2D Fung anisotropic material mdoel

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts
  • mirukpt
    Junior Member
    • Jun 2015
    • 19

    2D Fung anisotropic material mdoel

    Hello

    I am trying to model an artery using the 2D Fung anisotropic material model without including the shear components. This is a 4-parameter (3 parameters plus 'c') model and is defined as below:

    SED = (c/2)*(exp(Q) - 1); Q=A1.E11^2 +A2.E22^2 +2 A3.E11.E22;

    Is there a way to use this material model in Preview/FEBio?

    Thanks
    Mirunalini
  • ateshian
    Developer
    • Dec 2007
    • 1821

    #2
    Hi Mirunalini,

    You can use the "Fung-ortho-compressible" or "Fung orthotropic" materials and select the material properties as described in the User Manual. To understand how these properties related to the coefficients in your formula, please see this paper.

    Best,

    Gerard

    Comment

    • mirukpt
      Junior Member
      • Jun 2015
      • 19

      #3
      Hello Gerard,

      Thank you for the reference.. I was able to successfully write all my material model parameters in terms of Ei and Gij.

      1. Since I do not have any shear components in my material model (c7=c8=c9=0), all the Gij = 0. But this would imply perfectly incompressible material. Is there a value that you suggest I use for Gij to make it slightly compressible, so that my FEA solutions converge?

      2. Also, since I am assuming anisotropy, I can no longer use Hooke's law to determine the bulk modulus. what value of bulk modulus do you recommend? I assume that it should be a high value based on Holzapfel's penalty method.

      3. If I am not assuming anisotropy, would -nu12/E1 = -nu21/E2 still hold true? (These correspond to the 'lambda12' entries in the matrix shown in the user manual.)

      4. I tried to import a .nas file generated in ANSYS ICEM, but Preview crashes while importing it. I did not have any issues with importing a .nas file generated from a different mesh generation software.

      Thanks
      Mirunalini

      Comment

      • ateshian
        Developer
        • Dec 2007
        • 1821

        #4
        Hi Mirunalini,

        1. Since I do not have any shear components in my material model (c7=c8=c9=0), all the Gij = 0. But this would imply perfectly incompressible material. Is there a value that you suggest I use for Gij to make it slightly compressible, so that my FEA solutions converge?
        Setting Gij=0 does not make the material perfectly incompressible (these are unrelated). If you are having convergence issues, it could result from the fact that the material cannot resist shear, even while your model may be subjecting the material to shear. In that case, you can investigate iteratively which values of Gij help you achieve convergence. There is no value that we can suggest otherwise.

        2. Also, since I am assuming anisotropy, I can no longer use Hooke's law to determine the bulk modulus. what value of bulk modulus do you recommend? I assume that it should be a high value based on Holzapfel's penalty method.
        When using the uncoupled formulation for the Fung material, you can select the bulk modulus k independently of the other elastic constants. To enforce incompressibility, k should be much larger (e.g., 1000 times bigger) than the largest elastic modulus in the rest of your material definition.

        3. If I am not assuming anisotropy, would -nu12/E1 = -nu21/E2 still hold true? (These correspond to the 'lambda12' entries in the matrix shown in the user manual.)
        This relationship must hold true in the Fung material, no matter what else you assume. The lowest possible symmetry for the Fung material is orthotropic, but you can choose material properties that produce transversely isotropic or isotropic behaviors.

        4. I tried to import a .nas file generated in ANSYS ICEM, but Preview crashes while importing it. I did not have any issues with importing a .nas file generated from a different mesh generation software.
        I regret that I don't have expertise in this topic. Please submit a PreView bug report and attach the mesh file that is causing this problem.

        Best,

        Gerard

        Comment

        • mirukpt
          Junior Member
          • Jun 2015
          • 19

          #5
          Hello Gerard,

          I have another issue while translating Fung model parameters to Ei and Gij for input into FEBio. I understand that the spatial elasticity tensor should be first inverted and then equated to the stiffness matrix for orthotropic symmetry. I substituted the Lame like parameters (lambda ab and mu a) with equivalent expressions in terms of the Fung model constants and then inverted it. However, in my material model, since some constants are zero, the spatial elasticity tensor turns out to be singular. This does not allow me to obtain the values of Ei and Gij.

          My model is W=c/2(exp(Q)-1)
          Q=c3*E11^2+c2*E22^2+2*c5*E11*E22+2*c8*E12^2

          This renders the following constants to be zero, c1=c4=c6=c7=c9=0, which causes the determinant to be zero.
          Is there any other way this can be solved (without altering my model) other than by introducing an extra "c1*E33^2" term in my model?

          Thank you
          Mirunalini

          Comment

          • ateshian
            Developer
            • Dec 2007
            • 1821

            #6
            Hi Mirunalini,

            In a strict sense, when the determinant of the elasticity tensor is zero the material response is unstable (e.g., the volume collapses to zero upon loading). So the only solution is to create a material model that's not unstable. Your formulation is two-dimensional but being applied to three-dimensional space, which is the reason for this outcome.

            Best,

            Gerard

            Comment

            • mirukpt
              Junior Member
              • Jun 2015
              • 19

              #7
              Thank you for your reply, Gerard.

