Showing results for 
Search instead for 
Did you mean: 

FEM with 2D and 3D elements


I have an airplane seat with 3D and 2D elements. I might be doing the mating wrong because I can't seem to get the correct eigenvalues. My computer takes forever to solve and in the end it doesn't show me results. I've already done similar simulations with more elements and got good results, so the element number isn't the problem. Can anyone please enlighten me on how to do the mesh and the mating? The .zip file attached contains all the .stp, .prt, .fem and .sim files.


Thanks in advance,



Re: FEM with 2D and 3D elements

Siemens Phenom Siemens Phenom
Siemens Phenom

This model had 3 problems that I fixed. Then I was able to quickly get 10 modes above zero Hz. The first solve I ran was with your model as you delivered it. The errors listed in the NX solution monitor and NX Nastran F06 file stated:





The  M set refers to degrees of freedom that are dependent due to being connected to RBE2/3 elements or multipoint constraint equations (MPCs). The S set refers to degrees of freedom that have displacement constraints applied to them. Nastran by default doesn't allow DOF to be dependent and constrained at the same time. Your model has glue non-coincident mesh mating conditions that connect pins to lugs. The pins are fixed. Some of the pins' constrained nodes also connect to the lugs through the RBE3 elements. That's the root cause of this problem.


The solution was to set PARAM, AUTOMPC to YES. This lets NX Nastran adjust DOF dependencies automatically to overcome the constraint/dependency DOF conflicts. You define NX Nastran parameters in NX through the solution. Edit the solution, then go to the Parameters tab. Create a new parameters modeling object and set AUTOMPC to YES.


I ran a second solve and NX Nastran produced a bunch of MAXRATIO warnings, indicating that the stiffness matrix was unstable and ill conditioned. It tried to correct the ill conditioning, but it could not overcome it. Stiffness errors tend to be related to materials, physicals, or meshes. Knowing that you have shells in the model, past experience told me to look there first. It seems that you accidentally defined the shells as Plane Strain. I don't think you really want them to be plane strain, so I turned that option OFF.


My third solve got past the MAXRATIO warnings and the stiffness matrix seemed to be OK. But the eigenvalue solution was iterating too much. That's sometimes an indication of having unintended rigid body motion in the model. The solve completed and all 10 modes had frequencies all well below 1 (i.e. zero). They were all rigid body modes. The output showed that the shells on individual faces weren't connected to their neighboring faces. You have 2 options for solving this.


1. Sew the sheet bodies in your CAD model

2. Stitch coincident polygon edges together in the FEM


Sewing the sheet bodies in the CAD model is more efficient. After updating the meshes, I noticed that some of the automatic MMCs were lost (due to sheet bodies being from the model during the stitch operation and replaced by faces on a single sheet body). I recreated automatic MMCs. Then I solved again. The first mode was at 68.9 Hz and all looks much better. It's still not perfect. The lugs aren't connected to the spacers that connect to the seat. I really didn't spend time reviewing gaps between bodies and hoped that auto MMC with a search distance of 0.1mm would take care of things. Your geometry has gaps larger than 0.1mm.  Attached is my edited PRT/FEM/SIM data. It overcomes 99% of the difficulties you were having.






Mark Lamping

Simulation Product Management

Simulation and Test Solutions


Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

Re: FEM with 2D and 3D elements


Wow, thank you very much. You are a real life saver. You really helped me speed me my thesis. You really went the extra mile to solve my problem.


Thank you again.


Luís Ferreira