[ghorrocks]

Are you in China? If so then I suspect your government has blocked google which means my google drive link does not work.

[zhihuawan]

Originally Posted by ghorrocks

Are you in China? If so then I suspect your government has blocked google which means my google drive link does not work.

Yes,you are right,I am sorry that our country has block the google,I think the only way is to send the screen capture pictures to the CFD online,I know it is very disturbing you,if you are convinent ,I would hope you could help me,I am glad to recognize you ,you are friendly ,I wonder if the MSN can send to you ？Thank you.

[zhihuawan]

Originally Posted by ghorrocks

Are you in China? If so then I suspect your government has blocked google which means my google drive link does not work.

0GXL7ATS6FM8${%7UOL]Y7Q.png
IMG_4879.jpg
1Y)U(S9]N}LU}TSOKAM24.png


you can see my model ,in my model ,I choose the gas inlet,liquid inlet and outlet as a periodic interface,but the mass flow is to the all face ,I cannot give it to the liquid face,how can you solve it ?Thank you.

[ghorrocks]

As water has 1000 times the density of air, if you specify the water mass flow rate as the total mass flow rate you will not be off by much. Other errors will be larger than that.

[zhihuawan]

Originally Posted by ghorrocks

As water has 1000 times the density of air, if you specify the water mass flow rate as the total mass flow rate you will not be off by much. Other errors will be larger than that.

What is "off by much",I cannot understand your meaning,the mass flow is neither to the water nor to the air ,I do not know which fluid it will refer to, and I know this setting is wrong ,I want to see how you setting this mass flow rate ,maybe your model is different from me,can you send your setting images like my images sent to you to me ,thank you very much.

[ghorrocks]

If you say the flow rate is 1kg/s for water, but that is spread over a volume fraction of 50% water and 50% air, then you will be off by about 1 in 1000 from the density difference. That is a negligibly small error in most cases. So it is not worth spending much time fixing it as the error is very small. Spend your time on much larger errors like mesh refinement and convergence tolerance.

I have removed the results files from the example and this has made it small enough to email. Please PM me your email address and I will send it to you.

[zhihuawan]

Originally Posted by ghorrocks

If you say the flow rate is 1kg/s for water, but that is spread over a volume fraction of 50% water and 50% air, then you will be off by about 1 in 1000 from the density difference. That is a negligibly small error in most cases. So it is not worth spending much time fixing it as the error is very small. Spend your time on much larger errors like mesh refinement and convergence tolerance.

I have removed the results files from the example and this has made it small enough to email. Please PM me your email address and I will send it to you.

Thank you for your kindness.but I want the the volume of the liquid inlet is 100% ,the volume of the gas inlet is 100%,if I give the mass flow rate ,I cannot set this.My email is wanzhiha@stu.xjtu.edu.cn,
another email is hitzhwan@163.com，thank you very much.

[ghorrocks]

I have just emailed you the file. I have removed the results files so it is small enough to email.

[zhihuawan]

Originally Posted by ghorrocks

I have just emailed you the file. I have removed the results files so it is small enough to email.

I am extraordinary grateful for your sending the file to me, I find you are very intelligent to use the step function to solve the liquid and air inlet in the steady calculation,we can see a clear gas-liquid interface in the figure 1,but when I use your transient calculation with the result of steady result，the caculation step is about 300(Figure 2) ,but I find the clear interface of air and water is not clear,they are mixtured together,so I the uniform mass flow is not available way to solve the probelm, do you think so?Thank you very much.

[zhihuawan]

Originally Posted by ghorrocks

I have just emailed you the file. I have removed the results files so it is small enough to email.

fig1 steady.jpg


fig2 caculation.jpg


fig3 water volume fraction.jpg

This is figures,do you get the same result?

[ghorrocks]

When the solution goes all over the place (that is, not converging properly) then the interface will get smeared and you will not be able to recover it. You have to make sure the simulation converges for all time steps.

Also note I used a laminar flow model. The flow is probably turbulent so should have a turbulence model. It will be unstable with a laminar flow model.