              I have been assuming the constants in the thickness direction as mentioned in "Jermihov, Paul N. et al. “Effect of Geometry on the Leaflet Stresses in Simulated Models of Congenital Bicuspid Aortic Valves.” Cardiovascular engineering and technology 2.1 (2011): 48–56. PMC. Web. 10 Jan. 2016."

              verbatim :"To facilitate the analysis, the values of material constants in the thickness direction have to be assumed. Since the leaflet is thin and the thickness direction is not load-bearing, we expect the material to be even softer than the weaker in-plane direction and have minimal influence on the in-plane response. Based on this consideration, the material parameters are assumed to be equal to half of the radial direction in-plane material constants".

              However, this yields Poisson's ratio of .93 and .5 in the theta-r and r-theta directions respectively. So the above assumption of the remaining constants is not valid for my model.

              Comment

              • kostas
                Junior Member
                • Jul 2020
                • 13

                #8
                Hi Gerard,
                I realize this is an old thread but i was hoping for some further clarification on the Fung orthotropic SEF parameters. More specifically, I would like to know the relationship between the moduli appearing in PreView and the coefficients in Equation (b)/ page 3 of your paper :https://www.ncbi.nlm.nih.gov/pmc/articles/PMC3612496/ .
                Would be so kind as to confirm that the correct relationship between these two sets of coefficients is : c1=E1 / c2=E2 / c3=E3 / c4=v12 / c5=v23 / c6=v31 / c7=G12 / c8=G23 /c9=G31
                Thank you in advance,
                Kostas

                Comment

                • ateshian
                  Developer
                  • Dec 2007
                  • 1821

                  #9
                  Hi Kostas,

                  The formulas you wrote are not correct. The paper you cited relates the coefficients c1-c9 to the Lamé coefficients lambda_ab and mu_a (a,b=1,2,3). These Lamé coefficients are related to Young's moduli and Poisson's ratios of the Fung Orthotropic material according to the attached pages (which are from the User's Manual for FEBio3.0, to be released soon). Please take a look at those pages and let me know if this answers your question.

                  Best,

                  Gerard

                  FungOrthotropic.pdf.zip

                  Comment

                  • kostas
                    Junior Member
                    • Jul 2020
                    • 13

                    #10
                    Hi Gerard,

                    It does indeed answer my question. The pdf file was very helpful! Thank you for your time and your quick reply.

                    Best regards,
                    Kostas

                    Comment

                    • kostas
                      Junior Member
                      • Jul 2020
                      • 13

                      #11
                      Hi Gerard,

                      I defined the parameters successfully. Now I want to apply the Fung orthotropic material for a curved cylindrical artery geometry. As I understand, the material axes α (α=1,2,3) determine the E1,Ε2,Ε3,v12,...etc. Which are the default material axes according to the coordinate system? Is there any way to define the orientation for example of E1, E2 to correspond to circumferential and longitudinal direction? Can the Cartesian coordinate system be transformed to a cylindrical one?

                      Comment

                      • ateshian
                        Developer
                        • Dec 2007
                        • 1821

                        #12
                        Hi Kostas,

                        Please check this post regarding the FEBioStudio tool Set Axes from Curvature and let me know if it answers your query.

                        Best,

                        Gerard

                        Comment

                        • kostas
                          Junior Member
                          • Jul 2020
                          • 13

                          #13
                          Hi Gerard,

                          From what I gather from this post, the default material axes are the cartesian x,y,z. So what I need to do is change from a cartesian into a local coordinate system. I applied the "Set axes from curvature" option and "Executing command: Change mesh (Axes from Curvature)" appeared in the Log . I don't know if the changes were applied because when I tried to run the case it ended with the message "ERROR TERMINATION". Also, when applying the Fung-orthotropic material there is the property "Material axes" with the default value being "(none)". Do I need to change that ? Thank you in advance.

                          Comment

                          • ateshian
                            Developer
                            • Dec 2007
                            • 1821

                            #14
                            Hi Kostas,

                            To visualize the material axes in FEBioStudio, use View->Toggle Material Axes.

                            Material axes defined inside a material (such as in the Fung-orthotropic material) represent a further transformation of the underlying element material axes (which are either aligned with the global axes or vary with each element as done, for example, using Set axes from curvature). So, if you want your material axes to be transformed relative to the element axes, use the "Material axes" option in FEBioStudio for Fung-orthotropic.

                            BTW, if your material is a solid mixture, each solid constituent of the mixture can have its own material axes relative to the element material axes. This allows users to define multiple fibers (or fiber families), each with its unique orientation, within a mixture.

                            Best,

                            Gerard

                            Comment

                            • kostas
                              Junior Member
                              • Jul 2020
                              • 13

                              #15
                              Hi Gerard,

                              I used the "Toggle Material Axes" option after applying "Set axes from curvature" but it doesn't seem to work and I still have the cartesian coordinate system. Moreover, as you suggested, I tried using the "Material axes" by "local node numbering" option but I have trouble filling in the node values. I have a tetrahedral element mesh (TET4) but I don't know which nodes are which. What I mean is, to which nodes in my model do the values n0,n1,n2 correspond? I want to define a local coordinate system as shown in the screeshot below (please ignore the existing node values). Could you tell me what values do I need to isnert in order to achieve that? Also, for some reason, the node n2 cannot take any value besides 0. Thanks again!
                              local.png

                              Comment

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