Exercise: Office & Energy in Simulation CFD
In the following exercise, a small office space will be simulated to determine temperature distribution and energy implications of a design change. It is common for many AEC applications, including this one, to consider fluid flow and heat transfer together (i.e., conjugate heat transfer) to evaluate system performance.
Upon completion, please consider reviewing this alternate AEC Tutorial.
- Provide a concise overview of the typical AEC simulation process in Autodesk Simulation CFD.
- Determine the impact in energy savings of replacing single-pane windows with triple-pane windows for this office space.
The simulation will have several simplifying assumptions to reduce overall complexity and expedite completion of this introductory exercise:
- Empty office space with no occupants or equipment thermal loads.
- Buoyancy effects (natural convection) and solar radiation transmitted through windows is assumed to be negligible.
- All external surfaces are adiabatic (i.e. insulated) EXCEPT for the 3 windows.
NOTE: Later on, these initial assumptions will be addressed as more detail is added to the office space simulation.
- Total flow rate: 158 cfm
- Based on ~4 air exchanges per hour for a room volume of 2,370 cubic feet
- Summer conditions
- Supply air temperature: 65F
- Outside (ambient) air temperature: 90F
Single-pane, steel frame
Triple-pane, steel frame
|2||Inlets||79 cfm each @ 65F|
|3||Outlet||P = 0 psig|
A Simulation CFD Exercise
1. Download the exercise file here.
2. Load CAD geometry
a. Open up the Simulation CFD interface and click New in the upper left ribbon to start a new study.
Note: Simulations can also be directly launched from within most popular CAD platforms, including Autodesk Revit and Inventor. More information can be found here in the help. In this case, we are directly loading a CAD neutral file format.
b. Click the Browse … button, navigate to the folder where the exercise file has been saved and select the file CFD-Intro-Exercise1-office.sat.
Tip: CFD simulations require considerable reading/writing to the hard drive and should always be run on a fast local drive; shared network or USB drives must be avoided.
c. Type in the design study name as “CFD-Intro-Exercise1-office” and then click the Create new design study button.
d. Right click the Scenario 1 node in the Design Study Tree to the left, click on Rename and type in “SinglePane” for the scenario name.
3. Assign materials to the domain volumes:
a. Select the Materials button in the ribbon. Click Select All in the Selection ribbon (or right-click in the graphics window and click Select All).
b. Click Edit in the ribbon Materials menu (or right-click in graphics window and click Edit) to launch the Materials dialog box. Make sure that the column to the right of Type is set to Fluid.
c. Click in the column to the right of Name and click Air from the pulldown list.
d. Click the Apply button to assign the material. The color (light blue) of the domains will change to match the color in the lower left corner of the graphics window.
4. Allow heat to enter/exit through the windows:
a. Change the setup task to Boundary Conditions by clicking the Boundary Conditions button in the top ribbon (or click the Boundary Conditions node in the Design Study bar to the left).
b. Click directly on each of the 3 surfaces which represent the windows as depicted below.
c. Click on Edit in the ribbon Boundary Conditions menu.
d. In the Boundary Conditions dialog that pops up, click in the column to the right of Type, scroll down the pulldown list and click on Film Coefficient.
e. Click Coefficient Units and set to BTU/ft2/h/R.
f. Enter a Film Coefficient of 1.18 to represent a single-pane window.
g. Set the Temperature Units to Fahrenheit.
h. Set the Ref Temperature to 90 and hit the Apply button. A stripe will appear on the window surfaces confirming that they have an applied condition. The color of this stripe matches the legend in the lower left corner of the graphics window.
TIP: A film coefficient applied directly to the air surface represents the U-factor of the wall, window, door, etc.
5. Allow air to exit the simulation domain
a. Rotate the model if needed to see the outlet. Zoom in and click on the surface representing the single outlet, pictured below. Click on Edit in the ribbon Boundary Conditions menu.
b. In the Boundary Conditions dialog, click in the column to the right of Type, scroll down the pulldown list and click Pressure.
c. By default, the pressure is set to 0 gage. Click the Apply button.
6. Specify the inlet conditions coming from the HVAC system:
a. Rotate the model to see the underside of the floor and click directly on the 2 surfaces representing the inlets.
b. Click Edit in the ribbon Boundary Conditions menu.
c. In the Boundary Conditions dialog, click in the column to the right of Type, scroll down the pulldown list and click Volume Flow Rate.
d. Set the Unit to ft3/min.
e. Enter a Volume Flow Rate of 79 and click the Apply button.
f. In the ribbon Selection menu, click Select Previous (or right-click in graphics window and click Select Previous) to reselect the 2 inlet surfaces.
g. Click Edit in the ribbon Boundary Conditions menu.
h. In the Boundary Conditions dialog, click in the column to the right of Type, scroll down the pulldown list and click Temperature.
i. Set the Temperature Units to Fahrenheit.
j. Set the Temperature to 65 and click the Apply button. The boundary conditions in the study bar should now appear as follows:
7. Define a mesh for the simulation domain
a. Click Mesh Size in the ribbon Setup Tasks menu and then click the Autosize button in the ribbon over to the right.
b. Click on the single large air volume representing the office space and click on Edit in the ribbon. Move the Size Adjustment slider to the left to approximately 0.50 and then click the Apply button at the bottom of the meshing dialog.
c. Zoom in as needed and click on the 3 small air volumes representing the 2 inlets and single outlet and then click Edit in the ribbon. Move the Size Adjustment slider to roughly 0.25 and then click the Apply button.
