[Andrew Norfolk]

Hi,

I'm currently running a project in ANSYS Workbench where i'm generating thermal resistance curves for forced convection over a specific heat sink profile (varying the length of the heat sink extrusion and the inlet velocity). I am doing this using the parametric modelling feature which allows me to set up one numerical study and use identical settings for the mesh, setup etc. across all the simulations.

I have successfully run a total of 50 simulations which have output the required data for the varying inlet velocities and extrusion lengths.....

I have since noticed that I have not correctly defined the thermal resistance and need to modify the definition. When I try to change the definition it does not simply update all the thermal resistance values but rather wants me to rerun all of the simulations to get the results again! This should not be necessary as all the information needed to reevaluate the resistance can be found in the existing results file and I choose to retain all of the individual simulation data files (mesh, geometry, results etc.).

Does anybody know I can get all my design points to update their output parameters with having to re-mesh and re-solve each one?

Many thanks,

Andrew Norfolk

[Kapi]

You are basically running the model with different condition now hence it is asking you to re-run all the simulation again.
I dont think you can get results without re-running the simulations!

[Andrew Norfolk]

The thermal resistance value I have redefined is a CFD Post Processing output expression.

Thermal Resistance=(volumeAve(T)@HEATSINK-293.15[K])/power

Whereas before I made the silly mistake of forgetting to minus the input temperate:

Thermal Resistance=(volumeAve(T)@HEATSINK)/power

The way I see it, this expression can just be re-evaluated using existing results to solve the modified expression, there is no need to re-solve the entire problem as the physics has not changed!

[SalvusApfel]

Hey,
might be a bit too late but for future references:
Ansys Workbench supports the use of journals (Workbench -> File -> Scripting) which enables you to use python to update CFD-Post.
For example, I'm using this code to update 10 Desingpoints. Because the simulations are already done and I'd just added an additional CFD-post parameter, Ansys just updates CFD-Post module.


The code:

# encoding: utf-8
# 2020 R1
SetScriptVersion(Version="20.1.164")
for i in range(1, 10):
designPoint1 = Parameters.GetDesignPoint(Name=str(i))
Parameters.SetBaseDesignPoint(DesignPoint=designPo int1)
system1 = GetSystem(Name="CFX")
resultsComponent1 = system1.GetComponent(Name="Results")
resultsComponent1.Update(AllDependencies=True)


Regards