DEMO_febio_0004_beam_twist

Below is a demonstration for:

Building geometry for a beam with hexahedral elements
Defining the boundary conditions
Coding the febio structure
Running the model
Importing and visualizing the displacement 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
beam torsion twist loading
prescribed displacement boundary condition
hexahedral elements, hex8, hex20
beam, rectangular
static, solid, multi-step
hyperelastic, Ogden
displacement logfile
stress logfile

clear; close all; clc;

Plot settings

fontSize=20;
faceAlpha1=0.8;
markerSize=40;
markerSize2=20;
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

%Specifying dimensions and number of elements
beamWidth=10;
sampleWidth=beamWidth; %Width
sampleThickness=4*beamWidth; %Thickness
sampleHeight=beamWidth; %Height
pointSpacings=3*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

elementType='hex20'; %'hex8'

%Define applied torsion angle
alphaRotTotal=3*pi;%0.5*pi; %Total twist angle
numSteps=50; %Number of steps

%Material parameter set
c1=1e-3; %Shear-modulus-like parameter
m1=2; %Material parameter setting degree of non-linearity
k_factor=1e2; %Bulk modulus factor
k=c1*k_factor; %Bulk modulus

% FEA control settings
numTimeSteps=1; %Number of time steps desired
max_refs=25; %Max reforms
max_ups=0; %Set to zero to use full-Newton iterations
opt_iter=10; %Optimum number of iterations
max_retries=10; %Maximum number of retires
dtmin=(1/numTimeSteps)/100; %Minimum time step size
dtmax=1/numTimeSteps; %Maximum time step size

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
beamDimensions=[sampleWidth sampleThickness sampleHeight]; %Dimensions
beamElementNumbers=[numElementsWidth numElementsThickness numElementsHeight]; %Number of elements
outputStructType=2; %A structure compatible with mesh view
[meshStruct]=hexMeshBox(beamDimensions,beamElementNumbers,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

if strcmp(elementType,'hex20')
    [E,V,~,Fb]=hex8_hex20(E,V,{},Fb);
    meshStruct.elements=E;
    meshStruct.nodes=V;
    meshStruct.Fb=Fb;
end

Plotting model boundary surfaces and a cut view

hFig=cFigure;

subplot(1,2,1); hold on;
title('Model boundary surfaces and labels','FontSize',fontSize);
hp=gpatch(Fb,V,Cb,'k',faceAlpha1);
hp.Marker='.';
hp.MarkerSize=markerSize2;

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 set
logicFace=Cb==4; %Logic for current face set
Fr=Fb(logicFace,:); %The current face set
bcSupportList=unique(Fr(:)); %Node set part of selected face

%Prescribed force nodes
logicPrescribe=Cb==3; %Logic for current face set
Fr=Fb(logicPrescribe,:); %The current face set
bcPrescribeList=unique(Fr(:)); %Node set part of selected face

%Rotational settings
alphaRotStep=alphaRotTotal/numSteps; %The angular increment for each step
R=euler2DCM([0 alphaRotStep 0]); %The rotation tensor for each step
V2=V*R; %Rotated 1 part for visualization of stepwise amount

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,:),'k.','MarkerSize',markerSize);
hl(2)=plotV(V(bcPrescribeList,:),'r.','MarkerSize',markerSize);
hl(3)=plotV(V2(bcPrescribeList,:),'g.','MarkerSize',markerSize);

legend(hl,{'BC support','BC prescribe','BC prescribe 1 step'});

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';

%Create control structure for use by all steps
stepStruct.Control.analysis.ATTR.type='static';
stepStruct.Control.time_steps=numTimeSteps;
stepStruct.Control.step_size=1/numTimeSteps;
stepStruct.Control.time_stepper.dtmin=dtmin;
stepStruct.Control.time_stepper.dtmax=dtmax;
stepStruct.Control.time_stepper.max_retries=max_retries;
stepStruct.Control.time_stepper.opt_iter=opt_iter;
stepStruct.Control.max_refs=max_refs;
stepStruct.Control.max_ups=max_ups;

