Hi! I need an advice about the correct set-up of boundary condition in 3-D study of radial fan. I have got experimental results and I'm currently trying to reproduce one working point of fan characteristic curve. So far, I have worked in steady condition and I have imposed Pressure inlet condition (gauge of total pressure) at inlet and Pressure outlet condition at outlet (gauge static pressure). These conditions are imposed on the furthest surface of two plenum, one for the inlet and one (bigger) for the outlet, that I've modelled before. I know flow rate (m3/s), fan rpm and the value of the static pressure in a specific point after the exit of fan box. I have imposed at the inlet the gauge-total-pressure considering the value of dynamic pressure (I know flow rate) and at the outlet gauge-pressure=0 (p = p_amb = p_operating_pressure). Unfortunately I'm very far from the experimental static pressure value; my computational value is too low. I've surely made some mistakes (I expected a pressure flow field greater) but I can't understand which are.

Thanks a lot for any advice.

Hiras

I'd suggest you change the pressure outlet BC to "outflow" which is a less restrictive BC but depends quite a bit on whether you have a recirculation zone in that area, it may take longer to converge or diverge completely. But its fine if you have a "plug" flow at the outlet.

Then choose a proper reference pressure location (x,y,z) coordinates within the doman, at a point where you know the pressure (psia) for a fact. I'd suggest that you take a known value of the operating pressure (Pabs-Pguage) and stick it at that point. This should work.

Typically, the default pressure BCs are not accurate in fluent particularly if you need to check up with experimental data on pressures.

I am not completely sure, as am a new user myself but I've had some grief with this in a combustion case and this seems to work for me. (I use a mass flow inlet though)

Cheers

Sandeep.

Hi, first of all thanks for your advice.

I'd like to tell you some considerations about what you said.

When I use pressure-related boundary conditions (i.e. pressure inlet, pressure outlet...) the pressure location isn't important. In fact in the fluent user's manual it is said concerning this content: "If pressure boundaries are involved, the adjustment is not needed and the reference pressure location is ignored". So unless I impose, for example, mass_flow_inlet and outflow boundary conditions, I guess that parameter isn't involved in calcutation. Morever, if I impose Pressure_inlet and outflow boundary condition, this warning message appears: "Both outflow and pressure boundaries are present in the domain. This is an incompatibility and solution cannot proceed until this is fixed". All seems to make me choose Pressure_inlet and Pressure_outlet boundary condition.

Pretending to accept this fact, my doubts regard two things:

1. the correct value for Gauge_total_pressure in Pressure_inlet boundary condition form; this value is the relative total pressure referred to operating_pressure (in my case operating_pressure = p_amb = 101325 Pa). Now, I know the flow rate so I can calculate the value of dynamic pressure. What's the corret value for Gauge_total_pressure if I don't know the real value of static pressure at inlet? In any case it will be the sum of relative_static_pressure (that is unknown for me) and relative_dynamic_pressure (relative if I impose v_ref = 0 for the value of velocity in Reference value form)

2. is it correct modelling an exit plenum? How much large should I model it?

Thanks in advance for attention.

Hiras

umm... fluent provide information of gauge pressure result have to try to check the total pressre using contour view or XY plot?

Hi and thanks for your answer. I've checked all Pressure with contour but the values are too low and the inlet flow rate is too high (1 order of magnitude more or less).

It seems that the fan doesn't transfer energy to fluid. I'm worried because I don't see the physical behaviour neither.

Have you ever handled this type of study?

Thanks for your attention again.

Hiras

in case fan, fan transfered energy to fluid though fan in CFD simulated as fluid, but in this case u have to enter fan rpm and its axis.

if out let pressure for your case now is too low, i am agree with you that your fan doesnt transfer energy to fluid but act like turbine.

Ok but have you got any advice to solve this type of problem (validation of radial fan performance)? What's wrong in my set-up?

Hiras

PS: So far I'd like to remember you that I've used steady state solution, MRF, pressure-inlet/pressure outlet conditions, k-e standard.

Yes, you can't use the outflow BC with a pressure BC. Why not use a mass flux BC since you have the flow rate?

unless am missing something the static pressure can surely be calculated using the ideal gas law?

either that, or a mass flow rate can be calculated manually and used, since you have the flow rate, density and the area of cross section.

