Problem in Result in bottom outlet
 

Hello I have a question about boundary condition in a dam bottom outlet. Boundary conditions are given as follows:
Inlet1 (Water): pressure=1204000 pa
Inlet2 (Air): pressure=0 pa
Outlet: Pressure=0 pa
Problem is velocity value in air vent. Unfortunately, the speed obtained numerical model is much larger than the velocity in the physical model.
Also, the amount of air pressure in the tunnel after the gate have to be negative, while the pressure is zero at this point.
What is your suggestion to solve this problem?

http://alifallah92.persiangig.com/Capture.PNG

The air pressure in the air inlet and the outlet cannot be zero. There is going to be a small pressure difference across them which drives the air flow, but it will be tiny compared to the water inlet pressure.

But a more important point: Does this model need to be done as a multiphase model at all? At the massive pressure you have is the water confined to a known region at the bottom, so you could model this as a single phase water model (with the known free surface being modelled as a slip wall), and the air being modelled as a single phase with the free surface modelled as a wall with a tangential velocity equal to the water velocity?

What are you trying to learn with this model anyway?

A more accurate model is shown in Fig. As can be seen, there is a step in the model so that the air must be modeled in this situation.My goal is to compute the index Cavitation all over the tunnel.
The important thing is that flow before the gate is under pressure and after that is free surface.
Air duct air velocity calculated by the software is invalid.(about 120 m/s)While the speed limit is 50 m/s.
Where do you think the problem could be caused by?
This can be due to the size of the mesh or mesh type or incorrect boundary condition?
What is the correct boundary condition?(In Inlet1 pressure and flow rate is known.)
What is the correct initial condition?(For the initial conditions, the volume fraction of water before gate is assumed one and after that is zero. Also it is assumed that water velocity is zero.)
regards

http://alifallah92.persiangig.com/CFX2.png

This is an FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

I can see from the blockyness of your contours that your mesh is far too coarse. That is definitely one error, there may be others.

Thanks a lot for your kind help.

I have read the above file.
In a steady state, to achieve a reasonable answer, how many iterations are needed?
The answer does not converge to a residual set. What is the solution for this problem?
http://alifallah92.persiangig.com/image/Capture.PNG

This is an FAQ as well: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

physical time scale
 

How do you choose correct physical time scale?
FAQ said:
Use a larger physical time step. A time step approximately equal to the average residence time in the simulation domain is a good guide for most simulations. If it is a recirculating system without an inlet or outlet then use the turn over time of the largest flow feature. You can get the residence time in CFX-Post by placing a streamline and looking at the "Time" variable on it. The maximum value of time is the residence time.
Large and different quantities can be obtained with this method. Because I do not know what start from should be chosen in streamline window?
For example: 1.98e14 !!!!!
Which boundary should be chosen as start from? inlet1,inlet2,outlet,gate section or else?
Regards

As I said in the other post, start with auto time scale and use edit run in progress to increase it. Don't be timid, use time scale factors of 10, 100 or 1000. If it is too big it will start going numerically unstable. If it is too small it will take ages to converge or not converge at all.

I am really appreciate your help!:)

I used auto timescale with different timescale Factor.If it is greater than 12, the program gives error 255. With this timescale factor:
RMS U,V,W>1e-4
RMS air,water<1e-4
Velocity: is converged (50m/s)
Pressure is converged.
Imbalance: 0.04%
Is this an acceptable answer?
Why do not converge solution with increasing time step? Is it:
-The coarse mesh?
-Local effect?

Mesh used is as follows:
Mesh type: tetrahedral
Mesh sizing:
-Min size: .03
-Max face size: 1.5
-Max size: 2
Body sizing: .4 m
Face sizing: .2 m
Elements: 1602597
I used Aggressive, but the program gave Error.

I used High resolution in Turbulence Numeric, but the results did not change.

I used Blend factor .75 in Advection scheme , but the results did not change.

Rate is larger than .95. Is it a problem?

It is said MAX Residuals should be smaller than 1e-3 . Is it true?

It is said MAX should be one order larger than RMS? Is there this in my results?
I read manuals but:
:confused::confused::confused:

These pictures are added:

This question in an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Mesh quality will help, and I bet this simulation is not steady state anyway but requires transient for convergence. Just a guess, but I have seen this type of behaviour many times before :)

thanks.
Yes. I know my simulation is transient. At first I do so. But for compression with physical model I need to simulate steady.

thanks.
Yes. I know my simulation is transient. At first I do so. But for compression with physical model I need to simulate steady.

What do you mean by "But for compression with physical model I need to simulate steady."

Excuse me.
For Comparison with physical model I need to simulate steady.
I do not have result of physical model in different time.

If the simulation is really steady then a transient model will converge to the steady solution. So, as the FAQ says, try running transient and converge to steady state that way.

Is it correct that I simulate a steady simulation instead of transient?
How were pictures?

The FAQ I linked to explains it in detail. If you are having problems converging using a steady state model try a transient model. It often converges better and achieves your convergence tolerance. But you will need to run it for long enough to get the steady state result - if there is one.

