FLUENT - A possible procedure for modeling the soaking condition in automotive underhood simulations
The soaking condition would be the most challenging phase of the underhood simulation. Natural convection problems in general are highly unstable, because of the non-linearity due to strong coupling
between energy and the flow. The higher the temperature gradient, the more unstable the problem becomes. What makes it even more expensive is the transient simulation with radiation. Correct representation of the thermal mass of the engine becomes another problem. Another issue is the long time duration to be simulated (30 to 60 minutes) on mesh sizes ranging from 0.8 to 4.5 million cells!
The car is moving at a constant speed, and then it suddenly stops (with engine and cooling fan off). Then the car cools by natural convection.
Physically what happens:
As soon as the car is stopped, the flow develops very quickly, but the temperature of the solid cools down very slowly. So the time response for the flow is much faster than the time-response for the temperature. This was verified by runing a simple 2D case.
1. setup boundary conditions for forced flow with density as a function of temperature using incompressible-ideal-gas law
2. run flow equations (you may use k-omega turbulence with transition effects for natural convection)
3. run Energy and the Discrete Ordinates (DO) radiation model.
4. repeat above 2 steps until no changes to get the density variation
5. save case and data
6. setup boundary condition for natural convection
7. converge steady state solution of the natural convection flow. You may want to consider the following to speed up
1. iterate 100 times only DO and energy (2 energy iteration per 1 radiation iteration) using Uderrelaxation Factor (URF) of 1 for both.
2. iterate-to-converge DO and energy using URF of 0.8 for both
3. iterate flow 10 times (do no need to converge fully)
4. iterate 50 times only DO and energy (2 energy iteration per 1 radiation iteration) using Underrelaxatio Factor (URF) of 1 for both.
5. iterate-to-converge DO and energy using URF of 0.8 for both
6. repeat steps 3 and 4
8. save case and data into a new name
9. write out interpolated file for velocities, pressure, turbulence (File->Interpolate)
-select Write Data under Options
-select all fluid zones under Cell Zones
-select all variables except temperature under Fields
-click on Write
-provide name (flow-for-natural-convection.ip)
-click on OK
10. Read case and data for forced flow.
11. Read the interpolated file for the solid.
-Select Read and Interpolate under Options
-select fluid zones under Zones
-click on Read
-select the file flow-for-natural-convection.ip
-click on OK
Step 11 will overwrite only the flow field in the fluid and will leave the temperature unaltered.
12. Solve DO and Energy transient.
NOTE: Based on a simple 2d case of exhaust pipe and underbody (aluminum with thickness of 2mm), after the forced flow is stopped, the peak temperature occurs at about 90 to 100 seconds. And the flow due to natural convection becomes nearly steady at about 3 seconds.