In this example we want to shed some light on an important issue for all aquarium owners: Whats the magnitude of stress in the lumbar vertebra L5 during lifting of a 10 kg aquarium?
First we need a model to work on.
With the AnyBody Modeling System you already have a repository of models available, for details please see the AnyBody Assistant available from the menu. This tutorial has been written using the AnyBody Managed Model Repository Ver. 1.2 (AMMRV1.2) if you see differences between the tutorial text and your own results please download AMMRV1.2 from www.anybodytech.com/anybody.html?fwd=modelrepository
The starting point for this tutorial is the model: Applications/Examples/StandingLiftFEA/StandingLiftFEA.main.any
Please find the model and load it by pushing F7 and open a Model View. You should see something similar to the picture to the right. The vertebral body we want to analyze is marked with a circle on the zoomed-in picture.
This model is based on the StandingLift model of the AMMR Repository. It is a full body model lifting a box of 10 kg and therefore also imposing forces on the spine. In this tutorial we will be using a more basic representation of the L5 vertebra than the one included in the repository model. Our tutorial model lacks the pedicles and facets joints, consisting just of the vertebral body. This is done in order to simplify the FEA related processes which will be discussed later.
Another simplification will be that we only use the model with joint generating muscles; this will keep the force output files small. In order to export the forces acting on the vertebra we have to include the corresponding output function. Place your cursor inside the Study folder of the main file. Open the Classes tab in the tree view on the left side of the editor window and locate the AnyMechOutPutFileForceExport class. Right-click it and insert the class template:
AnyBodyStudy Study = {
AnyFolder &Model = .Model;
InverseDynamics.Criterion.Type = MR_MinMaxStrict;
tStart = 0.5;
tEnd = 0.5;
Gravity = {0.0001, -9.81, 0.0001};
nStep = 1;
AnyMechOutputFileForceExport <ObjectName> =
{
FileName = "";
/*NumberFormat =
{
Digits = 15;
Width = 22;
Style = ScientificNumber;
FormatStr = "";
};*/
//AllSegmentsInStudyOnOff = Off;
AnyValue/*Use a AnyValue-derived class*/ <Insert name0> = <Insert value or expression>;
//AnyValue/*Use a AnyValue-derived class*/ <Insert name1> = <Insert value or expression>;
//AnySeg &<Insert name0> = <Insert object reference (or full object definition)>;
};
};
Next we have to fill in the necessary information.
AnyMechOutputFileForceExport FEAoutput =
{
FileName = "FEAoutput.txt";
/*NumberFormat =
{
Digits = 15;
Width = 22;
Style = ScientificNumber;
FormatStr = "";
};*/
AllSegmentsInStudyOnOff = Off;
AnySeg &L5Seg = Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg;
};
The AllSegmentsInStudyOnOff switch decides if only
the forces of the listed segments will be exported or data
from all segments in the study. Usually you will only use a
selected amount of data to keep the file manageable. The
following segment points to the L5 segment which is the one
we like to analyze. You can fill in the path by browsing
the Model tab to the L5 segment, right-click it and choose
Insert Object Name in the drop down
menu.
Thats all you have to do for the force export.
Please reload the model by pressing F7. Open the Study tree
in the Operation tab in the left side of the main window
and choose InverseDynamicsAnalysis. Press the
Run button. The model will analyze one
timestep and write the FEAoutput.txt file which we have
specified before. Lets have a closer look on the
Output file. It is located inside your Application folder.
You can open it either directly in AnyBody or in any text
editor of your choice.
===================== Start of time-step =====================
TimeSample[0]:
t=5.000000000000000e-001;
Segment[0]:
Name=Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg;
m=2.085000000000000e+000;
Jmatrix=1.168885000000000e-003,-9.570149999999998e-004,0.000000000000000e+000;-9.570149999999998e-004,6.423084999999999e-003,0.000000000000000e+000;0.000000000000000e+000,0.000000000000000e+000,6.591969999999999e-003;
r=-4.191723282427327e-002;1.143386931706198e+000;-1.497737038225964e-004;
rDot=5.893342512209260e-003;2.446813630010483e-004;1.925491094541430e-004;
Omega=1.062708497851127e-002;1.762864022916421e-003;-5.853096975772747e-003;
rDDot=-1.156661004595328e-002;-4.599319370658593e-004;-5.426105181307061e-003;
OmegaDot=-2.994499467387653e-001;-4.974436887280604e-002;9.364055661513510e-003;
Forces(17):
Force[0]:
Name=Main.HumanModel.BodyModel.Trunk.JointMuscles.L5SacrumJnt.Extension.dof0.Muscle.PosMuscle;
Class=AnyMainFolder.AnyFolder.AnyFolder.AnyFolder.AnyFolder.AnyFolder.AnyFolder.AnyFolder.AnyFolder.AnyGeneralMuscle;
SegmentName=Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg;
SegmentID=0;
Pos=1.077503778883285e-003;1.138342420959186e+000;-7.537109318454295e-005;
RefFrame=Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg.L5SacrumJntNode;
Components(1):
F[0]=0.000000000000000e+000;0.000000000000000e+000;0.000000000000000e+000;
M[0]=-1.587641435713052e-002;5.682776806642225e-001;7.224660293361494e+001;
...
