Model Meshing Issues

[brut3]

I have a relatively simple part that I'm trying to run a stress analysis on. When trying to mesh the part I'm receiving an "unable to mesh part" error message. Additionally, there is nothing reported on the mesh error report. I've attached the part for your use, any help would be greatly appreciated.

 

[rb1957]

I have Inventor but not your version. post STP file

 

[brut3]

Below is a link to the STP file format:

Curved Metal Panel.stp

 

[rb1957]

meshed ok for me (using FeMap). what are you using ? PATRAN ?

 

[karachun]

Hello brut3. Can you show us pictures of your mesh or describe what type of mesh you want to get? Maybe you try to create solid mesh on this thin walled part and get errors.

 

[BlasMolero]

Dear Brut3,
This is a very thin plate, then is crazy to mesh using 3D solid elements (to account for stress gradient you need to mesh with minimum TWO elements in the thickness), the correct meshing workflow should be to create a midsurface and mesh with 2-D Plate/Shell CQUAD4 elements:



In fact, here you have the MIDSURFACE created in FEMAP V2406 MP1 ready to mesh with 2-D Plate/Shell elements (please note the curve imprints created in the midsurface to allow to generate automatic mapped mesh with excellent quality using the Approach on Surface = mapped four coner feature):



Mesh in FEMAP with the MESHING TOOLBOX using an element size = 6.35/4 = 1.5875 mm.
The quality of mesh is excellent: Jacobian check =0.387, well below the maximum allowable threshold (the limit is 0.6)



In summary: the target is to mesh with 2D Plate/Shell elements. Please note the plate thickness is very small, then a linear static analysis surely will be useless, the correct analysis type should be NonLinear activating large displacement effect to account for stress stiffneing effect (ie, account for membrane stiffness).

Best regards,
Blas.

 

[SWComposites]

agree 100% with Blas, this part should be modelled with shell elements.