IES-VE User Forum

Hi,

I am currently trying to get results on air temperature and velocity in a mechanically ventilated room with Microflo.
It is not clear to me whether the "Import opening flow" option is somehow linked to Macroflo or not and how it works.
If my room has overpressure (more supply air then return), will Microflo calculate the airflow through windows/doors or is that in input it needs from Macroflo?

Thank you

Bets

Hi,

One of our CFD consultants (Liam) has answered these queries and asked me to copy the response here (should be informative for other users as well):

It is not clear to me whether the "Import opening flow" option is somehow linked to Macroflo or not and how it works.

When you import opening flows Microflo reads a text file outputted by VE-VISTA. The text file is located in the VISTA subdirectory of your project and has the suffix "bcf" which stands for boundary condition file. This text files has

1) the temperatures of all the surfaces: ceilings, floors, walls, windows and doors.
2) the internal gains for people, lighting etc for each zone
3) Macroflo flows through openings in a zone, internal and external, cracks etc. The flow rates and the air temperature of the adjacency.

(3) comes from the Macroflo predictions.

Microflo will set up boundary conditions for each of the flows that lie along the boundary of the computational domain. If a flow is associated with an opening or crack inside the computational domain (away from the boundaries), e.g. a door between two zones when both zones are in the CFD model, then Microflo will not set up a boundary condition

If Macroflo predicts that flow enters the CFD domain through an opening then Microflo will set up a diffuser/supply boundary with the predicted flow rate and supply temperature. If Macroflo predicts that air exits the domain then Microflo will set up an extract boundary with the predicted flow rate.

Notice that the imported conditions, (1)-(3) above, does not include:

4) room conditioning/system stuff from the building template manager
5) air exchanges specified in the air exchanges tab in the building template manger.

These two extra items have to be set up manually. If you are using Macroflo then there might only be infiltration for (5) which will have only a small effect. (4) is very important to set up correctly. You can use the "convective plant load" from the VISTA results to work out how much heat or cooling is required to set up your CFD model to match the thermal model. Use the convective portion as the radiative portion goes into heating the room surfaces (well the vast majority anyway) which are already imported.

If my room has overpressure (more supply air then return), will Microflo calculate the airflow through windows/doors or is that in input it needs from Macroflo?

This question isn't easy to answer as

1) apacheSim/Macroflo doesn't include the physics to model pressurisation of a zone.
2) apacheHVAC/Macroflo has the physics but system data is not imported into Microflo so you still have things to setup manually anyway.
3) there are a number of ways to model mechanical ventilation, natural ventilation and mixed ventilation in the VE

In reality, if you are supplying air at a greater rate than extracting, the extra air leaks out of the building/zone somewhere until there is mass conservation, i.e. what goes in come out. Therefore if you are using apacheSim/Macroflo you can make an assumption of where the air leaks out. Usually the supply and extract rates are pretty close so you can just increase the extract rate from the boundary(s) that represent the extract for your system. OK all the air that would leak out of window cracks, under doorways, etc., is then assumed to exit the extract(s) but if the supply and extract rates are close this assumption will be fine.

Hi,

thank you for the quick reply. It just leaves me with few more questions:

PCully wrote:If Macroflo predicts that flow enters the CFD domain through an opening then Microflo will set up a diffuser/supply boundary with the predicted flow rate and supply temperature. If Macroflo predicts that air exits the domain then Microflo will set up an extract boundary with the predicted flow rate.

This will be automatically done by selecting the option "import opening flows", right?

PCully wrote:(4) is very important to set up correctly. You can use the "convective plant load" from the VISTA results to work out how much heat or cooling is required to set up your CFD model to match the thermal model.

Are you suggesting to use the "convective heat plant load" to determine flow rate and temperature of air to be supplied to the room in order to keep the set point temperature? Is there any other input to be set up in Microflo relative to (4)?

PCully wrote:In reality, if you are supplying air at a greater rate than extracting, the extra air leaks out of the building/zone somewhere until there is mass conservation, i.e. what goes in come out. Therefore if you are using apacheSim/Macroflo you can make an assumption of where the air leaks out.

I agree the extra air will leak out somewhere else, my problem is exactly to predict where the air leaks out (in my case the supply and extract rates are not close). Would it be correct to do as explained in the following points?

A. run Apachesim with active link to both Macroflo and ApacheHVAC (by setting the right supply and extract rates in ApacheHVAC I would expect to see where the extra air would leak out of the Macroflo openings)
B. import boundaries condition from the bcf to Microflo
C. set in Microflo the correct flow rates through HVAC diffusers/extracts (same as the flow rates set in ApacheHVAC - I am working with constant flow systems so flow rates are independent from other parameters)

Any suggestion on easier/quicker ways to model this is more than welcome

Thank you

Bets

This will be automatically done by selecting the option "import opening flows", right?

