Parameter Optimization for Biphasic Unconfined Compression Stress-Relaxation

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts
  • ateshian
    Developer
    • Dec 2007
    • 1824

    Parameter Optimization for Biphasic Unconfined Compression Stress-Relaxation

    This example describes a parameter optimization analysis for extracting material properties of cartilage from an unconfined compression stress-relaxation experiment. It uses experimental data from a stress-relaxation test performed on a disk of immature bovine articular cartilage (thanks to Brian Jones).

    In this analysis cartilage is modeled as a biphasic material whose porous matrix is described by a solid mixture of a "neo-Hookean" ground matrix (e.g., to model the contribution of proteoglycans to the compressive modulus) and a "spherical fiber distribution" to model the collagen fibrillar matrix (fibrils can only sustain tension). The hydraulic permeability is assumed to be constant.

    The model has a total of five material constants: Young's modulus (E) and Poisson's ratio (v) for the neo-Hookean solid, the fibril modulus ksi and the power-law exponent beta for the spherical fiber distribution, and the constant hydraulic permeability k. It is assumed a priori that v=0 and beta=2 so that the parameter optimization need only be performed on E, ksi and k.

    The material description in the model file (biphasic_ucsrlx_model.feb) is as follows:
    Code:
    		<material id="1" name="Cartilage" type="biphasic">
    			<phi0>0.2</phi0>
    			<solid type="solid mixture">
    				<solid name="fibers" type="spherical fiber distribution">
    					<beta>2</beta>
    					<ksi>4</ksi>
    				</solid>
    				<solid name="ground" type="neo-Hookean">
    					<density>1</density>
    					<E>0.33</E>
    					<v>0</v>
    				</solid>
    			</solid>
    			<permeability type="perm-const-iso">
    				<perm>0.001</perm>
    			</permeability>
    		</material>
    Notice that explicit names are provided for each <solid> component of the solid mixture, so that these names may be referenced in the optimization file (biphasic_ucsrlx_opt.feb) as follows:
    Code:
      <Parameters>
        <param name="Cartilage.permeability.perm">0.001, 0.0001, 0.002, 0.005</param>
        <param name="Cartilage.solid.ground.E">0.33, 0.1, 1, 1</param>
        <param name="Cartilage.solid.fibers.ksi">0.9, 0.2, 3, 1</param>
      </Parameters>
    This analysis is based on actual experimental data where the compressive displacement of the loading platen was recorded simultaneously with the platen load response. Though the desired platen displacement should have a linear ramp-and-hold profile, the actual displacement does not follow that profile exactly due to compliance in the loading apparatus. Therefore, the model file includes a load curve for the prescribed platen displacement which is based on the experimentally measured displacement.

    The parameter optimization analysis can be executed with the command
    Code:
    febio -s biphasic_ucsrlx_opt.feb
    The length units in this analysis are millimeters, force is in Newtons, time is in seconds. The analysis should converge to E=0.325 MPa, ksi=1.75 MPa and k=5.67E-04 mm^4/N.s. The quality of the fit is shown in the attached figure biphasic_ucsrlx_results.jpg.

    Gerard
    Last edited by ateshian; 12-04-2013, 09:31 AM.
  • ateshian
    Developer
    • Dec 2007
    • 1824

    #2
    To run this example in FEBio2, use biphasic_ucsrlx_model2.feb for the model file and biphasic_ucsrlx_opt2.feb for the optimization file. The command is
    Code:
    febio2 -i biphasic_ucsrlx_model2.feb -s biphasic_ucsrlx_opt2.feb
    Gerard

    Comment

    • fzmb treuter
      Member
      • Aug 2013
      • 79

      #3
      Hi Prof. Ateshian,

      I want to estimate the biomechanical properties of cartilage constructs from unconfined compression stress relaxation experiments. First I build the model and use biphasic theory (E, v and k). But no reaction force in z-direction are calculated. What is wrong? I have attached my model files. Please let me know what you think.

      ucc_rl_dtk1.prv

      Best regards,

      Thomas

      Comment

      • ateshian
        Developer
        • Dec 2007
        • 1824

        #4
        Hi Thomas,

        Would you please post the .feb file? I am unable to open the .prv file.