Before I simulate steady state, I did transient. But this way last 10 days!
In addition, results are not logical. In this case air velocity in inlet2 is very high!
(120m/s)

if you have a free surface in this model, the elevation where the interface is expected need to have a nicely resolved mesh, ie. fine mesh. If the mesh volumes are too large the interface will be one large blur spread over several large elements. In icem I would just put in a mesh density box where I expect it to be.

this geometry also looks like a prime candidate for a hex mesh, if you are familiar with it. If not, that tetra mesh needs to be improved in both resolution and quality.

you try running single phase with water only to fill the channel? Run that and see what the flow looks like, adjust the mesh as necessary. Check those yplus, at those water velocities, the near wall spacing needs to be done properly. Once you get a stable and accurate single phase, steady state solution, start adding complexity.

Ali: Have you read the FAQ I posted ages ago? http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

There are many things you need to check to have an accurate CFD model, and the more complex it is the more things you need to check.

Hello mjgraf
thanks for your advice.
I just have free surface flow down stream of gate.(Not in the whole tunnel) In upstream of gate, flow is pressurized. Resolution for interface is mesh adaption(criteria adaption:water volume fraction ). But unfortunately, in the end of first step gives error. (for example after 50 iteration)!
I think I have to simulate this simulation with two phase model. Because I need to see air velocity in the air vent after my gate.
At first I use hexahedral mesh, but my results were not as good as tetrahedral mesh. (body sizing:.4m face sizing:.2m)

Hello Glenn
thanks for your advice too.
I have read FAQ precisely. It is said:
If these parameters are not changing to an accuracy tolerance suitable for your simulation then your simulation is almost certainly OK as it is and no further work needs be done.
For 100 percent gate:
My important parameters(I mean air velocity in air vent(inlet2) and pressure in the beginning of my tunnel(inlet1)) sufficiently converged even though my specified criteria(1e-4) has not been met.
air velocity: 50m/s
water pressure: 1e6 pa
For 20 percent gate:
In this opening of gate with the same mesh (applied in 100 percent) I wonder why my pressure is so small.(6e5) Where as it should be 1.2e6.
In this opening my mass flow rate in inlet 1 is 34000kg/s. but in the 100 percent opening was 232000 kg/s.

How are you modelling the gate?

It is indicated in the following picture.

my suggestion still stands. no harm in running it without air to check stability, etc.

also, what is the outlet boundary condition?

I assume that knife edge block off in the channel is your gate?
Air inlet is there the large arrow is located?

Yes it is. Knife edge is my gate. I emphasize tunnel before gate is pressurized.(is not free surface flow) and after gate is free surface flow.
My air inlet is large arrow in the picture. Boundary condition for this inlet is pressure=0.(VFWater=0 VFAir=1)

My main inlet boundary condition main inlet can be specific mass flow rate or specific pressure.(VFWater=1 VFAir=0) But I prefer mass flow rate.

My outlet boundary condition is Pressure=0 but, for prevent error A wall has been placed in portion of an outlet, I assume there is water with depth .2 m in outlet boundary.

According you I decided to use icem for meshing. May be it is useful. But what is yplus? and how do I check this parameter? and What do you indicated with this parameter?

Mesh quality is very important for free surface models. Improving the mesh will be worthwhile.

Why model the flow upstream of the gate? Can't you specify the flow at the gate accurately enough? This would save a lot of meshed area so your simulation runs faster.

What is important to me is velocity and pressure downstream of the gate for estimate cavitation index. I can simulate shorter length of upstream of the gate. It only have conducted to ensure of my model .


By the way, How can I improve mesh quality in this model?
I do not know why my results are not good with hexahedral mesh? It is as follows:
Mesh sizing:
-Min size: .03
-Max face size: 1.5
-Max size: 2
Body sizing: .4 m
Face sizing: .2 m
I cannot use smaller mesh because of limitation in my computer.
In your opinion , It is useful icem mesh for my work?
Thanks for your attention.

You need to do a mesh sensitivity study for any simulation. If it says that you need a finer mesh then you need to find a way, get a bigger computer or say the required simulation accuracy is not possible with resources available.

I would also do some simple studies using simplified geometries before tackling the true geometry. Find out how important mesh size and quality is.

thanks a lot.
I have a problem in CFX Solver. I want to use Hp MPI Local Parallel in Run Mode. But after little time solver was stopped.
If MPI CH2 Local Parallel is applied, I face with Error 255.
My system CPU has 2 core. Solver set 2 partition automatically.
What is the solution to this problem?
Is there any setting in advanced controls that I must do?