As for a plenum attachment, its useful if you have flow physics changing at the outlet (for ex recirculation, shockwaves etc). If it is necessary you might want to extend it until a point where the flow is going straight out ie uniformly. It really depends on your flow.

Hi and thanks for your answer.

Through the simulation I'd like to reproduce experimental results so, in my opinion, the mass flow rate and the pressure flow field should be the consequence of energy transferred by fan motion.

Conceptually speaking, pressure is the most important variable in this type of cfd study so it should manage the flow field.

H

Hi hiras, which turbuence model are you using? k-epsilon? which near wall model? Standard wall function or Enhanced wall treatment? Do you have narrow passages in your model?

regards

better u changed your boundary condition by making inlet as mass flow rate since it's a gas (though compresibility effect is very small), outlet could be use as out flow or pressure out-let with gauge pressure set to be zero.

if u want to find the static pressure in oulet (after iteration), you have to calculate its by refer to reference condition(see help appendix for this formulation)

i hope this help

Hi, I'm using k-e, standard wall function and I haven't narrow passages.

I think these inputs are less important for radial blower macro-behaviour; they probably are more important for a finer analysis. I've asked further informations about experimental data. I'll tell you about any news.

Thanks a lot for now.

Hiras

Hi Hiras, ok, if you can afford to have y+>30 because you don't have narrow passages so std wall function should be ok.

Thanx to you too

Hi,

Based on your posts, You are getting very less pressure than experimental values. If i am correct, please check the rotation speed of the fan and rotation direction once again.

For cfd simulation of fans, velocity inlet and pressure outlet is most valid boundary conditions. From simulation, how much percentage variation you are getting than experimental data. Then what about velocity values?

With warm regards, JSM

Dear Hiras, CFD users,

Initially, I decided not to interfere with your discussion, and that because of several reasons. One of those reasons was the fear of being seen in a "who the hell this guy thinks he is?" way. But now I see that this forum, instead of being helpful at solving one's problems and at the same time giving others the opportunity to learn something, is just allowing some unexperienced users to express their opinion, which is not a bad thing for a classroom-type environment, where a "teacher" can limit and correct the effects on the others, but here this kind of liberty is making a lot of damage. So I will try to asume the role of the "teacher" in this particular thread.

People, let's stop for a minute and think.

What the ... is this thing called CFD after all? In my opinion, CFD is an incredibly refined engineering instrument, a high-precision tool. But that is all. Think of CFD like a Stradivarius violin. It is so beautiful, standing there behind the glass, its reputation is making everyone marvel, but give it to a I-don't-know-anything-about-music someone and the result will just be scratching your ears. This fine instrument can really move souls only in the hands of a master. A man who knows all its secrets and thouroughly understands how it works.

Now let's go back to the topic of this thread. We have to simulate a fan. What does a fan do? It moves a mass of fluid from one space to another, someone will answer. I say OK, this is what it does, but how? And here comes the theory. There are many probable answers from all of you, but let me suggest you something: what is the "driving force" behind all fluid phenomena? And the answer is: STATIC PRESSURE GRADIENT (SPG)! You don't believe me? Then tell me: why does the wind blow, why does a shock wave brake the window, why does a plane fly, and so on? SPG is responsible for all this. But how does this apply to our problem? Well, the fan does just one thing: it modifies the static pressure field around its blades, creating a negative SPG in front of it (thus moving the air inwards), and a positive SPG behind it (thus moving the air outwards). But to acomplish that, it requires mechanical energy to be transferred to its shaft. And the ratio of the absorbed mechanical energy vs. the energy actually transferred to the fluid (internal energy), is what we call the fan's efficiency.

Now, if we know the mechanism of this process, how should we model and simulate it correctly? There are three parameters that we can influence experimentally, and only three: total pressure in front of the fan, static pressure behind the fan and fan's RPM. So, to correctly reproduce the reality, we have to do the same in the virtual space. What are the BCs implemented in FLUENT that allow us to do this?

- pressure-inlet (to control the inlet SPG);

- pressure-outlet (to control the outlet SPG);

- fluid zone rotational properties (to control the mechanical energy available for the fan).

