ANSYS ICEM CFD extends ANSYS meshing capabilities with robust and varied geometry import, the ability to efficiently mesh large or complex models with extended meshing controls, advanced interactive blocking tools for structured or unstructured mesh generation, extended mesh diagnostics, advanced interactive mesh editing, and output to a wide variety of solver formats including CFD, FEA, and neutral formats.
ANSYS ICEM CFD can input geometry in almost any format, whether a commercial CAD design package, third-party universal database, scan data, point data, or even combinations of CAD, facets, and mesh. It includes a variety of "patch independent" meshing methods which are able to work with dirty cad and does not require that surfaces be formed into solids or that flow volumes be extracted. It does include a wide range of interactive geometry, blocking and mesh editing tools that can be used to generate advanced or high quality meshes for any application.
The data-integrated ICEM CFD component system, or “ANSYS ICEM CFD Add-in”, enables you to launch ICEM CFD from ANSYS Workbench and use it to build a project, with the option of adding upstream data from Geometry, Mesh, Mechanical Model, or combined Geometry and Mesh system components. You can also use ICEM CFD to provide data to downstream component systems, such as ANSYS Fluent, ANSYS CFX, ANSYS Polyflow, FENSAP-ICE, Mechanical APDL, and FE Modeler.


The ICEM CFD Component system contains the following cells:
The System Header identifies the component type and provides access to Workbench context menu options. The ICEM CFD system header context menu options include:
Refresh
Update
Duplicate
Clear Generated Data
Delete
Rename
Properties
Add/Edit Note
These standard actions are described in the System Header Context Menu Options, Duplicating Systems and Moving, Deleting, and Replacing Systems sections.
The Model cell is associated with the ICEM CFD application. You can use the Model cell to modify some aspects of the project. You can also double-click the Model cell to open the project in ICEM CFD. The Model cell context menu items include the following:
Edit: Opens the ICEM CFD application and loads an existing Geometry/ICEM CFD file.
Duplicate: Copies the entire geometry and mesh data, enabling you to edit the Model cell in the duplicate system to investigate an alternative modeling approach.
Transfer Data From New: Enables the transfer of data from upstream Geometry, Mesh, Mechanical Model, or combined Geometry and Mesh components.
Note: If the Geometry cell option Use Associativity is On (its default setting), Part Reference IDs are stored in a Workbench database and remain persistent in ICEM CFD even if the topology of the geometry is changed.
Transfer Data to New: Enables the transfer of data from an ICEM CFD project to downstream data-integrated system projects, such as:
Fluent
CFX
Polyflow
FENSAP-ICE
Mechanical APDL
FE Modeler
Update, Refresh, Reset, Rename, Properties, and Add/Edit Note. These standard actions are described in the System Header Context Menu Options, Duplicating Systems and Moving, Deleting, and Replacing Systems sections.
An additional property is Create Subset(s) from Named Selection. If this option is set, then overlapping named selections are transferred to multiple subsets instead of to exclusive parts. This enables the creation of geometry subsets instead of parts, allowing you determine the part to which the geometry entity (point/curve/surface) should be associated. When this option is disabled each geometry is assigned to only one part, thereby losing association with other Named Selections (which are mapped to parts).
The Parameters cell enables you to see and edit Input and Output parameters for ICEM CFD.
Note: Scripts written in ICEM CFD may not be parametric with upstream or downstream projects. Care should be taken to write scripts whose functions do not exceed the capabilities of the upstream or downstream component systems.
You can create an ICEM CFD component system in Workbench using any of these methods:
Double-click the ICEM CFD system template in the Toolbox.
Drag-and-drop the ICEM CFD system template onto the Project Schematic.
Right-click a Geometry or Mesh project and select Transfer Data to New > ICEM CFD.
Choose > to import a standalone ICEM CFD project into Workbench. When the Import dialog opens, choose ICEM CFD Project File (*.prj) and navigate to the project you want to import.
Updating a project in Workbench brings the entire ICEM CFD system up to the most current status, including upstream and downstream data.
Changes that require you to update your ICEM CFD project include changes to upstream data and changes you make in the ICEM CFD editor. When changes are made, the cell in the Project Schematic window indicates that an update is required. Note, however, that changes made in the ICEM CFD editor will not cause the system to go out of date until the project, tetin file (geometry), blocking file, and/or Replay file are saved.
The actions taken by Workbench depend on whether the following conditions are met:
Blocking exists.
A Replay file exists.
Blocking parameters are set.
Other input parameters are set.
The following table describes the actions performed by ICEM CFD according to these conditions:
Table 12: Updating ICEM CFD Projects
Blocking | Replay File | Blocking Input Parameters | Other Input Parameters | Actions performed by ICEM CFD |
|---|---|---|---|---|
| No | No | No | No |
|
| Yes | No | No | No |
|
No | No | No | Yes |
|
No | Yes | No | Yes |
|
No | Yes | Yes | Yes |
|
Yes | No | Yes | Yes |
|
Yes | Yes | Yes | Yes |
|
ICEM CFD saves the unstructured mesh and project only if the ICEM CFD project is closed and you update from Workbench. If the ICEM CFD project is open, you will need to manually save the unstructured mesh and project.
The order of operations is Meshing input parameters are set before the Replay file is run; Blocking Input parameters are set after a replay file is run, but only if blocking exists after the replay file is run.
If no Replay file exists, the default mesher is determined by the presence or absence of blocking: if no blocking exists in the project, tetra is the default. Conversely, if blocking exists in the project, hexa is the default mesher.
To update a project and refresh upstream and downstream data, right-click the Model cell and choose Update.
Note: If available, Update will use the ICEM CFD Replay file to update the ICEM CFD project.
The data-integrated ICEM CFD interface has been modified to provide additional functionality that enhances the integration of ICEM CFD and Workbench.
One-click menus that enable you to control basic project and Replay Recording functions.
Note: If you create Workbench Input Parameters and want to step through the script line-by-line or using a line range, you must open the dialog from this menu.
The Workbench Replay Control dialog enables you to test and edit Replay scripts created within Workbench.
You can ensure that you are working within the data integrated environment by checking the Message window within IICEM CFD. The first line identifies that the application is integrated in the Workbench Framework.


