Make Your MEP Design Better Using Autodesk CFD Simulation

M. MUNIRAJULU: Hi everybody. Good afternoon. Thank you for joining the session. My voice is a little hoarse because I got cold, so pardon me on that.

I'll try to unpack how we have used Autodesk CFD for better MEP designs. Let me introduce myself. My name is Munirajulu, and you can call me MM in short, if that is easier. OK. And I am working as Chief Engineering Manager, MEP-CFD. L&T Construction, Larsen & Toubro Limited, India. L&T Construction is a major player in the construction industry in India, and with the footprint overseas.

I have been using CFD analysis in the design process for the last 22 plus years, and out of the CFD I'm using for the last four years in MEP designs, my focus areas are data center cooling, basement car park ventilation, digital ventilation, smoke simulation in buildings, for life safety. And I was first time speaker last year, and this year also I was glad-- I was fortunate to be selected to speak here.

The goal of this today's session is better MEP designs using Autodesk CFD. I'll take you through four objectives that will help us understand how to reach that goal. You can see and understand airflow and heat transfer modeling, simulation strategies and techniques used in MEP design, and key results for evaluating the performance of MEP, and then some-- finally some advantages and limitations.

Autodesk CFP can be used in MEP systems in the design of MMP systems wherever there is airflow and heat transfer. And how airflow and heat transfer is modeled in Autodesk CFD, that plays a key role in reaching the design goal.

Now all of you probably would be knowing what is CFD? CFD stands for computational fluid dynamics, and it is a process and it involves four major stages. For stage A and B, we get the input from the design team. These inputs are CAD model and the material definition, and certain design parameters, which would become boundary conditions for the CFD analysis. For stage C and D, the CFD analyst does the job of meshing, solving, and extracting key results for evaluating the design.

For airflow modeling, typically we create a fluid region or domain, include all internal obstructions for the fluid flow. We also create geometrical features that represent supply and exhaust conditions. One important tip is, it is a good practice to extending inlet and outlets to avoid any divergence, a mass imbalance, and inaccuracy in results.

For heat transfer modeling we need to be aware what type of heat transfer happens-- forced convection, natural convection, or mixed convection, conjugated transfer. In forced convection, for example, air movement takes place by fans or blowers. And here, in Autodesk CFD, the flow and heat transfer can be solved successively. You solve for the flow first and then the heat transfer. They are decoupled, and that saves some time in the solution.

And in natural convection, air movement takes place because of buoyancy due to large temperature differences. And when we are solving for natural convection, flow and heat transfer are solved together. They are coupled.

Mixed convection-- heat transfer takes place by both the forced, as well as natural convection, and predominantly buoyancy-driven. Example is the Olympic flame. And in conjugated transfer, you have your transfer taking place through conduction through solids, and then convection by liquids, are the airflow. The example is the heat transfer heat exchanger.

Another important application of Autodesk CFD is for modeling rain water flow. For example, on the airport roofs and the water drains, we use what is called as free surface modeling in Autodesk CFD. This is specifically applicable for plumbing design.

So having covered some basics, I will take you through these simulation strategies and techniques that we have used in MEP design. The first case study, or the first project case study I'm going to cover is the DG room ventilation. Why CFD simulation for DG room? Actually we had existing DG room we had two issues in the operation of their DG room. The DG sets were tripping when loaded beyond 50% of the rated load, and then the ambient room temperature was rising sharply.

So we had to find out what it would cost, so we took up CFD analysis of the DG room. And the goal of the CFD analysis is to determine airflow and temperature distribution, and then identify the root cause, then recommend a solution. And we had to use a design performance criteria. We have used air temperature less than 50 degrees around engine, and 45 degrees around alternator.

Now we start with the CAD model from Revit, and we simplified geometrical details. And here we have simplified the electrical panels. We have modeled the electrical panels as rectangular solid blocks, instead of having all the details, because those details will not play a role in the airflow or heat transfer. And also we simplified the engine on the alternator as solids bonded by regular nice surfaces. Then we add inlet and outlet.

