Shell elements linear vs parabolic formulation give different reactions forces??

[PierreMalouf8976]

Using a simple shell model I have observed a difference in the calculated reaction forces by simply switching between linear and parabolic formulation. The load, boundary conditions and mesh are the same the only change is selecting linear and parabolic formulation for the mesh.

The "SPC Summation" feature is used to evaluate the reaction forces at the boundary conditions applied to the model. The correct reaction force should be 100,000 LB along the positive Z-axis, the model gives a difference of 9 LB for the linear formulation and 11,944 LB for the parabolic formulation.

Am I doing something wrong ? or has anybody else experienced this?

Following is the procedure I have used,

1. Create a simple model in SolidWorks, then import in Inventor Professional 2019.
2. Define the FEA model using the midsurface command. The model represent a center sill which is the main structural component of a railcar.
3. Select material ASTM A36, define thickness, fix the end of the center sill and apply a 100,000 LB compressive load.
4. Mesh the model with linear shell elements as shown in Photo 1.
5. Run the model and use the "SPC Summation" to calculate a reaction load of 99,991 LB at the applied boundary conditions at the end of the beam (center sill). There is a difference of 9 LB along the Z-axis.
6. Mesh the same model with parabolic shell elements as shown in Photos 3 and 4. The mesh size remains unchanged at 2 inches.
7. Run the model and use the "SPC Summation" to calculate a reaction load of 111,944 LB at the applied boundary conditions at the end of the beam (center sill). There is a difference of 11,944 LB along the Z-axis.

Regards to the group,

Pierre Malouf

Mechanical Engineer-Rolling Stock

[PierreMalouf8976]

Photo 5 did not upload in my previous post, here it is

[KubliJ]

Hi @PierreMalouf8976,

I think I am able to duplicate this on my machine.  The key issue seems to bet that contact (offset bonded) is required to hold the part together.  A continuous meshed part does not appear to generate any difference in results. 

I don't seem to be able to resolve it myself, so I'm reaching out to the team to see if someone has a suggestion.

Thanks,

James

[PierreMalouf8976]

Hi James,

The model I generated used offset bonded to hold the parts of the beam together. In the model I used there are three distinct parts a web with a top/bottom flange. I obtain different reaction forces measured with the "SPC Summation" when using linear or parabolic shell elements.

A continuous mesh was not used because other components will be added at a later date. I do this because the Nastran In CAD seems to be designed to use "offset bonded" to connect many parts in a model, is this correct?

In the past when I used "Continous Mesh" in the Mesh Settings I would get problems, it was recommended that I use offset bonded to address this.

I was surprised to see the different reactions forces when using "offset bonded", which prompted my question in this forum.

Regards,

Pierre Malouf

Mechanical Engineer-Rolling Stock

[KubliJ]

Hi @PierreMalouf8976,

The offset bonded contact is super handy when it comes to complex shell models.  A continuous mesh would be ideal as this would eliminate contact and the analysis time associated with them.  But there should be no issue with the use of contact.

I have ended up logging this with the developers as an issue with the software.  There is no clear explanation for the error in the reaction forces.  I also noted that the displacement and stress results would not match up with the linear elements no mater how refined I went with the linear mesh.  The two should in theory drive to the same results, it's just that the parabolic will reach the final result with a coarser mesh than the linear elements.

This issue seems to be a combination of things.  Linear elements, contact, and constraints.  I did find that if my constraints were away from any of the contact edges, I got correct reaction forces.  So for example in your I-beam.  The contact is along between the edges of the web and flanges.  Since you constrained the ends of the beam, the contact edge and constrained edges will end up sharing a node.  However, if you were to constrain the outer edges of the flanges, giving a separation between the contact edges and constraint edges, the reaction forces will be correct.

Depending on your model, it is probably just simplest to use the linear elements than to double check if your contact edges and constrained edges share any nodes.  Sorry for the inconvenience.

Thanks,

James