orientation about fung orthotropic material

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts
  • wlin1985
    Junior Member
    • Oct 2011
    • 13

    orientation about fung orthotropic material

    Hello,

    Now, I am doing a simple uniaxial compression with 0.1% strain via FEBio and ANSYS for verifing. Since the strain is very small, the Fung Orthotropic reduces to linear constitutive model. I tried to use <mat_axis type="vector"> <a>1,0,0</a> <d>0,1,0</d> </mat_axis> to define its directions. By changing the a and d, the results changed but there was still big difference between the results of FEBio and ANSYS.

    I want to know if the default initial directions of Fung Orthotropic material axes are the XYZ axises. If not, please help me to point it out.

    Thanks a lot,

    Lin
  • wlin1985
    Junior Member
    • Oct 2011
    • 13

    #2
    The attachment follows.

    Comment

    • ateshian
      Developer
      • Dec 2007
      • 1824

      #3
      Hi Lin,

      I want to know if the default initial directions of Fung Orthotropic material axes are the XYZ axises. If not, please help me to point it out.
      Yes, the default directions for orthotropic materials (if none are specified) are the XYZ axes.

      The file that you attached to your email shows axes orientations which are not aligned with the XYZ coordinates. Was that your intention?

      Are you comparing FEBio to ANSYS for a compressible orthotropic material? Or for a nearly-incompressible material? In FEBio, there are two Fung materials: "Fung orthotropic" (which you use in your example file), which is for nearly-incompressible materials, and "Fung-ortho-compressible." If your ANSYS analyses is for compressible materials, I suggest that you use the second model, and set the parameter "k" to zero.

      Let me know if that helps.

      Gerard

      Comment

      • wlin1985
        Junior Member
        • Oct 2011
        • 13

        #4
        Hi, Gerard,

        Appreciate for your reply.

        Yes, I defined the orientations to investigate the off-axis compression case. The mechanical properties for the material in the FEB file is some kind of wood, so it should be a compressible material. However, I can not find the "Fung-ortho-compressible" constitutive in the PreView 1.6. I think I should check other versions for PreView.

        Thanks a lot,

        Lin


        Originally posted by ateshian View Post
        Hi Lin,



        Yes, the default directions for orthotropic materials (if none are specified) are the XYZ axes.

        The file that you attached to your email shows axes orientations which are not aligned with the XYZ coordinates. Was that your intention?

        Are you comparing FEBio to ANSYS for a compressible orthotropic material? Or for a nearly-incompressible material? In FEBio, there are two Fung materials: "Fung orthotropic" (which you use in your example file), which is for nearly-incompressible materials, and "Fung-ortho-compressible." If your ANSYS analyses is for compressible materials, I suggest that you use the second model, and set the parameter "k" to zero.

        Let me know if that helps.

        Gerard

        Comment

        • ateshian
          Developer
          • Dec 2007
          • 1824

          #5
          Hi Lin,

          You can enter "Fung-ortho-compressible" directly into the .feb file using a text editor.

          Alternatively you can use the ”linear orthotropic” material.

          Best,

          Gerard

          Comment

          • wlin1985
            Junior Member
            • Oct 2011
            • 13

            #6
            Hello, Gerard,

            Fantastic! I am always disappointed about the lack of linear elastic isotropic and orthotropic models. You do help me a lot.

            By employing the linear orthotropic model, all results for on-axis compression cases are the same as ANSYS. Unfortunately, the off-axis compression case looks odd. Since it was an uniaxial compression, the stress along the compressive direction should be uniform while the stress along the two other directions, zero. However, the result did not show this characteristic.

            The FEB file is attached.

            BTW, I am sure that postview uses the Largerange strain for strain plot. So for the stress plot, engineering stress?

            Thanks,

            Lin

            Originally posted by ateshian View Post
            Hi Lin,

            You can enter "Fung-ortho-compressible" directly into the .feb file using a text editor.

            Alternatively you can use the ”linear orthotropic” material.

            Best,

            Gerard

            Comment

            • ateshian
              Developer
              • Dec 2007
              • 1824

              #7
              Hi Lin,

              For the off-axis compression, the state of stress is not uniform (unlike the on-axis loading). Therefore you have to be careful to pick a mesh that is sufficiently refined to capture the correct traction-free boundary conditions. See the attached OrthoWoodBM.feb file, where a biased mesh is used. If you run this problem, you will find that the stress Syy reduces to zero on the top face and Szz reduces to zero on the front face. (Actually, the values are not exactly zero, since they are evaluated at the center of the element, not on the face. The thinner the element, the closer this value should be to zero.) The other faces don't show zero stresses because of the boundary conditions applied on them (either symmetry conditions or prescribed displacement along x).

              In principle, you should see the same result in ANSYS.

              BTW, I am sure that postview uses the Largerange strain for strain plot. So for the stress plot, engineering stress?
              Yes, the strain is the Lagrangian strain. The stress is the Cauchy stress.

              Best,

              Gerard

              Comment

              • wlin1985
                Junior Member
                • Oct 2011
                • 13

                #8
                Hello, Gerard,

                I sincerely give thanks to you for your kindhearted helps and advices. I will do a further check about this case.

                Regards,

                Lin

                Originally posted by ateshian View Post
                Hi Lin,

                For the off-axis compression, the state of stress is not uniform (unlike the on-axis loading). Therefore you have to be careful to pick a mesh that is sufficiently refined to capture the correct traction-free boundary conditions. See the attached OrthoWoodBM.feb file, where a biased mesh is used. If you run this problem, you will find that the stress Syy reduces to zero on the top face and Szz reduces to zero on the front face. (Actually, the values are not exactly zero, since they are evaluated at the center of the element, not on the face. The thinner the element, the closer this value should be to zero.) The other faces don't show zero stresses because of the boundary conditions applied on them (either symmetry conditions or prescribed displacement along x).

                In principle, you should see the same result in ANSYS.



                Yes, the strain is the Lagrangian strain. The stress is the Cauchy stress.

                Best,

                Gerard

                Comment

                • wlin1985
                  Junior Member
                  • Oct 2011
                  • 13

                  #9
                  Hello, Gerard,

                  I just realized my mistake in ANSYS, the wrong use of symmetry boundary condition since the material is not symmetry. If using full model, the result seems similar as FEBio.

                  The problem occured now is when I using the full computational model in FEBio, it failed because of negative jacobian. Compared with 1/4 model, I think it was caused by insufficient boundary constraint. However, for simple compression case, fixed one area and given a prescribed displacement at its opposite area should be enough. Could you help me to point out the reason of this failure? Thanks a lot.

                  Lin



                  Originally posted by ateshian View Post
                  Hi Lin,

                  For the off-axis compression, the state of stress is not uniform (unlike the on-axis loading).

                  The other faces don't show zero stresses because of the boundary conditions applied on them (either symmetry conditions or prescribed displacement along x).

                  Gerard

                  Comment

                  • ateshian
                    Developer
                    • Dec 2007
                    • 1824

                    #10
                    Hi Lin,

                    Try solving the problem using the Full-Newton solver, instead of BFGS. That worked for me.

                    Gerard

                    Comment

                    Working...
                    X
                    😀
                    😂
                    🥰
                    😘
                    🤢
                    😎
                    😞
                    😡
                    👍
                    👎