Eigenvalue Buckling of thin walled cylinders and stiffened cylinders

KnHwKnHw Member

Hello,

 

i try to run some design Optimizations for a cylinder. Therefore i want to compare different stiffner typs and a unstiffened version. When i try to run the unstiffened Version, i alwys got the same total deformation(1;1,0001m) for several r/t(radius/wall thickness) ratios.When i try to simulate thin walls, Ansys can't "Performe Mode Extraction"(radius=750 thickness <20mm). I tried some settings explained in the Help-Section: Checking all specific settings for linear buckling, changing the solver to Subspace(default for linear is Direct) both didn't work.

Loads and Boundary conditions:

acceleration in axial and radial direction

fixed support on one front face

i turned of negative Load Factors

It did worked before, but there i mixed the Units for my Youngs' Module. (Now GPA then MPA->Factor 1000 more now)

 

Greetings KnHw

Comments

  • WenlongWenlong CanonsburgMember
    edited June 19

    Hello KnHw,

    Buckling mode shapes do not represent actual displacements but help you to visualize how a part or an assembly deforms when buckling.

    (Ref: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_buckling_analysis_type.html?q=displacement%20eigenvalue%20buckling)

    Regards,

    Wenlong

    ================ Note ====================

    If you have trouble opening the links I attached, please see the first useful link below

     

     

    ------------------------- Useful Links ----------------------------

     

  • KnHwKnHw Member
    edited June 20

    Hello Wenlong,

     

    thank you for your quick and helpful response. Maybe you also have an idea why i can't solve thin walls? If you need any further Information please ask

    Additionaly, is it possible to calculate the actual displacement?

     

    Regards

    KnHw

  • KnHwKnHw Member
    edited June 22

    Found a similar Post with no solution. I think it is a important question/Problem for multiple users

     

    https://studentcommunity.ansys.com/thread/eigenvalue-buckling-problem/?order=all#comment-58c4d644-0f7d-4b24-b433-ab3e0132bc40

  • WenlongWenlong CanonsburgMember
    edited June 22

    Hi KnHw,

    Sorry about the late reply. Could you please insert several images about your model boundary conditions and analysis settings?

    If you need the actual displacement, you would need to conduct a nonlinear eigenvalue buckling analysis. You can find more info here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v191/ans_str/Hlp_G_STR7_4.html

    Thanks,

    Regards,

    Wenlong

  • KnHwKnHw Member
    edited June 23

    Hi Wenlong,

    no worries, important is that i got a reply

    Thanks for the Link for actual displacement!

    Here are some images, please tell me if you need more! Workbench

    StaticStructuralSettingsOverview

    AnalysisSettings

    Fixed Support on the front face of the Cylinder

    Loadconditions: Acceleration

     

    thank you in advance!

     

    Best regards KnHw

  • WenlongWenlong CanonsburgMember
    edited June 23

    Hi KnHw,

    Your setup looks fine for me. I duplicated your setup and I am able to extract the modal shape. I am using a similar geometry size you described (radius 750mm, thickness 15mm). And I have tried solid and shell elements both work fine. 

    Can you please show me the exact error message? Also, what's the material property you are using? That could be the only input that's different from us. 

    Regards,

    Wenlong

     

  • KnHwKnHw Member
    edited June 23

    Hello Wenlong,

     

    can you plz try a thickness of less then 3mm? I could run a simulation today at my University and i was able to run 5mm (using the Subspace Solver) after changing the solver process settings(unchecking Distribute solution) .but less was not working. I got similar issues by using variuos stiffened shells (isogrid, orthogrid, trusscore and Honeycomb) modells. But i think for them i should open a new thread/ maybe the solution here will also work, then i would comment this here at the end.

    Error:

    Error message, Moden Extraction has no Progress

    on my other PC i got this solver output:

     

    *** NOTE ***                            CP =      30.594   TIME= 18:22:18

     

    The initial memory allocation (-m) has been exceeded.                  

     

      Supplemental memory allocations are being used.                       

     

     

     

      SUBSPACE CALCULATION OF UP TO    1 EIGENVECTORS.

