Tutorial Week 10 Internal bone remodelling

13 Pages·2016·1.03 MB·English

AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
Tutorial Week 10
Internal bone remodelling
Introduction
This tutorial will introduce the necessary steps to simulate internal bone remodelling
of an implanted femur using ANSYS. You will learn to:
• Setup and export mesh data from Workbench
• Generate an APDL input file for use with ANSYS Classic
• Call a pre-compiled Fortran subroutine during solution
Step 1: Prepare geometries for the femur and implant
The preparation of a realistic implanted femur geometry was detailed in week 4’s
tutorial. This involved the removal of the head and neck of the segmented femur in
ScanIP using the 3D editing tools. After completing the steps detailed in week 4’s
tutorial, you should end up with the following femur bone geometry.

Export this geometry from ScanIP as an IGS file. The femoral component of the hip
implant is available for download on the course website (FemoralImplant.IGS), under
the tutorial content for week 4, shown below.
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
Once you have both IGS geometries, they can be imported into Workbench. While it
is possible to import geometries directly into ANSYS Classic, the CAD interfaces in
Workbench are significantly more modern and work much better with external
geometry files. Start a new Mechanical Model module in the Workbench project
window. Double-click on geometry to open Design Modeler. Import both the femur
and implant geometries. They should look something like this:

The process of aligning these two geometries is provided in the week 4 tutorial. This
involves a simple body translation to move the implant into the correct position as
shown.

Once correctly aligned, a cavity for the implant in the femur is required. Use the
Boolean subtraction function provided in Design Modeler (Create > Boolean) to
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
create this cavity. Remember to select the femur as the target body and the implant
as the tool body, and ensure Preserve tool bodies is enabled (Yes).
Pay attention! At this point, the instructions deviate from week 4’s tutorial.
For this model, we are going to assume that the bone and implant are glued
together. We could allow Workbench to apply the default bonded condition to the
contact surfaces between these two geometries, but the simplest way to define this
relationship is to form a single part. Do this by selecting both geometries in the tree
outline, right-clicking and choosing Form New Part. For the mesh-savvy amongst
you, forming a new part enforces a contiguous mesh between the implant and the
bone. This means that the implant and bone will share the same nodes along their
interface, effectively gluing the two bodies together, and negating the need for
special contact conditions.

The result will be a single part containing two individual bodies. Don’t worry,
separate material properties may still be assigned to these two bodies. Close the
Design Modeler window, and it’s probably a good idea to save your project file at this
point.
Step 2: Generating the mesh in Workbench
Now the material properties can be set up in the Mechanical Model module. Open
Engineering Data and make two isotropic elastic materials: Bone and Implant. It
doesn’t matter what Young’s modulus and Poisson’s ratio you specify in this section;
they will just act as placeholders for the bone and implant mesh objects. A Young’s
modulus of 1 for the bone and Young’s modulus of 2 for the implant will suffice.
Close Engineering Data and open the Model component. This will launch the
Mechanical application window. First, assign the bone and implant materials to their
respective bodies. The next thing to do is generate a mesh for the model. For this
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
tutorial, it’s sufficient to just keep most of the default mesh settings. However, you
should keep element mid-side nodes to generate quadratic (second-order)
elements. Do this in the Advanced section of Mesh details, as shown below.

Although we should technically do a mesh convergence study to verify the accuracy
of our finite element model, we’re going to skip this for the sake of brevity.
The last thing we need to do in the Mechanical application is to define a named
selection for face on the neck of the femoral implant. Select the face and add it as a
named selection as below. This will make it easier to apply forces using APDL.
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
Step 3: Using FE Modeler to export the mesh
Once the mesh and named selection have been generated, close the Mechanical
application window. Insert an Finite Element Modeler module into the Workbench
project window, and link the model component of the Mechanical Model module to
it.

The FE Modeler module enables the export of mesh objects created in Workbench
to a variety of formats, including to ANSYS Classic by creating an APDL input file. It
will also translate the materials specified in Engineering Data and the Named
Selections defined in the Mechanical application to their APDL analogues.
Before opening FE Modeler, ensure that the unit used for the model are in metres,
not millimetres. You can do this by checking the Properties of the Assembly Mesh
in the Outline pane. If you don’t see Outline and Properties panes, go to View >
Outline and View > Properties in the project window.

