DEMO_febio_0013_disc_pressure_varying

Below is a demonstration for:

Building geometry for a thin disc 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
Creating model geometry and mesh
Defining the 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 2.5
febio, FEBio
pressure loading, spatially varying pressure, non-constant pressure
tetrahedral elements, hex4
tetgen
disc
static, solid
hyperelastic, Ogden
displacement logfile
stress logfile

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_stress=[febioFebFileNamePart,'_stress_out.txt']; %Log file name for exporting force

%Load
pressureValueMin=0.1e-3;
pressureValueMax=2.0e-3;
loadType='pressure';%'traction';

%Specifying dimensions and number of elements
pointSpacing=1;
inputStruct.cylRadius=30;
inputStruct.numRadial=round((inputStruct.cylRadius*pi)/pointSpacing);
inputStruct.cylHeight=3;
inputStruct.numHeight=round(inputStruct.cylHeight/pointSpacing);
inputStruct.meshType='tri';
inputStruct.closeOpt=1;

% Derive patch data for a cylinder
[Fs,Vs,Cs]=patchcylinder(inputStruct);

%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

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

Creating model geometry and mesh

The disc is meshed using tetrahedral elements using tetgen

inputStruct.stringOpt='-pq1.2AaY';
inputStruct.Faces=Fs;
inputStruct.Nodes=Vs;
inputStruct.holePoints=[];
inputStruct.faceBoundaryMarker=Cs; %Face boundary markers
inputStruct.regionPoints=getInnerPoint(Fs,Vs); %region points
inputStruct.regionA=tetVolMeanEst(Fs,Vs); %Volume for regular tets
inputStruct.minRegionMarker=2; %Minimum region marker
[meshStruct]=runTetGen(inputStruct); % Mesh model using tetrahedral elements using tetGen

 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- TETGEN Tetrahedral meshing --- 04-Jun-2019 12:46:47
 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- Writing SMESH file --- 04-Jun-2019 12:46:47
----> Adding node field
----> Adding facet field
----> Adding holes specification
----> Adding region specification
--- Done --- 04-Jun-2019 12:46:47
--- Running TetGen to mesh input boundary--- 04-Jun-2019 12:46:47
Opening /mnt/data/MATLAB/GIBBON/data/temp/temp.smesh.
Delaunizing vertices...
Delaunay seconds:  0.044101
Creating surface mesh ...
Surface mesh seconds:  0.004589
Recovering boundaries...
Boundary recovery seconds:  0.006526
Removing exterior tetrahedra ...
Spreading region attributes.
Exterior tets removal seconds:  0.000905
Recovering Delaunayness...
Delaunay recovery seconds:  0.015959
Refining mesh...
Refinement seconds:  0.036821
Optimizing mesh...
Optimization seconds:  0.001999

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:  0.028941
Total running seconds:  0.140045

Statistics:

  Input points: 1836
  Input facets: 3668
  Input segments: 5502
  Input holes: 0
  Input regions: 1

  Mesh points: 2883
  Mesh tetrahedra: 11786
  Mesh faces: 25406
  Mesh faces on exterior boundary: 3668
  Mesh faces on input facets: 3668
  Mesh edges on input segments: 5502
  Steiner points inside domain: 1047

--- Done --- 04-Jun-2019 12:46:47
 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- Importing TetGen files --- 04-Jun-2019 12:46:47
--- Done --- 04-Jun-2019 12:46:47

Access model element and patch data

Fb=meshStruct.facesBoundary;
Cb=meshStruct.boundaryMarker;
V=meshStruct.nodes;
CE=meshStruct.elementMaterialID;
E=meshStruct.elements;

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 disc. 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=unique(Fr(:)); %Node set part of selected face

logicFace=Cb==2; %Logic for current face set
F_pressure=fliplr(Fb(logicFace,:)); %The current face set

