# Unrealistic Pressure Values

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 2, 2010, 12:59 Unrealistic Pressure Values #1 New Member   Matt Join Date: Oct 2009 Posts: 7 Rep Power: 7 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

 February 2, 2010, 14:36 #2 New Member   A.R. Baserinia Join Date: Jan 2010 Location: Canada Posts: 24 Rep Power: 7 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

February 2, 2010, 17:27
#3
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,059
Rep Power: 86
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.

 February 4, 2010, 03:24 #4 New Member   Guohua Gao Join Date: Feb 2010 Posts: 3 Rep Power: 7 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.

 February 4, 2010, 06:02 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 11,059 Rep Power: 86 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.

 February 8, 2010, 13:04 #6 New Member   Matt Join Date: Oct 2009 Posts: 7 Rep Power: 7 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 Right-click Expressions in the tree view and select Insert > Expression. Set the name to UpH and click OK. Set Definition to 0.069 [m], and then click Apply. 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!

 February 8, 2010, 14:54 #7 Member   Reza Join Date: Mar 2009 Location: Appleton, WI Posts: 99 Rep Power: 8 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).

 February 8, 2010, 18:12 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 11,059 Rep Power: 86 Reza, please read my post above about a modified pressure. Do not add a source term, this is not required.

 February 8, 2010, 18:22 #9 Member   Reza Join Date: Mar 2009 Location: Appleton, WI Posts: 99 Rep Power: 8 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.

 March 11, 2010, 13:54 #10 New Member   Matt Join Date: Oct 2009 Posts: 7 Rep Power: 7 many thanks to all that replied, i managed to sort it!

 Tags pressure water nodes

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post pierresandre FLUENT 24 November 8, 2011 15:32 sidd CD-adapco 0 April 2, 2007 09:31 Antech Main CFD Forum 0 April 25, 2006 02:15 Christian FLUENT 0 April 15, 2003 07:24 HB &DS CFX 0 January 9, 2000 14:19

All times are GMT -4. The time now is 03:04.

 Contact Us - CFD Online - Top