CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Open Channel Flow (http://www.cfd-online.com/Forums/cfx/78441-open-channel-flow.html)

OffshoreStructuralEnginer July 22, 2010 00:07

Open Channel Flow
 
Howdy,

I am running a CFD using CFX-Ansys, open channel flow with two species, oil and water. I am new to CFD, and I have several problems. Do you think I could have some help from you Masters?


Background:
Open channel flow with underwater gate. Oil on the top and Seawater. I am trying to figure out how much oil mass will be restricted by the underwater gate. I have 3 Domains. The water, the oil on top, and the underwater gate. Inlets on the water and the oil, oil=oil, water=water. A outlet on the other side for both oil and water.

Problems
1. Defining crude oil- is this in one of the files that comes with Ansys or do I have to create this material from scratch?

2. How do I determine how much oil has traveled through my outlet? Is this a particle transport problem?

3. Ran the analysis, how do I change the following? I set the boom domain as a wall with no domain interference.

"If the isolated regions do not have the pressure level set either
by the boundary conditions or using a reference pressure equation,
you may encounter severe robustness problems.

This situation may have arisen because a domain interface was not
properly defined during problem setup. Please carefully check
the setup.

The solver will stop now and write a results file. The isolated
regions can be visualised in CFX Post by making plots of the
variable "Isolated Volumes".

If you are sure that the pressure level is set in each isolated
fluid region then you can force the solver to turn off this check
by setting the expert parameter "check isolated regions = f"."

Your the best,

ghorrocks July 22, 2010 06:36

Quote:

Defining crude oil- is this in one of the files that comes with Ansys or do I have to create this material from scratch?
The properties of crude oil vary greatly from place to place. You will have to define it yourself for the stuff you are interested in.

Quote:

How do I determine how much oil has traveled through my outlet? Is this a particle transport problem?
Integrate the mass flow rate of oil at the outlet. Easy done with a monitor point. It is not a particle transport problem.

As for your final question, does the oil float on top of the water? In that case you probably should not model it as multiple domains but as a multiphase fluid. This will allow the oil and water to flow around as they wish, displace each other and form waves and other cool stuff.

OffshoreStructuralEnginer July 26, 2010 18:51

Thanks GHORRocks, I did clean up and combine the 2 domains into one domain, which eliminated the "Isolated Doman Error".

Also I read up on mulitphase and multicomponent flow and switched my model from Lagragian to Eularian.

Volume Fractions is gicing me a real head ache, the oil is supposed to enter a vortex at the top of the underwater gate, but instead it is passing underneath. I have defined the bouyancy. For the initialization, the volume fraction of water is set to 1, and oil is set to 0. Hopefully this represents that there is no oil in the open channel at t=0. Also I have defined the outlet boundary as a Avg pressure equal to hydrostatic pressure. There is 9.8% flow back into the domain which is repeatidly blocked by the computer.

I still have no been able to use the model a monitor point that will provide mass information, just density. In fact I can't get mass to output at all.

Any other great suggestions.

ghorrocks July 26, 2010 19:00

Quote:

I did clean up and combine the 2 domains into one domain, which eliminated the "Isolated Doman Error".
:)

Quote:

Also I read up on mulitphase and multicomponent flow and switched my model from Lagragian to Eularian.
Sounds like progress.

Quote:

Volume Fractions is gicing me a real head ache...
Check your setup. Is the gravity vector in the right direction? Have you got your volume fractions the right way around?

Quote:

There is 9.8% flow back into the domain which is repeatidly blocked by the computer.
Inlets or outlets will always give you walls on backflow. If this is not right then you should not use inlet or outlets. You might be able to do it using an opening, but I suspect a better approach will be to model a section of the upstream or downstream geometry so the spurious walls do not affect the important part of your simulation.

Quote:

In fact I can't get mass to output at all.
The monitor I was referring to was a CEL expression, not a point. Something like massFlow()@Outlet should do it.

OffshoreStructuralEnginer July 26, 2010 20:12

You are such a big help. I really appreciate your thoughtful and macro approach.

I defined the element oil, well I figure that having actual oil, and not just water with oil density, will give me the results I am looking for.

