DEMO_febio_0017_cube_viscoelastic_load_unload

Below is a demonstration for:

Contents

Keywords

clear; close all; clc;

Plot settings

fontSize=20;
faceAlpha1=0.8;
markerSize=40;
lineWidth=3;

Control parameters

% Path names
defaultFolder = fileparts(fileparts(mfilename('fullpath')));
savePath=fullfile(defaultFolder,'data','temp');

% Defining file names
febioFebFileNamePart='tempModel';
febioFebFileName=fullfile(savePath,[febioFebFileNamePart,'.feb']); %FEB file name
febioLogFileName=fullfile(savePath,[febioFebFileNamePart,'.txt']); %FEBio log file name
febioLogFileName_disp=[febioFebFileNamePart,'_disp_out.txt']; %Log file name for exporting displacement
febioLogFileName_force=[febioFebFileNamePart,'_force_out.txt']; %Log file name for exporting force
febioLogFileName_stress=[febioFebFileNamePart,'_stress_out.txt']; %Log file name for exporting stress

%Specifying dimensions and number of elements
cubeSize=10;
sampleWidth=cubeSize; %Width
sampleThickness=cubeSize; %Thickness
sampleHeight=cubeSize; %Height
pointSpacings=2*ones(1,3); %Desired point spacing between nodes
numElementsWidth=round(sampleWidth/pointSpacings(1)); %Number of elemens in dir 1
numElementsThickness=round(sampleThickness/pointSpacings(2)); %Number of elemens in dir 2
numElementsHeight=round(sampleHeight/pointSpacings(3)); %Number of elemens in dir 3

%Define applied displacement
appliedStrain=0.3; %Linear strain (Only used to compute applied stretch)
loadingOption='compression'; % or 'tension'
switch loadingOption
    case 'compression'
        stretchLoad=1-appliedStrain; %The applied stretch for uniaxial loading
    case 'tension'
        stretchLoad=1+appliedStrain; %The applied stretch for uniaxial loading
end
displacementMagnitude=(stretchLoad*sampleHeight)-sampleHeight; %The displacement magnitude

%Material parameter set
c1=1e-3; %Shear-modulus-like parameter
m1=8; %Material parameter setting degree of non-linearity
k_factor=1e2; %Bulk modulus factor
k=c1*k_factor; %Bulk modulus
g1=30; %Viscoelastic QLV proportional coefficient
t1=6; %Viscoelastic QLV time coefficient
d=1e-9; %Density (not required for static analysis)
uncoupledLaw=1; %1=uncoupled, 2=coupled

analysisType='static';

% FEA control settings

t_load=2; %Time from start to max load
t_step_ini1=t_load/20; %Initial desired step size
numTimeSteps1=round(t_load/t_step_ini1); %Number of time steps desired
t_step1=t_load/numTimeSteps1; %Step size
dtmin1=t_step1/100; %Smallest allowed step size
dtmax1=t_step1; %Largest allowed step size

t_unload=t_load;
t_step_ini2=t_step_ini1; %Initial desired step size
numTimeSteps2=round(t_unload/t_step_ini2); %Number of time steps desired
t_step2=t_unload/numTimeSteps2; %Step size
dtmin2=t_step2/100; %Smallest allowed step size
dtmax2=t_step2; %Largest allowed step size


max_refs=25; %Max reforms
max_ups=0; %Set to zero to use full-Newton iterations
opt_iter=6; %Optimum number of iterations
max_retries=5; %Maximum number of retires

Creating model geometry and mesh

A box is created with tri-linear hexahedral (hex8) elements using the hexMeshBox function. The function offers the boundary faces with seperate labels for the top, bottom, left, right, front, and back sides. As such these can be used to define boundary conditions on the exterior.

% Create a box with hexahedral elements
cubeDimensions=[sampleWidth sampleThickness sampleHeight]; %Dimensions
cubeElementNumbers=[numElementsWidth numElementsThickness numElementsHeight]; %Number of elements
outputStructType=2; %A structure compatible with mesh view
[meshStruct]=hexMeshBox(cubeDimensions,cubeElementNumbers,outputStructType);

%Access elements, nodes, and faces from the structure
E=meshStruct.elements; %The elements
V=meshStruct.nodes; %The nodes (vertices)
Fb=meshStruct.facesBoundary; %The boundary faces
Cb=meshStruct.boundaryMarker; %The "colors" or labels for the boundary faces
elementMaterialIndices=ones(size(E,1),1); %Element material indices

Plotting model boundary surfaces and a cut view

hFig=cFigure;

subplot(1,2,1); hold on;
title('Model boundary surfaces and labels','FontSize',fontSize);
gpatch(Fb,V,Cb,'k',faceAlpha1);
colormap(gjet(6)); icolorbar;
axisGeom(gca,fontSize);

hs=subplot(1,2,2); hold on;
title('Cut view of solid mesh','FontSize',fontSize);
optionStruct.hFig=[hFig hs];
meshView(meshStruct,optionStruct);
axisGeom(gca,fontSize);

drawnow;

Defining the boundary conditions

The visualization of the model boundary shows colors for each side of the cube. These labels can be used to define boundary conditions.