[zhihuawan]

Originally Posted by ghorrocks

When the solution goes all over the place (that is, not converging properly) then the interface will get smeared and you will not be able to recover it. You have to make sure the simulation converges for all time steps.

Also note I used a laminar flow model. The flow is probably turbulent so should have a turbulence model. It will be unstable with a laminar flow model.

I have a different opinion to you.I think the reason is not it does not coverge,I the main reason is that you just calculate a few times which has clear water-air interface in the steady flow calculation,after the steady flow calucation,the layered water and air will flow out ,and the uniform air and water will flow in(the gas and liquid is mixtured with each other),so after a long time,there will not exist a clear interface between air and water.Do you think so?

In my simulation ,the velocity is small to 0.09m/s,so the Re number is less than 1000,so we can choose the laminar model ,the model may not be the problem ,as to your advice,I will change the setting to have a good coverging level,thank you very much.

[ghorrocks]

You can easily test whether your opinion or my opinion is correct by running a transient simulation which converges tightly at each time step. Having said that, you should be doing this anyway for a transient simulation where you want an accurate time history.

If your flow is in the laminar regime then just use a laminar flow model. Don't model physics which you know does not exist.

[zhihuawan]

Originally Posted by ghorrocks

You can easily test whether your opinion or my opinion is correct by running a transient simulation which converges tightly at each time step. Having said that, you should be doing this anyway for a transient simulation where you want an accurate time history.

If your flow is in the laminar regime then just use a laminar flow model. Don't model physics which you know does not exist.

I have done as you said ,I have choose inlet codition to the laminar flow ,but I met a error after it calculate a few times, this are the error images,I have send the case file to your e-mail, I find there are so many problems for me to solve.Thank you very much.
[ATTACH]error.jpg

error2.jpg

momentum and mass .jpg

user point.jpg

volume.jpg[/ATTACH]

[ghorrocks]

In future please just attach the output file. That gives all the details required to debug CFX. The error dialog boxes in Workbench are usually not very useful.

Again, this appears to be inadequate convergence. You need to make sure that every time step is converged.

In free surface models the time step required for good convergence can vary a bit due to surface waves on the surface. This means it is really good to use adaptive time steps, homing in on 3-5 coeff loops per iteration. This means the solution can adjust the time step as required.

[zhihuawan]

Originally Posted by ghorrocks

In future please just attach the output file. That gives all the details required to debug CFX. The error dialog boxes in Workbench are usually not very useful.

Again, this appears to be inadequate convergence. You need to make sure that every time step is converged.

In free surface models the time step required for good convergence can vary a bit due to surface waves on the surface. This means it is really good to use adaptive time steps, homing in on 3-5 coeff loops per iteration. This means the solution can adjust the time step as required.

(1)As you can see ,because it has debug,so there is no output files,so I just need adjust the solve setting.
(2)What is good adequate convergence,you mean every variables should below the 1e-4,I see the water-air interface in the steady calculation is not clear in my result ,which is different to your case.Can you receive my file from the e-mail?
(3)I find there is no adaptive time steps in the software when I choose the transient calculation,you can see the images,which one should I choose?analysis type.jpg

solve control.jpg

water volume.jpg

[ghorrocks]

1) If you don't have an output file then please attach the CCL.
2) The exact convergence tolerance required varies depending on the simulation. You may need to be higher or lower. Do a sensitivity analysis to find the convergence you require for accurate results.
3) The adaptive time step option is under the "Timesteps" option. You currently have that set to a fixed 0.0001[s]

[zhihuawan]

Originally Posted by ghorrocks

1) If you don't have an output file then please attach the CCL.
2) The exact convergence tolerance required varies depending on the simulation. You may need to be higher or lower. Do a sensitivity analysis to find the convergence you require for accurate results.
3) The adaptive time step option is under the "Timesteps" option. You currently have that set to a fixed 0.0001[s]

360??20180104084707877.jpg

when I try to set the timesteps to 1e-6,after a long time ,it will give a error ,the out files are as following:
This run of the CFX Release 18.0 Solver started at 21:39:13 on 03 Jan
2018 by user dell on DELL-PC (intel_xeon64.sse2_winnt) using the
command:


Setting up CFX Solver run ...