%Create spatially varying pressure
X=V(:,1);
C_pressure=mean(X(F_pressure),2); %Initialize as X-coordinate
C_pressure=C_pressure-min(C_pressure(:)); %Subtract minimum so range is 0-..
C_pressure=C_pressure./max(C_pressure(:)); %Devide by maximum so range is 0-1
C_pressure=C_pressure.^2;
C_pressure=C_pressure.*(pressureValueMax-pressureValueMin)+pressureValueMin; %Scale/offset to pressure range

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,:),'k.','MarkerSize',markerSize);
hl(2)=gpatch(F_pressure,V,C_pressure,'k',1);
patchNormPlot(F_pressure,V);
legend(hl,{'BC full support','Pressure surface'});
colormap(gjet(250)); colorbar;
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='Disc 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';
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}.k=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='Disc'; %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(:);

% -> Surfaces
febio_spec.Geometry.Surface{1}.ATTR.name='Pressure_surface';
febio_spec.Geometry.Surface{1}.tri3.ATTR.lid=(1:size(F_pressure,1))';
febio_spec.Geometry.Surface{1}.tri3.VAL=F_pressure;

%MeshData
switch loadType
    case 'pressure'
        febio_spec.MeshData.SurfaceData{1}.ATTR.name='pressure_values';
        febio_spec.MeshData.SurfaceData{1}.ATTR.data_type='scalar';
        febio_spec.MeshData.SurfaceData{1}.ATTR.surface=febio_spec.Geometry.Surface{1}.ATTR.name;
        febio_spec.MeshData.SurfaceData{1}.face.VAL=C_pressure;
        febio_spec.MeshData.SurfaceData{1}.face.ATTR.lid=(1:1:numel(C_pressure))';
    case 'traction'
        febio_spec.MeshData.SurfaceData{1}.ATTR.name='traction_value';
        febio_spec.MeshData.SurfaceData{1}.ATTR.data_type='vec3';
        febio_spec.MeshData.SurfaceData{1}.ATTR.surface=febio_spec.Geometry.Surface{1}.ATTR.name;
        febio_spec.MeshData.SurfaceData{1}.face.VAL=[zeros(size(C_pressure)) zeros(size(C_pressure)) -C_pressure];
        febio_spec.MeshData.SurfaceData{1}.face.ATTR.lid=(1:1:numel(C_pressure))';
end

%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;

%Loads
switch loadType
    case 'pressure'
        febio_spec.Loads.surface_load{1}.ATTR.type='pressure';
        febio_spec.Loads.surface_load{1}.ATTR.surface=febio_spec.Geometry.Surface{1}.ATTR.name;
        febio_spec.Loads.surface_load{1}.pressure.VAL=1;
        febio_spec.Loads.surface_load{1}.pressure.ATTR.lc=1;
        febio_spec.Loads.surface_load{1}.value.ATTR.surface_data=febio_spec.MeshData.SurfaceData{1}.ATTR.name;
    case 'traction'
        febio_spec.Loads.surface_load{1}.ATTR.type='traction';
        febio_spec.Loads.surface_load{1}.ATTR.surface=febio_spec.Geometry.Surface{1}.ATTR.name;
        febio_spec.Loads.surface_load{1}.scale.VAL=1;
        febio_spec.Loads.surface_load{1}.scale.ATTR.lc=1;
        febio_spec.Loads.surface_load{1}.traction.ATTR.surface_data=febio_spec.MeshData.SurfaceData{1}.ATTR.name;
end

%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.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
% febView(febioFebFileName);

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 12:46:52
Waiting for log file...
Proceeding to check log file...04-Jun-2019 12:46:54
------- converged at time : 0.1
------- converged at time : 0.181833
------- converged at time : 0.2654
------- converged at time : 0.350536
------- converged at time : 0.43709
------- converged at time : 0.524928
------- converged at time : 0.613926
------- converged at time : 0.703975
------- converged at time : 0.794973
------- converged at time : 0.88683
------- converged at time : 0.979465
------- converged at time : 1
--- Done --- 04-Jun-2019 12:46:58

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,'kw','none',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
    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;

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/.