ansys work bench

1. 1 © 2017 ANSYS, Inc. May 10, 2017
Workshop 04.1: Radiating System
18.0 Release
ANSYS Mechanical Heat Transfer

2. 2 © 2017 ANSYS, Inc. May 10, 2017
Problem Description
An aluminum section of a fin and tube heat
exchanger is to be analyzed. Since the model
represents an axially symmetric structure, a 90
degree section will be modeled.
The tube carries a contained hot fluid and the
interior wall is assumed to be at 300C.
The exterior surfaces experience a convective
condition.
We will add both convection and radiation
boundary conditions on the exterior surfaces to
evaluate the impact of heat losses due to each
mode of heat transfer.

3. 3 © 2017 ANSYS, Inc. May 10, 2017
Open Workbench and specify the unit system:
Metric (kg, mm, s, ºC, mA, N, mV)
Choose to “Display Values in Project Units”
Units Setup

4. 4 © 2017 ANSYS, Inc. May 10, 2017
• Open the Workbench Project
Schematic and choose a “Steady
State Thermal” analysis system
from the toolbox.
• Highlight the Geometry branch,
RMB, select Import geometry and
Browse ..., to file
“Fin_Tube_WS04.1.stp”.
• Double Click the Engineering Data
cell.
Model Setup

5. 5 © 2017 ANSYS, Inc. May 10, 2017
• You will be in the Engineering Data Application
tab. Activate the Engineering Data Sources
toggle and highlight General Materials.
• Add “Aluminum Alloy” to the current project
by pressing the “Add” button.
• Return to Project by pressing the Project tab.
• Double click the Model cell to open the
Mechanical application.
Model Setup

6. 6 © 2017 ANSYS, Inc. May 10, 2017
• Expand the Geometry branch and highlight the part
“FinTube”.
• In the details change the material assignment to
“Aluminum Alloy”.
A check in engineering data will confirm the aluminum’s
thermal conductivity property is temperature
dependent.
Preprocessing

7. 7 © 2017 ANSYS, Inc. May 10, 2017
• Highlight the mesh branch.
• Select the 2 symmetry faces, RMB > Insert > Sizing.
• Set “Element Size” to 2 mm.
• Highlight the mesh branch, RMB > Generate Mesh.
Preprocessing

8. 8 © 2017 ANSYS, Inc. May 10, 2017
• Highlight the “Steady State Thermal”
branch.
• Highlight the interior wall of the tube
section, RMB > Insert > Temperature.
• In the details for the temperature load enter
300 °C in the Magnitude field.
Preprocessing

9. 9 © 2017 ANSYS, Inc. May 10, 2017
Make sure surface select mode is active.
• In the graphics window, RMB > Select All.
• Use the control key and unselect the interior,
ends and symmetry faces of the fin tube
model (5 faces in all).
• You should have 33 faces selected.
• RMB > Insert > Convection.
Continued . . .
Preprocessing

10. 10 © 2017 ANSYS, Inc. May 10, 2017
• Enter a Film Coefficient = 5e-4 W/(mm^2-C) .
• Enter Ambient Temperature = 30C.
• Repeat selection steps from previous slide
(select 33 faces)
• RMB > Insert > Radiation.
• Enter Ambient Temperature = 30°C.
• Leave Emissivity = 1.
• Leave Correlation = To Ambient.
Preprocessing

11. 11 © 2017 ANSYS, Inc. May 10, 2017
Rt – Rc – Rr = Rtot 4785.2 – 4657.8 –127.43 = -0.03
• Solve:
• Highlight the Temperature, Convection and Radiation loads and
drag and drop them into the Solution branch, RMB > evaluate all
results:
• This is a shortcut to setting up reaction probes for boundary conditions.
• “Insert a Chart” with these three results selected, then the
results will be combined into a single chart & table.
• Analysis shows we have an energy balance.
Reactions show that radiation accounts for roughly 2.7% of heat losses from the system.
Solution

12. 12 © 2017 ANSYS, Inc. May 10, 2017
• If you have extra time, attempt to convert the To-Ambient radiation thermal
boundary condition to Surface-to-Surface (i.e. radiosity solver), as discussed
earlier.
Hints:
a) You will need to establish a Symmetry condition
(Periodic Region or Cyclic Region with a cylindrical
coordinate system) to achieve the proper view factors.
b) The enclosure should be “open” because the radiative
loss to ambient dominates.
c) Net loss due to radiation should be similar to the “To
Ambient” results obtained before.
Extra Challenge