+--------------------------------------------------------------------+
| |
| Partitioning |
| |
+--------------------------------------------------------------------+




+--------------------------------------------------------------------+
| |
| ANSYS CFX Partitioner 13.0 |
| |
| Version 2010.10.01-23.02 Sat Oct 2 02:26:59 GMTDT 2010 |
| |
| Executable Attributes |
| |
| single-int32-32bit-novc8-noifort-novc6-optimised-supfort-noprof-nos|
| |
| Copyright 2010 ANSYS Inc. |
+--------------------------------------------------------------------+





+--------------------------------------------------------------------+
| Job Information |
+--------------------------------------------------------------------+

Run mode: partitioning run

Host computer: IDEAL-PC (PID:1568)
Job started: Mon Jul 15 14:05:01 2013


+--------------------------------------------------------------------+
| Memory Allocated for Run (Actual usage may be less) |
+--------------------------------------------------------------------+

Data Type Kwords Words/Node Words/Elem Kbytes Bytes/Node

Real 2207.3 8.82 1.59 8622.4 35.28
Integer 25007.7 99.93 17.97 97686.1 399.74
Character 3232.9 12.92 2.32 3157.2 12.92
Logical 80.0 0.32 0.06 312.5 1.28
Double 600.5 2.40 0.43 4691.4 19.20

+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+

Domain Name : Default Domain

Total Number of Nodes = 250240

Total Number of Elements = 1391859
Total Number of Tetrahedrons = 1391859

Total Number of Faces = 68792

+--------------------------------------------------------------------+
| Vertex Based Partitioning |
+--------------------------------------------------------------------+

Partitioning of domain: Default Domain

- Partitioning tool: MeTiS multilevel k-way algorithm
- Number of partitions: 2
- Number of graph-nodes: 250240
- Number of graph-edges: 3352988

+--------------------------------------------------------------------+
| Partitioning Information |
+--------------------------------------------------------------------+

Partitioning information for domain: Default Domain

+------------------+------------------------+-----------------+
| Elements | Vertices | Faces |
+------+------------------+------------------------+-----------------+
| Part | Number % | Number % %Ovlp | Number % |
+------+------------------+------------------------+-----------------+
| Full | 1391859 | 250240 | 68792 |
+------+------------------+------------------------+-----------------+
| 1 | 683140 48.9 | 125603 49.9 0.7 | 42855 62.1 |
| 2 | 713299 51.1 | 126330 50.1 0.7 | 26119 37.9 |
+------+------------------+------------------------+-----------------+
| Sum | 1396439 100.0 | 251933 100.0 0.7 | 68974 100.0 |
+------+------------------+------------------------+-----------------+

+--------------------------------------------------------------------+
| Partitioning CPU-Time Requirements |
+--------------------------------------------------------------------+

- Preparations 2.200E+00 seconds
- Low-level mesh partitioning 2.652E-01 seconds
- Global partitioning information 3.120E-02 seconds
- Element and face partitioning information 4.680E-02 seconds
- Vertex partitioning information 1.560E-02 seconds
- Partitioning information compression 1.560E-02 seconds
- Summed CPU-time for mesh partitioning 2.590E+00 seconds


+--------------------------------------------------------------------+
| Job Information |
+--------------------------------------------------------------------+

Host computer: IDEAL-PC (PID:1568)
Job finished: Mon Jul 15 14:05:05 2013
Total CPU time: 3.245E+00 seconds
or: ( 0: 0: 0: 3.245 )
( Days: Hours: Minutes: Seconds )

Total wall clock time: 4.000E+00 seconds
or: ( 0: 0: 0: 4.000 )
( Days: Hours: Minutes: Seconds )


+--------------------------------------------------------------------+
| |
| Solver |
| |
+--

Have you followed the parallel installation instructions in the documentation?

Can you run something simple (such as a tutorial) in parallel?

Thanks for your good advice.
Yes,I followed the parallel installation instructions in the documentation.

I try two problems in the tutorial, but I can not run in parallel. These problems had exactly similar errors!

furthermore,When I want to select Type of Run to Full, Full is selected and it is unchangeable! Is it a problem?

I have another question about Y plus. What should be the range of y plus? In my simulation this is 5000 to 140000. Is it correct?

You obviously have a fundamental problem with your parallel setup. These are just about impossible to fix on the forum so we will not be able to help you much. I would remove the software and reinstall, and if that does not work talk to CFX support.

As for y+, you should do a sensitivity analysis and find out. But for simulations where boundary layer behaviour is important that y+ is almost certainly too big.

"Indirect start method returned non-zero exit code"Error
 

Hi friends.
I use six computers for solving my problem.
I cannot understand why following error is appeared?
"Indirect start method returned non-zero exit code"

suggestion you check the installation manual for setting up and using distributed computing in windows.

your ERROR: looked clear in the solver manager, non UNC path.

multizone in meshing
 

thanks.
I have another question. When I want to use multizone for meshing, the following error appears.(indicated in picture)
I want to use hexa mesh in my simulation.
In your opinion what should I do for this problem?
Even I used various Free Mesh Type, but did not produce any mesh!

This question is best asked on the ANSYS Geometry and meshing forum.

But I can tell you straight away that your geometry will require a tet mesh, unless you go to an advanced hex mesher like ICEM.