Figure 1.  Multiple zones in decomposed domain.
Zonal interface outlines may visually overload the model

There are 3 methods you can use to get rid of these zonal interface outlines. As an example, let’s focus on one of the blades of the model depicted in figure 1. The current state of the blade with zonal interfaces is presented in figure 2 below.

Figure 2.  Unwanted zonal interface outlines

Method 1: Using the Simplifying DTF option when importing the DTF file

With the Simplifying DTF option available during DTF file import you can merge contiguous volumes of same type and name together, as well as contiguous boundaries of same type and name. However, you might loose the original surface topology with this method.

For the example used in this tip, all blade surfaces are named “Blade”, so using the Simplifying option will import each blade as one surface only (see figure 8 below). Therefore, if you choose to use this option, you be careful when naming the volumes and boundaries in CFD-GEOM or CFD-ACE-GUI.

Figure 3.  Blade made up of one surface after Simplifying DTF import

Method 2: Turning the Outlines off

If you do not want the zonal interface outlines to be displayed, you can simply select all the surfaces that share the outline(s), and turn them off by clicking the Outline on/off icon from the Display Settings bar. Note that this option does not change the topology in any way.

Figure 4.  Blade with all outlines turned off

Method 2: Method 3: Using the Merge Surface tool

This method enables you to recover the original surface topology, i.e. the way it was before domain decomposition. The following steps will walk you through the procedure:

1. Select the surfaces you want to merge (either from the 3D Viewer or from the Object Explorer).

   

   Figure 5.  Selection of the two surfaces to be merged

2. Click on the “Surface Merge” button from the Operator Palette. This creates a new surface called “Merged Surface”. Note that the surfaces you selected for the merging operation are not deleted.

   

   Figure 6.  Surface Merge option (left) and resulting Merged Surface (right)

3. Select the surfaces that you just combined (from step 1) and hide them (click on the Hide icon from the Display Settings bar, or do Ctrl+b).

   

   Figure 7.  Blanked before-combined surfaces

4. Select the Merged Surface you created in step 2 from the object explorer and color it with the desired variable (or perform any other operation).

   

   Figure 8.  Resulting merged surface

You can also combine steps 1 and 3 into one step simply by hiding the surfaces immediately after selecting them in step 1.

Figure 9 below shows the result after repeating the procedure for all of the split surfaces of the blade. The original topology has been recovered, and you can notice that the merged surfaces do not have zonal interface outlines, thus giving a cleaner look to your CFD-VIEW model.

Figure 9.  Blade displays original surface topology (as it was before decomposition)

Note: tested with V2009.4

By default, CFD-VisCART is in Surface Selection mode. To switch to the Facet Selection mode, click on the "Pick individual facet" icon on the ToolBar, as shown in Figure 1.

Figure 1.  Facet selection tool on the Toolbar 

Now, click on any facet on a surface and it will be selected (and highlighted). Hold the Shift key to select multiple facets or keep the Shift key pressed and drag a window to select all facets within a given area. These selected facets can now be blanked out by clicking the “Blank the selected item(s) ” button below the explorer window or by simply pressing Ctrl-B. Note that if you select the facets with the "Shift key pressed and drag window" method, all facets within that window will be selected, even the underlying ones that are inside the model.

The following example shows how selecting facets and blanking them out can help improve model visualization.

Figure 2.  Pipe model in CFD-VisCART

Figure 3.  Facets selected and blanked out to visualize pipe interior

The selected facets can also be deleted. This can potentially be used to cut-out or trim model surfaces.

Note: tested with V2009.4

The BC/VC Queries tool can be found under the BC/VC panel, as shown in figure 1 below.

Figure 1.  BC/VC Queries tool

To utilize this tool, simply choose if you want to pick, unpick, blank or unblank the interfaces by selecting the appropriate option from the first drop-down list. Then, from the second drop-down list, select the type of interfaces you would like to act on. Finally, click on Go.

A situation where this tool is very useful is when you are setting boundary conditions. Consider the example below, in which we would like to set all external boundaries as Walls. Figure 2 shows the outer faces in purple and the Fluid/Fluid interfaces in green. A simple Ctrl+A would be sufficient to select all outer boundaries, but doing so would also select the interfaces inside the model.

Figure 2.  Example geometry showing the outer faces (left) and block interfaces (right).

To avoid this, first make all faces visible and pickable. Then, go to the BC/VC Queries tool, select “Blank” and “Fluid/Fluid” Interfaces, and click Go. Now that all interfaces are blanked, you can go to the Boundary Conditions tab to set your BC’s and do Ctrl+A to select all outer faces and set them as Walls.

This tool becomes very useful when dealing with models that contain a large number of domains and boundaries. Below are some other examples of situations for which this tool can be handy.

• When you want to look at the meshed model, but the mesh has a very large number of cells and the Turbo viewing option is disable, it can take time for the graphics window to refresh after you rotate/pan the model. Use the BC/VC Queries tool to blank all interfaces and make the graphics window more responsive.

• When a half model or one-fourth model is made and you would like to translate/rotate it, there may be a chance that overlapping boundaries are created (for example if the rotation angle is slightly off). If there is a proper connection between the domains, the original outer boundaries will become interfaces. However, in case of overlap or duplication, they will stay as walls. You can use the tool to blank/unblank the interfaces and see if the translation/rotation was correctly done.

Notes:
- It is recommended to assign the volume conditions first (fluid, solid, or block) and then use the BC/VC Queries Tool.
- The BC/VC Queries tool only works for 3D models.

