|
[Sponsors] |
![]() |
![]() |
#1 |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
I want to simulate a Wave maker in CFX.
My model: http://cdn.persiangig.com/download/9nOrkdEsFh/A.png/dl I dont know why this error occur? (DP 0) Update of the Solution component in Fluid Flow (CFX) failed: The solver failed with a non-zero exit code of : 2 |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Please attach your output file and some images of what you are modelling.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 | |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
Quote:
(DP 0) Update of the Solution component in Fluid Flow (CFX) failed: The solver failed with a non-zero exit code of : 2 I don't know why this error occur? Analsis type is transient... I attach an Image of my proplem model and boundry conditions Image Link:http://cdn.persiangig.com/download/9nOrkdEsFh/A.png/dl I define two Domin...One for Water and the other for Air...I define the boundry conditions as Image attached...I define a Experssion for moving wall velocity(=0.001*sin(100*ctstep)). I think I should Initialize the VOF for the Domains but I don't know how? |
||
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
M
Join Date: Dec 2017
Posts: 692
Rep Power: 12 ![]() |
1) Attach your files directly to the forum ... people dont like links where they dont know what the target is.
2) Maybe a screenshot will resolve my question, but why do you need two domains? You can have both phases in one domain. 3) Setting up multiphase simulations and initialising the phases (specifically for water and air setup) is covered in the cfx tutorials. E.g. 10. Free-surface flow over a bump. |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
It is a bad idea to make a domain boundary align with a free surface. It means the difficult numerics of the free surface is placed right on the bit where coupling over the domain boundary is difficult (at the interface).
Make your simulation a single domain. The error messages you report are workbench level error messages which tell you nothing. You need to look in the CFX output file (.out) for the details. That is why I asked for the output file in the first place.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#7 | |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
Quote:
I think some thin is wrong...because result is not acceptable... I cant upload the video here... I upload some pdf and a video about my case in WE transfer: https://we.tl/t-fpARQ9vS97 https://we.tl/t-MYIlet5TUL |
||
![]() |
![]() |
![]() |
![]() |
#8 |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
i managed to simulate the wave maker model in cfx . but the desired results were not achieved . in fact , the results do not match with the theory . I did the simulation in accordance with the Article .I attached the paper file and simulation results link below.
https://we.tl/t-1vZ8kX5nql |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
I don't have time to look at your results file and I don't click on strange links either.
Post images directly on the forum, and attach your output file directly on the forum. If you don't know how to do this have a look at the FAQ: https://www.cfd-online.com/Wiki/Ansy...n_the_forum.3F
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#10 |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
thank you...I solve that problem myself...But I ask a quesion...
I want to plot a point's elevation of water free surface According to simulation time. for example I want to plot free surface elevation in x=20 from t=0 s to t=20 s. aaaaaa.jpg |
|
![]() |
![]() |
![]() |
![]() |
#11 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
To get the average water height on a surface you can work out the wetted area by areaInt(water.volume fraction)@surface. You can calculate the average water height from there.
You can also do a line integral on a vertical line to get height at a point.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#12 |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
Thank you...I have an other problem...
I want to select some particle of water to plot path vs time...how could I define some particle of water? I want to plot path of 10 particle in some planes with equal span in x direction... what should I do? Untitled.jpg |
|
![]() |
![]() |
![]() |
![]() |
#13 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
I assume you want these particles to follow the transient flow.
In that case you are going to have to rerun the simulation, you cannot do it post-processing. In the solver you have a few options: * (easy) Add an additional convection variable, initialised to zero everywhere but 1 at your seed points. They will then convect around the flow. The problem with this approach is you are not modelling particles as such and the additional variable will dissipate away eventually. * (harder) Define a lagrangian particle phase. Define the particles to have almost zero mess and lots of drag. You can then track their motions in the post processor. This will slow the simulation down quite a bit. * (have not checked if this is possible) I vaguely recall there is a massless particle option in CFX. This would be the best way of doing it, but I am not sure how it is done, or even if it really is possible. I will leave further research of this comment to you ![]()
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#14 |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
thank you...But How I should define particles?...I want to define 10 particles in@some plan to plot particles paths and Velocties...in CFX-Pre how I define these particles?
|
|
![]() |
![]() |
![]() |
![]() |
#15 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
The only way I know to seed a flow with lagrangian particles at specific locations is with a user fortran routine to set the particle locations.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#16 |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
OK....How I should do that?...I don't know what should I do...There are any tutorial for particle path in VOF Multiphase model?
|
|
![]() |
![]() |
![]() |
![]() |
#17 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
No, the VOF Multiphase model is a Eularian model. You don't want that one. You want the Lagrangian particle tracking model.
It has been a while since I looked, but I think there is an example fortran file in the CFX installation somewhere. Have a look in the CFX documentation for user fortran for particles.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#18 |
Senior Member
M
Join Date: Dec 2017
Posts: 692
Rep Power: 12 ![]() |
Just a short warning: the particle tracking model gives you HUGE result files depending on how many particles you have inside the domain. Easily reaches 10 GB an more for a .res file. Make sure you have the resources to handle this as well.
|
|
![]() |
![]() |
![]() |
![]() |
#19 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
The huge result files are when you have zillions of particles. From what I understand of this application there should only be a handful of particles, so file size increase should be minimal.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#20 | |
Member
Saeed Pashazanousi
Join Date: Mar 2020
Location: Iran
Posts: 66
Rep Power: 6 ![]() |
Quote:
Untitled.jpg |
||
![]() |
![]() |
![]() |
Tags |
ansys 14 cfx, cfx |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
wave maker | wave maker | CFX | 12 | July 10, 2020 04:35 |
Coffee Coffee Maker Station Ways to Make | lichypanta | Main CFD Forum | 0 | June 16, 2016 03:18 |
Simulating Ice Accretion in CFX | agner583 | CFX | 3 | February 11, 2014 00:50 |
solving ocean wave with Fluent or CFX? | gholamghar | Main CFD Forum | 1 | March 21, 2009 12:49 |
Question about the shock wave in CFX software | nucharin | Main CFD Forum | 1 | January 25, 2005 08:26 |