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.