Open FE Modeler by double-clicking the Model component. Ensure that the Target
System is Mechanical APDL. You can check out the features of your mesh in the
outline tree. If all the instructions have been followed correctly, all you need to do is
click on Write Solver File. This writes all the mesh data to an APDL input file. You
can preview the contents of this file under Generate Data. Name your input file
“A3_mesh.inp” so it can be identified later.
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
Step 4: Editing the generated APDL input file
After saving the APDL input file from FE Modeler, close and save your Workbench
project file. The remainder of this project will take you through the steps needed to
create a solvable APDL input file.
APDL input files are just text files. You can open them in any text editor. The input
file generated from FE Modeler contains the locations of all the nodes, and the
definitions of all the elements from those nodes, and is therefore quite large for a text
file. Use Notepad++, which is available on the PCLAB computers, to open this input
file. Your input file will probably start off like this:
/PREP7
SHPP,OFF
/NOPR
!
! COORDINATE SYSTEMS
!
!
! MATERIAL PROPERTIES
!
/com, Materials <SECTION=MATERIALS>
! Origin Material Property ID - 23
MP,EX,1,1, ! Pa
MP,NUXY,1,0.3,
! Origin Material Property ID - 25
MP,EX,2,2, ! Pa
MP,NUXY,2,0.3,
!
! PHYSICAL PROPERTIES
!
!
! ELEMENT TYPES
!
/com, Element Types <SECTION=ELEMENTTYPES>
et,1,MESH200
keyopt,1,1,9

Some of these commands will be explained later in this tutorial when you work with
the template input file. The ! character denotes a comment, as does the /com
command. Briefly, the above set of commands opens the pre-processing module
(PREP7), sets up two materials (MP), with Young’s modulus (EX) and Poisson’s
ratio (NUXY), and then specifies a type of element to use (ET), which is called
MESH200. The Young’s modulus and Poisson’s ratio of the materials you specified
in Engineering Data previously should be reflected in the MP commands. All we want
in this input file is the definition of the nodes, elements, and the named selection,
which is called a component in APDL. So either delete, or comment out the above
selection of commands. You should end up with the nodal listing (list of node
numbers and their co-ordinates):
nblock,3
(1i8,3e20.9e3)
<nodes>
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
and the element listing (list of element numbers, the material number, element type,
and the nodes that are used to construct them):
eblock,19,solid,12307
(19i8)
<elements>

and the component listing (component from the Named Selection, and the
associated node numbers):

CMBLOCK,NECK ,NODE, 37
(8i10)
<nodes>

Note that the CMBLOCK command, which is used to define the component,
specifies 37 nodes. This is important later, when we apply forces on these nodes.
Then go to the very end of the input file (Ctrl+End), and delete the following
unnecessary commands.
!
! BOUNDARY CONDITIONS
!
!
! LOADS
!
!
! Solution
!
!
! Turn output back on
!
/GOPR
!
FINI
/GOPR

You can now save this input file.

Step 5: Generating a solvable APDL input file
Download the template APDL file from the course website, under the week 10
tutorial content, and open this in Notepad++. Most of the input file has been
commented in-line, however some important commands will be detailed here. Full
descriptions of each command and the associated options are detailed in ANSYS
Help (under Mechanical APDL > Command Reference).

To enable the set-up of model, /PREP7 command is issued to activate the pre-
processing modules in ANSYS. After this, we can define the materials, mesh, and
loads.
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
et,1,SOLID187 defines element type number 1 as a SOLID187, which is a 10-
node tetrahedral element (10 nodes means it has mid-side nodes and therefore has
quadratic shape functions). This matches the type of mesh we defined in Step 2.
Next we need to define the material properties of the femur bone (material number
1). As the Young’s modulus of the femur bone is going to change in response to a
mechanical stimulus, TB,ELASTIC,1 is used to make a material table that can be
used to define changing elastic material properties (i.e. Young’s modulus and
Poisson’s ratio).

In addition, we need a specify a user-defined field variable (UF01) that can be
changed in this manner using a subroutine. In this example, UF01 is going to be the
Young’s modulus, so the relationship between UF01 and the Young’s modulus in the
material table is going to be perfectly linear (with a gradient of 1). We can make this
happen by using the TBFIELD and TBDATA commands to define two points that will
define a straight line. See the table below to see what this means.

UF01 Young’s modulus (Pa)
1 1
1000000000000 1000000000000

This work-around allows us to directly change the Young’s modulus of the bone by
changing UF01 using a Fortran subroutine. Note that the Poisson’s ratio will stay the
same here.

TB,STATE,,1 is another work-around in the APDL input that allows us to store
custom data in the results. This defines a single state variable that we will use to
store bone density, which will then be plotted after the model is solved.

The implant is then given regular material properties using the MP command. You
can change the numbers to give the implant a Young’s modulus (EX) and Poisson’s
ratio (NUXY) of your own choosing.

