NASTRAN SOL 106 in SimCenter 3D - Shell Thickness Output? 1

[jmarkus]

Hi,

I'm just learning how to use SimCenter 3D. I'm working with the SOL 106 - nonlinear solution with shell elements (I don't have access to 401 or 402). Is there a way I can plot/output/measure the final thickness of shell elements?

Thanks,
Jeff

 

[sdm919]

Shell elements are by definition 2D. They are based on assuming a state of plane stress, that is sigma-zz (where x and y are the in-plane directions) is zero. Stresses and strains in the z-direction are not something a shell FEM computes.

However, using the equations of elasticity, you can get an estimate of the strains in the z-direction. For an isotropic material, and with sigma-zz=0, you get the normal strain epsilon-zz in terms of the in-plane stresses sigma-xx and sigma-yy.

epsilon-zz = (-nu/E)*(sigma-xx + sigma-yy)

So the change in thickness would be (original thickness)*(epsilon-zz).

You could start with the estimate given above. However, if you really think thru-the-thickness normal stresses/strains (sigma-zz, epsilon-zz) are a significant issue in your case, you might have to use 3D solid elements instead of shells.

 

[rb1957]

I don't know how NASTRAN optimises the shell thickness ... maybe it re-writes the PID card for the element. one way to infer the thickness is to print the three surface stress (top, middle and bottom). top should show t/2 (and bottom -t/2) in the output (.f06). But you'd think there was a more obvious way

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[karachun]

I found this paragraph in the documentation for the 106 solver (Simcenter Nastran Basic Nonlinear Analysis User's Guide basic_nonlinear.pdf section 1.1 Overview of Nonlinear Analysis and almost the same statement repeated at 3.7 Understanding Geometric Nonlinearity). This solver calculates elements in small displacements for all cases except for hyperelastic calculations (but hyperelastic calculation work only wits SOLID, Axisymmetric and Plane Strain elements and not Plane tress elements=PLATE elements). So the solver considers the change in thickness of PLATE elements to be zero. It also clearly states that this solver is not suitable for metal forming calculations.
So if your solution is within the limits of small strain then use the sdm919 solution .
If you need large strains like metal forming, then the 106 solver will give a wrong solution.

 

[SWComposites]

Jeff - what exactly are you modelling? and what material type and material model are you using? what is the need to determine the final thicknesses?

 

[jmarkus]

Currently I am just trying to wrap my head around the capabilities of SOL 106 (which is the only non-linear solution I have access to). I am planning to use this with parts made from steel sheet and aluminum sheets and extrusions. I am just starting with some simple models to wrap my head around what outputs I can get. One of my thoughts was to simulate a tensile test coupon to compare with some known results (both physical & virtual) to make sure my methods (& material models) make sense. The change in thickness was something that I thought I could use to validate my model, but I guess that might not be the best approach with this code.

 

[rb1957]

IDU ?

SOL 106 uses the standard PSHELL card, no? You define the thickness.

"change in thickness" ?? ... what, like under load, with the section plastically deforming ?? ... nah, or at least I don't think so.

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[sdm919]

In FEA, the nodes (grid points) move, but the properties do not change. Properties include area for 1D elements (CROD, CBAR) and thicknesses for 2D elements (CQUAD4/CTRIA3). 3D elements do not have section properties, because the "width" and "thickness" come from the node locations.

If you modeled a simple tension test with 1D CROD elements, you would get the axial extension, but not area change. If you modeled a flat tensile specimen with CQUAD4 elements, you would be the stretch, but you would also get the transverse contraction, because the nodes will move in that direction. But you will not get the contraction of thickness. If you truly want to see the contraction, both laterally and through the thickness, you would need to model your tension specimen with 3D solid (CHEXA) elements. But those changes in width and thickness come from the nodes moving, not from changes in the element section properties.

1D and 2D elements are engineering approximations, which are entirely adequate for solving many real engineering problems. I am not suggesting you need 3D solids for everything, it is just that you should be aware of the limitations of different types of modeling.

I would suggest another test case for SOL 106: a flat plate under uniform pressure. Make a square plate with all 4 sides simply supported. Apply a uniform normal pressure (PLOAD). Run it both linear (SOL 101) and nonlinear (SOL 106, large displacements but linear material). Analytical solutions are available for both cases, say in Timoshenko or Roark. At small loads, the models should give similar results. At higher loads, the nonlinear model should deflect much less than the linear one. This is because the linear model does not include the effect of membrane stiffening that occurs after the plate deflects more than about 1/2 the thickness.

Note that in a nonlinear solution, you really want to track the behavior, not just get to the end point all at once. You want to see how linear or nonlinear it really is, and if you are nearing a point of instability. Therefore you should get output at several increments of load along the way, not just at the final load. There are different ways to do this (see the documentation). In my example above, one thing you could track would be the deflection of the node at the center of the plate. Then you would have something to compare linear to nonlinear results. If the normal pressure was 10 psi, get results at 1, 2, 5, 10 psi to trace the curve.

P.S. It is always a good idea to run your models linearly first to debug them. Only when they are running correctly and giving expected results should you move on to the nonlinear runs.