I am experiencing an issue when using shell parts to build up my model. I have build the model and exported the CAD version as IGES. PrePoMax loads the geometry. I can get a beautiful mesh. I then define my sections (Three since the model has three different thicknesses for three different sections. I then defined the static step, applied the displacement/rotation boundary conditions and applied a pressure on the faces. I then run the analysis but I get Zero displacements and Zero stresses.
I have tried small solid and a shell model that has only one shell and get the expected results, but I have spent a long time and tried all possible combinations of constrains, contacts and boundary conditions to no avail.
Would really appreciate your observations and suggestions to make this work.
Are them connected, @FdoLorenzo ? When you import the file from CAD, do you make a compound part from them? Can you send your model, so we can help you better?
The best way to import a CAD geometry into PrePoMax is using the .step file format. In that way, all connected faces (bodies) are recognized as connected faces.
Thanks for taking the time to review my post. I create the CAD file using GiD. I export the file as either an .igs or .stp to open it with PrePoMax.
Directly from the .stp file created with GiD, PrePoMax opens it but no parts are shown.
I am attaching the Prepomax file, the .igs file and the .stp files for your review and comments.
One question that I have: What is the use or the need for making a compound?
The other observation is that the meshes created are not congruent, that is the meshes on two adjacent, connected shells do not share the same nodes.
One question, if you have to make a compound in order to get the proper results, wouldn’t that limit the number of materials that you can use in a model?
Thank you very much!
As I mentioned in my reply to Lucas, the CAD application that I use to create the .stp files created by my app cannot be viewed well with PrePoMax. The .igs work well.
Dear @FdoLorenzo , I have conducted a Frequency step on your model for the first 10 modes, and saw 10 rigid body modes. At least 2 parts are disconnected, but I think there are more.
When I did some tests the last month using parts with many partitions but connected to each other, this procedure guaranteed their contact and mesh connection. Hopefully it will work for your model as well.
I had no problems to model and export using FreeCAD, if you want to use open source software. Don’t know if it is a GiD bug when exporting shells, but maybe that would help you.
Maybe try the same procedure as described in: Compound part from IGES surfaces is empty to convert the .igs geometry to .stp geometry and then create a compound part.
After posting my question and reading your responses I tried all the suggestions, and this is what I found.
No Issues with PrePoMax if model comprises only one shell part or solid.
If model has more thjan one part, creating a compound does not appears to work. I am attaching one very simply model of half a sphere made using two parts.
One model created the mesh using prepomax not using a compound, and the second one creates the mesh using the compound. Netgen still makes a non-confromal mesh.
I even tried creating a mesh for the model that I sent recently using NGsolve, used the app to fix and stitch the parts and although you obtain a mesh that appears to be sound, I still get unconnected nodes at boundaries.
There appears to be no difference between using a version of my complex model if I export and iges or step file. still get the same wrong results due to non conformal meshing.
Any ideas or suggestions? Sphere-press-compound.pmx (896.9 KB) Sphere-press.pmx (892.3 KB)
The problem is the .igs geoemtry. I still have to determine what is cousing the problem and how to solve it but for the moment the solution is the same as already described. Using PrePoMax import the .igs. Then use PrePoMax to export the geometry into .step File->Export->Step. Then remove the .igs geoemtry from the model, import the created .step geoemtry and create the compound part. Meshing it should work now.
Dear Matej,
I really appreciate you taking the time to look at my issues. I did exactly what you indicated and the mesh, as you can see in the modified model is much better and it is now conformal.
I read the imported the igs model, exported as step, re imported the 28 step sections, made the compound, meshed the compound and define all the required conditions and properties, however, the solution is wrong.
I cannot figure out why it appears to be applying the pressure in the end face only.
Lucas, if you want to apply the frequency steps to check the mesh, do it by all means.
Thanks for all your help.
Best regards, F Lorenzo shell-6-13.pmx (1.9 MB)
I have checked your model and I wluld not say that the solution is wrong. You probably thought the solution is wrong since there are no colors in thre rest of the structure, only on the flat back surface. This surface gets deformaed so much that you can not see any other result. If you change the min/max limit on the legend and use much lower values for the max limit you will see color results in the rest of the model.
So the problem is a flat surface. Having a flat surface in a perssure vessel is a very bad idea, since most of the applied pressure is transformd into bending of such surfaces.
If you fix the entire flat back surface (all its nodes), you get this result:
Matej,
Thank you very much for the observations. I fail to do what you suggested and did not adjust the scale.
I agree with you that having a flat plate does not help with the integrity of the vessel. I am modelling this to see where the highest stresses where for powder trailer tank that failed and I am investigating. Needed an application that allow the use of 3D shell elements and PrePoMax is perfect, in addition to all the other nice features that I have been learning.
This is a low pressure multi compartment vessel (Design pressure 0.1 MPa) and I am modelling the most stressed part.
Matej,
I followed your advise, read more about the capabilities of PrePoMax and modifies the model to include the right section of the trailer. I am appending the equivalent Von Mises stresses. Because of some changes in the thickness of the plates in the actual model that I included in the model, there are some stress concentrations in the transitions. The actual model still uses a flat plate on the right, but because they reduced the exposed area to pressure, the deflection is smaller.
I need to continue working with igs CAD files but the procedure described works like a charm: Import the igs. => export the .stp file => create a new file and import the exported .step file => create a compound part and then mesh the compound! Works very well indeed!
I replied to given notify only, actually CalculiX is capable to modeling different thickness of shell element based on node
Edit keyword feature of PrePoMax can be user for simple model with structured quad mesh. However, it will be cumbersome for unstructured mesh and complex model.
This feature of variable thickness of shell element also has been discussed at another threads.
