|
[Sponsors] |
Simulate horizontal agitators by momentum source |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Tural
Join Date: Mar 2019
Posts: 6
Rep Power: 7 ![]() |
Dear Users,
I am new CFX user and want to simulate aeration and mixing processes in wastewater tank. My model is an open mixing tank which contains 2 horizontal agitators in different location and air diffuser grid on bottom of tank. it is a batch tank model. Instead of using propeller for agitators, I have created subdomain 1 and subdomain 2 for each agitators. I used general momentum source and gave values (including low and high) to the proper momentum source component in order to obtain water flow inside tank. However, there is only water flow inside and around of subdomains. Water velocity in the tank is zero. I have seen and read relevant momentum source posts here but I still can not solve this problem. What might be the main reasons of zero velocity in the tank? As far as I understand from the relevant posts, momentum source is the one of the main methods used to initialize the fluid flow. Thanks in advance |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Please post an image of what you are getting and your output file.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 | |
New Member
Tural
Join Date: Mar 2019
Posts: 6
Rep Power: 7 ![]() |
Quote:
I uploaded screenshot of CFD-post which shows the velocity but output file size exceeds the limit. Zip file size with compressed docx is still more than allowed size. |
||
![]() |
![]() |
![]() |
![]() |
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
The output file is a text file. Just post it as is, compressed if needs be. Don't put it in Word.
Your image is very weird. It shows some flow local to what I presume are the impellers, but also some bands of flow as well. This appears to not be conservative. Are you sure it is converged?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#5 | |
New Member
Tural
Join Date: Mar 2019
Posts: 6
Rep Power: 7 ![]() |
Quote:
I have applied momentum source term approach with different values. The images of water velocity vector, plane and output file are below. I used "axial thrust of the mixers per cylindrical volume of subdomain" as a general momentum source and pictures, output file are belong to this method. The result of simulation shows that water velocity vectors move out from the subdomain and return to backside by creating recirculation zone around of the each subdomain. Also, I have used -C( Water.Velocity w - wspec) equation for momentum source term with momentum source coefficient. When I use high values such as C=10^5, max value of the velocity is too high which is not acceptable. Although water velocity is not zero inside the tank, there is recirculation around the subdomains again with very high speed(~100 m/s). it seems like after high speed recirculation around the subdomains, water flow destroy the barrier in front of them. By decreasing value of C, I got reasonable values for water velocity, but there was no fluid motion inside the tank except around of subdomains like previous picture. And still have water flow recirculation around subdomains in each case. What can be the reason of recirculation? Thanks in advance. Last edited by Thural; April 4, 2019 at 07:49. |
||
![]() |
![]() |
![]() |
![]() |
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Firstly - in my previous post I requested you to just post the output text file, not to put it in word. But you have put it in word again. This is the last time I will look at a word file, I will be ignoring any future word files.
You have not defined a source term coefficient. It is very difficult to converge without this defined. Your problems look like you are just getting poor convergence and this is explained by you not using a source term coefficient.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
Tural
Join Date: Mar 2019
Posts: 6
Rep Power: 7 ![]() |
Thanks for your quick reply. I have already used momentum source coefficient in my previous simulations and got similar results.
|
|
![]() |
![]() |
![]() |
![]() |
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Can I have a look at your output file again? Just post it as a text file, compressed if needs be.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#9 |
New Member
Tural
Join Date: Mar 2019
Posts: 6
Rep Power: 7 ![]() |
Good evening,
You can find it in the following ZIP folder. |
|
![]() |
![]() |
![]() |
![]() |
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
* You are using single precision. Double precision will help.
* You have defined the time step size. How did you work this out? If it was a guess it is almost certainly wrong. Adaptive time stepping is recommended, homing in on 3-5 coeff loops per iteration. (UPDATE: I see your run is converging with 6 coeff loops per iteration so it is not too far off, but still a little bigger than recommended) * You have not defined momentum source term coefficient. This is very important, it won't converge without this set correctly. * you have set max coeff loops = 16, min=6. The recommended settings is max=10, min=0. * Have you checked your convergence criteria is good enough? Have you done a sensitivity analysis? * You can try the coupled volume fraction solver. Sometimes that helps a lot. * You have second order time stepping. I would use first order while you do this basic debugging, and go back to second order once it is working reliably.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#11 |
New Member
Tural
Join Date: Mar 2019
Posts: 6
Rep Power: 7 ![]() |
Mr. Horrocks,
Thank you for your detailed explanation and help. I am going to implement your ideas on the simulation as soon as possible. |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
[swak4Foam] swak4foam for OpenFOAM 4.0 | mnikku | OpenFOAM Community Contributions | 80 | May 17, 2022 08:06 |
[foam-extend.org] Problems installing foam-extend-4.0 on openSUSE 42.2 and Ubuntu 16.04 | ordinary | OpenFOAM Installation | 19 | September 3, 2019 18:13 |
[swak4Foam] groovyBC in openFOAM-2.0 for parabolic velocity bc | ofslcm | OpenFOAM Community Contributions | 25 | March 6, 2017 10:03 |
[OpenFOAM.org] Error creating ParaView-4.1.0 OpenFOAM 2.3.0 | tlcoons | OpenFOAM Installation | 13 | April 20, 2016 17:34 |
centOS 5.6 : paraFoam not working | yossi | OpenFOAM Installation | 2 | October 9, 2013 01:41 |