The following one-click menu options are available in the Toolbar when you open ICEM CFD from Workbench:
Save Project: Saves the entire project, including Workbench data.
Refresh Project: Refreshes the upstream data in the ICEM CFD project.
Update Project: Brings the entire ICEM CFD system up to the most current status, including upstream and downstream data.
Start Replay Recording: Begins recording the commands needed to generate a custom meshing process. All of the steps in the mesh development process are recorded, including blocking, mesh size, edge meshing, boundary condition definition, and final mesh generation. See Replay Scripts in the ANSYS ICEM CFD Help Manual. After you click the Start Replay Recording icon, the icon changes to the Stop Replay Recording icon. You can click this icon to stop recording.
You can also click the arrow to choose Pause Replay Recording, Run Replay File, Delete Replay File, and Replay Control, which opens the Workbench Replay Control dialog.

Note: If you create Workbench Input Parameters and want to step line by line or using a line range through a replay file, you must use the item from this menu to start the Workbench Replay Control dialog.
Output Mesh: You can choose to save the ICEM CFD mesh output to one of several formats including Fluent, CFX, Polyflow, ANSYS Meshing, or FENSAP-ICE projects.

The Replay Control dialog helps you create, test, and edit script files by performing operations in ANSYS ICEM CFD and recording the equivalent Tcl/Tk commands in a Replay file. You can then use the dialog to step through and edit the script.
The Workbench Replay Control dialog works exactly the same as the standalone Replay Control dialog, with two key exceptions:
The Workbench Replay Control dialog supports Workbench Input Parameters and allows you to step through them.
The dialog automatically loads the current Replay script file (ICM.rpl) instead of opening a file browser.

For more information, see the Replay Scripts section in the ANSYS ICEM CFD Help Manual.
Using input parameters in Workbench enables you to pass data to ICEM CFD, while output parameters allow you to receive data back from ICEM CFD. The interaction of parameters between applications provides you with greater flexibility and capabilities to run optimization and what-if scenarios. For more information about using parameters in Workbench, see Working with Parameters and Design Points.
Parameters may be set globally or individually, with individual parameters taking precedence over global values.
You can perform the following operations involving parameters:
Setting Input Parameters
Setting Workbench Mesh Parameters for Parts
Setting Parameters for Prism Meshing
Setting Output Parameters
Setting User Defined Parameters
Deleting Parameters
Clicking the box to the right of certain Meshing Input parameters enables you to select whether the parameter is controlled from within ICEM CFD or from within Workbench. A “P” in the check box indicates that it has been selected as a Workbench Input parameter. If the check box is empty, you can control the input from within ICEM CFD.

