Chip cooling ==> new solver available
Moderator: oliveroxtoby
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
Re: Chip cooling ==> new solver available
Hello,
Now it is ok for the convergence, thank you. The solver converges < 0.0001
I check y + for buoyantsimplefoam on the webb and it is very tricky.
https://www.cfd-online.com/Forums/openf ... error.html
I try to record the average temperatures from outlet and wall to be able to calculate exchanged powers.It is completly incoherent with y+ = 40 and the default wall function.
My case:
Duct with diameter of 100 mm lenght 2000 mm
Fluid air (default settings)
On wall heat exchange coef = 50 W/(m2.K) with Text = 290 K
Temp inlet fixed = 500 K with 2 velocities 5 m/s turbulent case, 0.1 m/s laminar case
Results
Turbulent case, air with v_inlet = 5 m/s
I obtain Toutlet = 301.9 K and Twall= 291.04 K
Pwall = 50 x 2 x pi x 0.05 x (291.04 - 290) = 33 W
Poutlet = (1.293 x 273 / 500) x 5 x pi x 0.05^2 x 1000 x (500 - 301.9) = 5.5 kW !!!
I try laminar case with y+ close to 1, it gives better results but it is again from from energy balance with tha same mesh.
Laminar case, air with v_inlet = 0.1 m/s
I obtain Toutlet = 298.4 K and Twall= 293 K
Pwall = 47 W
Poutlet = 112 W
I have done test cases with CHT solver in 2018, and I have differences lower than 25 % in energy balance on simple duct cases with very low y+ values.
To have a better understanding, I have try these 2 simple cases with a commercial software (in which the energy balance is respected) and results are very different...
Turbulent case: Pwall= Poutlet = 1284 W Toutlet = 449 K
Laminar case: Pwall = Poutlet = 94 W Toutlet = 322 K
Someone can give me advises how to run FC with buoyantsimplefoam solver please ?
Julien
Now it is ok for the convergence, thank you. The solver converges < 0.0001
I check y + for buoyantsimplefoam on the webb and it is very tricky.
https://www.cfd-online.com/Forums/openf ... error.html
I try to record the average temperatures from outlet and wall to be able to calculate exchanged powers.It is completly incoherent with y+ = 40 and the default wall function.
My case:
Duct with diameter of 100 mm lenght 2000 mm
Fluid air (default settings)
On wall heat exchange coef = 50 W/(m2.K) with Text = 290 K
Temp inlet fixed = 500 K with 2 velocities 5 m/s turbulent case, 0.1 m/s laminar case
Results
Turbulent case, air with v_inlet = 5 m/s
I obtain Toutlet = 301.9 K and Twall= 291.04 K
Pwall = 50 x 2 x pi x 0.05 x (291.04 - 290) = 33 W
Poutlet = (1.293 x 273 / 500) x 5 x pi x 0.05^2 x 1000 x (500 - 301.9) = 5.5 kW !!!
I try laminar case with y+ close to 1, it gives better results but it is again from from energy balance with tha same mesh.
Laminar case, air with v_inlet = 0.1 m/s
I obtain Toutlet = 298.4 K and Twall= 293 K
Pwall = 47 W
Poutlet = 112 W
I have done test cases with CHT solver in 2018, and I have differences lower than 25 % in energy balance on simple duct cases with very low y+ values.
To have a better understanding, I have try these 2 simple cases with a commercial software (in which the energy balance is respected) and results are very different...
Turbulent case: Pwall= Poutlet = 1284 W Toutlet = 449 K
Laminar case: Pwall = Poutlet = 94 W Toutlet = 322 K
Someone can give me advises how to run FC with buoyantsimplefoam solver please ?
Julien
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: Chip cooling ==> new solver available
y+ should be independent from the solver, otherwise this tutorial makes no sense:
https://www.youtube.com/watch?v=60fDz2cVdy8
(Aidan, if you read this: your tutorials are awesome!)
Some useful tools:
https://www.cfd-online.com/Tools/
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: Chip cooling ==> new solver available
Sorry, not yet. still learning...
I will try to rebuilt this
https://www.openfoam.com/documentation/ ... avity.html
http://info.tuwien.ac.at/cesbp/presenta ... shan-2.pdf
with FC to understand the solver. You will find the example in the bluecfd OF-tutorials.
Re: Chip cooling ==> new solver available
Thank you thschrader for your answer,
y+ value is dependant of what you want to calculate with your simulation. For drag and lift force (as describe in the video that you advise to me) the y+ value needs to be less than 5. It is also the case for energy exchange near walls.
The tutorial that you want to reproduce is far from my case, in which I have only forced convection in a duct. But it is interesting, and if you are able to get the same value than the tutorial, please let us know which parameters and BC you choose.
My understanding is, that for heat transfer with turbulence, y + need to be less than 1 and also resolve the flow without wallfunction.