Basic Settings
Option: Pure Substance
Material Group: User
Material Description: Crude Oil
Therm State: Liquid

Material Properties
Option: General Material
Thermo Prop
Equation of state
Option: Value
Molar Mass: 900 kg/kmol (this is for vegtable oil)
Density 1.77 Slug/ft^3

Reference State: Automatic

Transport Properties
Dynamic Viscosity: checked
Option: Value
Dynamic Viscosity: 4.177 lb*s/ft^2

That's it. I did not define Radiation Properties or Bouyancy Properties. This is a steady state (no thermal) model.

ghorrocks July 26, 2010 21:19

Have you worked through the tutorial example, I think it is free surface flow over a bump? This will show you how to set up a air/water model. You can use this as a template.

lihui54312 July 26, 2010 22:04

HI,
This is an multiphase problem, and you can use the freesurface model in CFX,and you can see the tutorial case,get the information how to set the model,this model is the VOF in fluent. good luck.

OffshoreStructuralEnginer July 30, 2010 20:35

lilhui, Could you please provide more information about the VOF model? Is it an example? What is the name of the example? Do you know precisely where it can be found?

I am sorry but Ansys Fluent Help is not user friendly on my computer.

OffshoreStructuralEnginer July 30, 2010 20:52

Analysis Type: Steady State

Default Domain:

Basic Settings
Fluid and Particle Definitions:
Air
Oil
Seawater

Morphology: Air
Option: Dispersed Fluid <- is this correct?
Mean Diameter: 0.015625 [in] sorry i guessed it would be 1/64 of an inch

Morphology: Oil
Option: Dispersed Fluid <-is this correct?
Mean Diameter: 0.3125 [in]

Morphology: Seawater
Option: Continuous Fluid

Domain Models
Pressure: Reference Pressure: 830 psf , hydrostatic pressure of water in 13ft depth

Bouyancy
Option: Buoyant
Gravity in X: 0
Gravity in y: 0
Gravity in z: -g <- z is positive away from ground
Buoyancy Ref Density: 1.99 slug ft^-3 <- assumed asking for density of principle fluid "Seawater". Is this a correct assumption? Is Buoyancy density different from regular density? Never heard of Buoyancy ref density in any class.
Buoyancy: Ref. Location: Automatic

Tab: Fluid Models
Multiphase: select Homogenous Model
Multiphase: Free Surface model: Standard
Heat Transfer:Homogenous Model: select
Heat Transfer: Option: Isothermal
Heat Transfer: Option: Fluid Temperature: 78F
Turbulance:K-Epsilon <----- from the example, Cfd-Post notifies that reynolds number is not right based on speed of 1.25 knots.

Anything stick out in your mind? I sure am learning alot! :) :p Lol

OffshoreStructuralEnginer July 31, 2010 16:56

One last question
 
So what I did to make a real difference was add velocity profiles to my walls. I set the top of the flume and the bottom as walls instead of openings. THis is valid since the water is standing still and the object is moving.

I can't get the time scale to move past 11 seconds. Can you tell me how to force the time scale to move to 120 sec?

ghorrocks August 1, 2010 06:25

Have you looked at the flow over a bump tutorial example? There are a number of errors in your setup and the example will show you how to set this up.

Forget lihui's comment about Fluent and VOF. Free surface modelling is very different in Fluent and you won't learn much by looking at that.

Quote:

I can't get the time scale to move past 11 seconds.
Why not? If you can't tell us what is stopping it running how do you expect us to help you?

OffshoreStructuralEnginer August 3, 2010 20:56

Looked over the tutorial. And changed a few boundary counditions. I would like to know what you think GHOR Rocks.?

Outlet boundary:
Velocity Cartesian: in Z direction 2.1 ft/s

Bottom:
Wall/ No Slip boundary/ Smooth/ Velocity in Z direction 2.1 ft/s

I had previously said this model was open channel flow. That was incorrect, I am actually pulling an object through the water. SO I modeled the object as stationary and the fluid as moving. Thank you Professor Einstein.

OffshoreStructuralEnginer August 3, 2010 21:20

Question about y
 
Question of the day:

I want "y" to be in feet. Ansys wants y to be in meters.

My equation for the pressure distribution of Hydrostatic pressure calls for

Press= WaterSpecificGravity*y

WaterSpecificGravity= 64 [lb ft^-3]
y = depth of water at any point

Obi Wan, you are my only hope!

OffshoreStructuralEnginer August 3, 2010 21:31

The Answer is WaterSpecificGravity = 64 [lbf ft^-3]

:) Me Happy!!! Today is MY Birthday!


All times are GMT -4. The time now is 11:51.