Setting Pressure Boundary Conditions in ANSYS CFX Pre
 

Hello every body,

I'm a novice user to ICEM CFD and CFX. I was trying to simulate in ANSYS CFX a hvac problem. The domain considered was a simple rectangular room with an inlet and outlet vents. However, there is a human being, a LCD monitor and a CPU with in the room. The monitor and the CPU being the heat sources in the room. It was intended to maintain an atmospheric pressure inside the room and a pressure lower than the atmospheric pressure at the outlet vents, a velocity boundary condition is used at the inlet. Accordingly I’ve specified in ANSYS CFX Pre, a reference pressure of 1 Atm in the basic settings for the domain and a relative static pressure of -0.7 Atm ( thinking that its absolute value will be 1-0.7 = 0.3 Atm ) at the outlet vents and a velocity of 2 m/s at the inlet. Material used is Air at 25 C.

Are you sure the outlet vent has a pressure of -0.7Atm? This would be a pressure difference enough to create flows of 100m/s in most rooms.

If the only thing setting the pressure level is the outlet pressure then that will set the pressure level (obviously!) So you need to have a think about how you have set your model up as your boundary condition selections are obviously not correct.

So you set the only pressure BC at -0.7 atm and a low flow rate and you are surprised that the operating pressure is . . . ~ -0.7 atm?

Yeah like I thought that the reference pressure set as 1 atm shall act as the operating pressure inside the room and because I applied this -0.7 as the static pressure, I did'nt expect that it will turn out to be the operating pressure inside the room.

As per the CFX help description for the Reference pressure, I suppose that when I set the ref.pressure = 1 atm. and the relative pressure at the outlet = -0.7. I thought that it will be applied as 0.3 atm at the outlet by the CFX.Please clarify if this conception is right (or) misleading.
I'm still in my 3rd year of engineering ( Bachelors ). I've taken up a project related to the CFD analysis of a HVAC room model and my guide has a limited knowledge of CFD. If you find these Boundary conditions to be absurd (or) unrealistic please suggest me some realistic boundary conditions which would make sense so that the results obtained are practically realisable.

The mass flow rate you are specifying is small. Therefor the pressure drop in your domain is small. Since you have fixed the outlet pressure at 0.3 atm absolute, and the pressure drop is small, then the pressure at the inlet is slightly above 0.3 atm absolute, meaning that your operating pressure in your domain is about 0.3 atm absolute, or -0.7 atm relative to the 1 atm reference pressure you specified.

Why are you specifying such a low outlet pressure, anyway? Is you room located 9 kilometers up in the sky or something?

By the way, I hope you are using Air Ideal Gas and not Air at 25C . . .

No I'm using Air at 25 C because I wanted my room temperature to be at 25 C before cooling so that imparting a cooling effect to such room would make some sense and my room is not located at such high altitudes the reason I chose to apply such low pressure at the outlet is only to have some sort of suction effect for the hot air to leave through.
Any way I some how now realise that I'm going in a wrong way as I told you I'm a newbie user and as my guide has a limited knowledge on this I'm not receiving any good help from him and that is the reason why I finally resorted to post my quieries on this forum.

I'd be really thankful if you can suggest me some reasonably good boundary conditions for this problem.

Best regards
Santhosh.

Firstly: In a normal room the outlet pressure is just a few Pa below ambient. -0.7 atmospheres is enough pressure to create a cyclone. So set a realistic outlet pressure.

Secondly: Set the outlet pressure to 0 and the reference pressure to the outlet absolute pressure. That will adequately set the reference pressure.

Third: Use "Air at 25C" if the flows are low Mach number and close to normal sea level conditions. If not you might need to consider the ideal gas model, but this is not needed for most HVAC work.

Four: Is buoyancy significant? You said there are computers and people in the room, they are all heat sources. If they are significant then you need to include buoyancy forces.

Address those issues and you should be getting closer to what you want.

Thanks for the reply glenn your suggestions worked. I've applied now a pressure of 0.997 atm for the simulation and in the post processing I could see that the global pressure range is around 0.997 atm.
Everything went fine when I was working with a single domain . Then I've used multiple domains by considering the CPU and Monitor as solid domains so as to account for Volumetric heating through sub domains with in them. In this case I could see pressures in the range of 18 to 50 pa. in post processing with the same pressure 0.997 atm taken as the outlet absolute pressure what can be the reason for this.

Best regards,
Santhosh.

Do you need to use solid domains for the heat sources? Can't you remove these domains and put the heat source on the boundary left behind? Only model the solid domain if you are interested in the heat distribution inside the domain.

Of course that is what I did before and it worked well but I just wanted to know what went wrong when I've worked with multiple domains.
Any way this problem was solved when the Reference pressure was set to 0 atm. and the outlet relative static pressure to 0.997 atm. instead of the other way around.
Now I'm really confused with the way the reference presure in CFX Pre works can you please clarify upon this. I've worked on some problems in CFX and most of the time I saw that everything works as expected only when the reference pressure is set to 0 why is it so ? Like when I worked with a reference pressure of 1 atm. and a relative static pressure of 0.3 atm at the outlet of the room ( I know that these BC s are not correct but just gave a try for some other reason. ). I was expecting that the presures in post processing will be around 1+0.3 = 1.3 atm but I was surprised to see them around 0.3 atm. this isn't what I expected after reading the CFX help on Reference pressure What can be the reason for this.

Best regards,
Santhosh.

