Manipulating Regions and Boundaries

In this section, you will combine the separate mesh blocks into a single contiguous mesh, then rename the mesh entities prior to continuing with the simulation.

In the intake window, open the Regions node.

You will see three separate regions, corresponding to the three mesh blocks that were imported.

Click to select each of the region nodes (Fluid_1, Fluid_1 2 and Fluid_1 3) in turn, and you will see that the selected region is highlighted and labeled in the Geometry Scene 1 display.

There are two alternative approaches for combining these regions so that information can propagate between them:

Create internal interfaces; or

fuse the regions and boundaries.

Using internal interfaces is advantageous if the mesh is to be manipulated further at a later stage, since interfaces can easily be deleted and created. However, there is likely to be some (most likely small) computational overhead associated with the interface. In this case, since the mesh will not need to be changed, we will combine the regions and fuse the adjacent boundaries, creating a single contiguous mesh. The process of "fusing" creates a (possibly non-conformal) interface, and then merges that interface into the mesh.

To combine the separate regions into one, use the <Shift><Click> approach to select all three region nodes.

Right-click and select Combine...

In the Combine Regions dialog, make sure all regions are in the Selected list box.

Only the top checkbox, Combine boundaries with similar names, should be ticked. In many situations, the Fuse adjacent boundaries option would also be used. However, in this case, the specified tolerance is not suitable for all the boundaries to be fused, so the fusing operations will be done later.

Click OK to combine the regions without fusing the boundaries.

Right-click on the Fluid_1 node and select Rename...

Change the name to Fluid. Click OK.

Now that the regions have been combined, you will fuse the adjacent boundaries that are currently separating the regions. The mesh is not conformal at these boundaries, so a non-conformal intersection needs to be computed as part of the fusing process. Essentially, an interface is created and then merged into the mesh.

The intersection process requires the specification of a tolerance. We will use the default value of 0.02 and then perform checks to ensure that this is suitable.

Before creating interfaces, the free-stream boundary types must be redefined as walls. This will allow the solution to be initialized without activating a flow model, normally a requirement of free-stream boundaries.

Open the Fluid > Boundaries node

Select all the free-stream boundary nodes: Free_Stream-31, Free_Stream-32, Free_Stream-4 and Free_Stream-6.

In the Properties window, set the Type property to Wall.

This will bypass the need to activate any models before initializing, the latter being a necessary step for testing the intersecting interface tolerance.

Select the Free_Stream-4 node, then Ctrl+click to select the Free_Stream-32 node (it is important to select the boundaries in this order)

Right-click and select Create Interface > In-place.

Open the resulting interface node, and select the Intersection node within the Physics Values node.

Click the

(Initialize Solution) button on the toolbar or select the Solution > Initialize Solution menu item.

To determine whether the test was successful, inspect boundaries Free_Stream-4 [In-place 1] and Free_Stream-32 [In-place 1] in the Geometry scene.

To gain access to them, first locate the Free-Stream 31 part by clicking on its node.

Right-click that part in the scene and select Hide.

Next, select the nodes of the two in-place interface boundaries, then click the

(Reset View) button on the toolbar to bring them into focus (zoom and rotate if necessary).

The parts appear intact, also showing that the interface was intersected correctly. This shows that the default tolerance value of 0.02 is the right one. Now delete the interface so that the boundaries can be fused.

Right-click on its node and select Delete.

Select the nodes of the Free_Stream-4 and Free_Stream-32 boundaries (in that order), right-click and select Fuse...

In the Fuse Boundaries dialog, make sure that these boundaries are in the Selected list box.

Click OK. You will notice that the nodes for both these boundaries disappear from the tree. This is because fusing boundaries incorporates them into the interior mesh grid.

Repeat the fusing process for the Symmetry-1 and Symmetry-7 boundaries (use the <Ctrl><Click> approach to select non-contiguous items). Again, use the default tolerance, 0.02.

Now combine (do not fuse) the Free_Stream-31 and Free_Stream-6 boundaries by selecting their nodes, right-clicking and selecting Combine. This creates a single free-stream boundary entity.

Select all the remaining symmetry plane nodes, right-click and select Combine.

Select the Wall-5 node and look in the Geometry scene. Click the

(Make Scene Transparent) button on the toolbar to see the part more clearly.

To correct this, right-click on the Wall-5 node and select Split Non-Contiguous.

Select the Wall-5 node and then the new Wall-5 2 node separately. The split action has made them into two separate boundaries.

Change the names of the boundaries to reflect their consolidation and indicate more clearly what they are.

Right-click on the Symmetry-3 node and rename it Symmetry.

Using the same technique as in the previous step, rename the other boundary nodes as follows:

Rename the Free_Stream-6 node Free_Stream.

Rename the Pressure-2 node Pressure.

Rename the Wall-1 node Cowl.

Rename the Wall-2 node Stbd Wall.

Rename the Wall-3 node Port Wall.

Rename the Wall-5 node Extension_Outer.

Rename the Wall-5 2 node Spinner.

Rename the Wall-6 node Extension_Inner.

This portion of the simulation tree should look as shown below when you are done.