This is a case study/tutorial prepared by Piotr Smardz so as to demonstrate how Fire Dynamic Symulator is used.
Smoke control system for a single-storey warehouse building
1.1 The aim of described FDS simulation
The objective of this exercise is to model a natural smoke ventilation system for a typical single-storey warehouse 50x30x10 m high. The building is subdivided by a smoke screen (4.5 m deep) into two smoke control zones, each 750 m2 in area. 8 smoke vents are provided for each zone. The total area of vents is 8×2=16 m2 per zone, which is equal to approx. 2% of the floor area (see Fig.1).
1.2 Design fire:
Fire area: Af =3×3 = 9 m2 (eg. “island” of stored goods)
Fire perimeter: P = 4×3 = 12 m
Heat release rate: q = 600 kW/m2
1.3 Setting up the FDS input file
The fire scenario to be modelled in FDS is described in a text file which is called the input file. When creating an input file it is necessary to observe a required syntax of input parameters. Each command starts with the character & and is terminated with the character /.
eg. &OBST XB=0.00,3.00,0.00,4.00,5.00,7.00 /
The first line of an input file is the HEAD namelist group which determines the name of the job (input parameter CHID) and provides a short description of the problem (input parameter TITLE):
&HEAD CHID=’warehouse’,TITLE=’ smoke clearance system for warehouse building’ /
The next step is to define the computational domain. A computational domain in FDS can consist of one or more rectangular meshes (we will use one mesh in this example). Each mesh is split into rectilinear grid of cells.
The size of the physical domain and its location in the global coordinate system is defined by PDIM namelist group. We can choose any location of our domain in the global coordinate system (eg. we can position the origin of the coordinate system in the left bottom corner of our building). It should be noted that for all symmetrical problems it is desirable to set the origin of the coordinate system in the geometrical centre of the domain, as this simplifies the definition of the elements of the building.
Variables XBAR0, YBAR0, ZBAR0 describe the origin of the domain. XBAR, YBAR, ZBAR describe the opposite corner of the domain. The default value for XBAR0, YBAR0, ZBAR0 is zero (e.g. if XBAR0, YBAR0, ZBAR0 are not defined, the physical dimensions of the domain are given as XBAR, YBAR, ZBAR)
The following line defines a computational domain 50x30x10 m high, positioned in such way that the origin of the coordinate system corresponds with the centre of the floor:
&PDIM XBAR0=-25.0,XBAR=25, YBAR0=-15, YBAR=15.0, ZBAR0=0, ZBAR=10.0/
The resolution of the grid is defined not be prescribing the size of the cell but by specifying the amount of cells in each direction.
If we want to use a grid with a cell size of 50 cm in our example, we need to use GRID namelist group to prescribe 100 cells in the x direction, 60 cells in the y direction and 20 cells in the z direction (note: the Z direction is assumed to be the vertical direction):
&GRID IBAR=100,JBAR=60,KBAR=20/
Input parameters IBAR,JBAR i KBAR must be integers and they should also be of the form 2l 3m 5n, where l,m,n are integers. For example 360 = 233251 is a good grid dimension but 140 is not as it can not be presented as a product 2l 3m 5n.
The next step is to prescribe the size and location of the smoke screen. Solid obstructions such as walls, floors, columns, beams etc. are defined using OBST namelist group. It is desirable that the size of an obstruction conforms with the grid resolution (e.g. if we use 0.25×0.25×0.25 m cells, the wall thickness should be 0.25 or 0.50 m but not 0.4 m)
In our problem the smoke screen should be 4.5 m deep and it should divide the building into two smoke control zones of an approximately equal size. For easier identification of the smoke screen in Smokeview program we will assign it green colour:
&OBST XB=0.00, 0.50, -15.00, 15.00, 5.50, 10.00, COLOR=’GREEN’/
The last element of the building geometry is the location and size of smoke vents. For each smoke control zone we propose 8 no. smoke vents 2.00 x 1.00 m. To simplify the problem we will assume that the vents are open from the beginning of the simulation.
By default the planes enclosing our computational domain are defined as solid walls (i.e. the domain is a closed box). Smoke vents are a particular case of a boundary condition. They are prescribed by VENT namelist group. If we want to create a passive opening to the outside we need to assign a value OPEN to the input parameter SURF_ID. Input parameter XB in VENT namelist is a sextuplet x1,x2,y1,y2,z1,z2 denoting a plane of the desired vent.
