DEMO_febio_0010_trabeculae_compression

Below is a demonstration for:

Building geometry for trabecular structure with tetrahedral elements
Defining the boundary conditions
Coding the febio structure
Running the model
Importing and visualizing the displacement and stress results

Keywords:
Plot settings
Control parameters
DEFINING GEOMETRY
Using grouping to keep only largest group
Remesh using geomgram
Tetrahedral meshing using tetgen (see also runTetGen)
Tetrahedral meshing using tetgen (see also runTetGen)
Visualizing mesh using meshView, see also anim8
Defining node labels
Define boundary conditions
Defining the FEBio input structure
Quick viewing of the FEBio input file structure
Exporting the FEBio input file
Running the FEBio analysis
Import FEBio results

Keywords:

febio_spec version 4.0
febio, FEBio
compression, tension, compressive, tensile
displacement control, displacement boundary condition
trabecular
tetgen, meshing
tetrahedral elements, tet4
static, solid
hyperelastic, Ogden
displacement logfile
Stress logfile

clear; close all; clc;

Plot settings

fontSize=20;
faceAlpha1=0.8;
markerSize=40;
lineWidth1=3;
lineWidth2=4;
markerSize1=25;

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=[febioFebFileNamePart,'.txt']; %FEBio log file name
febioLogFileName_disp=[febioFebFileNamePart,'_disp_out.txt']; %Log file name for exporting displacement
febioLogFileName_stress_prin=[febioFebFileNamePart,'_stress_prin_out.txt']; %Log file name for exporting stress
febioLogFileName_stress_full=[febioFebFileNamePart,'_stress_full_out.txt']; %Log file name for exporting stress

porousGeometryCase=1;

sampleSize=10; %Heigh of the sample
pointSpacing=sampleSize/25;
tolDir=pointSpacing/5; %Tolerance for detecting sides after remeshing

overSampleRatio=2;
numStepsLevelset=ceil(overSampleRatio.*(sampleSize./pointSpacing)); %Number of voxel steps across period for image data (roughly number of points on mesh period)

%Define applied displacement
appliedStrain=0.05; %Linear strain (Only used to compute applied stretch)

loadingOption='compression'; % or 'tension' or 'shear'
switch loadingOption
    case 'compression'
        stretchLoad=1-appliedStrain; %The applied stretch for uniaxial loading
        displacementMagnitude=(stretchLoad*sampleSize)-sampleSize; %The displacement magnitude
    case 'tension'
        stretchLoad=1+appliedStrain; %The applied stretch for uniaxial loading
        displacementMagnitude=(stretchLoad*sampleSize)-sampleSize; %The displacement magnitude
    case 'shear'
        stretchLoad=1+appliedStrain; %The applied stretch for uniaxial loading
        displacementMagnitude=(stretchLoad*sampleSize)-sampleSize; %The displacement magnitude
end

%Material parameter set
E_youngs=5; %Youngs modulus
nu=0.3; %Poisson's ratio
% mu=E_youngs/3;

%FEA control settings
numTimeSteps=10; %Number of time steps desired
max_refs=15; %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
dtmin=(1/numTimeSteps)/100; %Minimum time step size
dtmax=1/numTimeSteps; %Maximum time step size

runMode='external';% 'internal' or 'external'

DEFINING GEOMETRY

The trabecular structure is here simulated using

switch porousGeometryCase
    case 1 %Gyroid
        inputStruct.L=sampleSize; % characteristic length
        inputStruct.Ns=numStepsLevelset; % number of sampling points
        inputStruct.isocap=1; %Option to cap the isosurface
        inputStruct.surfaceCase='g'; %Surface type
        inputStruct.numPeriods=[2 2 2]; %Number of periods in each direction
        inputStruct.levelset=0.3; %Isosurface level

        [F,V,C,S]=triplyPeriodicMinimalSurface(inputStruct);
    case 2 %Stochastic structure
        inputStruct.L=1; % characteristic length
        inputStruct.Ns=numStepsLevelset; % number of sampling points
        inputStruct.Nw=60; % number of waves
        inputStruct.q0=25; % wave number
        inputStruct.relD=0.3; % relative density
        inputStruct.anisotropyFactors=[1 1 1]; %Anisotropy factors
        inputStruct.isocap=1; %Option to cap the isosurface

