# Lesson 3: Abaqus Interface¶

This chapter shows how forces calculated in AnyBody can be applied as boundary conditions to a FE Models generated for Abaqus.

Below you see the flowchart from the introduction of this tutorial extended with a converter step that converts the AnyFE output file to a format readable by Abaqus. This step is carried out by a small tool, called AnyFE2Abaqus.exe, which is available at AnyBody Technology webpage.

The model we will have a look at is a model of the claviclebone. We will analyze the muscle forces acting on the clavicle during lifting an arm and compute the stresses in the bone. The standard Standing model taken from the AMMR will be used (Notice, this tutorial was authored with AMMRV1.3.1. It should run equally well with newer versions of the AMMR, but the results may vary due to updates of the models).

We shall focus on the interfacing between AnyBody and Abaqus and therefore we will use a bone mesh derived from the standard scaled (=un-scaled) AnyBody model. Thereby, we can skip the step to do any scaling according to the subject data and in particular the bone geometry. This would have been needed if the bone model was derived from scanned data coming from another, significantly different, person than generic AnyBody model.

Let’s start with the AnyBody model. We have to make sure the FE and AnyBody models are aligned. The idea is to include local reference frames in both systems which will be used for all further data transfer. Open the Standing model from the AMMR, or better make a copy of the whole model folder and use this one. For convenience we will reduce the model detail by excluding the left arm and switching off the muscles in all body parts, except the right arm. This is done in the BodyPartsSetup.any file.

Next we define the local ref frame on the clavicle. All forces will be later exported with respect to this coordinate system. You can either use a pre-defined reference system in the AMS or create a new one. The following lines create a new node located in the Sternoclavicular joint:

AnySeg &RiArm = Main.HumanModel.BodyModel.Right.ShoulderArm.Seg.Clavicula;
RiArm = {
AnyRefNode localrefframe= {
sRel = {0,0,0};
// ARel = RotMat(0.5*pi,x);
AnyDrawRefFrame drws = {ScaleXYZ = {1,1,1}*0.3;RGB={0,0,1};};
};
};


Include them e.g. in the Environment file. After reload of the model the reference frame is shown

Download the prepared Abaqus file here and save it in your working directory. Please note that this FE model of clavicle was created in the same reference frame as the clavicle model in the AnyBody model, since we have actually used the STL exported from AMMR for this bone. Therefore, ‘localrefframe’ does not have to be displaced in order to match with the coordinate system of the FE mesh, but had the FE mesh been generated based on scanned data, the registration between AnyBody model’s clavicle and the FE mesh can be entered using localrefframe’s sRel and Arel members.

In a similar manner one could define a local reference frame in Abaqus by means of the *SYSTEM keyword; however, this is not advisable because the AnyFE Converter does not handle the *SYSTEM keyword in the supplied mesh file. We shall return to the issue of aligning the coordinate systems for the AnyBody forces and the mesh later, and so far we consider localrefframe to be aligned with the mesh coordinate system.

This figure above shows the clavicle bone mesh used for this example. This bone is modeled with a reduced stiffness, which can be interpreted as an osteoporotic bone.

Next we want to analyze the behavior of the bone subjected to the forces computed in the AMS. First, change the Mannequin file to create the desired physical activity. We want to analyze a simple lifting case, so all we specify is flexion in the shoulder joint. Open the Mannequin file and look for the PostureVel folder. Change the Glenohumeral flexion value to 50/Main.Study.tEnd, this determines the joint velocity necessary to reach 50 degree flexion taking into account the simulation time.

AnyFolder Right = {
//Arm
AnyVar SternoClavicularProtraction=0; //This value is not used for initial position
AnyVar SternoClavicularElevation=0; //This value is not used for initial position
AnyVar SternoClavicularAxialRotation=0; //This value is not used for initial position
AnyVar GlenohumeralFlexion =50/Main.Study.tEnd;


We also want to alter the initial starting position for the motion, enter the Posture position folder and make the changes indicated below.

AnyFolder Right = {
//Arm
AnyVar SternoClavicularProtraction=-23; //This value is not used for initial position
AnyVar SternoClavicularElevation=11.5; //This value is not used for initial position
AnyVar SternoClavicularAxialRotation=-20; //This value is not used for initial position
AnyVar GlenohumeralFlexion =0;
AnyVar GlenohumeralAbduction = 7;
AnyVar GlenohumeralExternalRotation = 0;
AnyVar ElbowFlexion = 5.0;
AnyVar ElbowPronation = -20.0;


We want this motion to be done in 10 seconds and analyze 5 time steps. This is set in the main file. Search the Study folder and change the end time of the study to 10 seconds and the number of time steps to 5.