Next step is to assign materials. We have assigned air material to the fluid domain, and aluminum material to the engine and the alternator. And see, one of the geometric simplifications that we have done is, louvers are replaced by a single, solid part. And this solid part we are assigning it assistance material-- basically that takes care of the free area, the porosity of the louver.

So we have assigned free area ratio of 0.55 in the through-flow direction. In other directions it's zero because we don't expect the flow to take place.

Boundary conditions, very important. We ought to apply correctly, otherwise the results that we get may not make sense. And here we have applied total heat generation boundary condition on the engine, alternator, and the radiator coil. These are based on the DG Indian specifications.

And then inlet BC is based on the ambient temperature and pressure, and the outlet is also ambient gauge pressure. And the flow is driven by the radiator fan, which is an internal fan.

Meshing-- Very important. The accuracy of the results depend on the meshing whether the scores are fine. So for the DC room we have used auto mesh for the overall domain, and we have given local refinement on the engine, on the alternator, and other important parts. I'll just show you those things.

So here we are given fine mesh on the engine and the alternator, this one. And then on the radiator fan we are given a uniform mesh of four to five elements here. That is important to capture the fan flow effects. And again, radiator coil. We are given the uniform mesh, and overall domain is auto mesh.

So after meshing, we set up these Solver Parameters. The heat transfer in the DG room is predominantly force convection type, so we can solve the flow first. And once the flow converges we can solve for v, heat transfer. That saves time. So here we have enabled the flow first for about 300 activations, and once that is flow parameters converge, we go to-- we switch up the flow.

We switch up the floor and then enable heat transfer here, and we solve for v, temperature distribution. OK.

Key results-- While evaluating the DG room ventilation performance we have considered three design options. The first one is our original proposed design which is an L design layout. And design option one-- we have fans installed on the roof. And design option two, we have the additional wall placed in between the alternator and the ventilation louvers.

I'll go through the results for all the three options, then we will conclude which one is better. So as-was layout-- Here, if you look at the velocity vectors in the vertical plane here, you see that the CFD results are showing the airflow is taking place directly to the radiator fan. It is actually bypassing the alternator and the engine. This ventilation air is supposed to cool the alternator and the engine, but it is actually not flowing over it, so there is a hot air recirculation happening. That is the reason why the DG room temperature is rising sharply.

So from the CFD analysis we could identify what is the root cause. The root causes, basically-- the ventilation air is bypassing the alternator and engine.

Now to solve that problem, we have considered two design options. For design option one, we are putting fans as I told you before, and these fans are actually pushing that incoming air downwards so that there is now flow happening on the alternator and on the engine. So that results into DG room temperature, which is acceptable. OK.

There is an option two, where we output the baffle plate here. The partition, it is actually gypsum board dropped from the roof. And the CFD analysis results, the velocity vector, shows that now the airflow actually happens from bottom to top, and flowing over the alternator on the engine. And this gives very good results for the DG room ambient temperature, less than 40 degree Celsius.

Now to conclude, we find the design option two is better, and it is cost effective because the cost is only the gypsum board, whereas in design option one you have installed fans and then it will involve running costs. So it is option two, it's cost effective. And we implemented this at the site, and we found that the [INAUDIBLE] are working now without tripping. And so we could avoid the warranty and performance issues. OK.

The next project case study I'm going to discuss is how we have used Autodesk CFD for smoke visibility and extraction calculations are related to smoke exhaust design. Now, the smoke exhaust design traditionally is based on air changes per hour, at least in India, but now the client and the consultants-- they are considering a performance-based design, which is based on the fire size. And, for that one, we have to use the CFD simulation and then evaluate or determine the smoke visibility, smoke temperature, air/smoke flow fields. Now, these results will be compared to the design performance criteria based on the British standard, which gives [INAUDIBLE] limits for smoke visibility and smoke temperature.