        [F,V,C,S]=stochasticMicrostructure(inputStruct);
        V=V.*sampleSize;
    case 3 %spinodoid
        inputStruct.isocap=true; % option to cap the isosurface
        inputStruct.domainSize=1; % domain size
        inputStruct.resolution=numStepsLevelset; % resolution for sampling GRF
        inputStruct.waveNumber=8*pi; % GRF wave number
        inputStruct.numWaves=500; % number of waves in GRF
        inputStruct.relativeDensity=0.5; % relative density: between [0.3,1]
        inputStruct.thetas=[90 0 0]; % conical half angles (in degrees) along xyz

        [F,V,C,S]=spinodoid(inputStruct);
        V=V.*sampleSize;
end

Using grouping to keep only largest group

groupOptStruct.outputType='label';
[G,~,groupSize]=tesgroup(F,groupOptStruct); %Group connected faces
[~,indKeep]=max(groupSize); %Index of largest group

%Keep only largest group
F=F(G==indKeep,:); %Trim faces
C=C(G==indKeep,:); %Trim color data
[F,V]=patchCleanUnused(F,V); %Remove unused nodes

% %% Remove non-manifold faces
% D=patchConnectivity(F,V,'ff');
% logicManifold=sum(D.face.face>0,2)==3;
% F=F(logicManifold,:);
% C=C(logicManifold,:);
% [F,V]=patchCleanUnused(F,V);

% %% Smoothen mesh
%
% %Smoothen surface mesh (isosurface does not yield high quality mesh)
% indKeep=F(C~=0,:);%F(size(Fi,1)+1:end,:);
% indKeep=unique(indKeep(:));
% cPar.n=75;
% cPar.RigidConstraints=indKeep; %Boundary nodes are held on to
% cPar.Method='HC';
% [V]=patchSmooth(F,V,[],cPar);

Visualizing geometry

cFigure; hold on;
title('Raw iso-surface based','FontSize',fontSize);
gpatch(F,V,C,'k',1);

% plotV(V(indKeep,:),'k.','MarkerSize',markerSize1);
axisGeom(gca,fontSize);
colormap gjet; icolorbar;
camlight headlight;
drawnow;

Remesh using geomgram

optionStruct.pointSpacing=pointSpacing;
% optionStruct.max_dist=0;
[F,V]=ggremesh(F,V,optionStruct);
C=zeros(size(F,1),1);

Visualizing geometry

cFigure; hold on;
title('Geogram remeshed','FontSize',fontSize);

gpatch(F,V,'w','k',1);

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

Tetrahedral meshing using tetgen (see also `runTetGen`)

% Create tetgen input structure
inputStruct.stringOpt='-pq1.2AaY';
inputStruct.Faces=F;

Tetrahedral meshing using tetgen (see also `runTetGen`)

% Create tetgen input structure
inputStruct.stringOpt='-pq1.2AaY';
inputStruct.Faces=F;
inputStruct.Nodes=V;
inputStruct.holePoints=[];
inputStruct.faceBoundaryMarker=C; %Face boundary markers
inputStruct.regionPoints=getInnerPoint(F,V); %region points
inputStruct.regionA=2*tetVolMeanEst(F,V);
inputStruct.minRegionMarker=2; %Minimum region marker

% Mesh model using tetrahedral elements using tetGen
[meshOutput]=runTetGen(inputStruct); %Run tetGen

% Access model element and patch data
Fb=meshOutput.facesBoundary;
Cb=meshOutput.boundaryMarker;
V=meshOutput.nodes;
CE=meshOutput.elementMaterialID;
E=meshOutput.elements;

 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- TETGEN Tetrahedral meshing --- 20-Apr-2023 10:39:56
 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- Writing SMESH file --- 20-Apr-2023 10:39:56
----> Adding node field
----> Adding facet field
----> Adding holes specification
----> Adding region specification
--- Done --- 20-Apr-2023 10:39:57
--- Running TetGen to mesh input boundary--- 20-Apr-2023 10:39:57
Opening /mnt/data/MATLAB/GIBBON/data/temp/temp.smesh.
Delaunizing vertices...
Delaunay seconds:  0.032603
Creating surface mesh ...
Surface mesh seconds:  0.01017
Recovering boundaries...
Boundary recovery seconds:  0.026791
Removing exterior tetrahedra ...
Spreading region attributes.
Exterior tets removal seconds:  0.015084
Recovering Delaunayness...
Delaunay recovery seconds:  0.011288
Refining mesh...
Refinement seconds:  0.150805
Smoothing vertices...
Mesh smoothing seconds:  0.276673
Improving mesh...
Mesh improvement seconds:  0.012198