As the VENT is always a plane, two of its six coordinates must be the same (in our case the z coordinates):
&VENT XB=6.50, 8.50, 2.50, 3.50, 10.00, 10.00, SURF_ID=’OPEN’/
The x,y coordinates of four first smoke vents are described in figure 2 below. Thanks to the proper use of the symmetry of our problem w can describe the remaining smoke vents by changing x and y coordinates into negative values (see Fig. 2)
In our simulation we will use the default mixture fraction model to describe the fire. Heat release rate of fire (per unit area) is defined by HRRPUA input parameter in SURF namelist group. We also need to assign a name to this boundary condition (e.g. fire), so that it can later be identified for a proper VENT namelist. HRRPUA is specified in KW/m2
& SURF ID=’FIRE’, HRRPUA=555/
Once heat release rate of fire is set, we can define the location and size of the area involved in fire. In FDS a fire is a particular type of a boundary condition and it is also described using VENT namelist with SURF_ID having the same value assigned as earlier describe by the relevant SURF command (in our case it is fire)
&VENT XB=-13.00,-10.00,-1.50,1.50,0.00,0.00, SURF_ID=’FIRE’/
The last parameter to define is for how long the simulation should run. In our example we will simulate 5 minutes (i.e. 300 seconds) of the fire. This is done using TIME command with variable TWFIN set to 300.
&TIME TWFIN=300/
Now that we have described our problem we need to decide which properties of the environment (e.g. smoke temperature, pressure, flow velocities etc.) we want to obtain as the result of our simulation
Gas temperatures, pressure etc. at certain point can be monitored using virtual thermocouple (THCP command). In our simulation we would like to measure the temperature of 4 different points within the hot layer (we can later use those measurements to calculate the average temperature of the hot layer). It is also interesting (as a comparison) to measure the temperature immediately above the fire.
The definition of the first thermocouple (locate 9 m above the floor) is as follows:
&THCP XYZ=-18.00,-8.00,9.00, QUANTITY=’TEMPERATURE’/
A very useful parameter that can be calculated in for any given x,y position is an averaged hot layer height (this property is often arrived at in hand calculations, hence it can be used to compare FDS results against crude estimations.
&THCP XYZ=-20.0,0.00,0.50, QUANTITY=’LAYER HEIGHT’,LABEL=’WysWG1’/
Only x and y coordinates prescribed above are meaningful as they describe the location where the hot layer height is to be measured. Z coordinate can be given any value in the range from ZBAR0 to ZBAR.
If we would like see a graphical representation of temperature field in any slice through the domain (e.g. in y=0.00 plane) we need to use SLCF command:
&SLCF PBY=0, QUANTITY=’TEMPERATURE’, VECTOR=.TRUE. /
Now we only need to save the created input file which we will name warehouse.data
The FDS simulation is started by invoking the following command in Windows command line:
C:nistfds fds4.exe < magazyn.data
The ready input file magazyn.data is presented below:
&HEAD CHID=’magazyn’,TITLE=’Symulacja pozaru w hali magazynowej’ /
&GRID IBAR=100,JBAR=60,KBAR=20 /
&PDIM XBAR0=-25.0,XBAR=25,YBAR0=-15,YBAR=15.0,ZBAR=10.0 /
&SURF ID=’FIRE’,HRRPUA= 555 /
&TIME TWFIN=300 /
&OBST XB=0.00,0.50,-15.00,15.00,5.50,10.00, COLOR=’GREEN’/
&VENT XB= 6.50,8.50,2.50,3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= 16.5,18.5,2.50,3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= 6.50,8.50,8.50,9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= 16.5,18.5,8.50,9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -6.50,-8.50,2.50,3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -16.5,-18.5,2.50,3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -6.50,-8.50,8.50,9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -16.5,-18.5,8.50,9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -6.50,-8.50,-2.50,-3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -16.5,-18.5,-2.50,-3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -6.50,-8.50,-8.50,-9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= -16.5,-18.5,-8.50,-9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= 6.50,8.50,-2.50,-3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= 16.5,18.5,-2.50,-3.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= 6.50,8.50,-8.50,-9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB= 16.5,18.5,-8.50,-9.50,10.00,10.00, SURF_ID=’OPEN’ /
&VENT XB=-13.00,-10.00,-1.50,1.50,0.00,0.00, SURF_ID=’FIRE’/
&SLCF PBY=0.00,QUANTITY=’TEMPERATURE’,VECTOR=.TRUE. /
&SLCF PBX=-11.50, QUANTITY=’TEMPERATURE’, VECTOR=.TRUE. /
&SLCF PBY=0.00,QUANTITY=’LAYER HEIGHT’ /
&THCP XYZ=-20.0,0.00,0.50, QUANTITY=’LAYER HEIGHT’,LABEL=’WysWG1’/
&THCP XYZ=-5.00,0.00,0.50, QUANTITY=’LAYER HEIGHT’,LABEL=’WysWG2’/
&THCP XYZ=-18.0,-8.0,9.00, QUANTITY=’TEMPERATURE’/
&THCP XYZ=-18.0,8.00,9.00, QUANTITY=’TEMPERATURE’/
&THCP XYZ=-6.00,-8.0,9.00, QUANTITY=’TEMPERATURE’/
&THCP XYZ=-6.00,8.00,9.00, QUANTITY=’TEMPERATURE’/
&THCP XYZ=-11.50,0.00,3.00, QUANTITY=’TEMPERATURE’/
1.4 Reading and analysing simulation results
We can retrieve the results of the simulation in two ways. We can run a visualisation tool called Smokeview which is a companion program to FDS. We can also analyse some of the output files (e.g. thermocouples’ reading file warehouse_tc.csv) which were created as the result of the simulation. As most of the output files are in Comma Separated Values (csv) format, they can be used to create graphs etc. using Microsoft Excel or similar computer package.
