Validation of Autonomous HVAC CFD methodology - The Comfortina benchmark case
Friday, July 10, 2020
Validation of Autonomous HVAC CFD methodology - The Comfortina benchmark case
Shadab Mohammed
Blog Author - Prathamesh Badadal
Written by Prathamesh Badadal
Blog Author - Shadab Mohammed
Written by Shadab Mohammed
15 Minutes Reading
15 Minutes Reading
In any office, hotels, classrooms, or other conditioned indoor spaces, there's almost always someone who's too cold, someone who's too hot. Achieving thermal comfort in the complete occupant zone is one of the main challenges faced by HVAC engineers while designing an HVAC system for any indoor space. Selecting a suitable method to deliver ventilation and conditioned air into the space is very critical in achieving this goal. HVAC engineers need a tool that allows them to identify hot and cold pockets in the space and optimize the diffuser positions for occupant thermal comfort upfront at the design stage itself.
In 2020 simulationHub embarked on a mission to revolutionize the HVAC industry. To address the concerns of HVAC designers in the case of indoor occupant thermal comfort, simulationHub introduced "Autonomous HVAC CFD", a fully autonomous CFD web app. Through this app, we provide the engineer and the designer with a solution to the problem of design optimization of the diffuser position, comparing the performance of different HVAC systems like overhead, underfloor or displacement ventilation and hence achieve thermal comfort.
To know more about the app and experience the future of HVAC design, please visit Link to the tech preview for a technological preview.
Autonomous HVAC CFD airflow animation
Figure 1: Diffuser airflow animation in Autonomous HVAC CFD.
CFD analysis involves stages like the creation of geometry models, meshing, and solving for the given physics. In any industry, this analysis is either done by an in house CFD team or outsourced to consultancy firms. The analysis requires High-Performance Computing machines(HPC), software that requires licensing and maintenance. This results in the whole process getting costly.
Autonomous HVAC CFD has automated the whole process of CFD analysis, especially for indoor rooms. All you need is a virtual model of the design, which can be created in the app as well, and with a few clicks, the results are ready to view. This reduces the effort required on part of the designer.
The distinct advantages of Autonomous HVAC CFD over other tools available in the industry are:
No inhouse HPC setup is required, as the app performs simulations on the cloud platform
No CFD expertise is required, all the CFD process are automated
Results are accessible to the user through the web browser
To summarize, all the worries of conducting the CFD analysis are taken care of by the app itself.
In line with simulationHub's constant endeavor to empower the designer, the whole process has been streamlined and automated to give the best results in a short time as possible. In this effort, the vast experience of simulationHub's CFD expertise has been used to give the user the best result.
Being autonomous is a great help, but it is also important that the solution we are offering is reliable and accurate as well. Hence to answer this question it is necessary to conduct a "Validation study" that ensures the accuracy of the results.
In the coming time, simulationHub will be showcasing the validation studies carried out to test the methodology used in the app. These will be covering the technical aspects of the app.
This blog will give a glimpse of one of the validation studies carried out using Autonomous HVAC CFD.
Objective of the CFD analysis
The goal of the analysis is to validate the app strategy developed. We will be validating the meshing, solver setup of the app through this analysis. For this, we have considered a standard benchmark case that has been developed by Nielsen et al. to study the indoor environment of space.
This study was part of a broad study to evaluate the indoor airflow as well as contaminant exposure. Prof. Nielsen of Aalborg University spearheaded the study.
For further information on the benchmark case, the reader can refer to
Case Description
A manikin is placed inside a rectangular wind tunnel of dimension 2.44 m x 2.46 m x 1.2 m. The air is entering the domain at 22°C from one side and exits through two circular outlets on the opposite surface. The manikin is in a seated position facing the uni-directional inlet air. Also, the manikin is placed symmetrically with respect to the z plane. The wind tunnel is placed in a large room as shown below in Figure-2.
Experimental Setup Image
Figure 2: Experimental setup for the benchmark case
The experimental study was conducted for 3 different inlet velocity values of 0.05, 0.2, and 0.5 m/s. The heat flux from the manikin was specified as a sensible heat load only. No latent heat load was considered in the manikin. The manikin was a non-breathing type. Velocity was measured at distinct points along planes D, E, and F at lines A, B, and C(in the z-direction) as shown in Figure 3.
Experimental Plane Location Image
Figure 3: Measurement locations corresponding to Nielsen et al. experiments.
(Lines A, B, and C on plane D, E, F are the locations where velocity has been measured)
Past studies on the benchmark case
Researchers across the world conducted various CFD studies on this case in order to test the prediction of their solver, schemes, etc. Their assumptions and findings are summarized below:
The uniform velocity assumption at the inlet was found to be incorrect. The velocity values from the CFD studies just downstream of the inlet were deviating by 100% at some points.
It is recommended that inlet velocity be modeled based on the experimental values measured just downstream of the inlet.
Of all the 2 equation turbulence models, SST k -⍵ has been found to give better results.