Writing /mnt/data/MATLAB/GIBBON/data/temp/temp.1.node.
Writing /mnt/data/MATLAB/GIBBON/data/temp/temp.1.ele.
Writing /mnt/data/MATLAB/GIBBON/data/temp/temp.1.face.
Writing /mnt/data/MATLAB/GIBBON/data/temp/temp.1.edge.

Output seconds:  0.098723
Total running seconds:  0.634884

Statistics:

  Input points: 6159
  Input facets: 12422
  Input segments: 18633
  Input holes: 0
  Input regions: 1

  Mesh points: 11238
  Mesh tetrahedra: 48639
  Mesh faces: 103489
  Mesh faces on exterior boundary: 12422
  Mesh faces on input facets: 12422
  Mesh edges on input segments: 18633
  Steiner points inside domain: 5079

--- Done --- 20-Apr-2023 10:39:58
 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- Importing TetGen files --- 20-Apr-2023 10:39:58
--- Done --- 20-Apr-2023 10:39:58

Visualizing mesh using `meshView`, see also `anim8`

meshView(meshOutput);

Defining node labels

C_vertex=zeros(size(V,1),1);
for q=1:3
    logic1=V(:,q)>(sampleSize-tolDir);
    logic2=V(:,q)<tolDir;
    C_vertex(logic1)=max(C_vertex(:))+1;
    C_vertex(logic2)=max(C_vertex(:))+1;
end

Visualizing vertex/node labels

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

gpatch(Fb,V,'w','none',1);

scatterV(V,50,C_vertex,'filled');

axisGeom(gca,fontSize);
colormap gjet; icolorbar;
camlight headlight;
drawnow;

Define boundary conditions

bcSupportList=find(C_vertex==6);
bcPrescribeList=find(C_vertex==5);

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,'w','k',1);

hl(1)=plotV(V(bcSupportList,:),'r.','MarkerSize',markerSize);
hl(2)=plotV(V(bcPrescribeList,:),'k.','MarkerSize',markerSize);

legend(hl,{'BC full 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='4.0';

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

%Control section
febio_spec.Control.analysis='STATIC';
febio_spec.Control.time_steps=numTimeSteps;
febio_spec.Control.step_size=1/numTimeSteps;
febio_spec.Control.solver.max_refs=max_refs;
febio_spec.Control.time_stepper.dtmin=dtmin;
febio_spec.Control.time_stepper.dtmax=dtmax;
febio_spec.Control.time_stepper.max_retries=max_retries;
febio_spec.Control.time_stepper.opt_iter=opt_iter;

%Material section
materialName1='Material1';
febio_spec.Material.material{1}.ATTR.name=materialName1;
febio_spec.Material.material{1}.ATTR.type='neo-Hookean';
febio_spec.Material.material{1}.ATTR.id=1;
febio_spec.Material.material{1}.E=E_youngs;
febio_spec.Material.material{1}.v=nu;

% Mesh section
% -> Nodes
febio_spec.Mesh.Nodes{1}.ATTR.name='Object1'; %The node set name
febio_spec.Mesh.Nodes{1}.node.ATTR.id=(1:size(V,1))'; %The node id's
febio_spec.Mesh.Nodes{1}.node.VAL=V; %The nodel coordinates

% -> Elements
partName1='Part1';
febio_spec.Mesh.Elements{1}.ATTR.name=partName1; %Name of this part
febio_spec.Mesh.Elements{1}.ATTR.type='tet4'; %Element type
febio_spec.Mesh.Elements{1}.elem.ATTR.id=(1:1:size(E,1))'; %Element id's
febio_spec.Mesh.Elements{1}.elem.VAL=E; %The element matrix