%Define supported node sets
logicFace=Cb==1; %Logic for current face set
Fr=Fb(logicFace,:); %The current face set
bcSupportList_X=unique(Fr(:)); %Node set part of selected face

logicFace=Cb==3; %Logic for current face set
Fr=Fb(logicFace,:); %The current face set
bcSupportList_Y=unique(Fr(:)); %Node set part of selected face

logicFace=Cb==5; %Logic for current face set
Fr=Fb(logicFace,:); %The current face set
bcSupportList_Z=unique(Fr(:)); %Node set part of selected face

%Prescribed displacement nodes
logicPrescribe=Cb==6; %Logic for current face set
Fr=Fb(logicPrescribe,:); %The current face set
bcPrescribeList=unique(Fr(:)); %Node set part of selected face

Visualizing boundary conditions. Markers plotted on the semi-transparent model denote the nodes in the various boundary condition lists.

hf=cFigure;
title('Boundary conditions','FontSize',fontSize);
xlabel('X','FontSize',fontSize); ylabel('Y','FontSize',fontSize); zlabel('Z','FontSize',fontSize);
hold on;

gpatch(Fb,V,'kw','k',0.5);

hl(1)=plotV(V(bcSupportList_X,:),'r.','MarkerSize',markerSize);
hl(2)=plotV(V(bcSupportList_Y,:),'g.','MarkerSize',markerSize);
hl(3)=plotV(V(bcSupportList_Z,:),'b.','MarkerSize',markerSize);
hl(4)=plotV(V(bcPrescribeList,:),'k.','MarkerSize',markerSize);

legend(hl,{'BC x support','BC y support','BC z support','BC z prescribe'});

axisGeom(gca,fontSize);
camlight headlight;
drawnow;

Defining the FEBio input structure

See also febioStructTemplate and febioStruct2xml and the FEBio user manual.

%Get a template with default settings
[febio_spec]=febioStructTemplate;

%febio_spec version
febio_spec.ATTR.version='2.5';

%Module section
febio_spec.Module.ATTR.type='solid';

%Get control section from template
stepStruct.Control=febio_spec.Control;

%Remove control field (part of template) since step specific control sections are used
febio_spec=rmfield(febio_spec,'Control');

%Control sections for each step
febio_spec.Step{1}.ATTR.id=1;
febio_spec.Step{1}.Control=stepStruct.Control;
febio_spec.Step{1}.Control.analysis.ATTR.type=analysisType;
febio_spec.Step{1}.Control.time_steps=numTimeSteps1;
febio_spec.Step{1}.Control.step_size=t_step1;
febio_spec.Step{1}.Control.time_stepper.dtmin=dtmin1;
febio_spec.Step{1}.Control.time_stepper.dtmax=dtmax1;
febio_spec.Step{1}.Control.time_stepper.max_retries=max_retries;
febio_spec.Step{1}.Control.time_stepper.opt_iter=opt_iter;
febio_spec.Step{1}.Control.max_refs=max_refs;
febio_spec.Step{1}.Control.max_ups=max_ups;

febio_spec.Step{2}.ATTR.id=2;
febio_spec.Step{2}.Control=stepStruct.Control;
febio_spec.Step{2}.Control.analysis.ATTR.type=analysisType;
febio_spec.Step{2}.Control.time_steps=numTimeSteps2;
febio_spec.Step{2}.Control.step_size=t_step2;
febio_spec.Step{2}.Control.time_stepper.dtmin=dtmin2;
febio_spec.Step{2}.Control.time_stepper.dtmax=dtmax2;
febio_spec.Step{2}.Control.time_stepper.max_retries=max_retries;
febio_spec.Step{2}.Control.time_stepper.opt_iter=opt_iter;
febio_spec.Step{2}.Control.max_refs=max_refs;
febio_spec.Step{2}.Control.max_ups=max_ups;