8. Assign solving parameters:
a. Click the Solve button in the ribbon
b. In the Control pane of the Solver dialogue, set the Iterations to Run to 300.
c. Click the Solution Control button, click the Advection … button, set the Advection scheme to ADV5. Click the OK button twice to return to the main Solve dialogue.
NOTE: Advection schemes are used to “tune” the solver for better accuracy and stability for certain applications. In this case, ADV5 is more adept at capturing flow recirculation and thermal stratification.
d. Click the Physics tab and then click on the box next to Heat Transfer to activate thermal calculations.
e. Click the Solve button to initiate the simulation. Once the solver starts, the interface automatically will go to Results mode and the ribbon menu will change.
NOTE: Depending on your hardware, it may take a minute or two for the solver to setup the model and initiate the solving sequence.
9. Results Visualization
a. While the simulation is solving, change the Global Result in the upper right corner of the ribbon from Velocity Magnitude to Temperature.
TIP: You can interact with the model and view preliminary results while the solution iterates to convergence, allowing any errors or omissions to be detected early on and corrected.
10. After the simulation is completed, clone the model to evaluate the following design change:
a. Right click on the SinglePane scenario, click Clone …, type in “TriplePane” and click on the OK button (or hit the Enter key).
b. Expand the Boundary Conditions branch in the Design Study Tree by clicking the small triangle to the left of Boundary Conditions.
c. Right click on the Film Coefficient boundary condition in the Study Bar and click on Edit …
d. Change the film coefficient from 1.18 to 0.39 to reflect the increased insulation of the triple pane window and click Apply.
11. Solve the cloned scenario
a. Click on Solve in the ribbon (or double click on the Solve node in the Study tree).
b. Click the Solve button to initiate solving.
NOTE: This performs a “restart” analysis from the end of the previous converged solution and solves faster since the flow field has already been developed. Changing the continue from option in the solver dialog to iteration 0 would start the analysis from the beginning.
12. Using the Decision Center to compare temperatures and the heat flux going through the windows:
a. Once the simulation has completed solving, click the Decision Center button in the ribbon (or hit the Spacebar once on your keyboard) to open the Decision Center bar in the lower left of the interface.
b. While still in Results mode change the Global result to Temperature if needed. Click on Summary Image once in the upper left corner of the Results ribbon. Note that a summary images is added to the Decision Center.
c. Now change the Global result to Wall Heat flux from Temperature and click Summary Image again.
d. In the Decision Center bar, right click the Design Review Center node and then click on Update all images.
e. In the Output bar in the bottom center of the interface, you will see 2 thumbnail images for Image 1 appear. Design1:SinglePane is already in the main graphics window. Click on the Design1:TriplePane thumbnail image and while holding the left mouse button down, drag it up to the main graphics window and release the button. The slider bar will now become active in the Output Bar. Move the slider back and forth and note how the temperatures on the windows are noticeably lower for the triple pane window.
f. Click on the Image 2 node in the Decision center and repeat the process of dragging the TriplePane thumbnail image up into the main graphics window. Using the slider, note how the heat flux going into the office also has been noticeably reduced with the triple pane windows.
|The left window in the SinglePane scenario has much more heat flux (mostly green on the legend) than the same window in the TriplePane version (light blue on the legend).|
Do these heat flux results make sense? Review the office layout again. Can you explain the reason why the window to the left has more flux than the other 2 windows? The answer is revealed in the summary below.
13. Evaluating Energy Implications
a. Click on the Wall Calculator button up in the Results ribbon to exit the Decision Center environment. Click on the 3 window surfaces, check the box next to Heat flux and then click the Calculate button. The total wattage entering the office space is approximately 40W.
b. Activate the SinglePane scenario by double clicking the SinglePane node in the Design Study Bar and then click on its Results node.
c. Repeat step (a.) above to calculate the flux entering the office with single pane windows. The wattage should read approximately 60W.
The triple pane window reduces the amount of energy entering the space by 20 Watts. This number can be used to calculate the total energy savings over a given period based on the time that the space is exposed to these conditions.
Did you come up with an explanation as to why the left window has more flux than the other windows? Heat flux flows in the direction of higher temperatures to lower temperatures and amount of heat flux is proportional to the difference of these temperatures. For the left window, the cold air inlet is centered below it so there is a plume of colder air directly behind this window (the inlet is located between the 2 windows in the other room). This plume of air increases the local temperature variation from outside to inside and results in a higher flux value. The velocity of the inlet air plumes can be visualized using planes or isosurfaces, as shown below:
|Velocity plumes from the supply inlets are visualized with cut planes on the left and by using an iso surface on the right.|
This is just one of the reasons why CFD insight is such a valuable asset for AEC applications. It directly reveals the hidden performance of complex situations that hand calculations, design guidelines, or intuition alone can miss.