Title: Accessing ANSYS Options
1Accessing ANSYS Options
2Chapter Overview
- In this chapter, the following ways of
interfacing with ANSYS will be covered - Named Selections and ANSYS Components
- Using Commands Objects
- Loading a Simulation Environment Directly in
ANSYS - The capabilities described in this section are
generally applicable to ANSYS Professional
licenses or above.
3A. Named Selections and ANSYS
- As will be seen subsequently, there are different
ways to interface with ANSYS to access advanced
functionality - However, when the model is transferred to ANSYS,
only node and element entities are sent - Solid model geometry is not referenced by the
ANSYS solver - Because of this, it may be difficult to select or
manipulate the model if only the finite element
mesh is present - Named Selections provide a convenient way of
selecting and manipulating the mesh - Named Selections are defined in Simulation
- These are transferred as Components in ANSYS,
where they can be selected or manipulated, as
needed. - To reference any geometry in ANSYS, the
geometry must first be defined as a Named
Component in Simulation
4 Transferring to ANSYS
- Named Selections transferred as ANSYS Components
- Vertex, edge, and surface named selections are
transferred as nodal components with the same
name - Named selections of solid, surface, and line
bodies transfer as element components with the
same name - Change the selection filter to Body. This
allows selection of surface and line bodies, not
just solid bodies! - The following conventions apply when Named
Selections in Simulation are transferred as ANSYS
Components - Names beginning with a number have the prefix
C_ added - Spaces will be replaced by underscores
- If multiple selection groups have the same name,
only the last one is converted as an ANSYS
component
5 Transferring to ANSYS
- Once Named Selections are transferred to ANSYS,
they can be referenced as Components to do the
following - Apply types of loads not supported in Simulation
- Change element attributes
- Define additional elements not supported in
Simulation - Special postprocessing tasks
- etc.
- Most ANSYS commands accept component names as an
argument, facilitating component use in ANSYS - Named Selections are associative with the CAD
geometry, so users do not have to worry if CAD
model is updated - Use of components is numbering-independent, so
users do not have to worry if the mesh changes
6B. Overview of Command Objects
- Command Objects enable users to add APDL (ANSYS
Parametric Design Language) commands, which
expose advanced ANSYS functionality not otherwise
available in Simulation - The Command objects requires that the user has
familiarity with APDL commands - Command objects can be inserted in the Part,
Contact, Environment or Solution branches - Part branch commands are inserted following the
material definition in ANSYS /prep7 - Contact branch commands are inserted following
the contact definitions in ANSYS /prep7 - Environment branch commands inserted prior to
the SOLVE command - Solution branch commands inserted after the
/POST1 command
7 Adding Command Objects
- Adding command objects is done by right-clicking
in the appropriate branch and using Insert gt
Commands - A new branch with a Worksheet view will be shown
where APDL commands can be inserted.
8 Parameterizing Command Objects
- The details window for each command object can
contain up to 9 parameter definitions (ARG1 to
ARG9). - Just as with other detail information throughout
Workbench these arguments can be made parametric.
In this example a command object placed in the
Environment branch contains the NSUB command.
The syntax of the command is NSUB, Initial
substeps, max substeps, min substeps Notice we
have substituted ARG1 in the command resulting
in Nsub, 10, arg1, 2 This parameter can be used
throughout Workbench including DesignXplorer
9. . . Specifying Material Properties
- Command objects inserted in part branches allow
quick material modification without having to
know each parts material number (ANSYS) - In the example below the mp command is used to
modify the Youngs modulus for the material used
for Part1. - Notice the parameter matid is inserted into the
command in place of the materials reference
number.
10. . . Specifying Contact Properties
- Contact branch command objects can be used to
modify ANSYS element type , real constant and
material number data using parametric references. - Can be used with symmetric or asymmetric contact
pairs. - Insert ANSYS commands using parametric references.
11 Obtaining Output Parameters
- Inserting a Command Object under the Solution
branch allows for the use of postprocessing
commands. - Certain types of APDL parameters may be retrieved
as Simulation parameters for use with design
studies - A output prefix is specified (default is
my_), so all APDL parameters with that prefix
will be searched and parsed. - Output parameters can be used with Parameter
Manager (discussed earlier in Chapter 10) or
DesignXplorer, enabling inclusion of APDL commands
12 Retrieving ANSYS Output Information
- Command objects placed in the Solution branch can
be used to retrieve plots from ANSYS - Place the appropriate plot formating information
(file type, size, etc.) in the command object. - Issue the desired plot commands.
- ANSYS plots are placed below the command object.
