Gasser-Ogden-Holzapfel-uncoupled model parameter setup

[SChen]

Hi,

I have a few questions regarding the parameter setup for the Gasser-Ogden-Holzapfel-uncoupled model.

<material id="1" name="Material1" type="Gasser-Ogden-Holzapfel-uncoupled">
<mat_axis type="vector">
<a>0,1,0</a>
<d>1,0,0</d>
</mat_axis>
<density>1</density>
<c>@c</c>
<k1>@k1</k1>
<k2>@k2</k2>
<kappa>0.15</kappa>
<gamma>41</gamma>
<k>@k</k>
</material>

For a parameter setup as above. <a> and <d> vectors would decide the e1, e2, e3.

Is e1 the bisector of the two fiber direction?

And are the two fiber families lie in the e1-e2 plane?

Is gamma the angle between e1 and each of the fiber famlily?

Is unit of gamma degree or radian?

Hope someone can help me out with this. The model parameters setup was not defined in the documentation.

Thank you!

Best,
Sheng

[ateshian]

Hi Sheng,

The Gasser-Ogden-Holzapfel-uncoupled model is undocumented because we have not been fully satisfied with the performance of our implementation. So please use it at your own risk (e.g., you have to first validate it against published results to convince yourself that it is working satisfactorily).

Is e1 the bisector of the two fiber direction?

Yes

And are the two fiber families lie in the e1-e2 plane?

Yes

Is gamma the angle between e1 and each of the fiber famlily?

Yes

Is unit of gamma degree or radian?

Radians

Best,

Gerard

[SChen]

Hi Gerard,

Thanks for the reply! Can I get a bit more info about what performance is not satisfiable so far, so that I know what to test and what the risk would be?

And just to confirm again, the unit of gamma is radian, correct? Since the angle parameters like phi and theta for fiber are in degrees. I assume gamma is in degree as well for consistency at first.

Thank you!

Best,
Sheng

[ateshian]

Hi Sheng,

This model is based on the paper by Gasser, Ogden and Holzapfel published in 2006 in J. R. Soc. Interface. In that paper, the authors present a number of test problems, not all of which seem to run successfully in our FEBio implementation. For example, the circumferential and axial cases presented in Fig. 9 of that paper run fine (kappa=0, no fiber dispersion), but the fiber dispersion case of Fig. 10b (kappa=0.226) does not converge beyond 2 mN of applied load, even though the paper shows result up to 1 N. Similarly, only the results for kappa=0 can be reproduced in Fig. 11 and not the results shown in Fig. 12.

Best,

Gerard

[cberggren]

Hi Gerard,

Have there been any changes in the status of the convergence issues for the Gasser-Ogden-Holzapfel model?

Thanks,

Caleb

[hik27]

Hi FEBio team,
I have a few questions regarding the Gasser-Ogden-Holzapfel-uncoupled model. I have a mesh with beam orientation assigned where I have the 3 eigen vectors & values for each element.

1. Is this model (Gasser-Ogden-Holzapfel-uncoupled model) working properly in FEBio studio? I checked the forum regarding this topic I saw some posts that suggest not to use it and another one saying it was working. I just wanted to confirm.

2. Also, how do we determine gamma if we are assigning orientation for each element? I used the HGO form in Abaqus before as given in this link (https://abaqus-docs.mit.edu/2017/Eng...stic-holzapfel). And the only parameters in Abaqus HGO are C10, D1, K1, K2, kappa. I was using the eigen vectors for orientation on each element. There is no variable gamma. I was wondering how I should determine gamma. Please advise.


Thanks,
Hirut

[ateshian]

Hi Hirut,

1. Is this model (Gasser-Ogden-Holzapfel-uncoupled model) working properly in FEBio studio? I checked the forum regarding this topic I saw some posts that suggest not to use it and another one saying it was working. I just wanted to confirm.

Yes, the HGO model is now documented, please see the User's Manual. This means that we consider it is working properly.

2. Also, how do we determine gamma if we are assigning orientation for each element? I used the HGO form in Abaqus before as given in this link (https://abaqus-docs.mit.edu/2017/Eng...stic-holzapfel). And the only parameters in Abaqus HGO are C10, D1, K1, K2, kappa. I was using the eigen vectors for orientation on each element. There is no variable gamma. I was wondering how I should determine gamma. Please advise.

The parameter gamma is defined in the paper by Gasser, Ogden and Holzapfel (T Christian Gasser, Ray W Ogden, Gerhard A Holzapfel. Hyperelastic modelling of arterial layers with distributed collagen fibre orientations. J R Soc Interface, 3(6):15-35, 2006). It represents the half-angle between the two fiber families. As explained in the User's Manual, the fiber families lie in the local x1-x2 (or x-y) plane. By default these axes are aligned with the global coordinate axes, however you can redefine the orientation of these axes using Material Axes, please see the section of the User's Manual that explains how to set material axes.

Best,

Gerard

[hik27]

Thank you for clarifying Dr Ateshian.

[biomath]

Hi, I'm trying to understand the specification of fiber angles for this model. (And in general). The angle gamma is the fiber angle in the e1-e2 plane relative to e1.

