Pressure Outlet Guage pressure
 

Absolute Pressure=Operating pressure+Guage pressure

I have 2 inlets and 1 outlet. The domain includes 2 phases, air and liquid solution. Vapors are generated due to high temperature in the domain. The guage pressures are known at the 2 inlets and 1 outlet (all boundaries). Velocities at the inlets are also known. hence, "velocity Inlet" boundary condition" at the inlets is used. Incompressible ideal gas law is used, which calculates pressure by operating Pressure, so i used the Pressures of the inlets (which is 2 Bar) as an operating pressure.

For the outlet (for air and vapor flow) I dont know the rate of mass flow of air and vapor at the outlet so I cannot use "Outflow" boundary condition. Now, i am left with "Pressure outlet boundary condition" at the outlet. For pressure outlet, I need guage pressure which is -6666Pa in my case.

My question is: what guage pressure should i use for Pressure outlet boundary condition used at the outlet. Would it be (-6666pa). Would it be ok to use negative value and would the change in operating presssure from 101325 Pa (default) to 2 bar effect the guage pressure here?

Thanks

Hi,

FLUENT accept negative signs; as you said, they are relative pressures.
Because of your specific state law which you have used, changing operating pressure would change results; i.e, in this state law, you have to set operating pressure wisely because it's used directly in state law. So if you want to use this state law, it's better to set a value which you'd have little pressure variation regard to that in whole domain; maybe an average of inlet and outlet will be good as first guess and you can improve that after results will be obtained.

Bests,

Amir, Thank you very much for your time.

The 2 inlets for N2 gas has a pressure of Pguage=200Kpa each.
The outlet is a suction which creates a vacuum pressure Pguage=-6666Pa. The operating Pressure used by me is Po=200Kpa (as the 2 inlets had this pressure)

For outlet boundary condition Pguage @the outlet is required.
Pguage=-6666Pa but It might be relative to 101,325 Pa. As operating pressure was changed by me from 101,325 Pa to 200 Kpa so Pguage may also be changed like this:

Pguage@outlet=-6666-200K =-206.66KPa

This negative value was input by me into the pressure outlet boundary condition for suction at the outlet.


Now, you mean to say that, I should not use 200Kpa value as operating pressure, rather, I should use the average of 200Kpa and -6666pa as the operating pressure. and you said, I can improve it after results. Could u elaborate on that? how can I improve it? Could you tell me the procedure.

thank you very much. So nice of you.

P_static@outlet=101.325-6.666=94.659K; P_gauge@outlet=94.659-200=-105.341K; right?

As I said before; FLUENT accept negative signs.
with op pressure=200K :
P_gauge@inlet=101.325K
P_gauge@outlet=-105.341K
I meant that; if you insist on using incompressible ideal gas law, in order to achieve more accurate density, set an operating pressure with minimum pressure deviation; I wasn't sure about static or gauge kind of pressure you've reported, but now it seems that 200kPa is a good choice as your first guess because deviation of pressure are almost equal. when you have got new results; you'll have pressure for each cell and by a statistical procedure you can find new op pressure which has minimum pressure deviation about. But this procedure wouldn't need if you use ideal gas law instead.;)

Bests,

Experimental Given Max guage pressure @2 inlets=200Kpa
Experimental Given Min guage Pressure @ 1 outlet suction= -6666Pa
Operating pressure used by me in FLUENT=200Kpa (as both inlets have same pressure so it seems a better option as opposed to the default 101,325Pa)

Based on these aforementionentioned values,

For Velocity_Inlet_Boundary_condition:
P_guage@inlet1=0
P_guage@inlet2=0

For Pressure Outlet Boundary condition:
P_guage@outelt-suction=-6666-200K =-206.66KPa

You said negative sign is not important but if i dont use negative sign with 206.66Kpa, it would mean that the P_Absolute @outelt-suction=206.66K+200K=406.66Kpa. Rather than, P_Absolute=-206.66K+200K=-6.66KPa

Secondly, could you please tell me that the values calculated by me are correct?

Third, I would use "ideal gas" instead of "Incompressible ideal gas law" as per our discussion of presure variations.