+--------------------------------------------------------------------+
| |
| CFX Command Language for Run |
| |
+--------------------------------------------------------------------+

LIBRARY:
CEL:
EXPRESSIONS:
Press = (1-step((y-0.0009[m])/1[m]))*960*cos(45)*g*y
END
END
MATERIAL: air 300K
Material Group = User
Option = Pure Substance
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1.1766 [kg m^-3]
Molar Mass = 1.0 [kg kmol^-1]
Option = Value
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.8537e-05 [Pa s]
Option = Value
END
END
END
MATERIAL: silicone oil
Material Group = User
Option = Pure Substance
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 960 [kg m^-3]
Molar Mass = 1.0 [kg kmol^-1]
Option = Value
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 0.0192 [Pa s]
Option = Value
END
END
END
END
FLOW: Flow Analysis 1
SOLUTION UNITS:
Angle Units = [rad]
Length Units = [m]
Mass Units = [kg]
Solid Angle Units = [sr]
Temperature Units = [K]
Time Units = [s]
END
ANALYSIS TYPE:
Option = Transient
EXTERNAL SOLVER COUPLING:
Option = None
END
INITIAL TIME:
Option = Automatic with Value
Time = 0 [s]
END
TIME DURATION:
Option = Total Time
Total Time = 1 [s]
END
TIME STEPS:
Option = Timesteps
Timesteps = 1e-006 [s]
END
END
DOMAIN: Default Domain
Coord Frame = Coord 0
Domain Type = Fluid
Location = fluid
BOUNDARY: Domain Interface 1 Side 1
Boundary Type = INTERFACE
Location = inlet
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 1 Side 2
Boundary Type = INTERFACE
Location = outlet
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: opening
Boundary Type = OPENING
Location = opening
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Opening Pressure and Direction
Relative Pressure = 0 [Pa]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
FLUID: air
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 1
END
END
END
FLUID: silicon oil
BOUNDARY CONDITIONS:
VOLUME FRACTION:
Option = Value
Volume Fraction = 0
END
END
END
END
BOUNDARY: side interface Side 1
Boundary Type = INTERFACE
Location = periodic
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: side interface Side 2
Boundary Type = INTERFACE
Location = periodic_shadow
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: wall
Boundary Type = WALL
Location = wall
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
FLUID PAIR: air | silicon oil
BOUNDARY CONDITIONS:
WALL ADHESION:
Option = Adhesive
Wall Contact Angle = 45 [degree]
END
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.1766 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = -g
Gravity Z Component = 0 [m s^-2]
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Option = Automatic
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: air
Material = air 300K
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID DEFINITION: silicon oil
Material = silicone oil
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
FLUID: air
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
FLUID: silicon oil
FLUID BUOYANCY MODEL:
Option = Density Difference
END
END
HEAT TRANSFER MODEL:
Homogeneous Model = Off
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k omega
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
FLUID PAIR: air | silicon oil
Surface Tension Coefficient = 0.0206 [N m^-1]
INTERPHASE TRANSFER MODEL:
Option = Free Surface
END
MASS TRANSFER:
Option = None
END
SURFACE TENSION MODEL:
Option = Continuum Surface Force
Primary Fluid = silicon oil
END
END
MULTIPHASE MODELS:
Homogeneous Model = On
FREE SURFACE MODEL:
Option = Standard
END
END
END
DOMAIN INTERFACE: Domain Interface 1
Boundary List1 = Domain Interface 1 Side 1
Boundary List2 = Domain Interface 1 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Translational Periodicity
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Mass Flow Rate = 0.57 [kg s^-1]
Option = Mass Flow Rate
END
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: side interface
Boundary List1 = side interface Side 1
Boundary List2 = side interface Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Translational Periodicity
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
END
MESH CONNECTION:
Option = Direct
END
END
OUTPUT CONTROL:
RESULTS:
File Compression Level = Default
Option = Standard
END
TRANSIENT RESULTS: Transient Results 1
File Compression Level = Default
Include Mesh = No
Option = Selected Variables
Output Variables List = Absolute Pressure,air.Volume \
Fraction,air.Velocity,silicon oil.Velocity,silicon oil.Volume Fraction
OUTPUT FREQUENCY:
Option = Timestep Interval
Timestep Interval = 10
END
END
END
SOLVER CONTROL:
Turbulence Numerics = First Order
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 50
Minimum Number of Coefficient Loops = 1
Timescale Control = Coefficient Loops
END
CONVERGENCE CRITERIA:
Domain Interface Target = 0.0001
Residual Target = 1.E-4
Residual Type = RMS
END
TRANSIENT SCHEME:
Option = Second Order Backward Euler
TIMESTEP INITIALISATION:
Option = Automatic
END
END
END
END
COMMAND FILE:
Version = 18.0
Results Version = 18.0
END
SIMULATION CONTROL:
EXECUTION CONTROL:
EXECUTABLE SELECTION:
Double Precision = No
Large Problem = No
END
INTERPOLATOR STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
END
PARALLEL HOST LIBRARY:
HOST DEFINITION: dellpc
Remote Host Name = DELL-PC
Installation Root = C:\Program Files\ANSYS Inc\v%v\CFX
Host Architecture String = winnt-amd64
END
END
PARTITIONER STEP CONTROL:
Multidomain Option = Automatic
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARTITION SMOOTHING:
Maximum Partition Smoothing Sweeps = 100
Option = Smooth
END
PARTITIONING TYPE:
MeTiS Type = k-way
Option = MeTiS
Partition Size Rule = Automatic
Partition Weight Factors = 0.12500, 0.12500, 0.12500, 0.12500, \
0.12500, 0.12500, 0.12500, 0.12500
END
END
RUN DEFINITION:
Solver Input File = E:\moni\yyq2\shuntai_005.res
Run Mode = Full
Solver Results File = E:\moni\yyq2\shuntai_006.res
END
SOLVER STEP CONTROL:
Runtime Priority = Standard
MEMORY CONTROL:
Memory Allocation Factor = 1.0
END
PARALLEL ENVIRONMENT:
Number of Processes = 8
Start Method = Intel MPI Local Parallel
Parallel Host List = dellpc*8
END
END
END
END