Correct.

Are you suggesting to use the "convective heat plant load" to determine flow rate and temperature of air to be supplied to the room in order to keep the set point temperature?

If your system provides heating or cooling by delivering air at a different temperature to the room air then use
Q = rho * vdot * Cp * (T_sup - T_ext)
where, Q is the convective room plant load (W), rho is the density of air which in Microflo is 1.2 kg/m3, vdot is the supply volumetric flow rate (m3/s), Cp is the specific heat capacity of air (J/kg/K), T_sup is the supply temperature, and T_ext is the extract temperature.

You don't know T_ext before the simulation is complete but it can be estimated from the air temperature prediction from apacheSim (Troom) which you can find in VE-VISTA. So

Q = rho * vdot * Cp * (T_sup - T_room)

Q, rho, Cp and T_room are known which leaves vdot and T_sup. Hopefully your system fixes either T_sup or vdot so the other can be calculated.

Once the CFD simulation is complete you can compare T_room to T_ext to see if they are similar. If they are similar then you have managed to produce a CFD simulation that represents the thermal model. If they are not similar then either:
1) you have setup your CFD model incorrectly, or
2) the 'stirred tank', or fully mixed air, assumption of the thermal model is invalid
You have to use your engineering judgement to determine where it is (1) or (2).

An example of (2): A small office space that has high level slot diffusers with a flow angle of 45 degrees from the vertical and the extract point is close to the ceiling. If you model this in apacheSim/apacheHVAC as one zone (which assumes one air temperature per zone) then basically the air temp at the ceiling is the same as that in the occupied region for both winter and summer, or in other words when you query VE-VISTA there is one air temperature for the room.

In a CFD model, in summer when the slot diffusers are supplying cool air, the air will descend to the occupied region and warmer stale air is extracted at high level. In this case the extract temperature will be very close to average air temperature of the room and the CFD and DTM (dynamic thermal model) will give a similar results (the average air temp over the whole CFD volume will be almost equal to the DTM value) and using Troom as a substitute for T_ext in the above equation will be accurate.

In winter, when the slot diffusers are supplying warm air, warmer supply air will stratify before being extracted at high level and will bypass the occupied region. In this case Troom from the DTM will not be equal to T_ext in the CFD model so you are not supplying the same Q in the CFD model to the DTM model. You can add the new CFD calculated value of T_ext back into the equation to predict what T_sup should be to give the correct Q and redo the CFD model. But this will change the CFD results again so you may have to hand iterate on T_sup.

You also have to be wary as you may be trying too hard to replicate the DTM results and instead you should admit that the DTM assumption of fully mixed air is not a valid one. It may be the case that you have to consider your control strategy and the positioning of you thermostats. The CFD may show you that in winter, because of stratification, you are not able to achieve thermal comfort with your design.

Is there any other input to be set up in Microflo relative to (4)?

If your system provides heating or cooling by means of radiators, chilled ceilings, etc., then the process is different to that described above.

If you have underfloor heating then you use Q from VE-VISTA to set up a "Heat" boundary on the floor surface. The "Heat" boundary requires the user to specify a heat flux (W/m2), therefore divide Q by the floor area of the zone in question. Similarly if you have a chilled ceiling a heat boundary with a negative heat flux value will supply cooling.

The confusing bit with using heat boundaries to set up the system in Microflo occurs when you have chosen to automatically import the convective room gains rather than setting them up manually. When you import room gains Microflo automatically spreads the room gains over the whole zone in question, from floor to ceiling height. Then Microflo allows the user to add some of those gains in manually.

E.g. For the timestep exported from VE-VISTA in a small office zone there are the following heat gains: convective occupant gain = 60W; convective lighting gain = 100W; and convective computer load = 100W.

When you first import the boundary conditions Microflo spreads 260W from floor to ceiling height. The 260W number can be found in "Model" mode (the highest level of Microflo) in the "Heat Gain (W)" text box. If you then choose to put in a 60W component to model the position of the person more accurately Microflo will subtract the 60W component you have in the model from the 260W and spread the resulting 200W from floor to ceiling height. There will then be 260W in the "Heat Gain (W)" text box and 60W in the "Inc. Heat" text box and even though you have added 60W into the model manually there will still be only 260W going into that zone.

If your heating/cooling system supplies air at a different temp to the room air there is nothing more to do but if the heating/cooling is done by a heat flux boundary it gets a little confusing.