Thanks a lot of your kindness.
Mohsin

:eek: I didn't say that! I meant FLUENT accept both positive and negative values and you don't need to concern about that, so it's not important but it's necessary:D; I thought you were not confident of setting negative values. I just wanted to say these are relative pressures and it's obvious that they may be positive or negative and you have to set correct sign hope that clear now! (I edited this doubting sentence)
I don't think so.
@inlet:P_static=301.325kPa so new gauge pressure=101.325kPa
@outlet:P_static=94.659KPa so new gauge pressure=-105.341kPa
and you have to consider signs as well.:D
maybe it's better to compute staic pressures with previous op pressure and then find new gauge ones; as done above.
yes, it's better for this case.;)

Bests,

Dear Amir

I agree with your values. I had made a mistake. So nice of you to help me to solve this issue.

Could you also put some light on this thread also:

http://www.cfd-online.com/Forums/flu...ry-inputs.html

Thanks

Dear Amir,

As I have already told u in the previous posts that my geometry contains 2 inlets and 1 outlet.

As you suggested the following values:

P operating= 200kPa
@inlet:P_static=301.325kPa so new gauge pressure@inlet=101.325kPa
@outlet:P_static=94.659KPa so new gauge pressure@outlet=-105.341kPa

Now, as

Absolute pressure=Static Pressure +Operating pressure

which in my case should be around 301.325Kpa at the inlets. However, after convergence, the contour plots for "Absolute pressure" at the inlets are not showing it to be anywhere near 301.325Kpa rather the contour plots are giving me a very lower value (close to outlet Pressure-rather it should be 301.325 Kpa). Why is it so? I am completly baffeled by this..Please help....

Dear Mohsin,

First of all, the above relation is not correct; correct form is something like this:
Secondly, you have to note that the value you've set in FLUENT for pressure-inlet boundaries is gauge total pressure and for pressure-outlet is gauge static pressure.

Bests,

Yes thank you for the correction

Total guage pressure=Static pressure+Dynamic Pressure
Absolute pressure=guage Pressure + Operating Pressure

Now, at the inlets, as the absolute pressure is about 3 bar, then why the absolute pressure is being shown at about 1 bar at the inlets. rather it should show 3 bar.

It is a little confusing.....

This equation is not correct again!
It's obvious, you've set gauge total pressure and you're seeing static pressure.

Bests,

Dear Amir,

Thank you for your reply. let me correct the equations:

Total guage pressure=Static guage pressure+Dynamic guage Pressure
Absolute pressure=guage Pressure + Operating Pressure

I am using "Velocity inlet BC" at the inlets and "Pressure outlet BC" at the outlets. For Velocity inlet BC "Initial Guage pressure" was required (which is the guage static pressure at the inlet).


Could you please elaborate on this:

"It's obvious, you've set gauge total pressure and you're seeing static pressure".

How can i see the correct Pabs. I will be really glad for your guidance.

I thought your inlet condition is pressure inlet; anyway, you're using velocity inlet and in density based solver it need out flow gauge pressure which is not a boundary condition for pressure it's just a threshold to enhance stability; here, you can see that inlet velocity will be shown correctly, right? so to achieve your pressure, maybe it's better to use pressure-inlet condition.

Bests,

oh so it means I have to simulate all over again by "Pressure inlet" boundary condition in order to simulate the correct pressure.

But

I have been given velocities at inlet and my goal is to change the velocities for various simulations to get the optimum condition for the geometry. If, I will use Pressure inlet boundary condition, how can it calculate the velocity? or which bounadry condition would be feasible in this case?

Secondly, which value of "Initial Guage pressure" should be specified in my case? or should it be 0?

thank you very much.

Dear Mohsin,
I think inlet pressure is more feasible for your purpose, you can set desired velocity by adjusting static and total pressure @ inlet; but an important note, these definition provided so far for total pressure are valid for incompressible flow, for compressible flow total pressure is evaluated via isentropic relation as a function of mach No.
So it depend on your case that which relation to use for computing total pressure.

