[Mohsin]

Dear Fluent users

In my geometry of spray Dryer, there are 2 inlets and 1 outlet. The outlet's BC is "Pressure outlet" and for both the inlets "Velocity Inlet" BC is used. When the flow field is calculated, the contours of static pressure at the inlets is giving inappropriate values. Static pressure values are being referenced to outlet's pressure values.

To get insight into this issue, rather than "velocity inlet" BC, I used "Pressure inlet" BC for the calculation of flow field. However this time, the velocity was calculated to be very high (as opposed to experimental results at the specified pressure).

My question is: Why is there such a difference?? While using "velocity Inlet" BC Static pressure values are being referenced to pressure outlet (Means the contours are showing the range of values used in the Pressure outlet. It is also not taking account the 'operating pressure' value given by me). On the other hand, while using "pressure inlet" BC, Static pressures at inlet come out be accurate but Velocity values are not appropriate....Could anyone tell me How to get the correct values of Static Pressure while using "velocity inlet" BC.

[santiagomarquezd]

Mohsin, respect of reference pressure, it is used only if no pressure BC is set in order to not obtain a "floating pressure" (https://www.sharcnet.ca/Software/Flu...ug/node375.htm). In addition setting pressures both at inlet and at outlets leads you to have to set total pressure at the inlets (https://www.sharcnet.ca/Software/Flu...ug/node219.htm), with

p_T=p_S+1/2*rho*V^2

Usually, using Velocity Inlet at inlets and Pressure Outlet at outlets behaves well, but if you want to compare with experimental values sometimes is useful to set the same values you had measured. Nevertheless in case you had measured velocities in all points, is it not suitable for BC's. You have to set V at inlets and P at outlets and then to check the velocity at the outlets.

Finally, in systems where fluxes are being mixed probably you need to set the BC's far from the mixing point in order not to have influence in the mixing process.

Some ideas, maybe you can post some pics about the results on the geometry.

Regards.

[shk12345]

Hello
I am doing the same simulation and also in my case the problem is same.
I also need the solution to this problem.
In my case even after using the pressure boundary conditions i am not getting that desired pressure profile in the computational domain.

Kindly help me as soon as it is possible.

Thanks
SHK

[Mohsin]

Dear Santiago Marquez

I am sorry for late reply. I couldn't read your reply in my inbox. Please have a look at this short issue. I have posted pictures also.

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 Static Pressure at Lower inlet)
The contours of static pressure are giving negative value (similar to the outlet Pressure values)
Picture 2: (contours of 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 static Pressure at outlet)
Here the contours are giving negative values as specified pressure outlet Boundary condition.
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? 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 that case, pressure values were given at inlets and static pressure values came out 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).
Question 2: how is FLUENT calculating velocity magnitude for Pressure inlet case? through Bernouli equation?

I'll be grateful for your guidance.
Mohsin

[shk12345]

The operating pressure influence the density of the fluids and not the inlet pressure.
You can try with operating pressure at the inlet and outlet boundary condition at the outlet.
In that case that i guess you can get some results. I have done some work consistently using VOF model and got some good results .But in my case i had only once inlet.
You can try that and tell me .

shk

[shk12345]

also you can try to use higher order descretization schemes for pressure and lower the under relaxation factors for it

[opop002]

can anyone tell me how to assign a udf temperature profile to an outflow BC in fluent or apply a udf velocity profile to a pressure outlet

[m.uzair]

I Know this is quite an old post, but I am facing the same problem

I am simulating a cold flow model of gas-solid fluidized bed. The problem I am having is with inlet boundary conditions.

At first I applied uniform inlet gas velocity (0.259m/s) at the inlet and pressure outlet at the other end. It worked perfectly. NOw I want to check the effect of variable inlet gas velocity by using pressure inlet boundary condition. I tried it both ways.. 1) by initializing 2) from the already running case of uniform inlet gas velocity (obtained total pressure of air and applied it at the pressure inlet (Gauge total pressure) ). The moment I do this, there is reverse flow at pressure inlet, the simulations show very abnormal behavior. Basically the solids spread all over the free-board. and the air velocity at the inlet reaches as high as 8 m/s(which should remain under 0.3 m/s or so).

What am I doing wrong?

Also can somebody please explain the relationship between pressure and velocity in this situation. How a constant pressure provides a variable velocity at the inlet. Or is there even any kind of relationship between pressure and velocity. If no, then what causes the change in velocity

Can anyone please help.

[r.d.]

Dear all, I know this is a old post, but I'm facing the same problem and I can't find an answer.


I simulated a pipe with a single hole-orifice plate (so the geometry is something like "full diameter pipe-constriction-sudden expansion-full diameter pipe"), only half domain because of the symmetry.



Since I had experimental measurments, I wanted to check if my simulation matched the measured values; in my circuit the op was downstream a circulation pump and I had one gauge pressure sensor upstream and another one downstream the orifice plate.



I started my simulations (steady state, incompressible flow, standard k-epsilon, standard wall functions) with inlet bc equal to the velocity obtained from the flow rate, but I noticed that the calculated pressure in the inlet section was lower than the measured (1 bar instead of 4); than I switched to the pressure inlet bc (total pressure 3 bar+dynamic pressure, initial pressure equal to the measured 3 bar), but this time the velocity in the inlet section resulted too high (2 m/s instead of 0.4).



It is clear to me that if I set the velocity inlet (that is the mass flow rate, in my case) this will drive the flow and fluent will calculate the corresponding pressure; conversely, if I impose a pressure drop (higher than the one in the velocity inlet bc case) fluent will calculate the corresponding mass flow rate (thus the velocity), that will be higher (the greater the pressure drop, the greater the flow rate).



What I still don't get is the reason of this mismatch; could it be a mesh quality problem, that is too coarse or bad in general? Or is it something else? How can I obtain the measured values of pressure and velocity?



Thanks in advance to everyone will spend some time to answer me and have a nice day!

[r.d.]

I discovered that I setted the planar geometry instead of the axisymmetryc; after correcting this, everything goes right (calculated pressure and velocity match the measured ones).


Roberta