Download and run a simulation of a 3D complex branching duct system.
What You'll Need
Several demonstration CFD models are included in the Azore installation files. For this tutorial you need the files located in the directory AzoreCFD-Documents-->Azore-Tutorials-->3D-ComplexDuct-Full.
Step 1: Introduction
Review the geometry of the Complex Duct.
Step 2: Import the Mesh & Check Grid
Select File→Import, navigate to the Azore-Tutorials folder and import the complex duct mesh. Select Grid→Check Grid to perform a check on the mesh.
Step 3: Define Physics
Select Database→Equations and choose Standard K epsilon from the dropdown menu. Select Database→Fluid Materials to confirm air as the working fluid.
Step 4: Set Boundary Conditions
Navigate to Database→Boundary Conditions→Exterior Surfaces. Highlight the inlet surface, press the Edit button, and select Normal Velocity from the dropdown menu in the dialog box. Set the velocity to 10.6 m/s. Select Turbulence and choose Intensity and Hydraulic Diameter from the dropdown menu. Set intensity to 0.1 and hydraulic diameter to 0.067 m.
Change the boundary type of outlet-1 from pressure to flow. When the Flow dialog box appears, set normal velocity to 5.0 m/s, intensity to 0.1, and hydraulic diameter to 0.067 m. For the remaining pressure surfaces (outlet-2 to outlet-8), under Momentum, set pressure at 0 Pa. Under Turbulence, set intensity at 0.1 and hydraulic diameter to 0.067 m. Change the name of outlet-1 to inlet-1 by double clicking the surface name.
Step 5: Prepare Simulation Monitors
Navigate to Database→Solution Monitors→Point to set up a point monitor at coordinate (1.31132, 0.293405, 0.55625). Select the Field Type as Total Velocity.
Navigate to Database→Solution Monitors→Surface and specify 7 as the number of surface monitors. For each surface, select Mass Flow as the Field Type. For the first surface monitor, press the surface button and choose outlet-2 for the monitored surface. For the remaining surfaces (2-7), select the other monitored surfaces as oulet-3 through outlet-8, respectively. Save the database by selecting File→Save Database As
Step 6: Run and Monitor the Simulation
Select File→Start Run and set the number of iterations to 1000. Check the box to connect to the solver to monitor solution progress.
Once the simulation is running, view the residuals by selecting Display→Monitors→Residuals. To view the outlet mass flow monitors, select Display→Monitors→Add Monitor. Navigate to Properties→Select Monitors and highlight all the outlet mass flow monitors. Use the same process to display the point monitor for total velocity. When the simulation is complete, load the results for post-processing.
Step 7: Explore the Rendering Options – Mesh/Features
Under the Edges tab, highlight wall-0 to display, pressing Generate if necessary. Use the color button to change the color if desired. Change the radio button to All Mesh to see the full mesh of wall-0.
Step 8: Explore the Rendering Options – Edges
Select Exterior in the surface list to display all exterior surfaces and change the render type to All Mesh. Next, uncheck the Apply to All checkbox below the surface list. Click on “Clear” below the secondary list to clear the selections. Select only the outlet-2 surface and then change the color. With outlet-2 still selected and the color changed, select additional outlet- surfaces and they will change to the same color as outlet-2. Press clear again and select the wall_0 surface and change the rendering type back to Features. Clear again and select the inlet surface, then change it to a different color.
With inlet still selected, right-click on one of the outlet- surfaces and choose Select All with Same Properties. To return to rendering all edges the same, re-check Apply to All.
Step 9: Explore the Rendering Options – Faces
Return the display of edges to be only wall_0, rendered as Features in white. Then switch to the Faces tab. Make sure Face Color is set to By Type below the surface list. Then select Exterior in the surface list to select all exterior surfaces. Try adjusting the color, opacity, and lighting.
Next, change Face Color to By Surface and uncheck Apply to All. Try adjusting the color, opacity, and lighting for an individual surface. Turn the lighting on/off for all displayed surfaces by right-clicking on Lighting and selecting the pop-up menu.
Step 10: Explore the Rendering Options – Paths
Under the Paths tab, press the Initialize Paths button. Highlight the two inlet surfaces to display pathlines for these surfaces. Uncheck the Distribute box to increase the number of lines. To better control the spacing between lines, check the Distribute box and change the distance apart by using the up/down arrows. To view the data as a field, select Color by: Field to color the lines based on Total Velocity. The shape of the path lines can be changed from Lines to Cylinders.
To show movement, press the Go/Stop button. Alternatively, press Options and check Animate. Change the FPS (Frames Per Second), Time Interval, and other options to see the effects on the movement. The Stats button can be selected in the primary Paths tab to summarize time and distances statistics in the log message area for the drawn path lines from inlet(s) to outlet(s). Before moving to the next step, turn off the display of faces and return the display of edges to be only wall_0, rendered as Features in white.
Step 11: Explore the Rendering Options – Contours
Go to the Contours tab and highlight the surface interior-1_2. Check the display range box to change the limits to the range on that surface. Press the Units button, and change the velocity units from m/s to ft/s. Change the display Category to Pressure and the Field selection to Total Pressure. Check the display range box.
Step 12: Create a Cutting Plane
Navigate to Display→Views and position the model in +Y_axis_Z_up position. The Drag Cutting Plane creation tool can be used to dynamically define where to place a cutting plane through the model. Press the shift key and the hold the right mouse button and drag the rubber band line over the centerline of the upper ductwork. Upon releasing the mouse and pressing OK, a new surface default-plane-0 will now be listed under Post at the bottom of the surface lists. Select this surface and rotate the model to visualize the new cutting plane. Set the category to Velocity and the field to Total Velocity. Select a display range from 0 to 50 ft/s.
Add vectors by navigating to the Vectors tab and highlighting default-plane-0. Reduce the Distribute value by clicking the down arrow and check the In Plane box. You can also adjust the length and scale of vectors under this tab.
Step 13: Extract Numerical Solution Data
Go to Reporting→Surface Data to calculate data for a particular surface. Highlight the interior-1_2 surface and press Report to print the surface data to the Log Messages Area. Select outlet-4 and Mass Flow and press Report. Similarly, choose interior-1_2 and Area Weighting RMS to report the RMS for the total velocity on this surface.
Save the database before closing.