% -> NodeSets
nodeSetName1='bcSupportList';
nodeSetName2='bcPrescribeList';

febio_spec.Mesh.NodeSet{1}.ATTR.name=nodeSetName1;
febio_spec.Mesh.NodeSet{1}.VAL=mrow(bcSupportList);

febio_spec.Mesh.NodeSet{2}.ATTR.name=nodeSetName2;
febio_spec.Mesh.NodeSet{2}.VAL=mrow(bcPrescribeList);

%MeshDomains section
febio_spec.MeshDomains.SolidDomain.ATTR.name=partName1;
febio_spec.MeshDomains.SolidDomain.ATTR.mat=materialName1;

%Boundary condition section
% -> Fix boundary conditions
switch loadingOption
    case 'shear'
        febio_spec.Boundary.bc{1}.ATTR.name='FixedDisplacement01';
        febio_spec.Boundary.bc{1}.ATTR.type='zero displacement';
        febio_spec.Boundary.bc{1}.ATTR.node_set=nodeSetName1;
        febio_spec.Boundary.bc{1}.x_dof=1;
        febio_spec.Boundary.bc{1}.y_dof=1;
        febio_spec.Boundary.bc{1}.z_dof=1;

        febio_spec.Boundary.bc{2}.ATTR.name='FixedDisplacement02';
        febio_spec.Boundary.bc{2}.ATTR.type='zero displacement';
        febio_spec.Boundary.bc{2}.ATTR.node_set=nodeSetName2;
        febio_spec.Boundary.bc{2}.x_dof=0;
        febio_spec.Boundary.bc{2}.y_dof=1;
        febio_spec.Boundary.bc{2}.z_dof=1;

        febio_spec.Boundary.bc{3}.ATTR.name='bcPrescribeList';
        febio_spec.Boundary.bc{3}.ATTR.type='prescribed displacement';
        febio_spec.Boundary.bc{3}.ATTR.node_set=nodeSetName2;
        febio_spec.Boundary.bc{3}.dof='x';
        febio_spec.Boundary.bc{3}.value.ATTR.lc=1;
        febio_spec.Boundary.bc{3}.value.VAL=displacementMagnitude;
        febio_spec.Boundary.bc{3}.relative=0;
    case 'compression'
        febio_spec.Boundary.bc{1}.ATTR.name='FixedDisplacement01';
        febio_spec.Boundary.bc{1}.ATTR.type='zero displacement';
        febio_spec.Boundary.bc{1}.ATTR.node_set=nodeSetName1;
        febio_spec.Boundary.bc{1}.x_dof=1;
        febio_spec.Boundary.bc{1}.y_dof=1;
        febio_spec.Boundary.bc{1}.z_dof=1;

        febio_spec.Boundary.bc{2}.ATTR.name='FixedDisplacement02';
        febio_spec.Boundary.bc{2}.ATTR.type='zero displacement';
        febio_spec.Boundary.bc{2}.ATTR.node_set=nodeSetName2;
        febio_spec.Boundary.bc{2}.x_dof=1;
        febio_spec.Boundary.bc{2}.y_dof=1;
        febio_spec.Boundary.bc{2}.z_dof=0;

        febio_spec.Boundary.bc{3}.ATTR.name='bcPrescribeList';
        febio_spec.Boundary.bc{3}.ATTR.type='prescribed displacement';
        febio_spec.Boundary.bc{3}.ATTR.node_set=nodeSetName2;
        febio_spec.Boundary.bc{3}.dof='z';
        febio_spec.Boundary.bc{3}.value.ATTR.lc=1;
        febio_spec.Boundary.bc{3}.value.VAL=displacementMagnitude;
        febio_spec.Boundary.bc{3}.relative=0;
    otherwise
        error('Invalid loadingOption provided');
end

%LoadData section
% -> load_controller
febio_spec.LoadData.load_controller{1}.ATTR.name='LC1';
febio_spec.LoadData.load_controller{1}.ATTR.id=1;
febio_spec.LoadData.load_controller{1}.ATTR.type='loadcurve';
febio_spec.LoadData.load_controller{1}.interpolate='LINEAR';
febio_spec.LoadData.load_controller{1}.extend='CONSTANT';
febio_spec.LoadData.load_controller{1}.points.pt.VAL=[0 0; 1 1];

%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.element_data{1}.ATTR.file=febioLogFileName_stress_prin;
febio_spec.Output.logfile.element_data{1}.ATTR.data='s1;s2;s3';
febio_spec.Output.logfile.element_data{1}.ATTR.delim=',';

febio_spec.Output.logfile.element_data{2}.ATTR.file=febioLogFileName_stress_full;
febio_spec.Output.logfile.element_data{2}.ATTR.data='sx;sy;sz;sxy;syz;sxz';
febio_spec.Output.logfile.element_data{2}.ATTR.delim=',';

febio_spec.Output.plotfile.compression=0;

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.runMode=runMode;

[runFlag]=runMonitorFEBio(febioAnalysis);%START FEBio NOW!!!!!!!!

