the surface analysis to compare the FE Results to the body analysis and discuss the differences. 

When analizing the part as a surface i  unfortunately receive enormous differences to the body analysis in displacement and mises tension. Is there any plausible explanation for this? 

The part is supposed to be able to rotate around the top corner where the roof and the plate meets so i realized that through putting a fixed clamp on just the edge of the part while on the surface part i just released one of the rotational degrees of freedom which is not possible the  body part.

I attached both files. Maybe someone can help me. 

I would appreciate any tips on what i am doing wrong. 

Kind regards,

Dogan

Adriano A. Koga

1) you CAN perform topology optimization in a surface model. Just make it 'design space' the same way you would do for any solid part.

The only difference is that you won't have as many controls for manufacturing as you would for solids parts (such as draw, extrusion, etc)

 

2) Solids and Shells have their differences, one of them as you've mentioned is related to their DOFs.

Solids have only the 3 translational DOFs, as shell model has all the 6 of them, so to compare both you need to be sure your constraints are physically the same in both.

But the most important point that I see in your model, is by turning on the mesh visualization on solid model.

You will see that as the model is really thin, Inspire is able to put only 1 layer of solid elements over your part, which is not enough to capture the stress field, specially over the thickness.

The shell model can accurately capture bending stresses (top and bottom layer). For the solid mesh, you would need at least 3 layers to start capturing the stress distribution over the thickness.

So imagine that your solid mesh is capturing just a averaged result of what is happening along the thickness.

Now it you imagine that bending is happening in one element, at one side it will be compression, and the other side it will be tension. So there's no way it could capture well both, with only 1 element along thickness.

But for your model, to have more layers, would increase a lot your model size. so I"d say: go for the surface/shell model.

Dogan_22589

Hello Adriano,

thanks a lot for your indepth answer. The reason why i said i cannot perform a topology optimization is because what i need to do is actually leave the layer that you marked as a design space as it is and add an extra layer on top of it to create some sort of rips and stiffener elements. It should look something like in the picture attached.

Is this also possible with a surface modell ? Extracting the MidSurface kind of takes away the ability to do this i believe. 

If its not possible does that mean that i should go for a topography optimization instead ? 

 

Thanks a lot 

Dogan