Again, for the this, also, we start with the CAD model. This building is a convention center exhibition hall, quite large. And this is divided into 10 smoke zones and we have done the CFD analysis for one typical zone. And here, also, we simplified geometry, especially the doors and then add inlet and outlet extensions. And, most importantly, we create fire part. Fire part is nothing but a short cylinder enclosed in a solid ring, which will act as a fire source in the CFD analysis. And the initial design for ventilation was based on well 12 air changes per hour for fire mode.

Materials are here. Fluid domain is assigned air material, but the material environment is variable. It means the software now will allow density variations with temperature. In the case of [INAUDIBLE] analysis, we have given the fixed properties, but here it's variable because smoke generation is driven by buoyancy.

Fire part material. We assign resistance with the high [INAUDIBLE] ratio and high thermal conductivity. And then the solid ring around it will be suppressed and the flow direction will be set to vertical. And we have to keep the fire part just above the floor, keeping a gap, this will ensure that cool air is done towards the fire source.

Boundary conditions. So here for the fire part we apply total heat generation boundary condition based on the heat release rate of the fire source, convective portion, and then we apply a scalar boundary condition of 1 that indicates that surface gives 100% of smoke.

Inlet BC. Apart from the ambient temperature and pressure, we have to specify a scalar value of 0. That means clean air is entering the building. Outlet BC is based on the volume flow rate, which is nothing but fan extract capacity.

Meshing. For evaluating the smoke generation and smoke spread, it is important that the fire part is meshed with a uniform mesh of four to five elements and then there is a good mesh below and above the fire part, so that the airflow and the smoke above will be calculated properly.

Solver settings. Now, the smoke analysis is [INAUDIBLE] driven, which means the heat transfer and the fluid flow happened simultaneously. So we have to use flow and heat transfer together. And we have set the solution mode as transient, meaning the temperature dependent analysis will be carried out with a time step of 0.5. And then for calculating the smoke visibility values, we are to set up-- we are to check the smoke visibility and then be able to give this smoke a visibility parameters-- extension coefficient, and the [INAUDIBLE] constant, and combustion particulate yield.

Since the smoke is calculated in Autodesk CFD as a scalar quantity, we are to enable general scalar with a non-zero diffusion coefficient. And then since buoyancy is involved, we set the gravity reduction in the vertically downward direction.

Key results. For evaluating the performance of the exhibition hall for smoke exhaust, we have used a three design options. The initial design is based on 20,000 CFM. And the Design Option 1 is 15,000, Design Option 2 is 12,000. So the design options are based only on the outlet boundary condition. So here we compare the smoke visibility results for all the options with respect to time from the start of fire. The 7-meter from floor-- this is the occupied space where we need the smoke free area for people to escape. So in all options-- all the design options we are seeing that the smoke is well above the 7-meter occupied space.

And, similarly, we compare the smoke temperature plots for all the three designs. So here also we see that the temperature doesn't fall below 60 degrees in the occupied space of 7-meter from the floor. The third important result is the airflow field. So here we compare that flow field and, of course, these values are acceptable because this is higher, this is a little less-- that is because of the CFM values. But the important thing is this smoke flow-- when the make up air comes in contact with a smoke flow, that velocity should be not high enough to deflect or dispose of this flow. So here we see that it is not happening. It is remaining as [INAUDIBLE] symmetric plume, that is good.

So, to conclude, all the three designs-- the initial design as well as the design options that we are consider-- all of them meet the design performance requirements. But one thing that you see here is that by doing the CFD analysis we are able to actually decide on the cost effective option-- that 12,000 CFM fan capacity-- because that will be cheaper. So you have a design option which is cheaper and which also will meet the performance requirements.

The next project case study I'm going to cover is on the basement car park ventilation. Nowadays, most commercial buildings and residential buildings, they have underground basement car parks. And there are two hazards for life safety in the basements. One of them is carbon monoxide emitted from the cars during normal use of the basement. The second one is smoke generated from the fire from the burning vehicle if there is a fire. So these-- and the ventilation system design is done with a view to either dilute these contaminants or remove them from the basement, so that life safety is ensured.