So my main question regards specifying e1 and e2. I am interested in a cylinder oriented along the z-axis. Within the HGO docs and menu I can specify angle, which then seems to correspond to local spherical coordinates, but here is where I'm getting a bit confused. I must sepcify theta and phi, but how do these correspond to the vectors e1 and e2 used to define the fibers.

I'd expect that for a given position (x,y,z) the change in coordinates is computed (i.e. the coordinates r, theta and phi are determined by x, y and z) and e_r, e_theta and e_phi are determined. Then I'd specify phi and theta and I'd define e_1 and e_2 for the fibers in terms of e_r, e_theta and e_phi. Do theta and phi correspond to the coefficients of a vector in terms of these basis vectors, i.e. e_1 = theta e_theta + phi e_phi? What is e_2 then? Then is the fiber direction at an angle gamma relative to e_1? It isn't entirely clear to me from the documentation if assigning theta and phi determine a change of coordinates or specify vectors somehow.

I guess that specifying the fibers withing HGO doesn't allow visualizing them in the graphics view of FEBio Studio. Toggle fibers doesn't show anything for me.

In any case, I'd like to have fibers oriented within the cylinder abd at an angle gamma relative to the cylinder axis, e_z in the global coordinate system. It seems like the cylinder specification could be used, but this is not available under HGO model? Should I use cylinder to create a local axis and then select 'local' in the HGO material?

[ateshian]

Hi,

Fiber angles are specified relative to the local coordinate system of each element. By default, each finite element in a mesh has a local coordinate system x1, x2, x3 (or x,y,z) aligned with the global coordinate system. However, there are many methods in FEBioStudio that allow you to create a local coordinate system in each finite element of the mesh. The mesh has to be editable (when the geometry is created within FEBioStudio, then meshed, one has to Convert to Editable Mesh -- otherwise, imported meshes are editable by default). The tools for assigning local material axes are available in the Mesh tab of the Build panel. Check out the two buttons labels "Set Axes" and "Set Axes from Curvature".

Toggle Material Axes and display the mesh in wireframe mode (Toggle Render Mode).

For example:

1) Build->Create->Tube
2) Mesh->Apply, then Convert->Editable Mesh
3) Select all faces on the cylindrical boundary, Set Axes from Curvature->generator: quadric (because this is a perfect cylindrical surface, i.e., a quadric surface), check Whole part, then Apply.
4) View->Toggle Material Axes, View->Toggle Render Mode (make sure that you have un-clicked the "Select faces" button, needed to display the wireframe mode). You will notice that the x-axis (red) is circumferential, the y-axis (green) is axial, and the z-axis (blue) is radial. This means that the plane tangent to the cylindrical surface is the local x-y plane.
5) Model->right click on Materials->Add Material->Category: uncoupled elastic->Material: Holzapfel-Gasser-Ogden.
6) Enter desired material properties.
7) Axes->angles, theta=gamma, phi=90. This means that the angle between x and y-axes is gamma, and the angle with the z-axis is 90, so that the fibers are in the plane tangent to the cylindrical surface.
8) Apply boundary conditions and a pressure (e.g., on the inner tube surface) and set up a structural analysis.

Here is an illustration of how I implemented this model: HGOexample.fsm

Since the Holzapfel-Gasser-Ogden model does not use the standard fiber model in FEBio (i.e., standard fiber model = a single fiber which sustains tension only, instead of a fiber bundle as in HGO, where the bundle sustains tension if the principal fiber direction is in tension), there is no mechanism to display the fiber vector for the principal fiber direction.

Alternatively, if you choose to use the old Holzapfel-Gasser-Ogden model from their 2000 paper, where they use a standard fiber model, you can create an uncoupled solid mixture with a Mooney-Rivlin ground matrix and two fiber-ex-pow-uncoupled fibers, oriented relative to the local material axes using the "angles" option. Then you can add custom plot variables to display the two fiber vectors, and label them as fiber1 and fiber2 (for example), as illustrated in the attached model file: HGOexample_alt.fsm

Best,

Gerard

[biomath]

Thanks, that helps a lot. I had slowly started to see how to do something like this, so great to confirm that I was starting to understand. I note that I was able to set axis with Mesh->Set Axis->Generator=cylindrical without explicitly making an editable mesh in case that is unintended behavior. I see that the method from curvature would generalize to non-idealized geometries.

I will just note that I get identical results using Axis=None and Axis=Angle, which makes sense to me. As I understood the documentation, Axis=None should default to using the Axis defined above, and then the fibers would be at angle gamma relative to the local x1 axis. Is that correct and then does that mean that the use of "Angles" option for Axes is only necessary to define fibers to be out of the x-y plane. (Is it possible to define phi as "depth"/location dependent?)

If one uses the "Angles" option for Axes does that mean that the value for gamma is redundant/irrelevant and overridden by theta?

Also, you say the angle between the x and y-axes is gamma, but gamma is actually the angle between the fiber direction and the x (e1) axis, right? Then the angle with y-axes would be 90-gamma, and the angle between x and y is always 90, right?

Best,
Jacob