Next, it’s time to import the mesh you defined in the “A3_mesh.inp” APDL file. You
can insert it using: /INPUT,A3_MESH,inp. This type of command can be used to
input any APDL code into the file without having to copy and paste it over.

Following this are commands that give an initial value to the UF01 field variable that
was defined earlier. The femur bone elements need this for the first time-step (before
any bone remodelling has occurred). In this example, we’ve assumed that the bone
is completely homogeneous, and has a Young’s modulus of approximately 10.5
GPa.

To fix the base of the femur, the nodes on the bottom face of the femur need to be
selected. The following commands select these nodes, set their displacements in the
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
X, Y, and Z directions to 0, and then re-select everything to prevent confusion with
the following commands.

NSEL,S,LOC,Z,-445.9e-3
D,ALL,UX,0
D,ALL,UY,0
D,ALL,UZ,0
ALLSEL

Forces in the Z direction (FZ) can be applied onto the component/named selection
that was defined from Workbench. Specify the name of the component (NECK) when
issuing the F command. Forces can also be applied in the X (FX) and Y (FY)
directions as well by issuing multiple commands. Note that the force is applied to
each node, so we divide the total force by the number of nodes noted earlier in the
component definition (37 nodes for the example given in Step 4).
The final part of the APDL input file specifies the solution settings.
antype,transient
time,24
deltim,1
outres,all,all
outres,svar,all
solve
finish
save

These commands specify a transient analysis type (ANTYPE), which will terminate at
time = 24 (TIME), in increments of 1 (DELTIM), and export all the results for all the
time-steps (OUTRES), including the state variable (SVAR) which will contain the bone
density data. SOLVE executes the solution. SAVE creates a .DB file that can be used
to reopen the model in the ANSYS Classic GUI.
You may add your own post-processing commands to save the bone density plots
automatically after it finishes solving (see Appendix). Once you have completed
creating the APDL input file, save it with a different filename (e.g. A3_solve.inp)
Step 6: Solving using the pre-compiled USERFLD
subroutine
As described in the lecture, the APDL input is a high-level scripting language, which
is interpreted line-by-line by the ANSYS program. In this tutorial, APDL input has
been used to define the nodes and elements of the model, and set up the various
boundary conditions and material properties.
To simulate the internal remodelling in the femur bone, a USERFLD subroutine
needs to be run at the end of every time-step to update the bone density, and
therefore, the Young’s modulus (which corresponded to the user-defined field, UF01
in the APDL file). These changes in Young’s modulus affect the mechanical stimulus
experienced by the femur bone in the next time-step. The subroutine is written in
AMME4981 Applied Biomedical Engineering
AMME9981 Computational Biomedical Engineering
Fortran, which is a lower-level programming language that needs to be compiled to
an executable object before ANSYS can execute it.
Luckily in this tutorial, we can use a pre-compiled subroutine, which saves a lot of
trouble. The commented source code and pre-compiled objects necessary to
solve the model are downloadable from the course website. Please download
this and examine the source code (USERFLD.F) to identify the steps and
relationships used to translate the mechanical stimulus to a change in bone density
and Young’s modulus. All the files should be placed in your working directory. It is
ideal to make the working directory as a new folder on the Desktop if you are in the
PCLAB.
The most efficient way of running ANSYS is using the batch interface. From the
Windows Start Menu, open cmd.exe. Use the cd command to navigate to your
working directory. An example navigating to the folder “assignment” on the Desktop
is provided below.
cd C:\Users\your_unikey\Desktop\assignment

Before we run our APDL input file (A3_solve.inp), ANSYS needs to know if there is a
subroutine we would like to use, and where it is located. Let’s assume you followed
the instructions above and put all the pre-compiled files into the working directory
(e.g. “assignment”). Use the following commands to set a temporary ANSYS
environmental variable, and check that it has been set properly.
set ANS_USER_PATH=C:\Users\your_unikey\Desktop\assignment
echo %ANS_USER_PATH%

Finally, it is time to run ANSYS.
“C:\Program Files\ANSYS Inc\v161\ansys\bin\winx64\ansys161.exe” –b –j
A3 –i A3_solve.inp –o A3.out

-b means batch mode
-j specifies the job name (and the name of the files that get dumped in your working
directory)
-i specifies the name of the APDL input file
-o specifies the name of an output file, from which you can monitor the status of
your job and any errors or warnings that occur. On UNIX systems, there is a tool
called tail, but on Windows, you can download a program called baretail.exe
to watch the output file as new events get added to it.
Once the job has completed successfully, you can open the generated .db file by
double-clicking on it, which will open the ANSYS Classic GUI.