But then why we are to use CFD simulation for this? We are to use the CFD simulation because we were not sure if the ducted ventilation system will work, which is based on the air changes per hour. So Autodesk CFD as a option by carrying out airflow analysis you can check in the LMA value calculations and then the CFD-- Autodesk CFD will give you the LMA values. LMA is nothing but local mean age that is equal to the air changes per hour locally in any location of the basement that you want, which is not possible in your hand calculations or the traditional designs.

And after doing-- after getting the LMA values, we evaluate the-- we compare the LMA values and then we recommend a better solution. So here design performance criteria that we have used is LMA values in the normal mode-- should be 950 seconds or less, which is approximately 15 minutes.

CAD model. This basement is quite large, about 46,500 square meters. And the normal mode ventilation is designed based on six air changes per hour and there are eight fan rooms, both supply and exhaust, and this is adapted ventilation system.

And, of course, for the basement analysis, you don't have very critical CFD parameters to think about it. You apply the air material to the fluid domain and then give the boundary conditions for the supply and the exhaust and then do the auto mesh, and, if required, use some refinement, and then you solve for the flow alone with LMA checked in, and so you will get the LMA values. So for-- the key results for evaluating the design performance of basement would be LMA values at the occupy level, which is 1.7 meter height from the floor.

We have done the CFD analysis for a number of iterations. So these are design variants-- are-- based on supply airflow and exhaust airflow directions as well as fan capacities. So you change the directions and the fan capacity, so you get one combination.

So we have done the CFD analysis for these variations and we can now compare the results. The initial design-- LMA values greater than 15 minutes for about 73% of the area, so which means design is not satisfactory. Anyone here aware of the LMA concept, Local Mean Age, for evaluating the ventilation? You are aware of it. OK, yeah. So LMA is nothing but local mean age. It is equivalent to air changes happening at a particular location for ventilation.

Under Design Option 1, we have increased the fan capacity by 30%-- keeping the supply and the exhaust flow directions as it is in the original design. And CFD results show that LMA values have become now less than 15 minutes for about 73% of the basement area. And Design Option 2-- we have kept five fans with 30% extra CFM and three fans we doubled the CFM. And here we change the supply to vertical direction-- keeping the exhaust in the horizontal direction. So this design variant use LMA values less than 15 minutes, but almost 89% of the basement area-- quite a significant improvement.

Design Option 3. This is same as Design Option 2, but we have made the supply and the exhaust both in the vertical direction. And this option gives LMA values less than 15 minutes for almost 90% of the basement area.

And then, finally, Design Option 4. Here flow rates are doubled for all the fans. And this gives the best results. The entire basement is having very good ventilation, 98% of the area less than 15 minutes.

But I'm going to show you that best is not the better because the Design Option 4 gives the best results, but then it comes with a cost. You are to double the fan capacities, whereas Design Option 3-- it provides acceptable ventilation, but at a reduced fan capacity. Almost 78% of the fan capacity gives the required ventilation. So it's better to choose the one which works rather than the best solution here because, always, cost effectiveness is better. So we are able to actually save the cost of the fans by 22% by choosing the Design Option 3.

The next product case study I'm going to talk about is how we have used Autodesk CFD for free surface flow simulation. And this is actually to find the root cause for rain water leakage in a airport roof. So this is a actual problem.

Due to heavy rain, water leaked from the roof into the passenger area in the airport and it was thought that this leakage could be from the skylight area in the roof. So one way to find out the root cause for this leakage is to do CFD analysis of the rain water flow happening on the roof and how it comes and flows over the skylight area. And if there is a water level going above the prescribed limits, then leakage can happen. So we wanted to see that from the CFD analysis.

So CF-- using CFD analysis we can predict the water levels in the roof channels. And, based on that, I'm going to show you how we have recommended a corrective action. And then the design performance criteria here is-- water level in the roof channel should be below 65 mm because roof channels standing seams are having a height of 60 mm. So water levels should not go about that level. So that is a reason for having this design performance criteria.