It starts with information on the included segment. All the
geometrical entries are listed. One nice feature here is
that all coordinates stated in this file are given in the
same (global) coordinate system. In the following all
forces acting on the segment are listed. In this case one
of the artificial joint moment generating muscles is shown.
The position of the force is given as well as all of its
components from AnyBody. Depending on the nature of the
underlying AnyForce class, which you can see in the
Class entry, there are a different number of
forces and moments listed. An AnyForce may have any number
of components, which may be a physical force or a torque,
but it may also be a more generalized load, not measured in
Newton or Newton-meter. Basically these force components
are related to the underlying kinematic measure, so that
force times kinematic displacement becomes work/energy; in
other words the kinematic measure decides the unit of the
force component. Anyway, these occasionally somewhat
artificial force measures present in the AnyBody model are
converted to real point forces and point torques, when
outputted to the AnyFE output file. Therefore, we find F[i]
and M[i] in the AnyFE, which are the point force and the
point torque associated the i 'th component of the
given AnyForce object. The total force acting in the global
direction at a point can be found by simply adding all the
components forces, i.e. summing F[i] for all i at
that location.
In many cases, the components are indeed simple such that component i=0 for instance is Fx as could be expected, but since this Fx may refer to a local coordinate system of a particular segment, a joint attachment node, or the like, F[i] and M[i] may still have three non-zero values when exported to the AnyFE file. This is because the data is tansformed while being exported so that the AnyFE is referring to a single coordinate system for all of the exported data; this system is often (by default) the global coordinate system or it can be a local coordinate system.
Let us have a look at the following entry which basically gives the joint constraints in the L5-Sacrum joint:
Force[12]:
Name=Main.HumanModel.BodyModel.Trunk.JointsLumbar.L5SacrumJnt.Constraints.Reaction;
Class=AnyMainFolder.AnyFolder.AnyFolder.AnyFolder.AnyFolder.AnySphericalJoint.AnyKinEq.AnyReacForce;
SegmentName=Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg;
SegmentID=0;
Pos=1.077503778883285e-003;1.138342420959186e+000;-7.537109318454295e-005;
RefFrame=Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg.L5SacrumJntNode;
Components(3):
F[0]=1.401363916972399e+001;4.096147301511706e-001;2.002355876380579e-004;
M[0]=0.000000000000000e+000;0.000000000000000e+000;0.000000000000000e+000;
F[1]=-1.375600406291832e+001;4.706177494369769e+002;-1.423747832550264e+000;
M[1]=0.000000000000000e+000;0.000000000000000e+000;0.000000000000000e+000;
F[2]=-1.455818281740253e-004;4.287178778727723e-003;1.418527218321406e+000;
M[2]=0.000000000000000e+000;0.000000000000000e+000;0.000000000000000e+000;
You can see the three moments have zero entries. This is
due to the fact that this joint is discretized as a
spherical joint which therefore cannot take up moments. In
the same manner all other joints are handled.
Next we need an object where we can apply our exported
forces. This is also quite simple. A facility is built in
the system (from Version 3.1) which allows the export of
all .anysurf and .stl geometries from your application in
the .stl format. The function will export the geometry in
its actual position, so please make sure that your model
has not been reloaded since the force export otherwise run
the InverseDynamicAnalysis again to bring it to right
position. Of course it also involves all scaling which has
been applied to the bones. Browse through the model tree to
the L5Seg
(Main\HumanModel\BodyModel\Trunk\SegmentsLumbar\L5Seg) in
order to export the L5 segment. Inside this folder you find
the DrawSTL folder. Right-click the folder and choose
Export Surface. Choose a convenient place to
store the file and give it the name L5.stl. A
dialog box will appear which allows you to specify a scale
value for the output file. The scaling can be useful to
switch from one units system to another. In our case we
have m as units in the AMS, but want to have mm for the FE
geometry. So choose as scale factor 1000. From the AnyBody
point of view, thats all we have to do. Please note
that not all bones which are right now in the Repository
may be suitable for a FEA. As the main intention is to have
graphical representation of the body it may appear that
some bone are simply to coarse for a detailed analysis. But
of course you are free to import your own .stl file into
the AnyBody Modeling System to substitute existing bones.
