Example of Extracting and Exporting a Table

This section illustrates how you would extract a table from one simulation to use as a boundary condition in another.

In this example, a channel flow simulation with periodic boundaries is used to create a fully developed channel flow profile. Values from an x-y plane cut across the fully developed channel are extracted into a table, exported and then used at the inlet of another simulation. This obviates the need to create a long inlet section in the second simulation to obtain the required fully developed conditions.

Create an xyz internal table. Make sure that the node of the new table is selected.

In the properties, set the Parts property by clicking the right half to activate the in-place object selector. In this example, plane section 1 is used.

Once you select the part, set the Scalars property. While the property allows text entries, it is much more convenient to use the property customizer ( ), which activates a scalars dialog.

This dialog works the same as the one you used for the part selection. In this example, Velocity: X-Component, Turbulent Kinetic Energy, and Turbulent Dissipation Rate are selected.

Extract the table data, then export the data to a .csv file.

In this example, the table is named inlet_rke.csv.

Open the simulation in which you want to use the profile. Then read the table file that you created in the other simulation.

In this example, the profiles that receive the data of this file are:

• Turbulent Dissipation Rate
• Turbulent Kinetic Energy
• Velocity: X-Component

They correspond to the scalars selected for the xyz table that was created earlier.

Open the Regions > [individual region node] > Boundaries > [individual boundary node] > Physics Values nodes, and select the profile node (Turbulent Dissipation Rate in the following screenshot).

Set the Method property to a tabular method (Table (x,y,z) in the following screenshot).

As a result of this action, the method node inside the profile node changes to a tabular method node. Its label matches the selection in the drop-down list, in this case Table (x,y,z). Select that node and set the Table property to the name of your table file. In this example, the name is inlet_rke.

Set the Table:Data property to the column of the scalar value, in this case Turbulent Dissipation Rate.

When you use Table (x,y,z) as the tabular method, once you set the Table and Table:Data properties, the other properties for the X, Y, and Z coordinates are read-only, since they map automatically to the columns in your table file with those headings.

In this example, in the same Physics Values node, these steps are repeated for Turbulent Kinetic Energy, its node depicted below.

In the same Physics Values node, a profile node for velocity is selected.

In this example, the velocity specification boundary condition has been set to Components, since only the X-component is being used in the table file. Hence, for this Velocity node, the Method property must be set to Composite, to use the composite vector profile method.

The next step, therefore, is to open the Velocity and Composite nodes. To use this approach, select the node of the components for which you want to plot data.

In this example, the X-component is selected, while the Y-component is a constant. (There is no Z-component because this case is two-dimensional.)

Set the Method property (Table (x,y,z) in the following screenshot).

As before, set the Table property to the name of your table file. Then set the Table:Data property to the column of the scalar value, in this example it is Velocity X-Component.

This completes the example of using a table file to transfer boundary conditions from one simulation to another.