That's why, I think, it is difficult with the current available settings of the cfdof buoyantsimplefoam solver to have realistic results. Modify by hand inside the openfoam case is needed. Ofcourse it is not a critical review against FreeCAD cfdOF work, which is very impressive and I am very happy to use cfdof. The user are also here to test and debbug things especially in opensource.
I will try to have coherent results with buoyantsimplefoam solver with forced convection and I let you know if I succeed.
Best regards.
Julien
y+ value is dependant of what you want to calculate with your simulation. For drag and lift force (as describe in the video that you advise to me) the y+ value needs to be less than 5. It is also the case for energy exchange near walls.
The tutorial that you want to reproduce is far from my case, in which I have only forced convection in a duct. But it is interesting, and if you are able to get the same value than the tutorial, please let us know which parameters and BC you choose.
My understanding is, that for heat transfer with turbulence, y + need to be less than 1 and also resolve the flow without wallfunction.
That's why, I think, it is difficult with the current available settings of the cfdof buoyantsimplefoam solver to have realistic results. Modify by hand inside the openfoam case is needed. Ofcourse it is not a critical review against FreeCAD cfdOF work, which is very impressive and I am very happy to use cfdof. The user are also here to test and debbug things especially in opensource.
I will try to have coherent results with buoyantsimplefoam solver with forced convection and I let you know if I succeed.
Best regards.
Julien
Re: Chip cooling ==> new solver available
To begin to confirm the simulation.
I have done an excel sheet with Colburn assumption in order to calculate the Nusselts number.
I obtain with the case parameters for temp outlet 443 K which is pretty close to the commercial software value.
I have done an excel sheet with Colburn assumption in order to calculate the Nusselts number.
I obtain with the case parameters for temp outlet 443 K which is pretty close to the commercial software value.
Re: Chip cooling ==> new solver available
Hello,
Let me share my results on buoyantSimpleFoam solver.
First I have mesh with Salome a 3 parts duct, 1000 mm with adiabatic wall for the mixing of the fluid, 2000 mm for the heat exchange zone (heat transfer coef) and 1000 mm more of adiabatic wall for outlet (I read this tip on cfdonline forum in order to have a good energy balance).
I start with laminar flow with bluecfdcore, the first cell layer at 1.3 mm. I add in the controlDict file postprocess tools to compute the average outlet temperature, pressure, mass flow and exchange power on the wall in order to be able to compare cases.
The results are in good agreement with commercial software and NUT analytic solution. The energy balance is good at less than 2 % BUT residualControl has to be decrease at 10^(-6) for energy h. The defaut setting 10^(-4) gives 25-30 % of difference between the power exchange on the wall and the power loss by the fluid (P=mCp(Toutlet-Tinlet)).
I switch on turbulent komegaSST model with bluecfdcore, first with wall functions by default used in cfdOF with y+ = 20.
The solution converged and the accuracy is very good between softwares and analytic result (with residualControl < 10^(-6) for energy h). But I need to change the fvScheme and fvSolutions files to achieve convergence. I notice a mistake in cfdOF when generating the case in the file "alphat" in the "0" directory, the object is instead of but it doenst generate warnings in log file.
I try also turbulent komegaSST model with bluecfdcore, first with y+ = 1 without wall function.
The simulation takes is quite longer but finishes to reach the same result the with the wall function. Everything is in order.
To finish I have run the same case 100% with cfdOF, meshing with cfMesh (adding manually postprocces utilities in the controlDict file for comparison) on the turbulent case but I am not able to converge. I see that the outlet temperature and the power exchaged on the wall are close to my previous results ...
I don't know if it is easy or not but it would be very cool to be able to choose some simple post process utilities via cfdOF, for example Temperature, velocity or pressure average on patches.
Julien
Let me share my results on buoyantSimpleFoam solver.
First I have mesh with Salome a 3 parts duct, 1000 mm with adiabatic wall for the mixing of the fluid, 2000 mm for the heat exchange zone (heat transfer coef) and 1000 mm more of adiabatic wall for outlet (I read this tip on cfdonline forum in order to have a good energy balance).
I start with laminar flow with bluecfdcore, the first cell layer at 1.3 mm. I add in the controlDict file postprocess tools to compute the average outlet temperature, pressure, mass flow and exchange power on the wall in order to be able to compare cases.
The results are in good agreement with commercial software and NUT analytic solution. The energy balance is good at less than 2 % BUT residualControl has to be decrease at 10^(-6) for energy h. The defaut setting 10^(-4) gives 25-30 % of difference between the power exchange on the wall and the power loss by the fluid (P=mCp(Toutlet-Tinlet)).
I switch on turbulent komegaSST model with bluecfdcore, first with wall functions by default used in cfdOF with y+ = 20.
The solution converged and the accuracy is very good between softwares and analytic result (with residualControl < 10^(-6) for energy h). But I need to change the fvScheme and fvSolutions files to achieve convergence. I notice a mistake in cfdOF when generating the case in the file "alphat" in the "0" directory, the object is
Code: Select all
object nut;
Code: Select all
object alphat;
I try also turbulent komegaSST model with bluecfdcore, first with y+ = 1 without wall function.
