I am working on Siemens NX 8.5 and my focus is topology optimization of a component. I watched some tutorials about it but I did not manage to find anything about how I can export a part file for the optimized component from the .sim file where I ran the simulation, in order to handle the part I get.
Can anybody help me?
Solved! Go to Solution.
The Topology Optimization in NX 8.5 allows you to export a facetted body of the optimization results. In your optimization Solution you see the link to the underlying Nastran Solution defintion and a "smoothing" taks. Right clicking on smoothing you can add a new smoothing task that will generate a smoothed surface result based upon you material distribution of the optimization results.
You can select to export an STL File when running the smoothing.
The STL File can then be imported in modeling into a new Part and you can start to generate your Design based on the proposal from topology optimization.
I hope that helps to close the loop in your design process.
thank you very much for your answer.
You solved my problem!
Moreover, do you know a way to perform a post-processing of the result obtained from the optimization simulation? Because I read that otherwise it should be performed by hand.
After the topology optimization is finished, you have all results of the final design cycle available in post. You can postprocess displacements, stresses, ... on the full model (with all void elements displayed). You can use groups or post view settings to setup an appropriate view.
The results are displayed on the original mesh - if you want to see results on the smoothed solution you have to do some manual works. Additionally to the output as STL, you can output a Nastran surface mesh (bdf). You have to generate a solid mesh (you can use Solid from Face Mesh), and reapply the boundary conditions.
I think I didn't understand the steps I must follow in order to see the results on the smoothed solution.
I tried to open a part file with the smoothed model and then I created a fem file in order to create the mesh the way you wrote. But I didn't manage to do it since in the fem file the model is not visible.
Is it the flow of steps to follow?
Moreover, once I create the bdf file, what do I have to do with it?
Sorry for the trouble.
if you want to see results on the smoothed solution you will definitely have to take som manual steps:
- Export the Smoothed surface as Surface Mesh (Select BDF additionally to STL in the Smoothing dialog)
- Read the surface Mesh to Advanced Simulation: "File -> Import -> Simulation" and select the bdf File
- Generate the solid mesh (Solid from Shell Mesh).
- If meshing fails, you might have self intersections in the surface mesh. You can remove these intersections using the "Node operations -> Node drag" Command.
- Reapply the boundary conditions (you can read the Simulation Entities to the Sim File using "Import -> Simulation Entities".
If you import an STL File to modeling, the facets are not transferred to Advanced Simulation.
I hope that helps.
I followed your steps and this is what I got.
Actually once I import the bdf file I got the optimized model which is already meshed. And I am not able to remesh it (I can't select the body while beeing in the Solid from Shell Mesh command).
I managed to import the boundary conditions from the sim file, but they are in the 'asleep' mode. How is it possible to 'defrost' them?
Because actually it's not feasible to work with facet features.
Moreover if I try to open the stl file in a model file and try to create new fem and sim files I cannot see the model in the latter two, so I can't work on it.
Actually I don't know why. Do you have any ideas?
Sorry again for the trouble.
what element Type did you select for the Solid from Shell Mesh? You need to use Tetra(4) as the Smooth Surface generates Tria(3) surface Elements. If you set the selection to Tetra(10) in the Solid from Shell Mesh command, you will not be able to select the surface mesh. Maybe that is your problem for the selection?
If you want to apply the boundary conditions to the new mesh and need to apply them to geometry, you can use the "Face from Mesh" Command and generate a polygone face on the mesh. These faces are associated to the mesh and can be used to apply the boundary condition.
the problem with the mesh was the one you thought. Now it is solved, as it is also solved the loads one as well. Face from Mesh is a command I did not know.
You made my day!
Thank you very much for your help.