If the reference pressure is 1atm and the relative pressure is 0.3atm then the post processer will report the pressure as 0.3atm and the absolute pressure as 1.3atm.

Thanks for the worthy replies Glenn. I checked up the absolute pressure values and everything goes fine now.I might have posed some newbie questions here but you were generous in answering them.

Best regards,
Santhosh.

pressure in cfx-pre résumé, wind in cfx-pre
 

Hello!

Thanks a lot Glenn, Michael and saisanthoshm88!
Thanks to this thread I think I understood what cfx means with relative and absolute pressures.
However I am not entirely sure. In the Following general questions about the pressure. I also fastly named my case because I realised that I was making allusions to it.

I write in the following what I set, resulting in a solver that does convergence, but I think the heat losses are wrong, and therefore this uncertainty.

• Basic Settings: There is a reference pressure in the "Basic Setings". This I set to 1 atm.
• Initiatlization: In the "initialization", you can also set a pressure, under "Static Pressure", called relative pressure. I initialize this as 1 atm.
• Boundary conditions: Then you can set a boundary pressure if you use an opening . This can be an opening pressure or a static pressure. If I expect flows out of this opening, I guess I would want to set the Static Pressure as 1 atm, as the velocity could create a total pressure increase. Or am I wrong? What would the opening pressure mean then?
• Boundary conditions: As we are there, I wanted to ask, what kind of a boundary condition do you use if you want to simulate wind. Do you set a flow direction in the "mass and momentum option"?

I have the problem of a cylinder who lies in an laminar 2 m/s monodirectional windfield. It is more complicated than that but here a 2D cut. The ______ represent the cylinder surface, ---- the wind which goes to the left.
At its end the cylinder is heated, which creates warm air and buoyancy driven effects.

-----------------------------------
-----------------------------------
__________________--------------
unknown inside flows --------------
__________________--------------
-----------------------------------
-----------------------------------

The cylinder opens into the wind and is closed at the other end, and I am astonished about the results I get, and this is why I ask you for help! I guess the best idea would be to create a "front geometry" so as to be more sure about the exactitude of the B.C.s?

A final résumé (guessing)
CFX PRE
Domain Default Definition of the air => Reference pressure: for most probs 1 atm
Initialisation => Relative pressure (under static pressure) : 1 atm
BCs=> many types, I also set 1 atm

So in the end I found that setting the same pressure everywhere was what I needed. My simulation isn't driven by pressure, but more by high temperature surfaces and buoyancy effects in this cylinder.

CFX POST
"Pressure" = static pressure p
"Total Pressure" = p + 1/2 rho v^2


I am sorry for the many questions.

Thanks in advance!
Lionel

Sorry, but I do not have time to read your post in detail. Can you post a brief paragraph explaining what your question is?

Hello!

Yes: you wrote on the 6/10/2010 that setting the outlet pressure to 0 and a reference pressure +/- 1 atm would initialize a flow correctly. My experience however has been that setting an outlet pressure of 0 would make the solver crash (i guess because in my case, as I don't have no inlet, the pressure cannot adjust in the cylinder.

So there is my question. How would you initialize a domain where inside as well as outside as well as the surrouding should have 1 atm pressure?
It seems like the only more or less converging setting is to set every pressure i can set at the same value.

Thanks a lot Glenn!

Little image
 

Hello!

Here a little image of my problem. Cut in the middle because symmetric. Gravity goes negative y.
The white opening opens into a wind flow (which in this case goes up into the sky, in positive y direction)
The red thing is a 1200 K no slip wall.
The blue surfaces are adiabatic walls.

If i set an opening pressure at my entrainment in the white front at 0 atm, the solver immediatly crashes.
So to set the same pressure everywhere (so no pressure gradients, I don't need no suction effect like saisanthoshm88), you have to write say "1 atm" everywhere, even in the category RELATIVE pressure? (I think your responses answer "yes" to this question.)

http://www.trebuchon.com/wp-content/...escription.jpg

Answer found to the question regarding wind
 

Hello dear Glenn and others!

Concerning wind, I am sorry for the not very thought-around question. I found my answer:

I just realized the importance of creating a volume in front of the body that is "attacked" by wind. You can set one surface as an inlet with a certain wind velocity (and temperature), the other surfaces of this front-volume as entrainments, as you are not sure how the wind flow will diverge when coming across the body.

Concerning pressure, I am still not sure, but to me the only thing that seems to work is to set all pressures everywhere equal to the reference pressure, so to write one reference pressure into a parameter (say "pamb") and to write "pamb" everywhere where they ask for a pressure.

This article as well as your answers state the contrary, but maybe it is just me as a non-native speaker not understanding the concept.
I post the link in case it helps others:
http://www.simutechgroup.com/CFD/cfd-tips-do-dont.html

Sorry Glenn for always making long posts. I should just make shorter posts.

Thanks in advance for any clarification!
Friendly greetings,
Lionel

If the domain is at approximately 1 atmosphere, and the flow creastes small pressure deviations from that, then the reference pressure should be 1 atmosphere and all bounary and initial conditions set to 0 pressure (or small values of pressure). The whole idea of the reference pressure is that the flow is small variations in pressure from the reference pressure to reduce round off error. It is a simple concept.

Hello dear Glenn!

Thanks a lot for the very nice answer! What you say makes perfect sense.
I must forget to set something somewhere, because everytime that I tried to solve something setting 0 pressure at a boundary, the solver crashes. Maybe I've also just been very unlucky and my license crashed every time I tried it.

But yes my question is answered by this.
Thanks!
Lionel