The Model Explorer allows you to copy and paste settings for the following objects (or group of objects):

• Boundary Conditions
• Volume Conditions (Properties)
• Initial Conditions
• Momentum Resistance Regions
• Multiple Reference Frame Regions
• Fan Models
• Macro Particle Settings
• Spray Injector Settings

The steps are similar to any other copy & paste procedure:

1. Select the object with the settings you wish to copy. It can be done by clicking on the object (BC/VC, Fan, etc.) in the Model Explorer or Viewer window.
2. Right-click the selected item. Choose "Copy ..." from the menu that pops up (see figure 1 below).

   
   

   Figure 1.  Copy/Paste feature in CFD-ACE-GUI

3. Select the objects (or a single object) on which you want to paste the settings. Right-click and choose "Paste from ..." as shown in figure 1.
4. Click "Apply" on the right panel to save the changes.

Tested with V2011.0

Figure 1.  Varying dihedral angle between adjacent patches

Generating a single domain volume mesh in CFD-VisCART for this case, with the ‘Preserve Features’ option activated, results in the surface mesh shown in figure 2. As can be observed, the boundary between the patches is captured very well where the dihedral angle is high, but as the dihedral angle decreases, the quality of boundary capture deteriorates.

Figure 2.  ‘Preserve Features’ option used with single domain mesher -
surface mesh shown

To address this issue, a new option called ‘Preserve Boundary Between Two Patches’ was introduced in CFD-VisCART V2011.0. It is available with the single domain mesher only and can be found under the Advanced tab in the Generate Mesh dialog, as depicted in figure 3 below. For the same model, activating this new option instead of the ‘Preserve Features’ option yields the surface mesh shown in figure 4. As can be seen, the boundary between the patches is captured along the entire length of the model.

Figure 3.  ‘Preserve Boundary Between Two Patches’ option

Figure 4.  ‘Preserve Boundary Between Two Patches’ option used with single domain mesher -
surface mesh shown

In addition to capturing explicit boundaries (boundaries between adjoining patches), this new option also enables the capture of implicit boundaries (for example, intersection of overlapping parts). Free boundaries though are not captured using this new option.

To summarize, if it is required to capture different types of features and boundaries in the model, our recommendation is to activate both the ‘Preserve Features’ and ‘Preserve Boundary Between Two Patches’ options for best results.

Tested with V2011.0

Suppressing an entity makes it invisible to the mesher during the mesh generation phase. The suppressed entity remains in the model and continues to be visible to the user. This allows for the quick and convenient addition/removal of parts to/from the final computational domain.

Below is an example of a car model where the simulation goal is to characterize the effects of the windshield position on the flowfield. Two simulations would be run, one for each windshield position, so the model contains two windshield parts. The second windshield part can be suppressed while the first is retained for the meshing phase, thus obtaining the first DTF simulation file. Then, another mesh can be generated by suppressing the first windshield and "unsuppressing" the second one, thus creating the second simulation file.

Figure 1.  Car model with two windshield parts

Figure 2.  Suppression option

Figure 3.  Mesh for each windshield position

The following entity types can be Suppressed/Unsuppressed:

• Geometry/Patches
• Domains
• Sources
• Gaps

NOTE: If you suppress a geometry part that has a source associated with it, you also need to suppress the source. Failing to do so will result in an unintended refinement in the mesh.

Note: tested with V2011.0

CFD-GEOM, an integrated geometry modeling and grid generation tool, supports the export of geometries and meshes in several different output formats. Traditionally,CFD-GEOM users have been able to write out ASCII STL files with consistent orientation from triangulated surface meshes. From V2008.2, CFD-GEOM also allows export of quad surface meshes (generated as structured or unstructured) into STL files. Quad facets are automatically split into triangles as per STL requirements. For structured meshes, only 2D blocks (not faces) can be exported.

Figure 1.  'Save STL files' option from File menu

These files can be opened later in any tool supporting STL files such as CFD-VisCART and CFD-VIEW for mesh generation or visualization purposes.

Figure 2.  Examples of exported STLs from triangular and quad surface meshes

The exported STL files can also be imported into CFD-GEOM as a discrete surface for further manipulations. A newly implemented discrete modeling engine in CFD-GEOM can import and manipulate meshed surfaces from several external grid formats.  Some of the available tools include:

1. Creation of discrete surfaces from lines and CAD surfaces
2. Extracting outlines and critical features
3. Split at outlines and critical features
4. Boolean operations on closed surfaces

Figure 3.  Discrete surface operations showing union of different closed surfaces,
intersection with a plane, and splitting using outlines and critical features

In future releases, CFD-GEOM users could expect more powerful features including re-meshing of imported discrete surfaces and tet mesh generation from re-meshed discrete surfaces.

A recent feature improvement makes working with cell-center data even more versatile, as it allows users to work with such data in batch mode. Indeed, the CFD-VIEW scripting function ImportDTF has been extended to include most of the options available from the GUI “Import Data File” facility, shown in figure 1 below. One of these added options is the “Cell” option, meaning that cell-center data can now be fully used with CFD-VIEW scripting, whether from the GUI or in batch mode.

Figure 1.  CFD-VIEW GUI “Import Data File” facility

The improved ImportDTF scripting function has the following prototype:

ImportDTF(filename, importMethod=DTF_ZONE_BASED, simnum=1, cell=0, spray=DTF_SPRAY_NONE, blanking=0, grouping=0, unscaled=0, nozero=0, animation=0)

Note that in usage, the names of the arguments should not be included, only the values should. For example if one wants to import a DTF in Zone Based mode, with Formatted Spray and Grouping options, one would use:

ImportDTF(“C:/docs/filename.DTF”, DTF_ZONE_BASED, 1, 0, DTF_SPRAY_FORMATTED, 0, 1, 0, 0, 0)

Example

Following is an example of a CFD-VIEW script that makes use of the ImportDTF function and the Calculator with cell-center data.

The simulation used is a 2D radial flow, as depicted in figure 2 below.

Figure 2.  Radial velocity simulation example -
Nodal velocity magnitude and vectors displayed

The script imports the DTF with cell-center data and calculates the cell-center radial and tangential velocity components in polar coordinates. It should be expected that the tangential component will essentially be zero, and that the radial component will carry the full magnitude of the velocity.

Below are the details of this script, which makes use of the improved ImportDTF function with “cell” option, as well as the extended calculator functionality for cell-center data support.

If you run this script in batch mode (<XCFD-VIEW -nogui -s polar_velocity.py>) and open the resulting MDL file, you can visualize the cell-center polar velocity components, presented in figure 3.

Figure 3.  Cell-center polar velocity components

You can download the DTF and Python script files used in the example by clicking on this link.

Note: tested with V2011.0