DEMO_febio_0010_trabeculae_compression

Below is a demonstration for:

Contents

Keywords:

clear; close all; clc;

Plot settings

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

porousGeometryCase='g';
ns=12; %Number of voxel steps across period for image data (roughly number of points on mesh period)
nPeriods=[2 2 2]; %Number of periods in each direction
sampleSize=10; %Heigh of the sample

%Define applied displacement
appliedStrain=0.2; %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*sampleSize)-sampleSize; %The displacement magnitude

%Material parameter set
c1=1e-3; %Solid shear-modulus-like parameter
m1=2; %Solid material parameter setting degree of non-linearity
k=c1; %Solid bulk modulus

% 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

DEFINING GEOMETRY

The trabecular structure is here simulated using isosurfaces on triply periodic minimal surfaces functions.

switch porousGeometryCase
    case 'g' %Gyroid
        n=nPeriods*ns; %Number of sample points
        isoLevel=0.; %Iso-surface level

        cutOffset=1/3*pi; %Cut level such that data "ends well"

        %Define coordinate limits
        xMin=0*pi;
        xMax=(xMin+2*pi*nPeriods(1))-cutOffset;
        yMin=0*pi;
        yMax=(yMin+2*pi*nPeriods(2))-cutOffset;
        zMin=0*pi;
        zMax=(zMin+2*pi*nPeriods(3))-cutOffset;
    case 'p' %Schwarz P
        n=nPeriods*ns; %Number of sample points
        isoLevel=0.; %Iso-surface level

        %Define coordinate limits
        xMin=0*pi;
        xMax=xMin+2*pi*nPeriods(1);
        yMin=0*pi;
        yMax=yMin+2*pi*nPeriods(2);
        zMin=0*pi;
        zMax=zMin+2*pi*nPeriods(3);
    case 'd' %Schwarz D
        n=nPeriods*ns; %Number of sample points
        isoLevel=0.; %Iso-surface level

        %Define coordinate limits
        xMin=0*pi;
        xMax=xMin+2*pi*nPeriods(1);
        yMin=0*pi;
        yMax=yMin+2*pi*nPeriods(2);
        zMin=0*pi;
        zMax=zMin+2*pi*nPeriods(3);
end

%Create coordinates
xRange=linspace(xMin,xMax,n(1));
yRange=linspace(yMin,yMax,n(2));
zRange=linspace(zMin,zMax,n(3));
[X,Y,Z]=meshgrid(xRange,yRange,zRange);
V=[X(:) Y(:) Z(:)];

%Calculate 3D image data
S=triplyPeriodicMinimal(V(:,1),V(:,2),V(:,3),porousGeometryCase);
S=reshape(S,size(X));

%Scaling coordinates
X=((X./abs(xMax-xMin)).*sampleSize)-sampleSize/2;
Y=((Y./abs(yMax-yMin)).*sampleSize)-sampleSize/2;
Z=((Z./abs(zMax-zMin)).*sampleSize)-sampleSize/2;

%Compute isosurface
[Fi,Vi] = isosurface(X,Y,Z,S,isoLevel); %main isosurface
Fi=fliplr(Fi); %Flip so normal faces outward

%Merge nodes
[Fi,Vi]=mergeVertices(Fi,Vi);
logicInvalid=any(diff(sort(Fi,2),[],2)==0,2);
Fi=Fi(~logicInvalid,:);

%Compute caps (to create closed surface)
[Fc,Vc] = isocaps(X,Y,Z,S,isoLevel); %Caps to close the shape
Fc=fliplr(Fc); %Flip so normal faces outward

%Merge nodes
[Fc,Vc]=mergeVertices(Fc,Vc);
logicInvalid=any(diff(sort(Fc,2),[],2)==0,2);
Fc=Fc(~logicInvalid,:);

%Join model segments (isosurface and caps)
V=[Vi;Vc];
F=[Fi;Fc+size(Vi,1)];

%Find top and bottom face sets
[Nc]=patchNormal(Fc,Vc);
logicTop_Fc=Nc(:,3)>0.5;
logicTop=[false(size(Fi,1),1);logicTop_Fc];

[Nc]=patchNormal(Fc,Vc);
logicBottom_Fc=Nc(:,3)<-0.5;
logicBottom=[false(size(Fi,1),1);logicBottom_Fc];

%Merge nodes
[F,V]=mergeVertices(F,V);

%Create faceboundary label
C=zeros(size(F,1),1);
C(logicTop)=1;
C(logicBottom)=2;

%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('Triply-periodic minimal surface derived model of trabecular structure','FontSize',fontSize);
gpatch(F,V,C,'k',1);