Bests,

Dear Amir,

Thank you so so much.

before concluding i have 2 short querries:

1. I am using Ideal gas law for compressible fluids to calculate density. As we discussed in the following thread that my domain has pressure gardients so Ideal gas law for compressible fluids would be effective in my case.

http://www.cfd-online.com/Forums/flu...essiblity.html

So, these relations for Total pressure are not valid in compressible case instead Mach number and isentropic flow relations are used.

Hence, Do u think, for calculating density I may change to "incompressible ideal gas law" (as Mach number is less than 0.1, but pressure variations are there) so that the equations for total pressure are valid? without much loss of accuracy?

2. Secondly, which value of "Initial Guage pressure" should be specified in my case? for pressure inlet boundary conditions?

As you know, ideal gas law is more general in comparison with incompressible type; I think you don't have better choice because incompressible type is proper just for cases in which pressure gradient is negligible.
Both total pressure equations have similar trends up to mach number 0.3; you can simply examine that.
There are some inconsistency in your boundary condition. Supersonic gauge pressure will be ignored in subsonic because it's not necessary for subsonic regime! If you have subsonic regime, you cannot set velocity inlet and also pressures on your boundaries simultaneously! In other words, in subsonic regime, it's impossible to change velocity with fixed pressure boundaries unless you would change pressure, this is result of elliptic nature of equations.

Bests,

Thank you Amir,

I followed what you said, I used "pressure inlet Bounadry condition" instead of "velocity Inlet" boundary condition. The continuity residual was difficult to reduce however it reduced to 10-3. and the other residulas for velocity and energy were well below 10^-5, along with mass flux showing convergence.

The absolute pressure at the inlet was shown properly. However, this time the velocity at inlet is being shown 60m/s on the average (In real situation it is 0.5m/s).

Pressure inlet boundary condition is giving velocity error now. Can you tell me what might be the reason of this higher velocity? how is the velocity calculated by FLUENT and/or do i need to more iterations or do i need to change the discretization scheme?

Please assist.

As I said before, because you're modelling subsonic regime, you cannot set both pressure and velocity. Here, you've set pressure and achieve velocity... . The difference between achieved velocity magnitude and expected one is high, so I think there should be fundamental issues. I have some suggestions which may help:
1) ensure parameters value which you have provided and their dimension are correct ....
2) use pressure based technique for coupling ...
3) use constant density and see what will happen!
4) estimate approximate average velocity if you have a pipe with one inlet and one outlet with outlet diameter and with such pressure difference via analytic solution.
5) use resolved grid near boundaries ...

Bests,

Thank you for your reply.

I will use Constant density and will see the result and post here by tomorow.

Just a question: what do u think, the results for "velocity inlet" case were fine? even though the Absolute pressure contours were not accurate in the contour report? Can they be used or they may be highly inaccurate??

You're talking about 2 different case; in one of them pressures are set and in the other velocity @ inlet and pressure @ outlet; upon your purpose you can use one of them; it's not a reasonable way to use part of one case for another, pressure and velocity are highly coupled! :eek:
Before changing density, estimate approximate velocity (No 4), also check thermal boundary conditions.

Bests,

Thank you for your reply Amir,

yes, I am talking about 1 of the cases. I was asking you would it be ok to use only 1 case for anlaysis. for instance, "velocity inlet" coz convergence was good in that case. I may discard the case in which "pressure inlet" is used. It gives absurd reports for Absolute pressure however, apparently I have no other solution. What do u say?

Velocity (no.4)? you mean the velocity at the inlet?

I have also simulated the results with constant density. The results are similar to compressible flow. Also, the thermal conditions used were also checked and seems to have no problems. Constant temperature is used at the inlets for the flow of N2.

Thanks again for your valuable responses.

It think the problem is resolved if you do this:
If you achieve good result in comparison with numeric one; you should check provided data more precisely. (I think this the case) because 0.5m/s seems to need lower pressure difference which both numeric results prooved that.

Bests,

Dear Mr. Amir

Please have a look at this short issue. I have posted pictures also.