%Material section
switch uncoupledLaw
    case 1
        %Viscoelastic part
        febio_spec.Material.material{1}.ATTR.type='uncoupled viscoelastic';
        febio_spec.Material.material{1}.ATTR.Name='Block_material';
        febio_spec.Material.material{1}.ATTR.id=1;
        febio_spec.Material.material{1}.g1=g1;
        febio_spec.Material.material{1}.t1=t1;
        febio_spec.Material.material{1}.density=d;

        %Elastic part
        febio_spec.Material.material{1}.elastic{1}.ATTR.type='Ogden';
        febio_spec.Material.material{1}.elastic{1}.c1=c1;
        febio_spec.Material.material{1}.elastic{1}.m1=m1;
        febio_spec.Material.material{1}.elastic{1}.c2=c1;
        febio_spec.Material.material{1}.elastic{1}.m2=-m1;
        febio_spec.Material.material{1}.elastic{1}.k=k;
        febio_spec.Material.material{1}.elastic{1}.density=d;
    case 2
        %Viscoelastic part
        febio_spec.Material.material{1}.ATTR.type='viscoelastic';
        febio_spec.Material.material{1}.ATTR.Name='Block_material';
        febio_spec.Material.material{1}.ATTR.id=1;
        febio_spec.Material.material{1}.g1=g1;
        febio_spec.Material.material{1}.t1=t1;
        febio_spec.Material.material{1}.density=d;

        %Elastic part
        febio_spec.Material.material{1}.elastic{1}.ATTR.type='Ogden unconstrained';
        febio_spec.Material.material{1}.elastic{1}.c1=c1;
        febio_spec.Material.material{1}.elastic{1}.m1=m1;
        febio_spec.Material.material{1}.elastic{1}.c2=c1;
        febio_spec.Material.material{1}.elastic{1}.m2=-m1;
        febio_spec.Material.material{1}.elastic{1}.cp=k;
        febio_spec.Material.material{1}.elastic{1}.density=d;
end

%Geometry section
% -> Nodes
febio_spec.Geometry.Nodes{1}.ATTR.name='nodeSet_all'; %The node set name
febio_spec.Geometry.Nodes{1}.node.ATTR.id=(1:size(V,1))'; %The node id's
febio_spec.Geometry.Nodes{1}.node.VAL=V; %The nodel coordinates

% -> Elements
febio_spec.Geometry.Elements{1}.ATTR.type='hex8'; %Element type of this set
febio_spec.Geometry.Elements{1}.ATTR.mat=1; %material index for this set
febio_spec.Geometry.Elements{1}.ATTR.name='Cube'; %Name of the element set
febio_spec.Geometry.Elements{1}.elem.ATTR.id=(1:1:size(E,1))'; %Element id's
febio_spec.Geometry.Elements{1}.elem.VAL=E;

% -> NodeSets
febio_spec.Geometry.NodeSet{1}.ATTR.name='bcSupportList_X';
febio_spec.Geometry.NodeSet{1}.node.ATTR.id=bcSupportList_X(:);

febio_spec.Geometry.NodeSet{2}.ATTR.name='bcSupportList_Y';
febio_spec.Geometry.NodeSet{2}.node.ATTR.id=bcSupportList_Y(:);

febio_spec.Geometry.NodeSet{3}.ATTR.name='bcSupportList_Z';
febio_spec.Geometry.NodeSet{3}.node.ATTR.id=bcSupportList_Z(:);

febio_spec.Geometry.NodeSet{4}.ATTR.name='bcPrescribeList';
febio_spec.Geometry.NodeSet{4}.node.ATTR.id=bcPrescribeList(:);

%Boundary condition section
% -> Fix boundary conditions
febio_spec.Boundary.fix{1}.ATTR.bc='x';
febio_spec.Boundary.fix{1}.ATTR.node_set=febio_spec.Geometry.NodeSet{1}.ATTR.name;
febio_spec.Boundary.fix{2}.ATTR.bc='y';
febio_spec.Boundary.fix{2}.ATTR.node_set=febio_spec.Geometry.NodeSet{2}.ATTR.name;
febio_spec.Boundary.fix{3}.ATTR.bc='z';
febio_spec.Boundary.fix{3}.ATTR.node_set=febio_spec.Geometry.NodeSet{3}.ATTR.name;

% -> Prescribe boundary conditions
febio_spec.Boundary.prescribe{1}.ATTR.bc='z';
febio_spec.Boundary.prescribe{1}.ATTR.node_set=febio_spec.Geometry.NodeSet{4}.ATTR.name;
febio_spec.Boundary.prescribe{1}.scale.ATTR.lc=1;
febio_spec.Boundary.prescribe{1}.scale.VAL=1;
febio_spec.Boundary.prescribe{1}.relative=1;
febio_spec.Boundary.prescribe{1}.value=displacementMagnitude;

