|
[Sponsors] |
![]() |
![]() |
#1 |
Member
Sara
Join Date: Nov 2020
Posts: 44
Rep Power: 5 ![]() |
Hi everyone!
I am simulating a model, and is only interested in the heat transfer behavior. I need to do a lot of simulations and due to limited time and space on my computer I was wondering if it was possible to reduce the computational calculations as I am only interested in the heat transfer. Thank you much ![]() |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
Join Date: Nov 2015
Posts: 246
Rep Power: 11 ![]() |
Replace Fluid domains with convection BC.
|
|
![]() |
![]() |
![]() |
![]() |
#3 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
You can freeze the fluids and turbulence by setting expert parameters:
solve fluids = f solve turbulence = f Then CFX only solves the remaining equations, like energy. In this way, you can solve a temperature field in a frozen flow field with various boundary conditions. This is of course only valid if the coupling between energy and fluids is negligible. |
|
![]() |
![]() |
![]() |
![]() |
#4 | |
Senior Member
Join Date: Jun 2009
Posts: 1,850
Rep Power: 33 ![]() |
Quote:
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
||
![]() |
![]() |
![]() |
![]() |
#5 |
Member
Sara
Join Date: Nov 2020
Posts: 44
Rep Power: 5 ![]() |
Hi
I am not expert in CFX and therefor as the manual recommend I should not change the expert control parameters if I am not experienced. Would you mind giving me a step by step description on how to change these parameters? |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Member
Sara
Join Date: Nov 2020
Posts: 44
Rep Power: 5 ![]() |
I was wondering if it was possible to do it that way.
CFX-pre --> "output control" --> "Resuls" --> for "option" --> selected variables for "output variable list" --> temperature Is it possible? |
|
![]() |
![]() |
![]() |
![]() |
#7 | |
Senior Member
Kira
Join Date: Nov 2020
Location: Canada
Posts: 435
Rep Power: 8 ![]() |
Quote:
To change the expert parameters, right click on the Solver folder and choose "Insert>Expert Parameter". Most of the parameters will appear in the GUI panel that comes up. If you need one that doesn't come up (i.e. an undocumented one), just add any of the ones shown to create the Expert Parameter object then right click on it and choose "Edit in Command Editor" to insert the parameter manually. |
||
![]() |
![]() |
![]() |
![]() |
#8 |
Senior Member
Kira
Join Date: Nov 2020
Location: Canada
Posts: 435
Rep Power: 8 ![]() |
Sure, it is possible but defeats the purpose of your question, since this would not reduce the number of computational calculations. Monitor points just monitor specified parameters, it would still calculate everything else as normal.
|
|
![]() |
![]() |
![]() |
![]() |
#9 | |
Member
Sara
Join Date: Nov 2020
Posts: 44
Rep Power: 5 ![]() |
Quote:
Can the monitoring option not reduce the simulation time my simulation takes approximatly a whole day right now and takes a lot of space on my harddisk ![]() |
||
![]() |
![]() |
![]() |
![]() |
#10 | |
Senior Member
Kira
Join Date: Nov 2020
Location: Canada
Posts: 435
Rep Power: 8 ![]() |
Quote:
You can try it out ![]() ![]() The only other way I can think of to only calculate certain parameters is to write and implement your own code, specifying what you want the solver to calculate (I've only done this once). |
||
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
As I mentioned earlier, in a frozen flow field, you can solve the energy equation solely by setting the other equations to false. Then since you only solve an energy equation that is not coupled to anything, you can simply increase the auto time scale from 1 to 10, 10000, 100000, or what so ever. Just give it a try untill you pushed it too far. Then the solver solves the equation at very high speed for you in a short period of time. You only need to make absolutely sure that:
- your energy residuals are low - the temperature in your monitoring points are constant. - your energy imbalance is zero (energy in = energy out). Then you can be sure that your energy equation is solved accurately. And again, remember your flow is frozen, so your solution only makes sense if there is no coupling between energy and any other variables. If you have an ideal gas, then you are already in trouble. Same hold for an temperature dependent viscosity. But judge for yourself. Don't hesitate to use expert parameters. You are already an expert since you are suspicious on the action that you take. Credits for you. |
|
![]() |
![]() |
![]() |
Tags |
heat transfer, reduce, space, time |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
LES Setting up Sensors on Model: Do I Need the Time Averaged or Also Space Averaged D | kepler123 | Main CFD Forum | 8 | February 7, 2020 18:31 |
higher order time and space discretisation for elliptic eq. with a transport eq. | emjay | Main CFD Forum | 1 | August 20, 2019 16:50 |
Run OpenFoam in 2 nodes of a cluster | WhiteW | OpenFOAM Running, Solving & CFD | 16 | December 20, 2016 00:51 |
Richardson Extrapolation to check time and space convergence | Hooman | Main CFD Forum | 0 | December 29, 2010 08:19 |
Time and Space Derivatives. | beezee99 | FLUENT | 0 | August 19, 2010 01:34 |