You can set the following input parameters in Workbench:
Global Mesh Size (See Global Mesh Size in the ANSYS ICEM CFD Help Manual.)
Shell Meshing (See Shell Meshing Parameters in the ANSYS ICEM CFD Help Manual).
Volume Meshing (See Volume Meshing Parameters in the ANSYS ICEM CFD Help Manual).
Prism Meshing (See Prism Meshing Parameters in the ANSYS ICEM CFD Help Manual).
Surface Mesh Setup (See Surface Mesh Setup in the ANSYS ICEM CFD Help Manual).
Curve Mesh Setup (See Curve Mesh Setup in the ANSYS ICEM CFD Help Manual).
Edge Params (See Edge Params in the ANSYS ICEM CFD Help Manual).
Vertex Location (See Set Location in the ANSYS ICEM CFD Help Manual)
For Surface Mesh Setup, Curve Mesh Setup, and Edge Params, you can set parameters for all existing surfaces, curves, or edges at once; in addition to setting a parameter for a single surface, curve, or edge.
Parameterized edges and vertices (location) can be easily located in the graphics display. Use > , under in the Display Tree to color all parameterized edges red. Similarly, > will color the parameterized vertex number red.
Note: If you create Workbench Input Parameters and want to step line by line or using a line range through a replay file, you must use the item from the One-Click menu to start the Workbench Replay Control dialog.
To set input parameters in Workbench:
Within ICEM CFD, choose any of the input parameters listed above.
Select the check box next to the parameter.
Click the Yes button in the message dialog box to confirm the selection. A P in the check box indicates that the parameter has been created for Workbench.
Note: You will not be able to edit the parameter within ICEM CFD unless you click the check box again and deselect the parameter.
In Workbench, double-click the project’s Parameters cell.
Edit the parameter values in the Outline of Schematic: Parameters window.

Click the Project tab to return to the Project Schematic window.
You can now update the project using the new parameter settings.
Within ICEM CFD, open the Surface Mesh Setup, Curve Mesh Setup, or Edge Params parameters from the Tab menu.
Click the Select button at the top of the Parameters window.
Click the Left Mouse button to select the curve, surface, or edge for which you want to set parameters.
Click the Middle Mouse button to complete the selection.
The surface, curve, or edge you selected are listed in the selection entry.

Select the check box next to the parameter you want as the input parameter.
Click the Yes button in the message dialog box to confirm the selection. A P in the check box indicates that the parameter for the single surface, curve or edge has been created for Workbench.
Within ICEM CFD, open the Surface Mesh Setup, Curve Mesh Setup, or Edge Params parameters from the Tab menu.
Leave the surface, curve or edge selection field empty (do not select any surface, curve or edge).
Select the check box next to the parameter you want as the input parameter.
Click the Yes button in the message dialog box to confirm the selection. A P in the check box indicates that the parameter for all existing surfaces, curves or edges has been created for Workbench.
The Part Mesh Setup parameters enable you to specify the mesh parameters for different parts of a geometry. See Part Mesh Setup in the ANSYS ICEM CFD Help Manual.
To create a Workbench mesh parameter for a part:
Click the Mesh tab.
Click the Part Mesh Setup icon.
In the Part Mesh Setup dialog, choose a part and assign non-zero values to one or more of its parameters.
Click in the Parameter column for the part.
A dialog asks you to confirm that you want to create a Workbench parameter for each value you’ve changed.
Note: If any Workbench parameters are already set for the part, a dialog will ask if you want to delete that Workbench parameter.
Parameters assigned as Workbench parameters are highlighted in blue.

To delete a parameter, click in the Parameter column. A dialog will ask you to confirm that you want to delete each individual Workbench parameter in the row.
As with ICEM CFD, the Apply inflation parameters to curves and Remove inflation parameters from curves options affect Workbench parameter behavior as well. The current value of Apply inflation parameters to curves is saved to the project file/.aienv_options file, so it is always available in GUI or Batch mode.
You can add prism meshing parameters using the Part Mesh Setup dialog:
Click the Mesh tab.
Click the Part Mesh Setup icon.
In the Part Mesh Setup dialog, choose a part and check the check box in the Prism column.
Click in the Parameter column for the part.
A dialog asks you to confirm that you want to create a Workbench parameter for Part PARTNAME: Prism.
Note: If any Workbench parameters are already set for the part, a dialog will ask if you want to delete that Workbench parameter.
You can set Workbench Output parameters to:
list unstruct mesh and pre-mesh blocking quality metrics
list the number of mesh errors and possible problems
list the number of element and block types created.
You set the output parameters within the ICEM CFD application, then view them in either Workbench or ICEM CFD.