You will have to tweak your CAD file a bit in order to make
it fit. Donation of
better quality CAD files of bones to the modelsis
most welcome.
Based on the exported forces and .stl file we can now build and analyze a FE model. Below we shall build an FE model applying the loads and other boundary conditions manually using non-commercially available software. However please notice that in the following lessons, we consider more smooth integration with selected commercial software by means of small converter software tools provided by AnyBody Technology. These tools automatically convert the AnyFE output file from AnyBody to input files for the particular FE software.
After building a FE model based on this data the internal stress in the bone tissue can be evaluated. Below are some von-Mises stress plots showing approximately the middle cross section of the vertebral body.
With a stress level of approx. 0.5 MPa in the cancellous
bone we are pretty far away from the yield strength, so we
can conclude that it appears to be ok for aquarium owners
to lift their pets in an aquariumof this size.
But of course we did some generous shortcuts to achieve
this goal and neglected a lot of detail which is provided
by the AnyBody Modeling System.
Building the FE-model
In this section a short description of how to build a
Finite Element model using AnyBody data is given. If you
are an experienced FE user you may want to skip this
section.
As this should be by no means a Finite Element tutorial we
will use some shortcuts to achieve our goal: We already
restricted the analyses to one time step. Further, we will
only take the joint reaction forces into account. How one
can handle muscle forces will be discussed below. And
finally the used geometry was simplified. Basically only
the vertebral body is used. The main reason for this is to
avoid getting lost in the jungle of meshing.
In the following, we will make use of two freely available
tools. Preprocessing (meshing and applying boundary
conditions) is done using IA-FEMesh provided by the University of Iowa. Calculix is used as solver and post-processor. This fine piece
of software is written and maintained by Guido Dhondt and
Klaus Wittig. Calculix v1.8 and IA-FEMesh v1.0 are used in
this tutorial. So things may slightly change with updates
on the programs. Please note that neither of these programs
is in related to AnyBody Technology.
Please follow the links shown above, download and install
the two programs if you want to do some hands-on
FEA.
Building the model - preprocessing
A file with the finished model is provided below, in
case you do not want to go through the entire model
building process.
Open IA-FEMesh and press the Surface tab to
load your (earlier exported) .stl file. After successful
loading we have to define a building block. The building
block is a prerequisite to the mesh generation and its
surfaces will be meshed and further projected on the bone.
For reasons of simplicity it has been prepared. Please
press the Block tab and chose
Load. Browse to the folder FEA
which is inside the StandingLiftFE
application folder. Choose the file
L5_block.vtk. Some boxes around the vertebral
body will appear.
In the next step, we will have a look at the local
mesh density and mesh the structure.
Press the Mesh tab and choose
Assign/Edit Mesh Seeds. By activating the
Color Code Mesh Seeds you can review the
settings for the mesh density which was set in the
predefined block. Just click on the different wireframes
and see the number of divisions per line. The density is
slightly increased in the regions of the vertebral
endplates.
Next is to generate the actual mesh. Open again the
Mesh tab and press Create. Fill
in n for node label and e for
element label, make sure that the volumetric mesh is chosen
and the perform smoothing" option is checked.
Apply will generate a nicely meshed vertebral
body (right)
After this we have to assign material properties to
the elements. Go to the Materials tab and
select User-Defined. You can simply give in
the Youngs modulus for the whole set of elements and
the Poissons ratio. Reasonable values may be an
average 1000 (MPa) for the modulus and 0.3 for the ratio.
But of course you may also want to model the bone in more
detail, separating the cortical shell and the cancellous
bone or even base the material properties on density data.
But this is surely not within the scope of this
tutorial.
In this example we will apply only the joint forces on the
endplates. Therefore we will not make explicit use of all
the information given by the AnyBody force export file.
We have to select two node sets to apply the boundary
condition. This is done by pressing the
Load/BC tab and the STEP-Load/BC
Assignments choose Node Set Definition
and use the appearing tools to define the node sets on both
endplates. You should use the option Visible surface
nodes and the + and tool to select the set.
You have to hold the Ctrl button to select nodes and
confirm your selection by right clicking on the selected
nodes. (In this case it is a rather good approximation to
select just a set of nodes on the endplates as force
application points. This may not be so easy for other
cases; in these the given information on the coordinates of
the forces is essential to apply the force in the right
way.)
