CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Unrealistic Pressure Values

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 2, 2010, 12:59
Default Unrealistic Pressure Values
  #1
New Member
 
Matt
Join Date: Oct 2009
Posts: 7
Rep Power: 7
mattyg88 is on a distinguished road
Good Afternoon,

To refresh your memory, I am a 3rd year MEng civil engineering student from the uk. I am currently working on my 30 credit project which is to analyse and design a contact mixing tank for wastewater treatment works.
I have generated my geometry and mesh for the tank in ansys workbench, inputted the boundry and flow conditions in cfx-pre, ran it in cfx-solver and post processed the results.
The results I feel I am getting for the pressures on the walls are very unrealistic with the average pressure being around 50Pa and the absolute pressure at 1.01E05 Pa for all the nodes on the outside mesh of the tank. I am aware I should be seeing pressures that are very similar to the static pressure caused by the weight of the water (static pressure = water density * gravity * hydraulic column = 1000 kg/m3 * 9.8 m/s2 * 3m = 29.43 kPa).
I have tried changing small things in ansys-pre but I keep getting the same results and its as if my simulation is not considering the weight of the water however stupid that sounds. My outlet of the tank is set at a position below the inlet so my flow should exit the tank via the outlet with zero energy costs. I have set my outlet to a static pressure of 0, is this correct? I also chop and change my wall boundrys from free slip to no slip but this doesnt seem to change the results.
If anybody has any idea of how to alter my system to produce some realistic results I would be extremely grateful .

Many thanks for your time,

Matt
mattyg88 is offline   Reply With Quote

Old   February 2, 2010, 14:36
Default
  #2
New Member
 
A.R. Baserinia
Join Date: Jan 2010
Location: Canada
Posts: 24
Rep Power: 7
baserinia is on a distinguished road
Did you activate the gravity in CFX-Pre? Gravity by default is zero unless you define the vector of gravity acceleration.

Amir

Last edited by baserinia; February 2, 2010 at 14:37. Reason: typo
baserinia is offline   Reply With Quote

Old   February 2, 2010, 17:27
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Have a look in the CFX documentation. Here's what the modelling guide/basic capabilities/physical models/buoyancy has to say:
Quote:
When buoyancy is activated, the pressure calculated by the solver excludes the hydrostatic pressure gradient. This modified pressure is often called motion pressure because it is responsible for driving the flow. All initial conditions and boundary conditions are interpreted in terms of this modified pressure. For details, see Buoyancy in the ANSYS CFX-Solver Theory Guide.
ghorrocks is offline   Reply With Quote

Old   February 4, 2010, 03:24
Default
  #4
New Member
 
Guohua Gao
Join Date: Feb 2010
Posts: 3
Rep Power: 7
gaoguohua is on a distinguished road
Did you use one phase or multiphase flow? If you choose one phase modeling, the gravity won't work even you define the vector of gravity acceleration.
gaoguohua is offline   Reply With Quote

Old   February 4, 2010, 06:02
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Incorrect, gravity also works on things like buoyancy driven flows and they are single phase. But in this case I doubt he is using a buoyancy driven flow so this is not relevant.
ghorrocks is offline   Reply With Quote

Old   February 8, 2010, 13:04
Default
  #6
New Member
 
Matt
Join Date: Oct 2009
Posts: 7
Rep Power: 7
mattyg88 is on a distinguished road
Many thanks to all that replied. I followed tutorial 7 to help me activate gravity and buoyancy on my model and have been getting some much better realistic pressure distribution results in cfx-post.

I used the following expressions on my model which are used in tutorial 7:
"Creating Expressions



  1. Right-click Expressions in the tree view and select Insert > Expression.
  2. Set the name to UpH and click OK.
  3. Set Definition to 0.069 [m], and then click Apply.
  4. Use the same method to create the expressions listed in the table below. These are expressions for the downstream free surface height, the density of the fluid, the upstream volume fractions of air and water, the upstream pressure distribution, the downstream volume fractions of air and water, and the downstream pressure distribution.

    DownH = 0.022 [m]
    DenH = 998 [kg m^-3]
    UpVFAir = step((y-UpH)/1[m])
    UpVFWater = 1-UpVFAir
    UpPres = DenH*g*UpVFWater*(UpH-y)
    DownVFAir = step((y-DownH)/1[m])
    DownVFWater = 1-DownVFAir
    DownPres = DenH*g*DownVFWater*(DownH-y)"
I am slightly confused as to what to set my upstream (UpH) and downstream (DownH) free surface height to as I am assuming my tank is full to the maximum height of 3.8m.
I set both UpH and DownH to 3.8m and my maximum pressure at the bottom of the tank 36.6Kpa seems fairly realistic so would anyone advise me that what I am doing is correct?

Many thanks!
mattyg88 is offline   Reply With Quote

Old   February 8, 2010, 14:54
Default
  #7
Member
 
Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 99
Rep Power: 8
triple_r is on a distinguished road
Hi,

I don't know if you have solved the problem or not, but another suggestion would be to add gravity as a source term into the momentum equations.

It is going to be a general source term with -g as the value that you enter for the z-momentum equation (I am assuming direction of gravity is -z) source and keep the others as zero.

I know if you activate buoyancy, it will not account for hydrostatic pressure, and I don't know if there is a place that you can specify gravity other than source term, or buoyancy options (Like what you do in fluent, entering it as an operating condition).
triple_r is offline   Reply With Quote

Old   February 8, 2010, 18:12
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Reza, please read my post above about a modified pressure. Do not add a source term, this is not required.
ghorrocks is offline   Reply With Quote

Old   February 8, 2010, 18:22
Unhappy
  #9
Member
 
Reza
Join Date: Mar 2009
Location: Appleton, WI
Posts: 99
Rep Power: 8
triple_r is on a distinguished road
Hi,

I am sorry for my not being very clear. I meant, if you don't enable the buoyancy, then you can add gravitational source terms to momentum equation, and that will take care of gravity without requiring you to solve thermal energy equations and having density being a function of temperature.

My suggestion was only based on that I thought the original poster wasn't intending to do a natural convection analysis.

Sorry again for not being clear about my suggestion.
triple_r is offline   Reply With Quote

Old   March 11, 2010, 13:54
Default
  #10
New Member
 
Matt
Join Date: Oct 2009
Posts: 7
Rep Power: 7
mattyg88 is on a distinguished road
many thanks to all that replied, i managed to sort it!
mattyg88 is offline   Reply With Quote

Reply

Tags
pressure water nodes

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Fluent natural ventilation pressure boundary condition pierresandre FLUENT 24 November 8, 2011 15:32
Pressure Condition sidd CD-adapco 0 April 2, 2007 09:31
Neumann pressure BC and velocity field Antech Main CFD Forum 0 April 25, 2006 02:15
Pressure inlet definitions Christian FLUENT 0 April 15, 2003 07:24
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 14:19


All times are GMT -4. The time now is 12:02.