Note: tested with V2009.4

As an example, consider the case of simple flow through a 3D cross channel, as shown in figure 1. We would like to resolve the intersection region with 12 x 12 cells. However, we do not need this much grid resolution across the inlet and outlet channels away from the intersection region.

To use the block coarsening feature, one needs to carefully divide the geometry into several blocks, based on the areas that need to be coarsen. The yellow and blue regions in figure 2 indicate the block structure we will use for the problem; the yellow regions are the areas we wish to coarsen.

Figure 1.  Flow through cross channel	Figure 2.  Break up into multiple blocks

Follow the steps below to use block coarsening and reduce the total number of cells in the computational domain.

1. Grid all the blocks with the same number of cells, using the finest grid resolution desired; in this case, 12 cells across the width of the channel.

   

   Figure 3.  All blocks have 12 cells across the width (1104 total cells)

2. Select the Coarsen Structured Domains tool, found under 'Mesh → Structured Domain Options', as shown in figure 4.

   

   Figure 4.  Coarsen Structured Domains tool

3. Apply the desired coarsening factor (a factor of 2 in this example). The coarsening factor (i.e. amount of coarsening) in a particular direction must exactly divide the original number of cells in that direction. CFD-GEOM will only display valid values based on that principle. Figure 5 below depicts the block coarsening procedure.

   Pick the block handle. It turns red and the block orientation axes appear.	Upon picking the block, the coarsening menu appears. Choose a factor and press Apply.

   Figure 5.  Coarsening procedure

Figure 6 shows the result of this operation, which coarsened the top block.

Figure 6.  Top block coarsened by a factor of 2

You can repeat the same procedure for the remaining outer regions of the cross channel. The resulting grid is 20% smaller. Furthermore, the grid is still completely connected (no arbitrary interface).

Here are a few things to keep in mind when using block coarsening:

1. It is recommended that you plan for block coarsening while constructing your geometry. Because coarsening applies to entire blocks, it may be necessary to break a block into smaller blocks, some of which will be coarsened. It is easier to do this early in the grid generation.
2. To ensure that a good solution is obtained, try to restrict block coarsening to factors of 2 in 3D and 4 in 2D.
3. The amount of coarsening applied to a block is relative to the original structured grid (i.e. it is not cumulative).  For example, if you coarsen a block in its I-direction by a factor of 2, and then coarsen the block again by a factor of 2, the result is a coarsening by a factor of 2, not 4.
4. The amount of coarsening (i.e. coarsening factor) in a particular direction must be such that the original the number of cells in that direction can be exactly divisible by the factor. CFD-GEOM will only allow you to select factors from a set of valid values. However, when writing CFD-GEOM scripts, you must ensure that the amount of coarsening you specify is valid, otherwise coarsening will fail.
5. For 3D cases: The boundary faces of a coarsened block are not coarsened; only the interior cells are. This causes a coarsened block (and its neighbor, if any) to become unstructured zones upon output to the DTF file. This is also the reason why in CFD-GEOM, CFD-ACE-GUI and CFD-VIEW you will see uncoarsened boundary faces on a block that you have coarsened, as shown in the figure 7 below.

   

   Figure 7.  Coarsened block showing uncoarsened boundary grids

The block coarsening feature is a very useful capability, allowing you to reduce the grid size and therefore the run time for a structured grid system, without introducing arbitrary interfaces.

Note: tested with V2009.4

CFD-ACE+ allows the user to work with particles of pre-defined shapes like sphere, spheroid, cube, cuboid, cylinder and cap cylinder (i.e. capsule) quite easily from built-in macro particle geometries available in CFD-ACE-GUI. For such built-in regularly shaped macro particles, CFD-ACE+ will assign Surface Marker points based on the Marker point density specified by the user (either from the GUI, an input file, or a user subroutine).

Additionally, CFD-ACE+ allows modeling of closed and open macro particles of arbitrary shape. An example of an open arbitrary macro particle would be a beaded string of point-mass particles of say colloids, macro-molecules and cells where there are gaps between two point-masses through which flow may pass. Please refer to CFD-ACE+ User manual for more details of Macro Particles. The shape of such arbitrary particles is entirely defined by the marker points position, which are fed to the solver through either an external input data file (*.dat file) or the user subroutine ‘upoint_init’.

This tip explains as how to define an arbitrary macro particle in CFD-ACE+ from the input data file.

First, you need to create the data file that contains:

• The macro particle name.
• The number of initial condition variables.
• The variables list for macro particle initial conditions.
• The number of marker points.
• The marker points specification. Each line corresponds to one marker point, and lists the variables value one by one separated by a 'tab'.

A section of the input file format for a closed wedge (or prism) shaped macro particle is given below.

Then, this file (or its path) should be specified in the GUI, as shown in figure 1 below:

Figure 1.  Reading the input file for an arbitrary Macro Particle in CFD-ACE-GUI

You can view the simulation results animation by clicking on figure 2.

Figure 2.  Wedge Macro Particle falling under gravity forces

You can download the files used in this 3D example by clicking here.

Note that:

• In the data file, there should be a space between the Hash sign (#) and the next character.
• The Particle name in the data file should match the particle name in CFD-ACE-GUI (“Arb_mac” in this case).
• When defining an open arbitrary macro particle using Marker Points, the diameter of the Marker points should not be zero, or the mass of the macro particle would be zero.
• When defining an arbitrary macro particle, the user should make sure that the marker points are non-collinear (do not lie on a straight line). At least one marker point should deviate slightly.
• Contrary to pre-defined macro particles, arbitrary macro particle cannot be displayed in CFD-ACE-GUI. Therefore, users will be able to see what the particle looks like only in CFD-VIEW.

Note: tested with V2009.4