+--------------------------------------------------------------------+
| |
| ---------+
| The Equations Solved in This Calculation |
+--------------------------------------------------------------------+

|
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver could not be started, or exited with return |
| code 255: . No results file has been created. |
+--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+
| The following transient and backup files written by the ANSYS CFX |
| solver have been saved in the directory E:\moni\yyq2\shuntai_006: |
| |
| 220.trn |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| E:\moni\yyq2\shuntai_006: |
| |
| pids, mon |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| After waiting for 60 seconds, 1 solver manager process(es) appear |
| not to have noticed that this run has ended. You may get errors |
| removing some files if they are still open in the solver manager. |
+--------------------------------------------------------------------+


This run of the ANSYS CFX Solver has finished.

can you help me ?I do not know how to send you file ?

[ghorrocks]

You are running a free surface simulation with surface tension. You will find that to get this to converge you will need amazingly small time steps. Surface tension modelling increases the simulation's sensitivity to time step size. So try smaller time steps. Even better, use the adaptive time steps I recommended before (adaptive time steps works very well for this class of simulations).

[zhihuawan]

Originally Posted by ghorrocks

You are running a free surface simulation with surface tension. You will find that to get this to converge you will need amazingly small time steps. Surface tension modelling increases the simulation's sensitivity to time step size. So try smaller time steps. Even better, use the adaptive time steps I recommended before (adaptive time steps works very well for this class of simulations).

I have tried so many times as you said ，but I failed all the time,I am very depressed ,I just want to abondon,can you help me?I just do not know how to do next?