This is the CAD model of the airport roof with the skylight portion. This is a skylight and this is the roof channel portion, so we are taking only a portion of the airport roof. And since the water flow is symmetrical about this skylight, we have taken axisymmetric model. And this is the axisymmetric model. This is the roof channels, and you have this connecting channel here, and this skylight is actually suppressed in this model because we don't need to have that here for the flow analysis.

CFD modeling. So we have to assign water to the fluid domain and boundary conditions. We are to apply velocity. This is based on the rainfall intensity at that particular location. Based on the rainfall intensity in the area of the roof, we can calculate the velocity. And as-- the solid parameters we set it default values in CFD software. And one other challenging thing here is that meshing. So this free surface simulation requests very fine mesh. And then the solution time can go on for days and weeks, so we have to be extra careful about the mesh size and the geometry that you are using for this analysis.

So this is the CAD model. This is the initial design, which is actually as implemented at site. So you have this connecting channel of 120 mm width in front of the skylight and we are taken about 2 and 1/2 meters of-- upstream of the skylight. And the height of each channel is 65 mm. That's why we are given that acceptance criteria of 65 mm. And this here-- the direction of water flow is shown from the roof channel it'll come and then it will join at the connecting channel. And then it'll flow over to the side channels because skylight will obstruct the water flow.

This is final design. In final design we have-- actually we have done quite a number of iterations, but I'm showing only the final design. So in the final design we have this connecting channel with 600 mm instead of 150. And we also have put extra fluid volume here to see if there is any possibility of overflow of water upstream of this.

Key results for rain water flow simulation. We use the volume of fluid as the key result and volume of fluid is nothing but-- it is fraction of water and the air. And if VOF is 0.5, that is basically the water and the air interface. So, based on this, we can decide that what are the water levels.

So here you see in the initial design-- without the VOF plots and this [INAUDIBLE] is actually-- water levels are above 65 mm. So here it-- this is a connecting channel, the water level is close to 150 mm here. And then the roof channels are actually now filled upstream to a length of about 2 meters, so, obviously, this is a problem. The water levels are basically overflowing on the roof channels and the roof channels are actually-- the standing seams are joined with a seal. That seal may not be perfect always, because it depends on the-- it is done manually. So there could be problems with sealing that perfectly. So if the water level goes above 65 mm, any gap there will lead to the leakage. So the initial design indicates basically the water levels are about 65 mm.

And then final design-- you'll see that water levels are actually confined to the connecting channel, which is basically the drain. So the goal is to ensure that the water is collected in the drain and it is diverted instead of piling up in the roof channels. So that's what we see here. And so nowhere in the channels we see the overflow of water, so it is below 65 mm here.

Conclusion. So for the final design water levels are less than 65 mm. And from this-- from the CFD results at least we can tell that water cannot leak, but then there is no guarantee, because we have not validated it. But then we implemented the solution at the actual site. We did a water flow test.

We connected some pumps and then allowed the same water to flow in the channels. And then we took videos of the water flow and measured the water levels in the connecting channel. And, surprisingly, what we have seen is the water flow pattern that you see here-- this water flow pattern-- the same thing we observed practically also. Most of the water actually getting collected here and it is not rising about 65 mm in the roof channels. So the practical test actually confirmed that the CFD results are close to the reality. And this solution was implemented and-- so now the airport is working perfectly OK and during the rainy season there is no complaints of water leakage into the passenger area. And I'm not showing that video because it's confidential. So.

So this is the conclusion. We basically-- by doing CFD analysis, we can find out the root cause, and then think about the design option, and then evaluate the design option to see if that gives you the-- or if that meets the performance criteria.

So we have seen all of the [INAUDIBLE] areas. We have seen [INAUDIBLE]. We have seen basement car park ventilation, we have seen smoke exhaust design, and then we have seen the plumbing design issue how we have resolved. So I have tried to cover how CFD can be used for all of these [INAUDIBLE] areas wherever there is a airflow and the heat transfer is involved. And we have seen that this is really beneficial. Because we are able to actually come out with a better design option and cost effective design. And also troubleshooting-- it really helps us to identify the root cause and then based on that you can suggest a solution. So having seen that, let's see what are the advantages and limitations.