In order to view the simulation results in graphical form we need to activate the menu by clicking the right mouse button anywhere in the Smokeview window. Then we select the desired result in the Load heading (e.g. temperature in slice y=0.00 – see figure 3 below). Only parameters defined as required results in the input file can be viewed.
Thermocouple measurements can be found in warehouse_tc.csv output file. This file can be viewed using any popular spreadsheet editor (e.g. MS Excel).
It should be remembered that a fire is an extremely dynamic phenomenon and therefore the thermocouple results will exhibit substantial readings fluctuations as indeed is the case in any real experiment.
If we want to compare the FDS results with hand calculations (which by their nature provide time and space averaged results) we need to calculate an average value of several readings. In our example it can be an average hot layer temperature based on 4 thermocouple readings. This mean value should further be averaged over certain time range (say 15 seconds) in order to eliminate the influence of short-term variation.
An exemplary printout of output file warehouse_tc.csv is presented below
Figure 4 presents hot layer height results for two locations (WysWG), hot layer temperature at four different locations (TC3 – TC6) and temperature reading 3 meters above the fire (TC7). The results are shown for the last ten seconds of the simulation.
1.5 Results validation
In the case of using FDS as an engineering tool for a real-life problem it is necessary to validate the obtained results by simple hand calculations. This will normally allow to detect any substantial mistakes that might have been made when defining the simulation.
We can use empirical correlations to obtain a “crude” check of our results.
If we assume hot layer height to be Y= 5.75 m, then the mass flow rate of smoke can be calculated as:
M = Ce P Y3/2
Ce coefficient is taken in the range from 0.188 to 0.21 depending on the building geometry (in our case we take Ce=0.21). Then
M = 0.21x12x5.751.5 = 34.7 kg/s
We can now calculate the average temperature rise in the hot layer, based on the obtained mass flow rate and the convective heat flux from fire. Let us assume that convective heat flux is approx. 2/3 (e.g. approx 70%) of the total heat relase.
Qc = 2/3 Q = 3300 kW cp = 1.01 kJ / kg K
q = Qc / (M x cp) q = 3300 / (34.7 x 1.01) = 94 oC
The average hot layer temperature is :
Tc = T0 + q = 20 + 94 = 114 oC (Tc= 387 K)
FDS results suggest lower smoke layer temperature i.e. approx. 80 oC. The difference between the two is roughly 50%. After analysing Heat Release output file warehouse_hrr.csv it is apparent that less then the assumed 66% of the total heat released in fire is transported by convection, which can partially explain the difference. Also, the results shown were obtained using a very crude grid resolution of 0.50 m, which could impact on their accuracy.
For the above parameters we can now calculate the required total area of smoke vents Av using the following formulae:
Coefficients of discharge Cv = Ci = 0.6
Outlet / inlet ratio Av / Ai = 1
Depth of smoke layer db= 10 – 5.75 = 4.25 m
The result is Av=16.3 m2 which is reasonably close to the vents area assumed in our FDS simulation.
1.6 Proposed modifications
In order to better understand the influence of certain physical parameters on the results of our simulation one can carry out the following variants of the simulation:
a) Decrease the area of replacement air inlets (i.e. the area of smoke vents in the adjacent smoke control zone) say down to 8 m2 while not changing the area of smoke vents in the zone affected by fire. It can be expected that the efficiency of the system will be decreased as an Av/Ai ratio is now increased to 2.
b) Increase the area of replacement air inlets (i.e. the area of smoke ven s in the adjacent smoke control zone) say up to 32 m2 while not changing the area of smoke vents in the zone affected by fire. It can be expected that the efficiency of the system will be increased (i.e. the smoke layer will be higher) as an Av/Ai ratio is now decreased to 0.5.
c) Change the fire location (e.g. to corner location)
If permitted by the computing power of the computer on which the simulations are carried out it is desirable to run the simulation with an increased grid resolution.
In the case of performing an FDS simulation for design purposes one should always check the sensitivity of the problem to grid resolution.
Please note that grid resolution can be easily increased two-fold by doubling all parameters of GRID command:
&GRID IBAR=200,JBAR=120,KBAR=40/
Our grid resolution is now 0.25 m and not 0.50 m as in the original example.
This modification will significantly increase the calculation time.
This article was first published on www.cfd.cad.pl
NOTE:
When preparing the above example care was taken to use realistic assumptions and input parameters. However, input properties such as design fire area, heat release rate or smoke vent area are not based on any actual design recommendations and were only selected to provide an easy illustration of the principles of modelling fire scenarios in Fire Dynamics Simulator. In the case of per
orming a computer modelling of an actual engineering problem the designer is the person solely responsible for using appropriate fire scenarios and input parameters.
