+47 67 57 21 00
+46 21 470 35 50
ANSYS Tutorial: Profile Boundary Conditions
At boundaries as inlet and outlets, variables like temperautes, velocity, pressure, mass flow rate and so on, are usually implmented as constant values. It is more acurate to use experiamental results and create profile boundary conditions based on interpolation of values from data files. Another option is to create a profile boundary from results at some loction in a previous simualtion – this technique will now be explained.
This tutorial shows how to use a swiriling flow from an outlet region as an inlet condition in a new analysis.
Although both systems can be analyzed toghether, separating components in the project can be more efficient and allows different configurations to be analyzed without solving the swirling flow again.
Figure 1: Swiriling flow from an outlet region
Export the Boundary Condtion profile
Start from your result file from which you want to use a section plane as boundary conditions. Export the Boundary Condtion profile from the outlet region as shown in Figure 2.
Figure2: Result file in CFD-post
Choose a suitable name for the .csv data file, and select type and location of the boundary profile that will be exported. The BC Profile option enables you to select a profile type, while Generic option makes it possible to choose from both scalars and vector component.
Make sure that the coordinate frame is specified relative to which the data will be exported and mark the variables you wish to export, see Figure 3. Save the file before you proceed to CFX-Pre.
Figure 3: Select location and variables that will be used as boundary condtions.
Import the profile data into CFX-pre
Start CFX-pre and import the geometry that will be used in the next simulation. The .csv files saved in CFD-post can now be imported directly into CFX-pre. Click Tools > Initialise Profile Data and load the .csv file. See Figure 4 and 5.
Figure 4: Import the profile data which was saved in CFD-post.
Figure 5: CFX-pre reads the file and creates functions that points to the variables available in the file. Make sure that all data is loaded and close the panel.
Assign the profile data to the correct boundary
The data you now have imported will be available under User Functions. Boundary conditions can now be set by interpolation of these values.
Figure 6: The outline three will now contain the new boundary functions.
Create a boundary condition Inlet and assign the profile data to the boundary condition in the Basic Setting tab. See example in Figure 7
Figure 7: Detailed information of the loaded boundary conditions.
Check of that you want to Use Profile Data and press Generate Data. Make sure that the functions refer to the correct coordinate frame. See Figure 8
Figure 8: Assign the profile data to the correct boundary and generate the boundary values.
Moving on to the Boundary Details panel you can shift a profile by modifying the x, y, z values passed into the function. As an example you can change the y-component in INLET.Veloctity v(x,y,z) to INLET.Velocity v(x, y + 2[m],z).
Details of inlet in air in Flow Analysis 1:
Figure 9: Make sure that correct inputs are used in the Boundary Details tab.
Visualize the imported boundary conditions
The boundary conditions can be visualized in CFX-pre as shown in Figure 10. You can create a Boundary Contour or a Boundary Vector plot of the profile data.
Figure 10: Boundary plot of the velocity vectors.
Notice that this method interpolates the exported values onto the new geometry . Since the mesh on the boundary of the two models may differ, the transition can result in slightly changed values. This difference is usually imperceptible.
Do you want to learn more?
Please contact ANSYS Technical Support at EDR on +4 6757 2120 for technical questions, or ask for a sales representative for questions about licensing.
...or simply send us your contact information and we will get back to you:
You will also find more tutorials in our ANSYS Blog!