%LoadData section
% -> Load curves
febio_spec.LoadData.loadcurve{1}.ATTR.id=1;
febio_spec.LoadData.loadcurve{1}.ATTR.type='linear';
febio_spec.LoadData.loadcurve{1}.point.VAL=[0 0;t_load 1;(t_load+t_unload) 0];

%Output section
% -> log file
febio_spec.Output.logfile.ATTR.file=febioLogFileName;
febio_spec.Output.logfile.node_data{1}.ATTR.file=febioLogFileName_disp;
febio_spec.Output.logfile.node_data{1}.ATTR.data='ux;uy;uz';
febio_spec.Output.logfile.node_data{1}.ATTR.delim=',';
febio_spec.Output.logfile.node_data{1}.VAL=1:size(V,1);

febio_spec.Output.logfile.node_data{2}.ATTR.file=febioLogFileName_force;
febio_spec.Output.logfile.node_data{2}.ATTR.data='Rx;Ry;Rz';
febio_spec.Output.logfile.node_data{2}.ATTR.delim=',';
febio_spec.Output.logfile.node_data{2}.VAL=1:size(V,1);

febio_spec.Output.logfile.element_data{1}.ATTR.file=febioLogFileName_stress;
febio_spec.Output.logfile.element_data{1}.ATTR.data='sz';
febio_spec.Output.logfile.element_data{1}.ATTR.delim=',';
febio_spec.Output.logfile.element_data{1}.VAL=1:size(E,1);

Quick viewing of the FEBio input file structure

The febView function can be used to view the xml structure in a MATLAB figure window.

febView(febio_spec); %Viewing the febio file

Exporting the FEBio input file

Exporting the febio_spec structure to an FEBio input file is done using the febioStruct2xml function.

febioStruct2xml(febio_spec,febioFebFileName); %Exporting to file and domNode

Running the FEBio analysis

To run the analysis defined by the created FEBio input file the runMonitorFEBio function is used. The input for this function is a structure defining job settings e.g. the FEBio input file name. The optional output runFlag informs the user if the analysis was run succesfully.

febioAnalysis.run_filename=febioFebFileName; %The input file name
febioAnalysis.run_logname=febioLogFileName; %The name for the log file
febioAnalysis.disp_on=1; %Display information on the command window
febioAnalysis.disp_log_on=1; %Display convergence information in the command window
febioAnalysis.runMode='external';%'internal';
febioAnalysis.t_check=0.25; %Time for checking log file (dont set too small)
febioAnalysis.maxtpi=1e99; %Max analysis time
febioAnalysis.maxLogCheckTime=3; %Max log file checking time

[runFlag]=runMonitorFEBio(febioAnalysis);%START FEBio NOW!!!!!!!!
 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- STARTING FEBIO JOB --- 04-Jun-2019 12:48:45
Waiting for log file...
Proceeding to check log file...04-Jun-2019 12:48:47
------- converged at time : 0.1
------- converged at time : 0.2
------- converged at time : 0.3
------- converged at time : 0.4
------- converged at time : 0.5
------- converged at time : 0.6
------- converged at time : 0.7
------- converged at time : 0.8
------- converged at time : 0.9
------- converged at time : 1
------- converged at time : 1.1
------- converged at time : 1.2
------- converged at time : 1.3
------- converged at time : 1.4
------- converged at time : 1.5
------- converged at time : 1.6
------- converged at time : 1.7
------- converged at time : 1.8
------- converged at time : 1.9
------- converged at time : 2
------- converged at time : 2.1
------- converged at time : 2.2
------- converged at time : 2.3
------- converged at time : 2.4
------- converged at time : 2.5
------- converged at time : 2.6
------- converged at time : 2.7
------- converged at time : 2.8
------- converged at time : 2.9
------- converged at time : 3
------- converged at time : 3.1
------- converged at time : 3.2
------- converged at time : 3.3
------- converged at time : 3.4
------- converged at time : 3.5
------- converged at time : 3.6
------- converged at time : 3.7
------- converged at time : 3.8
------- converged at time : 3.9
------- converged at time : 4
--- Done --- 04-Jun-2019 12:48:47

Import FEBio results

if runFlag==1 %i.e. a succesful run
    % Importing nodal displacements from a log file
    [~, N_disp_mat,~]=importFEBio_logfile(fullfile(savePath,febioLogFileName_disp)); %Nodal displacements

