Ansys Learning Forum Maintenance

NOTICE: We will be performing backend maintenance of our Learning Forum from April 5 to April 12, 2021. The result will be a new infrastructure but with little impact to user experience and design. Currently the forum is accessible in read-only mode as we complete our final migration. Thank you for your patience. For urgent issues please visit HERE.


Large Deflection — Ansys Learning Forum

Large Deflection

Hello everyone!

I solve a problem with thin shells, with a static calculation I have no problems, when I connect large defomations, I have no solution convergence. How can convergence be improved or what could be the problem?

Best Answers

Answers

  • peteroznewmanpeteroznewman Member Posts: 11,369
    Accepted Answer

    @Evgenii_K

    Under Analysis Settings, turn on Large Deflection. Turn on Auto Time Stepping. Set the Initial and Minimum Substeps to 100, and the Maximum Substeps to 1000.

    Click on the Solution Information folder and type 3 into the Newton-Raphson Residual plots in case you fail to converge.

    Reply with an image of the Newton-Raphson Convergence Plot.

  • Evgenii_KEvgenii_K Member Posts: 31

    Unable to converge.

    Newton-Raphson Residual Force

    Newton-Raphson Residual Force 2

    Newton-Raphson Residual Force 3


  • peteroznewmanpeteroznewman Member Posts: 11,369

    @Evgenii_K

    Do you have contact in the model? If so, reducing the Normal Stiffness of the contact by a factor of 0.1 can help convergence.

    The N-R Residual Force plots show you where to improve the mesh. Use smaller elements at these locations.

    Please show the mesh at these locations before and after the mesh improvement. Are these shell or solid elements?

  • Evgenii_KEvgenii_K Member Posts: 31

    There are no contacts in the model!

    Residual force NR is displayed over the entire model shell.

    The shell in the modoli is broken with a 1000 mm mesh.

    This is -  SHELL181; keyopt=1

    It became impossible to solve the whole model with a 100 mm grid, so I made a test model with one span. But even a solution with such a fine grid could not be found.

    The grid that was before - 1000 mm

    Mesh which has become - 100 mm


  • peteroznewmanpeteroznewman Member Posts: 11,369
    edited March 1

    @Evgenii_K

    Please describe the loads and supports on the shell.

    If there is a pressure on the convex side or a large compressive load in the membrane direction of the shell, then the reason for the lack of convergence could be due to the load approaching a buckling load. That can be a reason why a Static Structural model will converge with Large Deflection turned off, but will fail to converge with Large Deflection turned on. The structure becomes unstable as the load approaches the instability. With stabilization or arc-length methods, the solution can proceed past the critical load and show post-buckled results.

    Buckling can also be mesh dependent, and we see some evidence of that since the coarse mesh got a little further than the fine mesh.

  • Evgenii_KEvgenii_K Member Posts: 31

    You are absolutely right! The casing consists of a technical fabric 1 mm thick (the fabric is very strong and can withstand heavy loads) stretched over a steel frame, a static load is applied to the casing - pressure. Is there a way to solve this convergence problem?

  • peteroznewmanpeteroznewman Member Posts: 11,369
    edited March 2 Accepted Answer

    @Evgenii_K

    Getting a structure with an applied pressure to show post-buckled results is challenging. Get ready for days (weeks?) of research. One requirement is to introduce some tiny amount of non-uniformity into the model to seed the buckled shape. This can be done by reshaping the geometry with a small amount of the linear elastic buckled shape, or you can apply a small force that will help it to buckle. Here is a YouTube video that explains that.

    https://www.youtube.com/watch?v=j_hdimE35hs

    You can learn something about the critical buckling load and the buckled shape using the linear Eigenvalue Buckling analysis.

    Start by taking the Structural Instabilities Course.

    https://courses.ansys.com/index.php/courses/structural-instabilities/

    Here are the discussions on linear Eigenvalue Buckling

    https://www.google.com/search?q=site%3Aforum.ansys.com+eigenvalue+buckling&oq=site%3Aforum.ansys.com+eigenvalue+buckling

    Here are the discussions on nonlinear post buckled analysis.

    https://www.google.com/search?q=site%3Aforum.ansys.com+nonlinear+post+buckling+stabilization+arc-length&oq=site%3Aforum.ansys.com+nonlinear+post+buckling+stabilization+arc-length

  • Evgenii_KEvgenii_K Member Posts: 31
    edited March 3

    I already studied this problem and came to the conclusion that it can be solved using Hill's fluidity, I even asked a question on this forum about how Hill's theory can be applied, I wrote to technical support, and wrote on other forums, no one could give an even answer. Your answer about how you can solve this problem is the most complete and fairly objective.

  • Evgenii_KEvgenii_K Member Posts: 31

    Peter, please tell me! I have a test of the shell we discussed. The shell was tested for biaxial tension, the test was carried out at the University of Newcastle. Is this data sufficient to compose the matrix and is it necessary to degenerate the stress through the deviator?


  • peteroznewmanpeteroznewman Member Posts: 11,369

    @Evgenii_K

    On sheet 1 I can see the UTS, but what you want is the Modulus. Do you have a copy of MSAJ/M-02-1995 to see how that test is performed?

  • Evgenii_KEvgenii_K Member Posts: 31

    Here is the full report, that's all there is. Pay attention to the unit of measurement of the results, especially the Poisson's ratio which is greater than 0.5 as I understand it can be greater than 0.5 if the material is anisotropic.


  • peteroznewmanpeteroznewman Member Posts: 11,369

    @Evgenii_K

    This is a woven fabric, so there are different properties in the Warp and Fill directions.

    What is the sheet thickness?

    What is the fiber material?

    What is the binder material?

    Do you have the material properties of the fiber and binder?

    ANSYS has ACP/Pre that allows you to define a composite material and put fibers down in two directions and hold them together with a binder.

  • Evgenii_KEvgenii_K Member Posts: 31

    ACP / Pre, I have already checked it will not work. To solve the problem, I need to convert the units of measurement to MPa and assign the properties of the material in the third direction. But those properties of the material that I have, they are not required for Hill's fluidity, for this task the stresses radiated during stretching and sliding are needed, and this experiment must be done three times, but I only have this data with them and I need to work with them. The question is, how can the experimental data be reduced to MPa and is it possible to take voltages from the diagram ?! The diagrams that in the report I converted into an electronic version and tried to use them in the model of hyperelastic materials, but here too, failure.

    Material thickness 1 mm, base material polymer reinforced with fiberglass mesh

Sign In or Register to comment.