Advantages. Autodesk CFD, anybody has used here? OK. So it's very easy to use. And, if done properly, it can give you better designs as I have shown you. And since the CFD results give engineering data, which is not available to you otherwise-- like velocity distribution, temperature distribution, and the scalar distribution-- so based on these values and their pattern, you can actually think about a innovative solution for the problem. And you can also come out with a cost effective design.

And, moreover, if we do the CFD analysis during the design stage itself, we can actually avoid performance or warranty issues later on. So it's a-- it will-- at least we have found it's a good practice to carry out CFD analysis, and to see that the design is meeting the performance requirements, and then go ahead with the detailed design drawings.

Limitations. As you maybe knowing, CFD model is basically an approximation to the real problem and that approximation is based on assumptions. So the CFD analysis is as good as assumptions. And it's computationally intensive. Some problems can take few hours, but some can take days and some weeks. For example, the rain water flow, it took a few weeks for us to come out with a solution. And whereas the [INAUDIBLE], we could do the analysis in 1 and 1/2 days. And if we think about the accuracy of the CFD results, we don't have actually vast amount of tested data to validate the CFD results. There is a limited test data, but that may not represent the real life situation. But with experience, and knowledge of fluid dynamics, and the software-- how the software works, you can make a good engineering judgment, so advantages actually outweigh these limitations.

So you can-- I finished quite early actually, so you can give your feedback in the AU mobile app and I'll be ready to take any of your questions now.

AUDIENCE: Do you have a place where we can look up coefficients, and something kind of like a data book--

M. MUNIRAJULU: Yeah.

AUDIENCE: --that would be useful for designs. [INAUDIBLE].

M. MUNIRAJULU: Yeah, for smoke analysis, what we require is the tenability criteria-- tenability for smoke visibility and smoke temperature. So that is a direct output from the Autodesk CFD. Now, that can be compared with the code requirements and see if they're meeting the requirements or not.

So I'm not sure if any other coefficient is required to evaluate it.

AUDIENCE: So it's just out-of-the-box [INAUDIBLE]?

M. MUNIRAJULU: Sorry?

AUDIENCE: [INAUDIBLE] Autodesk CFD?

M. MUNIRAJULU: Sorry?

AUDIENCE: These go under the default setting?

M. MUNIRAJULU: Default setting. No, no. Default settings will not work for all the problems. It depends on the problem. You have to, for example, in smoke analysis, default settings will not work. You have to choose settings. For example, if the combustion-- if the fire is flaming combustion or a smoldering combustion, based on that, the extension coefficient will be different.

Similarly, the exit signs, if they are reflective, the sign constant will be different. If they are illuminated, sign constant will be different. Sorry?

AUDIENCE: Where can we find all that data?

M. MUNIRAJULU: Sorry?

AUDIENCE: Where can I find that data?

M. MUNIRAJULU: Yeah. The fire engineering report will give that data. Normally the design team will have a fire engineering, mechanical fire engineering department. So they will have the life safety report. And it will be mentioned there. So it'll be there in the specifications for fire safety when we submit a report. So all that data is actually compiled, which we use in the safety analysis.

And another source is the SFPFPE-- Society for Fire Protection and Fire Protection Engineering. So that handbook gives a lot of data on this, the combustion particulate [INAUDIBLE], and things like that. Yeah.

AUDIENCE: Question. Is the software able to model [INAUDIBLE] of specific diffusers, like [INAUDIBLE] diffusers, for HVAC and cooling applications?

M. MUNIRAJULU: Yes, it is. Yeah, you can do that. You can do that.

AUDIENCE: Is it generic Autodesk diffuser or is it Titus model PSS I6 so that it's actually accurate [INAUDIBLE]?