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

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 --- 04-Jun-2019 12:45:42
 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- Writing SMESH file --- 04-Jun-2019 12:45:42
----> Adding node field
----> Adding facet field
----> Adding holes specification
----> Adding region specification
--- Done --- 04-Jun-2019 12:45:42
--- Running TetGen to mesh input boundary--- 04-Jun-2019 12:45:42
Opening /mnt/data/MATLAB/GIBBON/data/temp/temp.smesh.
Delaunizing vertices...
Delaunay seconds:  0.050275
Creating surface mesh ...
Surface mesh seconds:  0.012693
Recovering boundaries...
Boundary recovery seconds:  0.036602
Removing exterior tetrahedra ...
Spreading region attributes.
Exterior tets removal seconds:  0.016278
Recovering Delaunayness...
Delaunay recovery seconds:  0.015396
Refining mesh...
Refinement seconds:  0.186243
Optimizing mesh...
Optimization seconds:  0.01364

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:  0.13563
Total running seconds:  0.467165

Statistics:

  Input points: 6733
  Input facets: 13546
  Input segments: 20319
  Input holes: 0
  Input regions: 1

  Mesh points: 13530
  Mesh tetrahedra: 64186
  Mesh faces: 135145
  Mesh faces on exterior boundary: 13546
  Mesh faces on input facets: 13546
  Mesh edges on input segments: 20319
  Steiner points inside domain: 6797

--- Done --- 04-Jun-2019 12:45:43
 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- Importing TetGen files --- 04-Jun-2019 12:45:43
--- Done --- 04-Jun-2019 12:45:43

Visualizing mesh using meshView, see also anim8

meshView(meshOutput);

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==2; %Logic for current face set
Fr=Fb(logicFace,:); %The current face set
bcSupportList=unique(Fr(:)); %Node set part of selected face

%Prescribed displacement nodes
logicPrescribe=Cb==1; %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','none',0.5);

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='2.5';

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

%Control section
febio_spec.Control.analysis.ATTR.type='static';
febio_spec.Control.title='Cube analysis';
febio_spec.Control.time_steps=numTimeSteps;
febio_spec.Control.step_size=1/numTimeSteps;
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;
febio_spec.Control.max_refs=max_refs;
febio_spec.Control.max_ups=max_ups;

% Material section
febio_spec.Material.material{1}.ATTR.type='Ogden unconstrained';
febio_spec.Material.material{1}.ATTR.id=1;
febio_spec.Material.material{1}.c1=c1;
febio_spec.Material.material{1}.m1=m1;
febio_spec.Material.material{1}.c2=c1;
febio_spec.Material.material{1}.m2=-m1;
febio_spec.Material.material{1}.cp=k;

%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='tet4'; %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='Bone sample'; %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';
febio_spec.Geometry.NodeSet{1}.node.ATTR.id=bcSupportList(:);

febio_spec.Geometry.NodeSet{2}.ATTR.name='bcPrescribeList';
febio_spec.Geometry.NodeSet{2}.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{1}.ATTR.name;
febio_spec.Boundary.fix{3}.ATTR.bc='z';
febio_spec.Boundary.fix{3}.ATTR.node_set=febio_spec.Geometry.NodeSet{1}.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{2}.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;

febio_spec.Boundary.prescribe{2}.ATTR.bc='x';
febio_spec.Boundary.prescribe{2}.ATTR.node_set=febio_spec.Geometry.NodeSet{2}.ATTR.name;
febio_spec.Boundary.prescribe{2}.scale.ATTR.lc=1;
febio_spec.Boundary.prescribe{2}.scale.VAL=1;
febio_spec.Boundary.prescribe{2}.relative=1;
febio_spec.Boundary.prescribe{2}.value=0;

febio_spec.Boundary.prescribe{3}.ATTR.bc='y';
febio_spec.Boundary.prescribe{3}.ATTR.node_set=febio_spec.Geometry.NodeSet{2}.ATTR.name;
febio_spec.Boundary.prescribe{3}.scale.ATTR.lc=1;
febio_spec.Boundary.prescribe{3}.scale.VAL=1;
febio_spec.Boundary.prescribe{3}.relative=1;
febio_spec.Boundary.prescribe{3}.value=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);

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 12:45:48
Waiting for log file...
Proceeding to check log file...04-Jun-2019 12:45:49
------- 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
--- Done --- 04-Jun-2019 12:46:07

Import FEBio results

if runFlag==1 %i.e. a succesful run
    % Importing nodal displacements from a log file
    [time_mat, N_disp_mat,~]=importFEBio_logfile(fullfile(savePath,febioLogFileName_disp)); %Nodal displacements
    time_mat=[0; time_mat(:)]; %Time

    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;

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,DN_magnitude,'k',1,1); %Add graphics object to animate

    gpatch(Fb,V,0.5*ones(1,3),'none',0.1); %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;
    drawnow;

    % 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(:,3).^2,2)); %Current displacement magnitude
        V_def=V+DN; %Current nodal coordinates

        %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,DN_magnitude}; %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.

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/.