        Thanks,

        Gerard

        Comment

        • fzmb treuter
          Member
          • Aug 2013
          • 79

          #5
          Hi Prof. Ateshian,

          sorry for the late answer. Here is the .feb file. Please let me know what you think.

          ucc_rl_dtk1.feb

          Best regards,

          Thomas

          Comment

          • fzmb treuter
            Member
            • Aug 2013
            • 79

            #6
            Hi Prof. Ateshian,

            I cannot find the problem in my model. The reaction force in z-direction are not calculated. What is wrong! Please let me know what you think. I have attached my model files.

            ucc_rl_dtk1.feb

            Best,

            Thomas

            Comment

            • ateshian
              Developer
              • Dec 2007
              • 1824

              #7
              Hi Thomas,

              It appears that the loading platen has its outward normal facing up (away from the cartilage surface). You need to flip the platen 180 degrees so that the normal faces down toward the cartilage surface.

              Also, your symmetry plane has a width that matches the radius of the cartilage wedge exactly. This means that with compression, as the cartilage expands laterally, it will lose contact with the symmetry plane. I recommend that you increase the width of that plane.

              Best,

              Gerard

              Comment

              • fzmb treuter
                Member
                • Aug 2013
                • 79

                #8
                Hi Prof. Ateshian,

                thanks a lot. Now it works. The compression plot shows a little bit strange! Because the last part of the cartilage surface has no contact to the plate during the compression phase. Please, look at the following picture.

                compression.jpg

                Although the model is attached.

                ucc_rl_dtk1.feb

                Please, let me know what you thing. Maybe I have to change the biphasic contact?

                Best,

                Thomas

                Comment

                • ateshian
                  Developer
                  • Dec 2007
                  • 1824

                  #9
                  Hi Thomas,

                  From the picture it seems that you anchored the bottom surface to prevent it from moving in the radial direction. If it was your intention to model an adhesive interface, this result is not surprising, but you would have to add more elements along the axial direction to accurately reflect the response using this boundary condition. Otherwise, if your intent is to have a frictionless interface at the bottom, you should release the fixed conditions that constrain the radial expansion. In that case you will not observe a loss of contact at the radial edge.

                  Best,

                  Gerard

                  Comment

                  • fzmb treuter
                    Member
                    • Aug 2013
                    • 79

                    #10
                    Hi Prof. Ateshian,

                    thanks a lot! Now, the model works well.

                    Best,

                    Thomas

                    Comment

                    • fzmb treuter
                      Member
                      • Aug 2013
                      • 79

                      #11
                      Hi Prof. Ateshian,

                      why we use only one element in axial direction and many elements in radial direction? Because of the p=0 in radial direction?

                      Best regards,

                      Thomas

                      Comment

                      • Wilhelm
                        Junior Member
                        • Nov 2015
                        • 2

                        #12
                        Hi Prof. Ateshian,

                        I hope this threat is not dead by now.

                        I tried to run the example files in FeBio2; but with the message:
                        FATAL ERROR: the variable Cartilage.solid.ground.E is not recognized

                        Failed initializing the task: optimize

                        I am trying to find out what could be the reason; but first searches gave me material from 2 years ago. Back these days it was often referred to not actual versions of FeBio- i cannot imagine that I (after two years) would have an outdated version though.
                        I thought about a problem caused by changed syntax.

                        Can you give me a hint for my search?


                        Thanks in advance and best regards,

                        Alex

                        Comment

                        • ateshian
                          Developer
                          • Dec 2007
                          • 1824

                          #13
                          Hi Alex,

                          I checked the FEBio source code and it appears that changes were made to the method by which material parameters are read. In other words a bug crept into FEBio 2.4.0 and we will need to fix that. (The bug is fixed in the current development version, but we need to transfer that fix to a new release version 2.4.1.) In the meantime, you should be able to run this analysis with an earlier version.

                          Best,

                          Gerard

                          Comment

                          • ateshian
                            Developer
                            • Dec 2007
                            • 1824

                            #14
                            Hi Thomas,

                            The reason for using only one element along the axial direction is that the solid strain and fluid pressure are homogeneous in that direction. One element is enough to capture this response. (Strain is not homogeneous along the radial direction because p=0 as you surmised, leading to an inhomogeneous radial fluid flux, fluid pressure and strain.) This type of simplification only occurs for specialized geometries and boundary conditions, as in this example of unconfined compression with frictionless platens.

                            Best,

                            Gerard

                            Comment

                            • dsrawlins
                              Developer
                              • Dec 2008
                              • 366

                              #15
                              Hi Thomas,

                              The bug has been fixed and I've uploaded version 2.4.1 to the web site.

                              Cheers,

                              Dave
                              Department of Bioengineering, University of Utah
                              Scientific Computing and Imaging institute, University of Utah

                              Comment

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