Within ICEM CFD, choose > > .
Optionally, click the Output quality metrics check box to select quality metrics.
Use the Quality Metrics drop-down menu to choose the metric you want to set.
Click the radio buttons to select the mesh types to check for the metric.
Optionally, click the Output number of elements check box.
Check the boxes next to the element types for which you want you want an output.
Optionally, click the Output Check Mesh check box.
Check the boxes next to the errors you want to have tallied in the output results. ICEM CFD will perform an analysis as part of the meshing process and list the results in the Output window and in the Workbench Parameters window.
Similarly, check the boxes for Output Pre-Mesh Quality and Output Number of Blocks to set the Blocking Output Parameters.
For more information about pre-mesh quality, see Determining the Pre-Mesh Quality in the ANSYS ICEM CFD User's Manual.
For more information about Hexa Block types, see Hexa Block Types in the ANSYS ICEM CFD User's Manual.
Within ICEM CFD, choose > > .
In the Workbench Output Parameters window, check one or more of Delete all quality metrics output parameters, Delete all number of elements output parameters, Delete all Pre-Mesh Quality output parameters, or Delete all Number of Blocks output parameters as required.
Click OK.
Setting User Defined Parameters gives greater flexibility and control over the meshing operation. For example, parameters that cannot be applied as single input parameters can be individually set with User-Defined Parameters.
Note: See the ANSYS ICEM CFD Programmer's Guide for information about using user-defined parameters with replay scripting.
Within ICEM CFD, choose > > .
In the Workbench User Defined Input/Output Parameters window, check the Create Input Parameter check box.
Enter a value for the Parameter name.
Enter a value for the Parameter. This value must not be empty.

Click Apply or OK.
You can edit this value in the Outline of Schematic: Parameters window.
Within ICEM CFD, choose > > .
In the Workbench User Defined Input/Output Parameters window, check the Create Output Parameter check box.
Enter a value for the Parameter name.
Enter a value for the IC Function.
The IC Function must start with
ic_geo_ or
ic_uns_ or
ic_hex_ and must return an
integer or a float value.

Note: See the ANSYS ICEM CFD Programmer's Guide for information about IC functions.
Click Apply or OK.
You can use this procedure to delete any input or output parameter, whether user-defined or otherwise.
Within ICEM CFD, choose > > .
In the Workbench User Defined Input/Output Parameters window, check the Delete Input/Output Parameter check box.
Use the drop-down menu to choose the name of the parameter you want to delete.
Click Apply or OK.
This example illustrates how you can use user-defined parameters to test different meshing scenarios for a simple box:
In the Workbench Toolbox, double-click the ICEM CFD component to start the data-integrated ICEM CFD component system.
Double-click the Model cell to open ICEM CFD.
First, create an Input parameter, ZSIZE, that you can manipulate from Workbench.
Choose > > .
Click Create Input Parameter.
Name the Parameter ZSIZE and set
the Parameter Value as
2.

Click OK to finish.
Now create a box model upon which you will perform a meshing operation. Record the process so the operation can be performed again when you update it from Workbench.
Click the Start Replay button.
Click the Geometry tab and choose Create/Modify Surface.
Choose Standard Shape from the Create/Modify Surface window.
Choose Box and click Apply.
Click the Mesh tab and choose Compute Mesh.
Choose Volume Mesh and click Compute.
Click Yes on the message dialog box to use autosizing for the mesh size.
Click the Stop Replay Recording button.
Choose > to save the project.
Next, edit the script to use the input parameter.
Choose Workbench Replay Control from the One-Click Replay Recording menu.
Click the Edit button.
Edit Line 15 (or whichever line is
appropriate), ic_vid_objectbox8 GEOM 00 {0 0 0} 1 1
1, to ic_vid_object box8 GEOM 00 {0 0 0} 1 1
[ic_wb2_get_parameter user_defined ZSIZE]
Choose > .
Close the Edit window.
Click the Save button and save ICM.rpl.
Click the Done button. Do not close ICEM CFD.

Now you can change the Input parameter through Workbench.
In the Workbench Project Schematic window, double-click the Parameters cell of the ICEM CFD component.
Change the value of ZSIZE to 5 and return to the Project tab.
Right-click the Model cell and choose Update.
You can watch the Replay script run using the new parameter in the ICEM CFD interface. Each time you change the ZSIZE parameter in Workbench, a new part will be generated and meshed with the new ZSIZE parameter value.
When you create a project that transfers ICEM CFD data downstream to a Static Structural system, data that is applied to the geometry, such as load data, is not transferred to the structural system. To work around this limitation, you can use a Finite Element Modeler (FE Modeler) system as a bridge between the two systems, then manually set the connections between them.
To transfer an ICEM CFD project to Static Structural:
Start with an ICEM CFD component.
Choose > to select an existing ICEM CFD project, or;
Drag an ICEM CFD component system into the Project Schematic window, then click the model to open the ICEM CFD Add-In and create your model.
Drag out an FE Modeler system and drop it on the ICEM CFD system.
Note that they are connected through the Model cell.
Drag out a Static Structural system as a Standalone system.
Tip: If you drag the Static Structural system out and drop it on the FE Modeler system, the two cells will link Model to Engineering data, and model information will not be passed downstream.
Drag the Model cell from the FE Modeler system and drop it on the Model cell of the Static Structural system.
Right-click the Model cell of the ICEM CFD system and choose Update.
Right-click the Model cell of the FE Modeler system and choose Update.
The model is now ready to use within Static Structural.