Exercise: Boundary Conditions in Simulation CFD

To demonstrate the use of boundary conditions, the office space will now be enhanced with more detail, including wall and ceiling U-factors along with heat generation for the occupant and computer. The additional boundary conditions will more accurately depict reality and increase simulation fidelity.

Learning Objectives

  • Gain experience working with multiple boundary conditions.
  • Observe physical effects of boundary conditions in a model.

 

Assumptions

The simulation will have several simplifying assumptions to reduce overall complexity and expedite completion of this boundary conditions tutorial.

  • Time of day fixed with sun directly above the office.
  • Solar radiation transmitted through windows is assumed to be negligible.
  • Attic space (not shown) will dampen heat flux from the sun.
  • Floor is considered adiabatic (i.e. insulated).

NOTE:  Setup will begin from a support file where all setup tasks (except boundary conditions) will be defined. 

Simulation Parameters

  • Total flow rate:158 cfm, split between two air inlets (~4 air exchanges per hour)
  • Summer conditions
    • Room Inlet Temperature: 65F
    • Ambient Air Temperature (outside): 90F
  • Heat load from the seated person is 60 Watts
  • Computer generates 100 Watts with a fan pushing air at 60 CFM
  • Net solar load through the ceiling is 11 W/m^2/k

Simulation Process

1. Open share file

a. Open the Simulation CFD interface and click Open in the upper left ribbon to access the CFD-Exercise 3.cfz file which can be downloaded here.

NOTE: The .cfz file must be downloaded to a local drive with read and write privileges. When opened, a design study folder will be created in the same location as the .cfz file by default.

2. Specify the inlet conditions coming from the HVAC system

a. Rotate the model to see the underside of the floor and click on the 2 surfaces representing the inlets.


The above image shows two (2) inlets selected.

b. Click Edit in the ribbon Boundary Conditions menu.

c. Change the Type to Volume Flow Rate

d. Change the Unit to ft^3/min from the dropdown menu.

e. Enter a Volume Flow Rate of 79

NOTE:  Ensure the arrows indicate the flow direction as moving into the space, if the arrow on the inlet is not entering the space use the “Reverse Normal” button to correct the flow direction.

f. Click the Apply button.

g. In the ribbon Selection menu found in the setup tab, click Select Previous (or right-click in graphics window and click Select Previous) to reselect the 2 inlet surfaces.

h. Click Edit in the ribbon Boundary Conditions menu.

i. In the Boundary Conditions dialog, click in the column to the right of Type, scroll down the pull-down list and click Temperature.

j. Set the Temperature Units to Fahrenheit.

k. Set the Temperature to 65 and click the Apply button. 

3. Allow air to exit the model

a. Change the orientation of the model and select the outlet extension.


Above shows location for outlet pressure to be applied.

b. Click Edit in the Boundary Conditions section of the ribbon (or right-click in graphics window and click Edit) to launch the Boundary Conditions dialog box.

c. Change the Type to Pressure by clicking on velocity next to type and using the drop down menu.

d. The default 0 gage pressure value will be used

1. P=0 is a standard outlet condition

e. Click the Apply button to assign the boundary condition. 

TIP:  A stripe will appear on the outlet surface confirming that it has an applied condition.  The color of this stripe matches the legend in the lower left corner of the graphics window.

4. Allow heat to enter/exit through the windows

a. Click directly on the 3 surfaces which represent the windows.  Selected items are rendered as red (depicted in next image).

b. Click on Edit in the ribbon Boundary Conditions menu.


Three window surfaces selected is shown above.

c. In the Boundary Conditions dialog that pops up, click in the column to the right of Type, scroll down the pull-down list and click on Film Coefficient.

d. Click Coefficient Units and set to BTU/ft2/h/R.

e. Enter a Film Coefficient of .39 to represent a triple-pane window.

f.  Set the Temperature Units to Fahrenheit.

g. Set the Ref Temperature to 90 and hit the Apply button. 

TIP: A film coefficient applied directly to the air surface represents the U-factor of the wall, window, door, etc. 

