Showing results for 
Search instead for 
Do you mean 

The constraint doesn't work?


Dear All,


I'm working on a blade model of a wind turbine. I want to calculate the mode shape of the model after fixing it at the right end. So I fixed several nodes on the surface. But the boundary condition doesn’t work. Femap gave me the same result as by free free condition, and the surface isn't fixed in the result.


I don’t know whether I defined the wrong boundary condition. Theres no problem when I tried to calculate the mode shape with free free condition. Can anyone please help me with it?




Thanks in advance!




The following are the link to my model and some screen shots


Define the constrant on the nodes


Fix the nodes


Analysis options



Constraint before simulation



mode shape after simulation





Re: The constraint doesn't work?

It appears your shell and solid meshes are not congruent at the wing root. Your constraints appear to be on the solid mesh nodes which allows the shell mesh nodes to move. Unless you actually intended for the solid and shell to move indepently, then you will need to remesh and make sure the meshes are congruent, or use glue contact to attach the shells to the solids.





Re: The constraint doesn't work?

Hi Joe,


thanks a lot for your answer. But even the solid elements are not fixed. 


I also tried to fixed both the shell and the solid elements, but still it doesn't work. Do you have any idea why is that?





Re: The constraint doesn't work?

Dear Felix,

For any reason you have a problem with the constraints definition (the mesh is properly associated with geometry, not problem here): the next picture show the mesh of the 2-D COMPOSITE skin elements, together with nodes & constraints: you can see that constraints are applied to midside nodes that belongs only to TET10 elements.


and this is the mesh of composite + solid CTETRA elements, nodal constraints are only applied to midside nodes, not connected at all wirh Shell COMPOSITE elements.constraints-skin-solid.png

Simply click with the RMB the constrainst definition and select EDIT WHERE APPLIED, click in RESET and use METHOD > ON SURFACE and select the two surfaces where you want to apply the fixed constraints, and you are done!!.

Repeat the Normal modes analysis with NX NASTRAN (SOL103) and you will see now different results:constraints-solved.png

Best regards,

Blas Molero Hidalgo, Ingeniero Industrial, Director
Blog Femap-NX Nastran:

Re: The constraint doesn't work?

Thanks a lot! Your method works. Problem solved!