Is it common to get drastically different results between Beam Elements and Brick elements while using MES with Nonlinear Material Models? My modle is drastically different then when I try a simple model (one beam supported at one end) this also yeilds different results.
In general, the results should be similar. Of course, brick elements provide a lot of additional results (von Mises stress) that beam elements do not provide, so this is one source of potential differences. And because of the very nature of the two element types (3D versus line), it can be easy to create models that are not identical.
To answer the many questions that come to mind, it would be best if you post an archive of your model.
16 years experience with Simulation Mechanical
This will probably need some input from a developer on MES for some of the technical details, but here's what I see.
- With the midside nodes included in the brick model, the displacemet is 2.28 inches. This is closer to the beam displacement of 4 inches.
- The displacements are close while the structure remains in the elastic region. See the attached images.
- The structure yields in the last 2 or 3 time steps of the analysis. You may want to include more time steps at the end of the analysis to better capture the transition from elastic to plastic.
- Because the entire cross-section goes plastic and experiences very large displacement, the inertial effects may be important. Running each analysis as nonlinear static would show if those effects are important or not.
- Because the dimensions of the cross-section (2.5 inches square) are large compared to the length (22 inches), how the mass is distributed could be important. If the beam element assumes the mass is concentrated at the centroid, the inertia effects could be different than the distributed mass of the brick model. (I do not know how MES distributes the mass of the beam elements.)
- I do not know whether beam elements assume the cross-section remains planar or not. This could have an effect on the results.
- A higher integration order on the beam elements may give more accurate results for that analysis.
So, I think the brick model will give more accurate results in this structure.
16 years experience with Simulation Mechanical
The results are so different because your loads are different. In the brick model, your load is 5,000 lbf; in the beam model, your load is 10,000 lbf.
I personally think the beam based model should have more accurate results (if its length is larger enough than its width). This is because the nature of brick element itself.
FIrst, for the model with beam, the length of the area with beam ditributed loads is 2.5 in, while the for the model with brick element, the length (Z-direction) of the area with surface forces is 2.66 inch, and the width (Y-direction) is 1.79332 and 1.79755 on the two sides.
Secondly, even the dimensions of the areas with forces are well set up, finer mesh (especially along the thickness direction) should be used for the modele with brick to obtain better bending simulation.
If the length (along Z-direction) of the model is much larger than the other two dimensions, well setup model should provide similar results for beam element and brick element.
To verify the statement that “brick element model should provide similar results to the beam element model if the mesh is fine enough”, I did an analysis with much finer mesh size (40%) and increased number of layers to 6. (This probably is the finest mesh size we usually would go with a CAD model especially when I have a larger multi-parts assembly.)
I have attached the displacement graph plot. The brick model’s displacements do not change too much, and the brick model still gets much smaller displacement than the beam model does at the end of 1 sec.
One thing I don’t understand regarding Shoubing’s reply. He says that the surface force was only applied on the width (Y-direction) of 1.79332” (not 2.5”) in brick model. I understand he means that the radius=0.375” transition areas did not get the surface force.
However, in the beam model, an aisc2005 HSS 2-1/2x2-1/2x3/16 square tube was selected from cross-section library, which should contains the radiuses, too – I assume. When the Beam distributed load is added along the length of 2.5 inch, is it applied on the flat face plus the radius transition areas?? If it’s YES, probably most people did not realize it -- because it is not real situation in most applications.
Well, the length of the area with beam ditributed loads is 2.5 in, while the for the model with brick element, the length (Z-direction) of the area with surface forces is 2.66 inch (rather than 2.5 inch).
And if the length (along Z-direction) of the model is much larger than the other two dimensions, then a well setup model should provide similar results for beam element and brick element.
This does deserve a verification test.