    N_disp_mat=N_disp_mat(:,2:end,:);
    sizImport=size(N_disp_mat);
    sizImport(3)=sizImport(3)+1;
    N_disp_mat_n=zeros(sizImport);
    N_disp_mat_n(:,:,2:end)=N_disp_mat;
    N_disp_mat=N_disp_mat_n;
    DN=N_disp_mat(:,:,end);
    DN_magnitude=sqrt(sum(DN(:,3).^2,2));
    V_def=V+DN;
    [CF]=vertexToFaceMeasure(Fb,DN_magnitude);

    % Importing element stress from a log file
    [time_mat, E_stress_mat,~]=importFEBio_logfile(fullfile(savePath,febioLogFileName_stress)); %Nodal forces
    time_mat=[0; time_mat(:)]; %Time
    stress_cauchy_sim=[0; mean(squeeze(E_stress_mat(:,end,:)),1)'];

Plotting the simulated results using anim8 to visualize and animate deformations

    % Create basic view and store graphics handle to initiate animation
    hf=cFigure; %Open figure
    gtitle([febioFebFileNamePart,': Press play to animate']);
    hp=gpatch(Fb,V_def,CF,'k',1); %Add graphics object to animate
    gpatch(Fb,V,0.5*ones(1,3),'k',0.25); %A static graphics object

    axisGeom(gca,fontSize);
    colormap(gjet(250)); colorbar;
    caxis([0 max(DN_magnitude)]);
    axis([min(V_def(:,1)) max(V_def(:,1)) min(V_def(:,2)) max(V_def(:,2)) min(V_def(:,3)) max(V_def(:,3))]); %Set axis limits statically
    view(130,25); %Set view direction
    camlight headlight;

    % Set up animation features
    animStruct.Time=time_mat; %The time vector
    for qt=1:1:size(N_disp_mat,3) %Loop over time increments
        DN=N_disp_mat(:,:,qt); %Current displacement
        DN_magnitude=sqrt(sum(DN.^2,2)); %Current displacement magnitude
        V_def=V+DN; %Current nodal coordinates
        [CF]=vertexToFaceMeasure(Fb,DN_magnitude); %Current color data to use

        %Set entries in animation structure
        animStruct.Handles{qt}=[hp hp]; %Handles of objects to animate
        animStruct.Props{qt}={'Vertices','CData'}; %Properties of objects to animate
        animStruct.Set{qt}={V_def,CF}; %Property values for to set in order to animate
    end
    anim8(hf,animStruct); %Initiate animation feature
    drawnow;

Calculate the simulated applied uniaxial stretch

    displacement_Z=N_disp_mat(bcPrescribeList,end,:); %Z displacements of the prescribed set
    displacement_Z=mean(displacement_Z,1); %Calculate mean Z displacements across nodes
    stretch_sim=(displacement_Z(:)+sampleHeight)./sampleHeight; %Derive stretch

Visualize stress-stretch curve

    cFigure;
    hold on;
    title('Cauchy stress-displacement curve','FontSize',fontSize);
    xlabel('Displacement [mm]','FontSize',fontSize); ylabel('\sigma Cauchy stress [kPa]','FontSize',fontSize);

    plot(displacement_Z(:),stress_cauchy_sim(:),'r-','lineWidth',lineWidth);

    view(2); axis tight;  grid on; axis square; box on;
    set(gca,'FontSize',fontSize);
    drawnow;


    cFigure;
    hold on;
    title('Cauchy stress-time curve','FontSize',fontSize);
    xlabel('time [s]','FontSize',fontSize); ylabel('\sigma Cauchy stress [kPa]','FontSize',fontSize);

    plot(time_mat(:),stress_cauchy_sim(:),'r-','lineWidth',lineWidth);

    view(2); axis tight;  grid on; axis square; box on;
    set(gca,'FontSize',fontSize);
    drawnow;
end

GIBBON www.gibboncode.org

Kevin Mattheus Moerman, [email protected]

GIBBON footer text

License: https://github.com/gibbonCode/GIBBON/blob/master/LICENSE

GIBBON: The Geometry and Image-based Bioengineering add-On. A toolbox for image segmentation, image-based modeling, meshing, and finite element analysis.

Copyright (C) 2019 Kevin Mattheus Moerman

This program is free software: you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation, either version 3 of the License, or (at your option) any later version.

This program is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details.

You should have received a copy of the GNU General Public License along with this program. If not, see http://www.gnu.org/licenses/.