E.g. if you have underfloor heating of 1000W in the same zone, which you add using a heat flux boundary, then you have to increase the number in the "Heat Gain (W)" text box by 1000W to 1260W. Then Microflo will add 1000W through the floor, 60W through the component, and 200W into the air spread over the whole volume from floor to ceiling.

If you don't increase the number in the heat gain text box then Microflo will add 1000W through the floor, 60W through the component, and 200W-1000W=-800W into the air spread over the whole volume from floor to ceiling. In other words there will be 1000+60-800=260W in the model, which is the number in the "heat gain (W)" text box.

If this is confusing you have the option of not automatically importing the room heat gains and instead to set up all the room gains manually using components and boundary conditions. Remember only use the convective portion of these gains as the radiative portion is already counted for. The values can be found in VE-VISTA for the timestep exported.

I agree the extra air will leak out somewhere else, my problem is exactly to predict where the air leaks out (in my case the supply and extract rates are not close). Would it be correct to do as explained in the following points?

A. run Apachesim with active link to both Macroflo and ApacheHVAC (by setting the right supply and extract rates in ApacheHVAC I would expect to see where the extra air would leak out of the Macroflo openings)
B. import boundaries condition from the bcf to Microflo
C. set in Microflo the correct flow rates through HVAC diffusers/extracts (same as the flow rates set in ApacheHVAC - I am working with constant flow systems so flow rates are independent from other parameters)

Yes that methodology would work but I would take care to set realistic wind pressure coefficients via the choice of exposure type in Macroflo.

To be honest though there are loads of ways of modelling these things and you would have to do a validation study to prove if one way was better than another, e.g.
1) use CFD to predict the whole problem, airflow around the building, flow through the openings and the internal flow. Problems: Complicated, Microflo can't do it coupled (internal and external flow at the same time), plus very difficult to treat crack flows
2) if you have open windows then most of the extra airflow will choose this easier path than flowing through cracks in the building fabric so you can just assume that the extra supply air affects each window flow rate by the same amount
3) use of pressure boundaries rather than supply and extract boundaries in the CFD model. Problem: what pressure to assume if there are multiple boundaries, where to place the pressure boundaries.
4) use a mass sink in the CFD model spread over the whole zone that removes air directly from each cell in the CFD mesh. Problem: Not very accurate if there is a large difference in inflow to outflow, plus Microflo doesn't have this facility

Thank you very much Liam for the thorough explanation. It really helps understanding how Microflo works.

One more advise: how would you suggest to model an air supply through a perforated steel sheet? Is it possible to model a turbulent flow or should I just use a general diffuser to which assign the same air speed and total flow rate of the perforated steel sheet?

Cheers

Bets

Hi Bets,

One more advise: how would you suggest to model an air supply through a perforated steel sheet? Is it possible to model a turbulent flow or should I just use a general diffuser to which assign the same air speed and total flow rate of the perforated steel sheet?

All the air streams passing through the perforations should merge to produce a single jet so using a single general diffuser will be fine.

You should definitely set the correct volumetric flow rate (and hence mass flow rate) as this is the most important parameter. Velocity is important to throw but the measuring technique to supply a velocity in the data specs of different diffusers can vary significantly, so worry less about this.

You can skip the section in red as you don;t need to know this for a perforated diffuser but it may be of help if you are setting supplies that have blades to direct flow.

Microflo requires two bits of info, either
1) volumetric flow (vdot) and area (A), or
2) velocity (V) and area

If you supply (1) then Microflo calculates velocity as V= Vdot/A.

If you supply (2) then Microflo calculate the volumetric flow rate as Vdot = V * A.

But velocity V in the above equations is the velocity normal to the plane of the supply boundary.

If there is an angle to the flow out of the diffuser then the velocity normal to the surface V_norm = Vdot/A but the velocity is the direction of flow becomes

Vdot/A/cos(d)

where d is the angle of discharge to the surface normal.

You don't have to worry about this but I am telling you to show that you must be careful in specifying velocity of a diffuser rather than flow rate because flow rate is the most important number to get correct.

In your case just draw the supply diffuser to the same dimensions as the bit of the diffuser which has the perforations, i.e. don't make it as big as the total area of the diffuser if it has a big border around it that doesn't let flow out.

The flow out of the diffuser that you set up will be turbulent in the Microflo model but the user doesn't have the ability to change the turbulence values in Microflo. To be honest though setting turbulence at supplies in CFD models is a bit of an unknown in most cases and most times people just guess at it. Also if there is anything creating turbulence downstream of the inlet boundary the choice of turbulence values at the inflow boundary (within reasonable values) will have very little effect of the results.

It is much more important to get a fine mesh than worry about the inflow boundary turbulence values in my opinion.

Regards,
Liam