As, I have already descirbed in the previous posts, I have 2 inlets and 1 outlet. The lower inlet is having a "velocity inlet" BC with a velocity magnitude of 4.678m/s. The upper inlet is also having a "velocity inlet" BC with a velocity magnitude= 0.3 m/s. The operating pressure is 297458 Pa (as the flow is considered incompressible and this value is used to compute the density of the flow, hence, this value is set according to mean flow pressure of the inlets). The outlet is creating a suction and it has a Pressure outlet" BC with a guage pressure value of -196623.3 Pa (i-e Absolute pressure=100834.7 Pa, as guage pressure will be added to operating pressure for absolute pressure). After simulation: The solution gives appropriate velocity contours but the pressure contour plots for the inlets are strange.

Picture 1: (Contours of Guage Static Pressure at Lower inlet)
The contours of guage static pressure are giving negative values (similar to the outlet Pressure values).
Picture 2: (contours of Guage static pressure at Upper Inlet)
Here, also the contours of static pressure are giving negative value (similar to the outlet Pressure values)
Picture 3: (contours of Guage static Pressure at outlet)
Here the contours are giving negative values as specified pressure outlet Boundary condition.So, it seems to be fine.
Question 1: Shouldn't the contours of static pressure be similar to operating pressure value (which is 297458 Pa-mean flow pressure)? What is actually operating pressure? Does operating pressure is the pressure outside the domain? Why is the contour plots at the inlets are giving pressure values relative to outlet pressure values and not the one specified in operating pressure.

To check this confusion, I calculated the solution with "pressure inlet" BC at inlets and "pressure outlet" BC at outlets. In this case, As, it is pressure Inlet boundary condition, so pressure values were given at inlets. The simulation results show the static pressure values to be appropriate but the velocity values at the inlets were calculated very high (i-e 100m/s, actually it should be 4.678 m/s according to the flow rate given to me).

Question 2: how is FLUENT calculating velocity magnitude for Pressure inlet case? through Bernouli equation?

I'll be grateful for your guidance.
Mohsin

Dear Mohsin,
It seems that your case is not pressure driven one. As I said before op. pressure is just a reference for incompressible flow and not necessarily the pressure of outside the domain. All the pressure are relative to the op. one. you can set op. pressure to zero and see that the pressure different between 2 specified point wouldn't change. this can be done by a simple try and error if you want to set the density properly as a function of average pressure. (note that in incompressible flow the pressure differents are important not the absolute value!). I think that you're not sure about the physical value for BCs. find them specifically and then think about the reference value.
Consider a volume adjacent to the inlet; when the continuity condition is satisfied for this control volume, the unknown inlet flux in obtain.

Bests,

Dear Amir, Thank you so much for your kind consideration.


You mean that Absolute pressure or Guage static pressure are not important in incompressible flow. So, the values of static pressure obtained at the inlets should not be seen. Only the difference of static/dynamic/absolute pressures should be noted. As in my case, the static pressure contours, at the inlets, are very strange (giving negative values; picture 1 and 2 above), the results may be ok as the difference is important and not the absolute values.


Could you please clarify why absolute values are not important and only pressure difference is important in incompressible flows?

Dear Mohsin,

As you know ; so you can add any constant to your pressure field without changing the momentum equation; i.e., the solver works with relative pressures.
Note that it's not strange that inlet pressure is negative because your op. pressure is relatively large!
In the other word, op. pressure is not used in the solver in incompressible flow, so you can set op. pressure to zero and the results are gauge pressures.
Don't hesitate to ask if this is not clear.

Bests,

I am afraid I am unable to understand what you mean by this? Could you please elaborate on this?

It means that static pressure values (which are calculated negative, as my op.pressure is large) has no effect on the results. Only the difference of static/dynamic pressure (between 2 points in the flow) is important.


As you said, op. pressure is not used in incompressible flows; then how is the static pressure, at the inlet, is calculated when "velocity inlet" BC is used at the inlets?


Thank you so much.

Sure; the only equation in incompressible flows which has the pressure term is the momentum equation where you can find there. In mathematical point of view, only the gradient (variation) of the pressure is included and affects the momentum equation. Consequently, you can add any constant to the pressure term without changing the momentum equation because:
because
Exactly. setting different op. pressure just shifts the pressure values but the differences are equal. this is because of that you've set the pressure BC according to the op. pressure.
Yes, it's not used in the solver but you can see its effects indirectly in shifting the pressure field. ( because you've set the pressure BC according to the op. pressure). When you've set the velocity at the boundary, the inlet pressure is calculated via conservation of momentum in adjacent boundary cells.