The heat flux from the manikin in the experiment is 76 W, but in case if only convection is to be considered, then the value heat flux should be 38 W
From CFD studies it is observed that the maximum deviation of velocity value occurs on the plane F at the B midline of the z plane. Hence researchers tend to compare their velocity values specifically at this line sometimes.
Using these experiences we conducted the CFD analysis of the benchmark case.
CFD study
Below we describe the steps carried out in the CFD analysis of the benchmark case. As is the case in any CFD study we will elaborate on the pre-processing (geometry, meshing), solving the case(numerical setup), and finally the discussion of the results. The methodology is completely based on the app.
Geometry and mesh
In any CFD analysis after the problem formulation, the next step is the determination of the domain to be considered. We have tried to maintain the similarity of the experimental and CFD setup.
Experimental Setup Image
Figure 4: The computational domain of the CFD analysis.
In the experiments conducted, the feet of the manikin was not attached to the floor, but in our analysis to avoid the bad quality mesh, we have kept the feet attached as shown in the figure below.
Manikin Foot Image
Figure 5: Geometrical approximation of the manikin foot
The meshing was done as that is being used in the app. Mesh around the manikin was fine enough to resolve the surface features as well as able to address the requirements of the flow and turbulence model.
Manikin Mesh Image
Figure 6: Mesh resolution around the manikin.
Boundary Conditions and the numerical setup
We will be considering the 0.2 m/s inlet velocity case of the experimental study. A complete summary of the boundary conditions considered in the analysis is as follows:
Boundary conditions Inlet Manikin Outlet Walls
Velocity Velocity profile No-slip Zero gradient No-slip
Pressure FixedFlux FixedFlux FixedValue FixedFlux
Turbulence In accordance with the velocity values, length scale, and turbulent intensity Wall function for ⍵ and 1E-10 for k Zero gradient Wall function for ⍵ and 1E-10 for k
Although at the inlet we have assumed a velocity profile, we have kept the mean value to be 0.2 m/s which matches the experimental case.
The manikin heat flux is taken to be 38 W as we would be considering only convection (​Although we have considered only convection the Autonomous HVAC CFD solver is capable of including radiation effects)
The turbulence model considered is the SST k-⍵ model.
The numerical schemes have been set up in accordance with the app strategy. Residual convergence was set up to 10-6 while the outlet temperature was monitored as well.
The inlet velocity was modeled in accordance with the experimental values just downstream of the inlet. The velocity profile was 6th order polynomial. On implementing the profile it was determined that the new velocity profile matches the experimental value of 0.2m/s.
Once the velocity profile was verified a mesh independence study was performed with different mesh sizes as well as the meshing strategy used in the app. After analyzing the results, it was determined that the current meshing strategy of the app was fine enough.
Results and discussion
Following are the results obtained from the simulation based on the app methodology.
Velocity Mid-Plane Result
Figure 7: Velocity contours at midplane z=0.
Temperature Mid-Plane Result
Figure 8: Temperature contours at midplane z=0.
From Figure 7 it is clear that there is sudden acceleration at the outlets. Also the wake region extends all the way from manikin to the wall near the outlet. The temperature contour at the same plane shows that the heat is quickly dissipated by the incoming air.
Temperature on Manikin Surface
Figure 9: Temperature distribution on the manikin surface.
The temperature distribution on manikin is shown in Figure 9. In the region where the velocity of the air is low, the convective heat transfer is also less. This results in high temperature on the manikin surface especially on the back region as the velocity there is low due to the wake region as seen in Figure 8.
Velocity Result at Plane-D
Figure 10: Velocity profiles at plane D.
( circle represents experimental data, the continuous line represents CFD data )
Velocity Result at Plane-E
Figure 11: Velocity profiles at plane E.
( circle represents experimental data, the continuous line represents CFD data )
Velocity Result at Plane-F
Figure 12: Velocity profiles at plane F.
( circle represents experimental data, the continuous line represents CFD data )
For plane D the velocity results from the CFD analysis are matching with experimental results. While for plane E and F the velocity values from the CFD analysis are following the trends of experimental velocity values
The velocity at z=0 on plane F is slightly overshooting in CFD analysis as compared to the experimental measurements
For all considered points on plane F (at the respective z values), the mean relative deviation is observed to 4.47 % while the standard deviation is 18.29% with respect to experimental velocity values
The causes of deviation can be attributed to the geometry differences between experimental and CFD study, inlet velocity profile and the distribution of heat flux on the manikin.
From the above qualitative and quantitative comparisons, it is observed that our CFD results are matching well with experimental velocities and it is also following the experimental trend of velocity.
To summarize, the results reflect that the app methodology is capable of predicting the indoor environment flow physics to a good level of accuracy.
P.V.Nielsen, S.Murakami, S.Kato, et al. "Benchmark test for Computer Simulated Person" Aalborg University, 2003
N. Martinho,A.Lopes,et al. "CFD modelling of benchmark tests for flow around a detailed computer simulated person", 7th International Thermal Manikin and Modelling Meeting - University of Coimbra, September 2008
Blog Author - Prathamesh Badadal
Written by Prathamesh Badadal
Blog Author - Shadab Mohammed
Written by Shadab Mohammed