Accessing ANSYS Options

1
Accessing ANSYS Options

• Chapter 5

2
Chapter 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.

3
A. 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

6
B. 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.

16
C. 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)

23
Accessing ANSYS Options Hyperelastic with
Contact Nonlinear Analysis of a Keyboard

• Workshop 5

24
D. 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.

25
Workshop 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

26
Workshop 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
27
Workshop 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.

28
Workshop 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.

29
Workshop 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

30
Workshop 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.

31
Workshop 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

32
Workshop 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

33
Workshop 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

34
Workshop 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.

35
Workshop 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

36
Workshop 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

37
Workshop 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

38
Workshop 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

39
Workshop 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.

40
Workshop 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.

41
Workshop 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.

42
Workshop 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.

43
Workshop 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.

44
Workshop 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.