 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
-------->    RUNNING/MONITORING FEBIO JOB    <-------- 20-Apr-2023 10:40:05
FEBio path: /home/kevin/FEBioStudio2/bin/febio4
# Attempt removal of existing log files                20-Apr-2023 10:40:05
 * Removal succesful                                   20-Apr-2023 10:40:05
# Attempt removal of existing .xplt files              20-Apr-2023 10:40:05
 * Removal succesful                                   20-Apr-2023 10:40:05
# Starting FEBio...                                    20-Apr-2023 10:40:05
  Max. total analysis time is: Inf s
 * Waiting for log file creation                       20-Apr-2023 10:40:05
   Max. wait time: 30 s
 * Log file found.                                     20-Apr-2023 10:40:06
# Parsing log file...                                  20-Apr-2023 10:40:06
    number of iterations   : 2                         20-Apr-2023 10:40:07
    number of reformations : 2                         20-Apr-2023 10:40:07
------- converged at time : 0.1                        20-Apr-2023 10:40:07
    number of iterations   : 2                         20-Apr-2023 10:40:08
------- converged at time : 0.2                        20-Apr-2023 10:40:09
    number of iterations   : 2                         20-Apr-2023 10:40:10
    number of reformations : 2                         20-Apr-2023 10:40:10
------- converged at time : 0.3                        20-Apr-2023 10:40:10
    number of iterations   : 2                         20-Apr-2023 10:40:12
    number of reformations : 2                         20-Apr-2023 10:40:12
    number of iterations   : 3                         20-Apr-2023 10:40:14
    number of reformations : 3                         20-Apr-2023 10:40:14
------- converged at time : 0.5                        20-Apr-2023 10:40:14
    number of iterations   : 3                         20-Apr-2023 10:40:17
    number of reformations : 3                         20-Apr-2023 10:40:17
------- converged at time : 0.6                        20-Apr-2023 10:40:17
    number of iterations   : 3                         20-Apr-2023 10:40:19
    number of reformations : 3                         20-Apr-2023 10:40:19
------- converged at time : 0.7                        20-Apr-2023 10:40:19
    number of iterations   : 3                         20-Apr-2023 10:40:21
    number of reformations : 3                         20-Apr-2023 10:40:21
------- converged at time : 0.8                        20-Apr-2023 10:40:21
    number of iterations   : 3                         20-Apr-2023 10:40:23
    number of reformations : 3                         20-Apr-2023 10:40:23
------- converged at time : 0.9                        20-Apr-2023 10:40:23
    number of iterations   : 3                         20-Apr-2023 10:40:26
    number of reformations : 3                         20-Apr-2023 10:40:26
------- converged at time : 1                          20-Apr-2023 10:40:26
 Elapsed time : 0:00:20                                20-Apr-2023 10:40:27
 N O R M A L   T E R M I N A T I O N
# Done                                                 20-Apr-2023 10:40:27
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

Import FEBio results

if runFlag==1 %i.e. a succesful run

Importing nodal displacements from a log file

    dataStruct=importFEBio_logfile(fullfile(savePath,febioLogFileName_disp),0,1);

    %Access data
    N_disp_mat=dataStruct.data; %Displacement
    timeVec=dataStruct.time; %Time

    %Create deformed coordinate set
    V_DEF=N_disp_mat+repmat(V,[1 1 size(N_disp_mat,3)]);

Importing element stress from a log file

    dataStruct=importFEBio_logfile(fullfile(savePath,febioLogFileName_stress_prin),0,1);

    %Access data
    E_stress_mat=dataStruct.data;

    E_stress_mat(isnan(E_stress_mat))=0;