After the definition of a node set on both endplates
we have to provide the boundary conditions. For this we
need our force export file. Please open the file (it should
be located in your StandingLiftFEA application folder) in
an editor and scroll down to Force[12]. This force is the
joint reaction on the L5-Sacrum joint.
Force[12]:
Name=Main.HumanModel.BodyModel.Trunk.JointsLumbar.L5SacrumJnt.Constraints.Reaction
Class=AnyMainFolder.AnyFolder.AnyFolder.AnyFolder.AnyFolder.AnySphericalJoint.AnyKinEq.AnyReacForce
Segment=Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg
SegmentID=0
Pos=1.077503784652309e-003;1.138342420959032e+000;-7.537109341625460e-005;
RefFrame=Main.HumanModel.BodyModel.Trunk.SegmentsLumbar.L5Seg.L5SacrumJntNode
NumComponents=3
F[0]=1.401363929748741e+001;4.096147338026376e-001;2.002355902030428e-004;
M[0]=0.000000000000000e+000;0.000000000000000e+000;0.000000000000000e+000;
F[1]=-1.375600406286652e+001;4.706177495305955e+002;-1.423747837481083e+000;
M[1]=0.000000000000000e+000;0.000000000000000e+000;0.000000000000000e+000;
F[2]=-1.455818161773931e-004;4.287178425936316e-003;1.418527096959978e+000;
M[2]=0.000000000000000e+000;0.000000000000000e+000;0.000000000000000e+000;
By summing up the rows for the forces F[0], F[1], and F[2]
we get the resulting components for the joint reaction
load. This can be directly used in the force definition as
they are given in the same coordinate system. In this case
only the Y-force component is of interest as all other
forces are pretty small. Choose Force and
your defined node set for the lower endplate. Specify the
Y-force to 471 (N). Make sure to confirm with
Apply. Select the node-set on the opposite
endplate and set the displacement to be 0 in all direction,
confirm again with Apply. (Next also the
moment generating muscles could be taken into account in a
similar manner, but this will be skipped here.)
The model is now finished. Now we have to export the model.
This export can be found under Load/BC.
Choose Export ABAQUS File. This will write an
ABAQUS style input file for a FE-Solver. This is the format
Calculix can read. Press Apply and name the
file L5FEA and save.
There is one more thing that has to be defined preliminary
to the FEA - the desired output. Please open a text editor
and load the L5FEA.inp file. In this file the whole
analysis is defined, using a reference to the node and
elements file.
**=========================================================================
**
HISTORY
DATA
**
**=========================================================================
**------------------------------------------------------------STEP
1
*STEP, INC=100, NLGEOM=YES, UNSYMM=YES
*STATIC
1.0, 1.0
**
*BOUNDARY, OP=NEW
unten, 1, 1, 0
unten, 2, 2, 0
unten, 3, 3, 0
**
*CLOAD
EndplateB, 2, 2.2488
**
**------- Output Requests --->
**
*NODE FILE
U
*EL FILE
S,
**
**
**
*END STEP
Please include the Output Requests (see
red lines above). This will make sure we get some results
to look at. Save the file and close the editor.
Solve and postprocessing
If you have somehow screwed up your model or simply
didnt want to go through the model building process,
you can find a working model here:
StandingLiftFEA\FEA\L5FEABackup.inp. (In this model also
different materials for the cortical shell (E = 12000 MPa)
and the cancellous bone structure (E = 200 MPa) have been
assigned.
If you want to use this model instead of your own build,
please change the following comments
involvingL5FEA to
L5FEABackup.)
Open up the Calculix command shell and browse to the
directory where you placed the L5FEA.inp file. Now
type
ccx L5FEA
and press return. This will push the model forward to the solver and start the analysis. Within a few seconds a nice JOB FINISHED should appear. Now, lets have look at the results: Therefore, type
cgx L5FEA.frd
This will call the Calculix (pre- and) postprocessor.
A graphical window showing the vertebrae will appear.
Clicking on the left side will give you a panel to
visualize the results. First you have to choose the dataset
you want to access. For example click on Datasets>Stress
to activate the stress dataset. After this you can choose
the desired Entry, e.g. Mises Stress. You can assess the
results in more detail using different Viewing settings
(Please have a look at the Calculix help file for more
information on this). Here are two examples for the
von-Mises stresses in the middle of the cross section of
the vertebral body:
This completes Lesson 1.
In the following lessons, we show somewhat more automatic interfaces to selected commercial FE packages using small interface tools
Click here to continue to