- Plots are static images (see next page).
13 Retrieving ANSYS Output Information
- ANSYS plots are retrieved below the command
object.
14 Linking with Text File
- The Command Objects contents can be exported or
imported to/from a text file - The Command Object contents can be refreshed to
reflect current text file contents - In Details view, linked filename will be shown
15 Command Objects Summary
- Command Objects provide a convenient means of
adding APDL commands to a Simulation model in
order to access advanced ANSYS functionality not
otherwise exposed - Commands branch provides pre- and post-processing
access inside of ANSYS, including linking
contents with external text files (e.g., ANSYS
input or macro files) - When used for post-processing, certain parameters
with a given prefix may be retrieved back into
Simulation. This is useful not only to view APDL
parameter output but also for design studies,
such as with Parameter Manager or DesignXplorer - For users not as familiar with APDL commands, the
Preprocessing and Postprocessing Commands
branches, discussed next, provide an alternate
means of including ANSYS functionality within
Simulation.
16C. Transferring Models to ANSYS
- As seen in the previous section, the two types of
Commands branches allow the user to add ANSYS
APDL commands within the Simulation environment
to access advanced functionality - In some cases, users may wish to transfer the
Simulation model into ANSYS directly and run the
model from there - All of these options will transfer the mesh only,
not the solid model geometry, to ANSYS - There are three ways to transfer the mesh/loads
to ANSYS - Saving the Environment as a binary ANSYS database
- Saving the Environment as an ASCII ANSYS input
file - Loading the Environment in an ANSYS session
17 Saving the ANSYS Database
- During solution, the ANSYS binary database can be
saved - In the Details view of the Solution branch,
change Save ANSYS db to Yes - Specify the ANSYS database filename in the ANSYS
db File Name textbox, which will appear
underneath - Solve the model, which will initiate solution and
save the ANSYS database (.db) - Things to keep in mind
- A solution must be initiated to create/save the
.db file - The ANSYS .db file will be saved in the active
units (Units menu) - This is also used in conjunction with saving
ANSYS result files after a solution (see next
slide)
18 Saving Other ANSYS Binary Files
- ANSYS files written during solution may also be
saved - Use with the Postprocessing Commands Builder
- Enable use to manually post-process within ANSYS
later - In the Tools menu gt Options gt Simulation
Solution, user can save ANSYS files as well as
specify where these files are stored. To save
ANSYS files for each Simulation database, use the
option Use Project Directory.
19 Writing an ANSYS Input File
- An ANSYS input file may be generated,
independent of the Simulation solution - Select a Solution branch
- Select Tools gt Write ANSYS Input File and
enter the name and location of the input file - Things to keep in mind
- As with saving the binary ANSYS database, only
the currently selected Environment will be
written. Write multiple input files for each
Environment branch to be saved. - Unlike saving the binary ANSYS database, this
option does not require a Simulation solution.
If loads/supports and requested results are
incomplete, Simulation will not know what type of
analysis to specify, so the model may be
transferred as MESH200 generic mesh-only
elements. Otherwise, see previous chapters as to
how the model will be translated to ANSYS - There will be an /EOF command prior to SOLVE
- To make the input file generate the mesh and
solve, simply remove the /EOF line in any text
editor
20 Loading Environment in ANSYS
- It is possible to load an Environment directly
into ANSYS - In the Workbench Project page, select a Model
- On the right-side menu, one can list Environments
contained in that Model branch - Select the Environment of interest to load into
ANSYS
21 Loading Environment in ANSYS
- After selecting the Environment, the ANSYS Output
Window will appear, and the Workbench GUI will
change to ANSYS - The analysis may be continued from within ANSYS
- Note that any actions performed in ANSYS will be
captured in an ANSYS log file, but these will not
be stored in Simulation - When leaving ANSYS, the user will be prompted to
save files
22 Loading Environment in ANSYS
- All pertinent files from the ANSYS session will
be stored in a new subdirectory in the Solver
Working Directory - The subdirectory name will be called
filename_num where filename is the name of
the .dsdb file and num is the numerical
Environment number - For example, for the third environment branch of
a Project.dsdb file, the subdirectory will be
named Project_3 - All ANSYS-generated files, including the input
file, error file, log file, and database, will be
contained in the subdirectory - filename_AWE.inp text input file generated from
Simulation and automatically read into ANSYS - filename.db (optional) binary ANSYS database of
mesh and loads - filename.err text file containing all error or
warning messages - filename.log text file containing ANSYS command
history - filename.page temporary binary file (leave
untouched)
23Accessing ANSYS Options Hyperelastic with
Contact Nonlinear Analysis of a Keyboard
24D. Workshop 5 Hyperelastic with Contact
- This exercise will cover accessing ANSYS options
through the Commands object. A 2D analysis of a
portion of a hyperelastic keyboard will be
performed, as shown below. - General use of Commandsobject in the
Geometry,Environment, and Solutionbranches - Use of Named Selections willfacilitate
manipulating datain ANSYS - Output parameters and plotswill be retrieved
from thesolution - Items shown with roundbullet points are tasks to
beperformed.
