[pashazanousi]

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

[ghorrocks]

Please attach your output file and some images of what you are modelling.

[pashazanousi]

Originally Posted by ghorrocks

Please attach your output file and some images of what you are modelling.

CFX Solver give followin error:
(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?

[AtoHM]

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.

[pashazanousi]

Thanks for your attention
A.jpg

[ghorrocks]

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.

[pashazanousi]

Originally Posted by ghorrocks

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.

I simulate the piston type wave maker with wall velocity(0.5cos(10*time)).I do it in transient Analysis type and active dynamic mesh in Unspecified.
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

[pashazanousi]

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

[ghorrocks]

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

[pashazanousi]

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

[ghorrocks]

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.

[pashazanousi]

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

[ghorrocks]

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

[pashazanousi]

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?

[ghorrocks]

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.

[pashazanousi]

Originally Posted by ghorrocks

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.

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?

[ghorrocks]

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.

[AtoHM]

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.

[ghorrocks]

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.

[pashazanousi]

Originally Posted by ghorrocks

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.

I just need some particles path...If I don't use VOF Model then How I simulate the free surface tank?...How I define materials and simulation setup?...I search Web,papers and every thing to learn but I can't...I'm confused
Untitled.jpg