AnyBodyStudy Study = {
AnyFolder &Model = .Model;
tEnd = 10.0;
Gravity = {0.0, -9.81, 0.0};
nStep = 5;


Now we have to specify which forces we want to export to the FE model. For this we make use of the Class inserter. Place you cursor in the Study folder in the main file, below the code shown above and select the Classes tab on the left side of the main file window. Search for the class named AnyMechOutputFileForceExport right click on it and choose Insert class template. This will insert the class necessary for force export.

AnyMechOutputFileForceExport <ObjectName> =
{
FileName = "";
/*NumberFormat =
{
Digits = 15;
Width = 22;
Style = ScientificNumber;
FormatStr = "";
};*/
//UseRefFrameOnOff = Off;
//AllSegmentsInStudyOnOff = Off;
//XMLformatOnOff = Off;
//AnyRefFrame &<Insert name0> = <Insert object reference (or full object definition)>; You can make any number of these objects!
//AnySeg &<Insert name0> = <Insert object reference (or full object definition)>; You can make any number of these objects!
};


Create a folder in your Standing model folder named files_in and one called files_out. This will be used to store the FE files. Change the FE_out object as shown below. These definitions specify that all forces acting on the segment Clavicula will be written in the xml file clavload. It is important to use the xml format, since the AnyFE converter only reads this format.

The UseRefFrameOnOff option enables specification of a reference frame in which all forces and positions are reported. Switch this option on and name the ref frame (the one we created before). You can find the path to the ref frame by browsing the model tree on the left side of the main file window to the right clavicle and right click Insert object name.

AnyMechOutputFileForceExport FE_out =
{
UseRefFrameOnOff = On;
AnyRefFrame &ref1 =
Main.HumanModel.BodyModel.Right.ShoulderArm.Seg.Clavicula.localrefframe;
AllSegmentsInStudyOnOff = Off;
XMLformatOnOff = On;
//AllSegmentsInStudyOnOff = Off;
AnySeg &clav = Main.HumanModel.BodyModel.Right.ShoulderArm.Seg.Clavicula;
};


This object will write all the muscle and joint forces for all time steps in one xml file.

We are now ready to execute the AnyFE converter and transform the generic AnyFE XML file to an Abaqus readable INP file. The AneFE converter tool is available at the AnyBody Technology webpage. Unpack the files in your model folder. These files include the AnyFE converter, which is an executable called AnyFE2Abq.exe. It can convert the xml code to Abaqus keyword sequence and combine it with the FE model.

The AnyFE converter is a command line tool with options controlled by program arguments. Running the program with the –h, i.e. AnyFE2Abq.exe –h. We shall briefly go through the important options here.

The –i and –o options specify the input AnyFE xml file (-i) and the output file (-o), respectively. The –m option is used to specify a FE model without boundary conditions. This Abaqus INP file, containing the mesh only, will be included in the converter output INP file by means of an include-statement.

Another significant option is –e, which is the radius of muscle/ligament attachment area. This radius (default value is 1 cm) is used for the construction of coupling constraint between a loaded point and the surface of the bone. Please note that this radius is used on all loads applied, not only muscles and ligaments, but also joint reactions, applied loads, etc. This parameter is not a physiological parameter. Please also note that in case of complex concave geometries these constraints may select wrong parts of the bone surface and may require some manual adjustment.

You can call the converter either from a shell prompt or from inside the AnyBody system. The latter can be done by using the following class: AnyOperationShellExec. The names for the executable, its working directory and the options for the call of the exe file have to be given. Please adjust the path corresponding to your setup and insert this code below the study folder:

AnyOperationShellExec ConvertToAbq={
Show=On;
FileName = "AnyFE2Abq.exe";
Arguments = "-i ..\files_in\clavload.xml -o ..\files_out\output.inp -m .\clavicula.inp";
WorkDir=".\ ";
};


This will enter an operation called ‘ ConvertToAbq’ into the model and running this will execute the AnyFE converter. From the shell prompt you write the following to get the same result:

AnyFE2Abq.exe -i ..\files_in\clavload.xml -o ..\files_out\output.inp -m .\clavicula.inp


At this point, let us return to the issue of the coordinate systems that we have used so far and an alternative option. In the example we have exported all the positions and forces with reference to a given manually defined system attached to the clavicle, i.e. the ‘localrefframe’. The AnyFE converter will by default will transfer all positions and forces directly, i.e., in the same coordinate system as exported the AnyFE XML file. In the above, we have therefore considered ‘localrefframe’ to be the coordinate system of the FE model, which is also the CT/MRI scan system. Notice that in the given case, the segment reference and the output reference are aligned since the FE mesh was based on the original bone geometry from the AnyBody model, i.e. sRel= {0, 0, 0}.