    %Compute Von Mises
    S_vm_ND = sqrt( 0.5*((E_stress_mat(:,1,:)-E_stress_mat(:,2,:)).^2 + (E_stress_mat(:,2,:)-E_stress_mat(:,3,:)).^2 + (E_stress_mat(:,1,:)-E_stress_mat(:,3,:)).^2));

    %Compute volume weighted mean Von Mises stress

    elemVol=tetVol(E,V); %Element volumes
    totalVol=sum(elemVol); %Total volume
    S_vm_mean=squeeze(sum(S_vm_ND.*repmat(elemVol,[1 1 size(S_vm_ND,3)]),1)./totalVol); %Mean Von Mises stress

    appliedDisplacement=dataStruct.time.*displacementMagnitude;

    cFigure; hold on;
    xlabel('u [mm]','FontSize',fontSize,'Interpreter','Latex');
    ylabel('$\sigma_{vm}$ [MPa]','FontSize',fontSize,'Interpreter','Latex');

    plot(appliedDisplacement,S_vm_mean,'b','LineWidth',lineWidth1);

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

Plotting the simulated results using anim8 to visualize and animate deformations

    DN_magnitude=sqrt(sum(N_disp_mat(:,:,end).^2,2)); %Current displacement magnitude

    % Create basic view and store graphics handle to initiate animation
    hf=cFigure; %Open figure
    gtitle([febioFebFileNamePart,': Press play to animate']);
    title('Displacement magnitude [mm]','Interpreter','Latex')
    hp=gpatch(Fb,V_DEF(:,:,end),DN_magnitude,'k',1); %Add graphics object to animate
    hp.FaceColor='interp';

    axisGeom(gca,fontSize);
    colormap(gjet(250)); colorbar;
    caxis([0 max(DN_magnitude)]);
    axis(axisLim(V_DEF)); %Set axis limits statically
    camlight headlight;

    % Set up animation features
    animStruct.Time=timeVec; %The time vector
    for qt=1:1:size(N_disp_mat,3) %Loop over time increments
        DN_magnitude=sqrt(sum(N_disp_mat(:,:,qt).^2,2)); %Current displacement magnitude

        %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(:,:,qt),DN_magnitude}; %Property values for to set in order to animate
    end
    anim8(hf,animStruct); %Initiate animation feature
    drawnow;

Plotting the simulated results using anim8 to visualize and animate deformations

    [CV]=faceToVertexMeasure(E,V,S_vm_ND(:,:,end));

    % Create basic view and store graphics handle to initiate animation
    hf=cFigure; %Open figure
    gtitle([febioFebFileNamePart,': Press play to animate']);
    title('$\sigma_{1}$ [MPa]','Interpreter','Latex')
    hp=gpatch(Fb,V_DEF(:,:,end),CV,'k',1); %Add graphics object to animate

    hp.FaceColor='interp';

    axisGeom(gca,fontSize);
    colormap(gjet(250)); colorbar;
    caxis([min(S_vm_ND(:)) max(S_vm_ND(:))]/4);
    axis(axisLim(V_DEF)); %Set axis limits statically
    camlight headlight;

    % Set up animation features
    animStruct.Time=timeVec; %The time vector
    for qt=1:1:size(N_disp_mat,3) %Loop over time increments

        [CV]=faceToVertexMeasure(E,V,S_vm_ND(:,:,qt));

        %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(:,:,qt),CV}; %Property values for to set in order to animate
    end
    anim8(hf,animStruct); %Initiate animation feature
    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.

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/.

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.

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

DEMO_febio_0010_trabeculae_compression

Contents

Keywords:

Plot settings

Control parameters

DEFINING GEOMETRY

Using grouping to keep only largest group

Remesh using geomgram

Tetrahedral meshing using tetgen (see also runTetGen)

Tetrahedral meshing using tetgen (see also runTetGen)

Visualizing mesh using meshView, see also anim8

Defining node labels

Define boundary conditions

Defining the FEBio input structure

Quick viewing of the FEBio input file structure

Exporting the FEBio input file

Running the FEBio analysis

Import FEBio results

Tetrahedral meshing using tetgen (see also `runTetGen`)

Tetrahedral meshing using tetgen (see also `runTetGen`)

Visualizing mesh using `meshView`, see also `anim8`