The simulation takes is quite longer but finishes to reach the same result the with the wall function. Everything is in order.
To finish I have run the same case 100% with cfdOF, meshing with cfMesh (adding manually postprocces utilities in the controlDict file for comparison) on the turbulent case but I am not able to converge. I see that the outlet temperature and the power exchaged on the wall are close to my previous results ...
I don't know if it is easy or not but it would be very cool to be able to choose some simple post process utilities via cfdOF, for example Temperature, velocity or pressure average on patches.
Julien
- Attachments
-
- fvSolution .txt
- (3.32 KiB) Downloaded 87 times
-
- fvSchemes.txt
- (2.21 KiB) Downloaded 88 times
- oliveroxtoby
- Posts: 812
- Joined: Fri Dec 23, 2016 9:43 am
- Location: South Africa
Re: Chip cooling ==> new solver available
Hi Julienjulieng wrote: ↑Wed Dec 16, 2020 11:02 pm Hello,
Let me share my results on buoyantSimpleFoam solver.
First I have mesh with Salome a 3 parts duct, 1000 mm with adiabatic wall for the mixing of the fluid, 2000 mm for the heat exchange zone (heat transfer coef) and 1000 mm more of adiabatic wall for outlet (I read this tip on cfdonline forum in order to have a good energy balance).
I start with laminar flow with bluecfdcore, the first cell layer at 1.3 mm. I add in the controlDict file postprocess tools to compute the average outlet temperature, pressure, mass flow and exchange power on the wall in order to be able to compare cases.
The results are in good agreement with commercial software and NUT analytic solution. The energy balance is good at less than 2 % BUT residualControl has to be decrease at 10^(-6) for energy h. The defaut setting 10^(-4) gives 25-30 % of difference between the power exchange on the wall and the power loss by the fluid (P=mCp(Toutlet-Tinlet)).
I switch on turbulent komegaSST model with bluecfdcore, first with wall functions by default used in cfdOF with y+ = 20.
The solution converged and the accuracy is very good between softwares and analytic result (with residualControl < 10^(-6) for energy h). But I need to change the fvScheme and fvSolutions files to achieve convergence. I notice a mistake in cfdOF when generating the case in the file "alphat" in the "0" directory, the object isinstead ofCode: Select all
object nut;
but it doenst generate warnings in log file.Code: Select all
object alphat;
I try also turbulent komegaSST model with bluecfdcore, first with y+ = 1 without wall function.
The simulation takes is quite longer but finishes to reach the same result the with the wall function. Everything is in order.
To finish I have run the same case 100% with cfdOF, meshing with cfMesh (adding manually postprocces utilities in the controlDict file for comparison) on the turbulent case but I am not able to converge. I see that the outlet temperature and the power exchaged on the wall are close to my previous results ...
This is really valuable feedback - thank you! Is there any chance you could share your setup as I would like to experiment with the default schemes so that this case would converge without any intervention?
Re: Chip cooling ==> new solver available
Hello,
The case is attached without the polyMesh folder (too big). The Mesh has been generated with Salome 9.5.
The residual control < 10^(-6) for h. It converges in 1800 iterations
In the controlDict file, the postreatment for wall power takes into account the variable density and thermal conductivity of the gas.
The is 1.25 % of difference between power exchange on the wall and fluid convected power.
Best regards
The case is attached without the polyMesh folder (too big). The Mesh has been generated with Salome 9.5.
The residual control < 10^(-6) for h. It converges in 1800 iterations
In the controlDict file, the postreatment for wall power takes into account the variable density and thermal conductivity of the gas.
The is 1.25 % of difference between power exchange on the wall and fluid convected power.
Best regards
- Attachments
-
- buoyantSimpleFoam_turbulent_compressible_without_polyMesh.zip
- (11.13 KiB) Downloaded 96 times
- oliveroxtoby
- Posts: 812
- Joined: Fri Dec 23, 2016 9:43 am
- Location: South Africa
Re: Chip cooling ==> new solver available
Thank you! Sorry to be a nuisance, but I was actually wanting the case setup that you did in FreeCAD/CfdOF (.FCStd file), so that I can try running in CfdOF using various tweaked settings similar to your successful setup, to hopefully achieve a better set of defaults.julieng wrote: ↑Fri Dec 18, 2020 8:09 pm Hello,
The case is attached without the polyMesh folder (too big). The Mesh has been generated with Salome 9.5.
The residual control < 10^(-6) for h. It converges in 1800 iterations
In the controlDict file, the postreatment for wall power takes into account the variable density and thermal conductivity of the gas.
The is 1.25 % of difference between power exchange on the wall and fluid convected power.
Best regards
Re: Chip cooling ==> new solver available
You are welcome, glad to contribute.
- Attachments
-
- pipe_3_morceaux.FCStd
- (67.99 KiB) Downloaded 118 times