     

      NUMBER OF EQUATIONS              =       612864

     

      MAXIMUM WAVEFRONT                =          147

     

      MAXIMUM MODES STORED             =            1

     

      MINIMUM EIGENVALUE               =  0.00000E+00

     

      MAXIMUM EIGENVALUE               =  0.10000E+31

     

     

     

      Memory allocated for solver              =  4180.559 MB

     

      Memory required for in-core solution     =  3983.583 MB

     

      Memory required for out-of-core solution =   545.658 MB

     

     

     

    *** NOTE ***                            CP =      99.406   TIME= 18:22:45

     

    The Sparse Matrix Solver is currently running in the in-core memory    

     

     mode.  This memory mode uses the most amount of memory in order to     

     

     avoid using the hard drive as much as possible, which most often       

     

     results in the fastest solution time.  This mode is recommended if     

     

     enough physical memory is present to accommodate all of the solver     

     

     data.

     

     

     

    Material properties:

    and the secon material is used:

     

    When i quit the solving process i got this message on my workbench:

    (DP 1) Update of the Lösung component in Eigenwert-Beulanalyse for Design Point 1 failed: Error updating cell Lösung in system Eigenwert-Beulanalyse for design point 1.

     

    Best regards Bastian

  • KnHwKnHw Member
    edited June 24

    Hello Wenlong,

     

    just giving you a short update, I tried some different boundary conditions for another Load Case with a deplacement on the top and the Bottom:

    it worked out fine, so thats why i am thinking it is not working because of the fixed support. One Guy from the Team mentioned that he had some Problems with thin shells because of the inertial Relief settings in the structual settings-> I tried to simulate the shell, while inertial relief was turned on but I got the error message that inertial relief is not working for Buckling prestress analysis. Is it right, that i have to turn it of for Buckling analysis?

     

    Dealing with this i got a Meeting with the guy from the University and we want to analyse a different Loading Case if this one is not working, maybe you can answer one short question for this Loading case:

    Is it possible to give the add a deplacement for the Centroid of the Geometry? So that i can actually see the Buckling, when this Cylinder is accelerated without any external support.

     

    Thank you very much for your support!

     

    Best regards

    KnHw

  • WenlongWenlong CanonsburgMember
    edited June 25

    Hi KnHw,

    Regarding assigning displacement to the centroid of the geometry, you can try "remote displacement". Then when you assign the remote displacement location, you can select the cylinder body and Ansys will find out the centroid for you. 

    Regards,

    Wenlong

     

  • KnHwKnHw Member
    edited June 26

    Hello Wenlong,

     

    ok thank you for this advise,  I could select the faces of my cylinders but not the body is this a problem?

     Secondly I have a problem using inertial relief and buckling analsys. I read in some forums that it is possible to use it in other FEA Software, so i think it is also in ANSYS but i missed some settings.

    In the end my Task is to simulate a Rocketsell while it is accelerated, so it should not have any supports. Thats why i think i need inertial relief and a remote displacement. Maybe you got another idea?

     

    Here is my new set up: I have a remote Displacement with a pinbal of 0.75m.

    load stays the same acceleration in lateral and axial axis.

    Running my static strutural parts works fine. But then when i try to use Buckling analysis i got this message: Inertial Relief is not valid for Prestress Environment

     

    Can some one explain me why i can't or how i can use interial relief with eigenvalue buckling?

     

    Thanks in Advance

     

    Best regards KnHw

  • WenlongWenlong CanonsburgMember
    edited June 26

    Hi KnHw,

    In your case, I think assigning acceleration and remote disp will be enough, right? Inertia relief is used to calculate accelerations to counterbalance the applied loads in static analysis. Also please note below ( https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/wb_sim/ds_Solver_Controls.html?q=inertia%20relief): 

    If the Inertial Relief property is set to On, then any analysis linked to the Static Structural analysis is invalid. This includes a Static Structural analysis linked to the following analysis types:

    • Pre-stressed Modal

    • Eigenvalue Buckling

    • Pre-stressed FULL Harmonic Response

    • Pre-stressed MSUP Harmonic Response

    • Pre-stressed MSUP Transient

    • Pre-stressed Response Spectrum

    • Pre-stressed Random Vibration

    Regards,

    Wenlong

     

Sign In or Register to comment.