Rotational Symmetry in Buckling Analysis

Please login with a confirmed email address before reporting spam

Hi everyone,

I'm currently trying to reduce the size of my model by applying symmetry. While I’ve had some success with basic symmetry cases, I’m still struggling to correctly define rotational symmetry for my cross-section.

I’m performing a linear buckling analysis, and my geometry has a three-fold (120°) rotational symmetry. Despite experimenting with simpler models, I haven't been able to set it up properly in COMSOL.

Could someone please guide me on how to define and implement this type of symmetry in my model? I’ve attached a simple sketch of both the full and reduced models for reference.

Thank you very much in advance for your help!

Best regards, https://drive.google.com/file/d/1-ygSbmOydDTfKx1leXw_7t2vOn5RRqnV/view?usp=drive_link

sketch


5 Replies Last Post 2025年4月15日 GMT-4 07:32
Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 1 week ago 2025年4月9日 GMT-4 09:58

It is unsafe to use symmetry for buckling problems, since the buckling modes may be nonsymmetric, even though geometry and loading are symmetric.

-------------------
Henrik Sönnerlind
COMSOL
It is unsafe to use symmetry for buckling problems, since the buckling modes may be nonsymmetric, even though geometry and loading are symmetric.

Please login with a confirmed email address before reporting spam

Posted: 1 week ago 2025年4月9日 GMT-4 14:40

It is unsafe to use symmetry for buckling problems, since the buckling modes may be nonsymmetric, even though geometry and loading are symmetric.

Dear Henrik Sönnerlind,

Thank you for your quick and helpful response.

I was wondering—is there a way to reduce the model size in a buckling analysis?

Best regards, Mirhan

>It is unsafe to use symmetry for buckling problems, since the buckling modes may be nonsymmetric, even though geometry and loading are symmetric. Dear Henrik Sönnerlind, Thank you for your quick and helpful response. I was wondering—is there a way to reduce the model size in a buckling analysis? Best regards, Mirhan

Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 6 days ago 2025年4月10日 GMT-4 07:29
Updated: 6 days ago 2025年4月10日 GMT-4 10:47

For structures with a single symmetry plane, you can analyze half of the structure using symmetry boundary conditions as one case, and antisymmetry boundary conditions as the other. This will give you all modes and corresponding buckling loads.

With two orthogonal symmetry planes, you would need four sets of boundary conditions on a quarter of the structure.

For rotational symmetry it is more complicated. Buckling modes can have different types of cyclic behavior. Such problems can be treated using Floquet Theory, but that is not a built-in functionality. It is, however, possible to set up such boundary conditions by editing Periodic Condition constraints in Equation View.

-------------------
Henrik Sönnerlind
COMSOL
For structures with a single symmetry plane, you can analyze half of the structure using symmetry boundary conditions as one case, and antisymmetry boundary conditions as the other. This will give you all modes and corresponding buckling loads. With two orthogonal symmetry planes, you would need four sets of boundary conditions on a quarter of the structure. For rotational symmetry it is more complicated. Buckling modes can have different types of cyclic behavior. Such problems can be treated using Floquet Theory, but that is not a built-in functionality. It is, however, possible to set up such boundary conditions by editing *Periodic Condition* constraints in *Equation View*.

Please login with a confirmed email address before reporting spam

Posted: 2 days ago 2025年4月14日 GMT-4 08:13

Dear Henrik Sönnerlind,

Thank you very much for your response! I’ll look into the suggested solutions and do my best to implement them as advised.

Best regards, Mirhan

Dear Henrik Sönnerlind, Thank you very much for your response! I’ll look into the suggested solutions and do my best to implement them as advised. Best regards, Mirhan

Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 1 day ago 2025年4月15日 GMT-4 07:32
Updated: 8 hours ago 2025年4月16日 GMT-4 08:22

Hi Mirhan,

Thanks for your input here. As an effect of your questions, we have now implemented Floquet periodicity for buckling. It will be available in the next major release.

I the meantime, you can use the method shown in the attached model. The important things are the following:

  • Two different Periodic Condition nodes are used: One for the stationary step, and one for the linear buckling step.
  • The second one is edited in two ways in Equation view: New expressions for the constraints are used, and the variable solid.pc2.mFloquet is hardwired to the azimuthal mode number.
  • A sector 3D dataset has been added in order to visualize the modes for a full model.
  • Note that some of the modes computed do not have the number of periods given by the azimuthal mode number. This is not an error. Those modes are also true solutions. The reason that they appear can be 'left as an exersise to the reader'. Hint : phase angles are only unique up to a factor 2*pi.

The user forum, just as questions asked in support, provide us with a lot of useful feedback and influences future development.

-------------------
Henrik Sönnerlind
COMSOL
Hi Mirhan, Thanks for your input here. As an effect of your questions, we have now implemented Floquet periodicity for buckling. It will be available in the next major release. I the meantime, you can use the method shown in the attached model. The important things are the following: * Two different *Periodic Condition* nodes are used: One for the stationary step, and one for the linear buckling step. * The second one is edited in two ways in *Equation view*: New expressions for the constraints are used, and the variable *solid.pc2.mFloquet* is hardwired to the azimuthal mode number. * A *sector 3D* dataset has been added in order to visualize the modes for a full model. * Note that some of the modes computed do not have the number of periods given by the azimuthal mode number. This is not an error. Those modes are also true solutions. The reason that they appear can be 'left as an exersise to the reader'. Hint : phase angles are only unique up to a factor 2\*pi. The user forum, just as questions asked in support, provide us with a lot of useful feedback and influences future development.

Reply

Please read the discussion forum rules before posting.

Please log in to post a reply.

Note that while COMSOL employees may participate in the discussion forum, COMSOL® software users who are on-subscription should submit their questions via the Support Center for a more comprehensive response from the Technical Support team.