25Workshop 5 Hyperelastic with Contact
- Launch Workbench and open a new Simulation
session - Under the Geometry branch in the Details view
- Turn off import of solid and line bodies and only
select import of surface bodies - Change the Analysis Type to 2-D
- From the Context toolbar, choose Geometry gt From
File and select the Parasolid file
keyboard.x_t - The model will be attached to Simulation, as
shown next
26Workshop 5 Hyperelastic with Contact
- Select the menu item Units gt Metric (mm, kg, N,
C, s, mV, mA) - Right-click on Part 1 and select Rename to
rename it to ground - Likewise, right-click on Part 2 and rename it
to keyboard - Right-click on keyboard and select Insert gt
Commands from the pop-up menu - In the contents of the Commands object, type the
following
mpdele,all,MATID tb,hyper,MATID,1,,neo tbdata,1,80
.194
27Workshop 5 Hyperelastic with Contact
- The commands that were added in the previous
slide delete the existing material properties for
the keyboard part and replace it with a
neo-Hookean hyperelastic model. - The matid parameter is used to reference the
material ID for that given part, so the element
type or material can easily be changed using
ANSYS commands - The active Simulation units are used during
analysis, so it is important that all materials
defined in the Commands object have the same
units as the active Simulation Units.
28Workshop 5 Hyperelastic with Contact
- Using the Control Key, select both ground and
keyboard from the Geometry branch - In the Details view, ensure that Plane Stress
is the Behavior - Enter 10 mm for the Thickness
- In this example, the keyboard is assumed to have
a plane stress state with a thickness of 10 mm.
29Workshop 5 Hyperelastic with Contact
- Right-click on Contact Region under the Contact
branch and select Rename Based on Geometry - The contact pair will be renamed to ground To
keyboard, as shown on the right - In this case, the automatic contact detection
selected the top of the ground as the contact
surface (red). We need to flip the contact pair
such that the top of the ground is the target,
as it is the stiffer material. - Right click on ground To keyboard and select
Flip Contact/Target
30Workshop 5 Hyperelastic with Contact
- In the Details view, select Contact.
- The bottom of the keyboard will be highlighted.
With the Edge selection active and the Control
key pressed, select the other two lines as shown
on the right, as these will be expected to touch
the ground - Click on Apply to complete the selection
- Change Type to Frictionless
- Change Behavior to Asymmetric
- Change Formulation to Augmented Lagrange
- Toggle Pinball Region to Radius and enter
10 mm for the radius.
31Workshop 5 Hyperelastic with Contact
- Select the Mesh branch and, in the Details view,
toggle the Global Control to Advanced - The Element Size should be set to 1 mm
- Change Curve/Proximity to 100
- The Shape Checking can be switched to
Aggressive - Change the selection filter to Face and select
the ground part. From the Context toolbar,
select Mesh Control gt Mapped Face Meshing, as
shown on the right - The Element Shape can be set to Quadrilaterals
32Workshop 5 Hyperelastic with Contact
- Change the selection filter back to Edge and
select the four lines of the ground part, as
shown on the right - From the Context toolbar, select Mesh Control gt
Sizing - In the Details view, change Type to Number of
Divisions, with the number of divisions being 1 - In this example, the ground is not of interest
and is much stiffer than the keyboard, so it will
be meshed with just one element. - Right click on the Mesh branch and select
Preview Mesh
33Workshop 5 Hyperelastic with Contact
- Select the topmost line of the keyboard part
and select the Create Selection Group icon - When asked for a name, enter PUSH_TOP
- A new Named Selection branch and PUSH_TOP object
will be created in the Tree. - The Named Selection can be referenced as a nodal
component in ANSYS Command objects in order to
manipulate the model. In this case, a special
loading will be applied to the nodes in PUSH_TOP
34Workshop 5 Hyperelastic with Contact
- Highlight the Environment branch, then select the
leftmost line of the keyboard part - From the Context toolbar, select Structural gt
Frictionless Support - Do the same for the rightmost line of the
keyboard part and add a Frictionless Support
there as well.
