I hope you are all doing well. I am currently working on a project involving the stress analysis of a one-sixth fractional motor rotor using PrePoMax (CalculiX FEA). I have prepared the model file and have also included two screenshots of the setup. However, I am facing difficulties in obtaining the desired simulation results.
To troubleshoot the issue, I followed relevant tutorials on YouTube, including “PrePoMax (CalculiX FEA) - Tutorial 6 - Rotating disc” and “PrePoMax (CalculiX FEA) - Tutorial 17 - Plane strain analysis of a composite pipe.” These tutorials covered topics related to contact and rotation settings, which are crucial for my simulation setup.
Despite my efforts, I have been unable to generate the expected results. I suspect that I might have overlooked some critical steps or misconfigured certain parameters in PrePoMax. Specifically, I am facing challenges with contact definitions, rotation settings, and possibly constraints.
Therefore, I am reaching out to the community for guidance and support. If anyone has experience with PrePoMax (CalculiX FEA) and has successfully performed stress analysis on rotating structures or similar cases, I would greatly appreciate your input.
Thank you for your time and consideration. Looking forward to your assistance and knowledge-sharing.
Check this thread with a discussion about a very similar model: Request for feedback
The magnets are initially unconstrained, there’s only contact between them and the rotor. You may have to use a different approach - prescribed rotation (displacement control is always better for convergence than force control) or magnets tied to the rotor (probably not exactly what you want to achieve but it can be a good starting point).
In those youtube examples, FEAnalyst used displacement BC’s in X and Y directions, because his model was 90 degree sector and cyclic boundraies were on X and Y axis exactly. But, your model is a 60 degree sector and you cannot use displacement boundaries directly. You should improve your cyclic symmetry definition for accurate results.
You should rotate nodal coordinates of cyclic boundary nodes to cylindirical coordinate system. Then you can fix displacements in tangential Y direction.
I used tied contacts in your model. You can follow FEAnalyst’s suggestions for better contact definition.
You also fixed inner diamter of the rotor. I donot know if this is the case for your system. I would keep it free if there is no feature which will prevent radial growth of inner diameter.
The problem with this model hard contact was exposed in the calculix forum. Once it starts rotating the magnets fly away due to the lack of friction or lateral constrain.
Look at this video to see what am I refering too.
It can be solved for example extending the contact area to the lower corner of the magnet.
Thanks a lot for the suggestions from @FEAnalyst, @furkan and @ANYS!
Your insights and suggestions have been incredibly helpful in guiding my progress.
As per your recommendations, I incorporated the following modifications to my model:
Tie Contraints : I implemented tie constraints to simulate contact between different components.
Coordinate Transformation : Following furkan’s advice, I transformed the nodal coordinates of cyclic boundary nodes to cylindrical coordinate systems.
I am pleased to share that these adjustments have yielded promising outcomes, and I can now consistently obtain results in the simulation.
Next, I plan to further enhance the contact definition based on FEAnalyst’s suggestions and address the concerns raised by ANYS to ensure the stability and accuracy of the simulation.
I am excited to share my progress with the community and seek additional feedback to refine the analysis and validate the model.
Once again, I extend my heartfelt gratitude for your generous support and expertise.