M. MUNIRAJULU: Yeah. Actually Autodesk, they have simplified some diffusers to enable you to give the correct floor directions and the flow parameters. That, you can use it. But if you're using it for some kind of a research purpose, then you have to use actual diffuser geometry.

And then-- but it is very time consuming and computationally very intensive. So I think the Autodesk approach of approximating the users through direction on the flow rate, that's quite OK. Yeah?

AUDIENCE: Any thermal comfort ranges, like [INAUDIBLE] displacement ventilation like that, air velocities?

M. MUNIRAJULU: Thermal comfort?

AUDIENCE: [INAUDIBLE] and stuff like that.

M. MUNIRAJULU: Thermal comfort? Yeah. Autodesk CFD can be definitely used for evaluating the thermal comfort in terms of--

AUDIENCE: Like that [INAUDIBLE]?

M. MUNIRAJULU: Yeah. So yeah. Yes. For thermal comfort, we use what is called is the PPV and the PME values. Make it basically a number of people dissatisfied and you know, those values.

So those ranges are available from ASHRAE. So we can use that as a guideline. And the software also will give you that output, PME output in terms of a range of values it will get. Similarly, PPV values also it will give. Yeah.

AUDIENCE: What CFD software were you using before Autodesk. And what was it that you liked about Autodesk software that made you switch?

M. MUNIRAJULU: Actually, I have used Fluent. I have used CFX. I have used also, Star CCM Plus. Then the latest is Autodesk CFD. And I recently we have purchased Fluent, which is a specific HVAC software.

But the problem with the HVAC, the flow interned-- there is one more software called FDS, fire dynamic simulator, which is specifically used for a fire simulation. So this Fluent and FDS, they are based on the directly near coordinates. So capturing the code geometry will be like a little challenging in those software. But in Autodesk CFD, which is based on finite volume method, you don't have that problem. The geometry will be well resolved.

And you will not lose the geometry data in Autodesk CFD. But the other softwares like Fluent and FDS, it is based on finite volume method, and based on the regular rectilinear grade. So you will lose basically geometrical data. And if you don't want to lose the data, then you ought to actually refine the message so much, it will be almost impossible for you to solve some practical problems.

So I find Autodesk CFD that way practically useful, because you have the CAD model and the Revit. And then you take the CAD model, import it into the CFD. And then before that, you can clean up a bit, because you don't need all the details from the Revit model. And so that works fine, actually. But there are limitations in the Autodesk CFD.

For example, for basement ventilation, we will be able to get only LMA values, local mean age values, but you won't be able to get carbon monoxide levels in PPM, because some standards like ASHRAE, they mention CO level should be below 50 PPM like that. So Autodesk CFD has a limit. It doesn't have actually that capability of calculating CO levels or any contaminant level in terms of PPM, because it uses what is called a scalar diffusion option, which will be in the range of 0 to 1. So that is a limitation here.

And Autodesk CFD, another problem is if you want to calculate variation related problems, we have found there is a difficulty in getting meaningful results. If you include variation, the convergence issues and meaningfulness of the reserves. So we really stop trying variation problems with Autodesk CFD. But for all other purposes, we found it very practical and useful. And we are using it extensively.

AUDIENCE: Have you used CFD for wind analysis on buildings?

M. MUNIRAJULU: Yes, wind analysis, we have used actually. Recently, the prime minister of India has inaugurated the tallest statue in India that is actually taller than the Statue of Liberty. And that project we did it. Design and engineering and construction, we did that project. And there I, was involved in the CFD analysis.

So that statue is supposed to be ventilated inside. So the ventilation air should come from outside. Now that ventilation effect depends on the wind speed and direction and things like that. So we did the external flow analysis over the statue. And we found out what are the pressures on that statue at various locations.

And then based on the pressure coefficients, our engineering team identified what should be the ventilation lower sizes and things like that. So external aerodynamics is possible with Autodesk CFD. We have done it.

It gives whatever results you want, basically the pressure ratios, pressure coefficients. Any more questions?