35Workshop 5 Hyperelastic with Contact
- Select the bottommost line of the ground part
- Add Structural gt Fixed Support from the Context
toolbar - Right-click on the Environment branch and select
Insert gt Commands - In the Commands object, select Import from the
Context toolbar - Select keyboard2.mac as the file
- The contents of keyboard2.mac will be inserted
into the Commands object
36Workshop 5 Hyperelastic with Contact
- It may be worth pausing for a moment to examine
the commands inserted from keyboard2.mac - All results are saved for each substep
- The nodal component (Named Selection) called
PUSH_NODE is selected, and a coupled set for
the y-direction is created for all of the nodes - A displacement of 54 mm is applied in the
y-direction on the master node of the coupled
set. - An element plot is generated, so the user can see
the mesh and boundary conditions in Workbench
Simulation
37Workshop 5 Hyperelastic with Contact
- Select the Solution branch. In the Details view,
change the following - Solver Type to Direct
- This model has hyperelastic and steel materials,
so the matrix may be ill-conditioned. The sparse
direct solver will suffice for such a small
problem. - Weak Springs to Off
- Large Deflection to On
- Although the text box may change to yellow, this
is because no results have been requested yet. - Auto Time Stepping to On
- Initial Substeps and Minimum Substeps of 10
and Maximum Substeps of 1000
38Workshop 5 Hyperelastic with Contact
- From the Context toolbar, select the following
- Stress gt Equivalent (von-Mises)
- Strain gt Equivalent (von-Mises)
- Deformation gt Total
- Tools gt Solution Information
- Tools gt Contact Tool
- Change the Contact Tool detail to Worksheet,
change Contact Side to Contact gt Apply. - Then RMB gt Insert
- Contact gt Pressure
- Contact gt Penetration
39Workshop 5 Hyperelastic with Contact
- There are some type of results that cannot be
viewed directly from Simulation. These include
load-history response (POST26) as well as element
table items - Right-click on the Solution branch and Insert gt
Commands - From the Context toolbar, select Import and
read in the keyboard3.mac file - The contents will be displayed in the worksheet.
Notice the inclusion of the output parameter
MY_REACTION in the Details view.
40Workshop 5 Hyperelastic with Contact
- The keyboard3.mac contains postprocessing ANSYS
commands - The Time-History Post-processor is used to
plotforce vs. displacement at thetop of the
keyboard - The General Postprocessoris then used to get
thereaction force due to pushingthe keyboard
down. This isreported as MY_REACTION,which
is also recognized bySimulation as an
outputparameter that can be usedwith the
Parameter Manageror DesignXplorer - The resulting thicknesses are also plotted.
41Workshop 5 Hyperelastic with Contact
- Click on the Solve icon to initiate the
solution. - Select the Solution Information branch to
review the contents of the Output window. - The Force Convergence graph can also be
reviewed during solution to monitor the progress
of the analysis - At the end of the solution, a warning message may
appear. The user does not have to worry about
this, as the frictionless supports used in this
example are fine for this large-deflection
solution.
42Workshop 5 Hyperelastic with Contact
- Select Equivalent Elastic Strain and review the
strains. - Change the scaling in the Context toolbar to 1.0
(True Scale) - The undeformed model may also be superimposed to
get a better sense of how much the keyboard
deformed. - Note that the equivalent elastic strains are very
large (66), as this is a hyperelastic model. - Review other results, such as stresses,
deformation, and contact results. Contact
pressure distribution is shown on the right.
43Workshop 5 Hyperelastic with Contact
- Note that under the Commands object in the
Solution branch, there are four Post Output
objects - If no objects are shown under the Commands
branch, click on the Workbench Project tab on the
very top, then return back to Simulation tab to
refresh the window - Select Post Output 2 this is a plot of force
vs. deflection in the y-direction. - Note that the force is relatively small at first.
Then, the slope changes when the front of the
keyboard initiates contact. Another change in
slope occurs when the middle contacts the ground.
44Workshop 5 Hyperelastic with Contact
- Post Output 4 shows the final thicknesses
- Recall that the initial thickness was 10 mm (Step
3) - Because of the incompressibility of the
hyperelastic material, some areas (yellow) became
thinner while other areas (red) became thicker. - Post Output 3 shows equivalent stresses
- Note that the max stress in ANSYS is 141 MPa
while max stress is 140 MPa in Simulation. This
slight difference is due to the fact that ANSYS
has different options for output, including
averaged or unaveraged stresses, so the user has
more control over output results with the
Commands object.