To be able to assess the effects of one parameter on the fan's performance, we must allow only one parameter to be modified. Then, we have three possibilities:

- modify total inlet pressure (to simulate a fan that sucks air from a chamber);

- modify static outlet pressure (to simulate a fan that blows air into a chamber);

- modify RPM (available in both cases and for simulating a recirculating fan).

By modifying the pressure at constant RPM we will calculate several working points on the same working line. To calculate other working lines, we must adjust RPM and re-modify pressure. This way we can obtain the full range of fan performance levels.

Are velocity-inlet or mass-flow-inlet BCs wrong? No, though they are not natural but FORCED BCs. Both BCs impose mass-flow, which must actually be a RESULT of the simulation, as it is for the real fan!!!

Finally, I'd like to present an example: let's say we have an axial fan in a tube, and both ends of this tube are directly connected to the atmosphere. How do we correctly simulate such a fan?

* What we do know: total pressure at inlet end (atmospheric pressure), static pressure at outlet end (atmospheric pressure), fan's RPM.

* What we don't know: static pressure at inlet end, total pressure at outlet end, mass flow.

So, we impose a 0Pa gauge total pressure at inlet, a 0Pa gauge static pressure at inlet, and fluid zone RPM. And we get the mass flow. To modify mass flow, we must adjust fluid zone RPM (inlet and outlet BCs remain unchanged no matter what is the RPM).

I hope that this was clear enough for everybody, especially for Hiras. And thank you for your patience.

All the best,

Razvan

thanks to æake the things clearer and to share your knowledge with great patience and talent

Thank you Razvan. I started reading this forum only short time ago, and found all your posts really clarifying and helpful. Just one thing: in your post you said pstatic is known at outlet and is pstat=0, than two lines below I think you made typing mistake saying "0Pa gauge static pressure at inlet". Surely you meant at outlet. Razvan ca you please ocnfirm. Thank you Jo

Hi Jo,

Indeed, there is a mistake. Here is the errata:

"So, we impose a 0Pa gauge total pressure at inlet, a 0Pa gauge static pressure at inlet, and fluid zone RPM"

must be corrected to:

"So, we impose a 0Pa gauge total pressure at inlet, a 0Pa gauge static pressure at outlet, and fluid zone RPM".

Please accept my appologies.

Razvan

Hi Razvan first of all thanks for what you wrote. I'd would add something. My set-up is the same as you suggested. I agree with you and with your items (as you can read in previous answers).

Experimental structure is this: inlet-plenum -> inlet-duct (in the middle of this there is a point of gauge static pressure measurement) -> radil-blower -> outlet-duct -> p=p_amb=101325 Pa. At outlet duct flow rate was measured (so I can draw out dynamic pressure at inlet).

My boundary conditions are: Inlet (surface in which there is the measurement point): gauge_total_pressure (gauge_static_pressure_value + dinamic_pressure) fan: RPM= cost, MRF, k-e..... Outlet: Gauge_static_pressure=0

Considering that experimental data report:

1. the values of gauge static pressure at measurement-point in inlet duct are always positive

2. if previous value dicreases, increases mass flow rate.

The fact is CFD simulations give me the opposite behaviour.

Now:

1. CDF is wrong (I'm just joking)

2. I did big mistake (and I haven't found it jet....)

3. My set-up (model) is different from experimental data

The last item made me ask further information about data obtained.

I'll tell you about news. Thanks another time.

Hiras

[chaudhry_hashim]

Hi I am quite new to CFD i am trying to find out the fan curve. My fan diameter is 71mm and what did uptill now I made inlet duct 15 times of fan dia with pressure inlet (0.0 Pa), outlet duct 30 times of fan dia with pressure outlet (0.0 Pa) and I am giving fixed rpm to the rotating region in between. I am measuring pressure in inlet and outlet duct at a position 10 times of fan dia. but Still I didnt find the relevant pressure difference across the fan and also the solution is not converges. If i want to give the value of dynamic pressure at the inlet then how can i calculate this value as i know the flowrate.
Although I am working in the same way as hiras worked that I am using steady state solution, MRF, pressure-inlet/pressure outlet conditions, k-e standard.
I have attached the pictures of model and mesh kindly take a look and also let me know whether my geometry is correct or not

I would be very grateful if you people help me out