4. Allow heat to enter/exit through the door:

a. Click on the surface which represents the door. 

b. Click on Edit in the ribbon Boundary Conditions menu.

c. In the Boundary Conditions dialog that pops up, click in the column to the right of Type, scroll down the pull-down list and click on Film Coefficient.

d. Click Coefficient Units and set to  BTU/ft2/h/R.

e. Enter a Film Coefficient of .64 to represent a 1 inch thick wood door.

f.  Set the Temperature Units to Fahrenheit.

g. Set the Ref Temperature to 90 and hit the Apply button.


The door selection is shown above.

5. Allow heat to enter/exit through most of the walls (inner faces between two spaces will be neglected as these are internal walls):

a. Click directly on the 6 surfaces which represent the walls.  Selected items are rendered as red as depicted in this image:


Above shows three surfaces of the exterior walls selected, rotate the model to select the other three.

b. Click on Edit in the ribbon Boundary Conditions menu.

c. In the Boundary Conditions dialog that pops up, click in the column to the right of Type, scroll down the pull-down list and click on Film Coefficient.

d. Click Coefficient Units and set to BTU/ft2/h/R.

e. Enter a Film Coefficient of .08 to represent R-13 wood stud wall.

f. Set the Temperature Units to Fahrenheit.

g.  Set the Ref Temperature to 90 and hit the Apply button. 

NOTE:  A Film Coefficient will be applied on the roof to consider solar heat being added that would have to pass through an attic space.  The same U-factor for our R-13 studded wall will be used with a reference temperature of the attic space rather than the outside ambient. 

5. Allow heat to enter through the roof:

a. Select the 6 surfaces of the raised ceiling

b. Click on Edit in the ribbon Boundary Conditions menu.

c. 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.

d. Click Coefficient Units and set to BTU/ft2/h/R.

e. Enter a Value of .08.

f.  Set the Temperature Units to Fahrenheit.

g. Set the Ref Temperature to 115 and hit the Apply button.  


Above shows the selections of roof for solar loading.

7. Apply heat generation from the computer.

a. Change the selection type to Volume (in the selection section of the ribbon or right click menu)

b. Hide the main air volume (CTRL+MMB)

TIP: If Volume selection is not active only surfaces will hide, not the entire volume.  Set selection to Volume, RMB -> Show All, and then hide the main air volume.

c. Select the computer.

d. Click Edit in the ribbon while in Boundary Condition Task.

e. Enter 100 W in the Total Heat Generation value section and hit Apply.


Image shows the computer selected.

8. Apply heat generation to the occupant.

a. Select the person.

b. Click Edit in the ribbon.

c. Enter 60 W in the Total Heat Generation value section and hit Apply.



Image shows the occupant selected.

The boundary conditions in the study bar should now appear as follows:


Above is the list of Boundary Conditions that should be in the design study bar (verifying the boundary conditions have proper values/units and a proper count of surfaces and volumes that they are applied to can save time instead of stopping and modifying settings).

Note: Mesh size and solver settings are already implemented in the share file (.cfz) to keep the emphasis on boundary conditions.

9. Solve the analysis

a. Click on Solve in the Ribbon.

b. Click on the Solve button

NOTE:  Exploring the results can be done while the model is solving or after the solve is finished.  Anticipate up to 1 hour or more for simulation to complete.

10. Change global Result

a. In the ribbon change the Global Result to Temperature using the dropdown menu

11. Create a Cut Plane

a. Click on the Planes task in the ribbon.

b. Click on the Add button..

c. Click on the plane and select the Y button which reorients the plane.

d. Right click on the Temperature Legend, in the Units menu select Fahrenheit.

e. Right Click on the legend again and select Options.

f.  Check the checkbox for User specified range at the top and type in 90 for the Max value and close the dialog box.

NOTE: Can you set the scale to help visualize thermal stratification in the space

Above shows the cut plane with the legend specified to a max of 90 F.

Summary

The additional environment and operational conditions considered and characterized by boundary conditions increase the fidelity of the results by accounting for more of the environment’s influence on the simulation model.

Accounting for the heat generated by occupants, equipment, and system U-factors in this exercise captures more reality and improves the fidelity of simulation results such as thermal stratification in the space.

AttachmentSize
Package icon cfd-exercise_3.zip3.41 MB