|
[Sponsors] |
How to perform a simulation with User Function |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
February 27, 2024, 15:06 |
How to perform a simulation with User Function
|
#1 |
New Member
Felipe Roque
Join Date: Feb 2024
Posts: 5
Rep Power: 2 |
Hi Folks!
There are some data i would like to use as input in my CFX simulation. My problem relies in a retangular resevoir and one small quadratic area in one of his face which is a boundary condition applied as heat flux. The data i have it's from a simulation my collegue perfom, which there are two columns time (s) and heat flux (W/mē). I usually use a fixed value as input of heat flux, but since i'm trying to perfom a more accurate transient analysis on my simulation i would like to use this data that i have. The normal procedure i use is: create a BC for heat flux>"boundary details"> "Options"> select "heat flux"> "Heat flux in "i added the fixed value i have, for example -400 W/mē". What i would like: create a BC for heat flux > "boundary details> "Options"> select "heat flux"> "Heat flux in "insert the data i have">. While i was searching i found that i need to create a "User Function" but when i create appears some boxes that i don't know what i should filled with. Like where "Argument Units", "Result Units"...and where i added the file containing my data i like to use? |
|
February 27, 2024, 16:34 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
You are using the correct function, you just need to specify the units correctly.
The argument unit is "t" as argument for looking up the function is time. The result unit is "W/m2" You can input this function in several ways, the way I do it is to set up the basic function and then edit the CCL of the function to copy/paste all the data points in. When you have this set up then you can just define your heat flux boundary to have the heat flux defined by the user function.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
February 27, 2024, 17:39 |
|
#3 |
New Member
Felipe Roque
Join Date: Feb 2024
Posts: 5
Rep Power: 2 |
When i set the "Result Units" to "W/m2" CFX return an error (see the img attch). I need to put the "W/m2" to "Wm^-2"?
|
|
February 27, 2024, 17:42 |
|
#4 | |
Senior Member
Join Date: Jun 2009
Posts: 1,860
Rep Power: 33 |
Quote:
for time.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
||
February 27, 2024, 17:53 |
|
#5 |
New Member
Felipe Roque
Join Date: Feb 2024
Posts: 5
Rep Power: 2 |
Okay, thx. I change the Argument Unit to "s" and Result Unit to "W m^-2" and works!
|
|
February 27, 2024, 18:49 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
Sorry, yes: the variable is "t" but the unit is "s". Thanks for correcting that.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
February 28, 2024, 10:22 |
|
#7 |
New Member
Felipe Roque
Join Date: Feb 2024
Posts: 5
Rep Power: 2 |
after the setup of "User Function" what should i do on "Solver Control" configuration? I ask this because the data mentioned have 5400s of simulation so i need to config this amount of time? i did some runnings but seams like the simulation don't stop when the limit of data are reached...i wounder why?
|
|
February 28, 2024, 16:58 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
You have set the simulation to run for 5400s of total time at 0.5s timesteps, so it should do those time steps and stop at 5400s (unless it stops with an error before this). Your user function has no effect on total simulation time - when your user function runs out it will do what you set the user function to do when it goes out of range (that is the "Extend min" and "Extend Max options") - this only sets what the user function returns, it will not stop the simulation.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
February 29, 2024, 05:48 |
|
#9 | |
Member
Evelyn
Join Date: Mar 2021
Posts: 32
Rep Power: 5 |
Quote:
__________________
biofluid mechanics;Hemodynamics |
||
March 1, 2024, 07:13 |
|
#10 |
New Member
Felipe Roque
Join Date: Feb 2024
Posts: 5
Rep Power: 2 |
thank you very much!
|
|
Tags |
ansys, cfx, data input, doubt, user function |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[mesh manipulation] RefineMesh Error and Foam warning | jiahui_93 | OpenFOAM Meshing & Mesh Conversion | 4 | March 3, 2018 11:32 |
[mesh manipulation] refineMesh Error | mohsen.boojari | OpenFOAM Meshing & Mesh Conversion | 3 | March 1, 2018 22:07 |
Version 15 on Mac OS X | gschaider | OpenFOAM Installation | 113 | December 2, 2009 10:23 |
Compilation errors in ThirdPartymallochoard | feng_w | OpenFOAM Installation | 1 | January 25, 2009 06:59 |
Problem with compile the setParabolicInlet | ivanyao | OpenFOAM Running, Solving & CFD | 6 | September 5, 2008 20:50 |