%Add template based default settings to proposed control section
[stepStruct.Control]=structComplete(stepStruct.Control,febio_spec.Control,1); %Complement provided with default if missing

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

%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=elementType; %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='Beam'; %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(:);


%Create steps
V2=V; %Coordinate set
nodeSetName=febio_spec.Geometry.NodeSet{2}.ATTR.name;
febio_spec.MeshData.NodeData=[];%Initialize so we can use end+1 indexing
bcNames={'x','y','z'};
for q=1:1:numSteps
    %Step specific control section
    febio_spec.Step{q}.ATTR.id=q;
    febio_spec.Step{q}.Control=stepStruct.Control;

    %Rotate coordinates
    V2n=V2; %The current set
    V2=V2*R; %Rotated further

    %Define prescribed displacements
    bcPrescribeMagnitudesStep=V2(bcPrescribeList,:)-V2n(bcPrescribeList,:);

    %Define mesh data and prescribed displacements
    for q_dir=1:1:3 %Loop over coordinates dimensions

        %Define mesh data for displacement increments
        c=numel(febio_spec.MeshData.NodeData)+1; %Current step index
        febio_spec.MeshData.NodeData{c}.ATTR.name=['displacement_',bcNames{q_dir},'_step_',num2str(q)];
        febio_spec.MeshData.NodeData{c}.ATTR.node_set=nodeSetName;
        febio_spec.MeshData.NodeData{c}.node.ATTR.lid=(1:1:numel(bcPrescribeList))';
        febio_spec.MeshData.NodeData{c}.node.VAL=bcPrescribeMagnitudesStep(:,q_dir);

        %Define prescribed displacements
        febio_spec.Step{q}.Boundary.prescribe{q_dir}.ATTR.bc=bcNames{q_dir};
        febio_spec.Step{q}.Boundary.prescribe{q_dir}.ATTR.relative=1;
        febio_spec.Step{q}.Boundary.prescribe{q_dir}.ATTR.node_set=nodeSetName;
        febio_spec.Step{q}.Boundary.prescribe{q_dir}.scale.ATTR.lc=1;
        febio_spec.Step{q}.Boundary.prescribe{q_dir}.scale.VAL=1;
        febio_spec.Step{q}.Boundary.prescribe{q_dir}.relative=1;
        febio_spec.Step{q}.Boundary.prescribe{q_dir}.value.ATTR.node_data=febio_spec.MeshData.NodeData{c}.ATTR.name;
    end
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;

%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);

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=10; %Max log file checking time

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

 
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
--- STARTING FEBIO JOB --- 12-Aug-2020 11:14:01
Waiting for log file...
Proceeding to check log file...12-Aug-2020 11:14:01
------- converged at time : 1
------- converged at time : 2
------- converged at time : 3
------- converged at time : 4
------- converged at time : 5
------- converged at time : 6
------- converged at time : 7
------- converged at time : 8
------- converged at time : 9
------- converged at time : 10
------- converged at time : 11
------- converged at time : 12
------- converged at time : 13
------- converged at time : 14
------- converged at time : 15
------- converged at time : 16
------- converged at time : 17
------- converged at time : 18
------- converged at time : 19
------- converged at time : 20
------- converged at time : 21
------- converged at time : 22
------- converged at time : 23
------- converged at time : 24
------- converged at time : 25
------- converged at time : 26
------- converged at time : 27
------- converged at time : 28
------- converged at time : 29
------- converged at time : 30
------- converged at time : 31
------- converged at time : 32
------- converged at time : 33
------- converged at time : 34
------- converged at time : 35
------- converged at time : 36
------- converged at time : 37
------- converged at time : 38
------- converged at time : 39
------- converged at time : 40
------- converged at time : 41
------- converged at time : 42
------- converged at time : 43
------- converged at time : 44
------- converged at time : 45
------- converged at time : 46
------- converged at time : 47
------- converged at time : 48
------- converged at time : 49
------- converged at time : 50
--- Done --- 12-Aug-2020 11:14:17

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),1,1);

    %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)]);

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.Marker='.';
    hp.MarkerSize=markerSize2;
    hp.FaceColor='interp';
    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(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;

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/.