As an alternatively, you can export the AnyFE XML file in another reference frame, even the global system in AnyBody (UseRefFrameOnOff=Off) for that matter. This implies that the data of the AnyFE XML file may or may not contain motion of the bone and it will probably.not be aligned with the FE mesh/CT/MRI scan system. If you chose this an option, the AnyFE Converter can remove the rigid body motion by using the –r option equal to ‘segment’:

AnyFE2Abq.exe -i ..\files_in\clavload.xml -o ..\files_out\output.inp -m .\clavicula.inp –r segment


This makes all AnyFE data from the AnyFE Converter being transformed to the local frame of the segment, here the clavicle segment, before applied to the FE model and outputted.

If the reference frame of the segment is not identical to the one of the FE mesh, one can apply a constant transformation to all data accommodating for this misalignment. The –t option allows you to enter the transformation as a string containing space separated numbers. The command line will look like:

AnyFE2Abq.exe -i ..\files_in\clavload.xml -o ..\files_out\output.inp -m .\clavicula.inp –r segment –t "a11 a12 a13 a21 a22 a23 a31 a32 a33 dx dy dz"


The transformation may contain either 9 or 12 numbers. The first nine, aij, must be the orthogonal rotational transformation matrix and the latter optional three, dx, dy, and dz, are the translations.

These options allow you to handle the coordinate systems differences using the AnyFE Converter, i.e., outside AnyBody. For instance this implies that you do not have to redo simulations just to apply the same forces to another FE mesh with another local frame; this can all be done with adjustment of the parameters for the AnyFE converter.

Now we have looked at how to execute the AnyFE converter properly, so let us have a look at what it does.

Please notice that the AnyFE Converter is reading Abaqus input file (INP) and it is only expecting a simple mesh specification. This reader is not fully compatible with the INP keyword language for Abaqus. Basically, it only reads in the first block of nodes (*NODE section) and it does not accept commands that may interfere with the interpretation of this node section. This implies that many Abaqus keywords are not allowed in front of the first node section. This also implies that subsequent node sections are not read and therefore, not used for application of forces.

The AnyFE Converter performs the following actions:

• Maps all AnyBody exported forces, i.e., joint reactions, muscle forces and applied forces to the provided FE mesh. Mass related forces are neglected, i.e., gravitational and acceleration equivalent forces.

• Defines nodes in the positions from the AnyFE output file, i.e. the position of all loads (this includes muscle/ligament attachment nodes)

• Defines amplitudes for each force/moment component in the AnyFE output file

• Defines concentrated loads (*CLOAD) in each of these nodes

• Defines coupling constraints between the created nodes and a part of the surface of the bone

• The mesh in included

• Adds inertia relief loads (*INERTIA RELIEF)

Please note that the inertia relief loads will automatically be added to the model in order to provide a full set of boundary conditions. However, these loads require a density value in the material definition section. Absence of this density value will result in the error during the FE analysis. In case when additional constraints are present in the model, e.g. environment support, contact with another bone, etc., the inertia loads can be suppressed or removed.

Now we are ready to run the analysis and convert the data. Reload the model in the AMS. Select RunApplication in the Operations tree. This will automatically run the Calibration and InverseDynamics studies. Next select ConvertToAbq operation and run it. This will create a new Abaqus input file in the files_out folder.

Open Abaqus and import the input file from the output directory. This will load the clavicle mesh model, apply the boundary conditions. Next step is to make your custom final adjustments, run the FE solver, and when finished, post-process the results. The image below shows the results of running the model without any custom adjustments, however in the following we shall consider modification of the load application regions.

On the following picture, you can see the muscle attachments nodes and coupling constraints that are applied to the finite element model.

Bear in mind that the muscle attachment area is considered to have a constant radius, however, in many cases these areas are elongated and have irregular pattern. Let us assume that the area for the sternocleidomastoid muscle has to be changed to fit better the user’s expectations, for example, to be more physiological. That can be done by defining the desired muscle attachment area as a new surface in the FE model and changing the relevant coupling constraint to refer to this surface. In our example, we create a surface on the posteriormedial side of the clavicle as it shown on the following pictures. Please note that you will also need to set the influence radius option to ´To outermost point of the region´ in order to make sure that you now make the coupling to the whole surface.

The following picture shows how the modified constraint looks like; the sternocleidomastoid muscle attachment patch is now spread on the surface elements of the clavicle mesh.

We can run the solver again and inspect the results, see the image below. In the crude model, we have worked with in this case, we do not see significant changes due to the modification in the overall picture.