Bests,

Dear Amir, thank you very much for you valuble discussion.

Now, it is clear that FLUENT deals with relative pressures in incompressible flows, as the only term involving pressure is the momentum equation and the momentum equation contains pressure gradient which means that momentum equation will deal with only change of pressures in respective directions.

The momentum equation is shown in picture. Just out of curiosity, what do you mean by "Constant" in this

Right. it means, if I want to check the pressure values in the domain, I should only check absolute pressures and not the static pressure (which is the pressure relative to op.pressure and which may look absurd because of negative values caused by high op.pressure). Correct?

Inlet pressure is calculated via conservation of momentum in adjacent boundary cells, but what about the inlet cell (not the adjacent one)? The inlet cell is the cell on which I have specified the velocity magnitude of 4.678 m/s in the "velocity inlet" BC. I think, on this cell, the initial guessed value of pressure is used (which you specify in the solution initialization panel)?? Right?

Dear Mohsin,
The constant value can be any reference magnitude such as op. pressure; i.e.: (note that the value of this constant should be the same in all the cells)

Firstly, your definition for static pressure is not correct; here you mean gauge pressure. (note that FLUENT shows gauge static pressure instead of pure static one)
But the meaning of your statement is generally correct but it depends on different applications. Note that you can easily add arbitrary values to your pressure field in post processing stage via "custom field functions".
No, it's not correct. What I was talking about adjacent cell is exactly what you are thinking about; that's a cell which one of its faces located at the boundary. here the pressure over this face is unknown and will be found by solving momentum conservation over this cell. There are also some discussion regarding the staggered grid in numerical codes which is not related to your general question.

Bests,

I was wondering, If I use "velocity inlet BC" and initialize (standard) my flow with inlet in "solution initialization" panel. Then, how is fluent using the initial guessed value of "pressure"? Previosuly I was of a view that, on the face in question (boundary face), the initial guessed pressure value is used. Could you please clarify me on that?

Hi,
Yes; you're right. the initial guessed is used for pressure but just for initialization! This value should be corrected during iterations and what I was talking about is a procedure for its corrections. But to avoid special numerical responses; the pressure is calculated at the cell centers and the velocities at appropriate faces which is a staggered procedure (other cell or node values can be found with proper interpolations). This may be done by introducing virtual cell layer at the boundaries and so on. This is not a point you care about; these are just initial values and corrected by iterations in way that conservation of momentum would be satisfied in all the cells, so the unknown boundary pressure is corrected in this manner.

Bests,

Thank you so much. I am so glad that people, like you, spare their time for this kind of valuable discussion. Everything regarding my long awaited puzzle is clear now.

have you came across or can you recommend any FLUENT manual/guide/book (other than the FLUENT USER GUIDE) which can give more insight into its solution procedures?

Dear Mohsin,

If you want to dig further into numerical procedures basically I can recommend these famous and valuable CFD books:

• Computational Methods for Fluid Dynamics; Ferziger J. H., Peric M.
• Numerical Heat Transfer and Fluid Flow; Patankar S. V.
• Computational Fluid Dynamics; Anderson J. D.

But regarding the FLUENT software specifically, I haven't seen other referenced better than the manual.
Hope that help you.

Bests,

Hello!
I am confused at your discussion.
what is the difference between static gauge pressure and total gauge pressure?


I have to apply vacuum pressure at the one side of outlet.
I set operating pressure 101.325 kPa. i have to apply 96.825 kPa absolute pressure. so guage pressure will be -4.5 kPa that i should set?
Am i right?

total pressure (or stagnation pressure) is a hypothetical property of the flow. Stagnation pressure is the static pressure a fluid element would have if it were brought to rest (usually through an isentropic process). Static & total pressure can be referred to from any gauge. Hence you can have absolute static pressure, gauge static pressure, absolute total pressure, or gauge total pressure.

-4.5 kPa is what you need to set at the outlet, that is correct.