Download Computational Hydraulics, Lecture Notes- Physics - 4 and more Study notes Physics in PDF only on Docsity!
STAR-CCM+ Exercise SPRING 2011 Deadline: Friday 8 April, 10 am
- Notes on the software
- Assigned exercise 1. Notes on the Software
1.1 Features
New features introduced in this exercise include:
- passive scalar ā an additional scalar-transport equation for concentration of pollutant
- user-defined field functions ā to set inflow profiles, calculate and plot new functions
- reports ā extract forces, averages, max and min etc. on specified parts
- extraction and export of data at specified points
- x-y plots
- additional derived parts ā line probes, isosurface, etc.
Most of these will be demonstrated in class; refer to the help system for further guidance.
1.2 Summary of Main Steps in a Simulation
0. Start server process (File > New Simulation) 1. Create a model geometry: 1.1 Create a solid model (Geometry > 3D CAD Models) 1.2 Create a geometry part ([rc the CAD model] > New geometry part) 1.3 Create a Region ([rc the geometry part] > Set region) Specific boundaries are best named at the CAD stage, but can be manipulated later. 2. Define a fluid continuum and model equations: 2.1 Set up (Continua [rc] > New > Physics Continuum) 2.2 Choose model equations (Continua > Physics > Models [rc]) 3. Define boundary conditions: 3.1 Define types (Regions > Body > Boundaries) **3.2 Set inflow boundary variables
- Generate a mesh:** 4.1 Set up (Continua [rc] > New > Mesh Continuum) 4.2 Choose mesh type (Continua > Mesh > Models [rc]) 4.3 Set default mesh parameters 4.4 Set part-specific mesh parameters (if required) 4.5 Generate mesh (button on toolbar) **5. Set up any reports, monitors or scenes used to check progress
- Set stopping criteria** (Stopping Criteria [rc] > Create from Monitor) 7. Run (button on toolbar) 8. Analysis and plotting (reports/derived parts/scenes, ā¦)
Use the residuals plot to check convergence. Check that any monitors have reached a steady value. Watch the Output window for āinterestingā warnings.
1.3 Model Physics
To have better control over the choice of models, uncheck the āAuto-select recommended physics modelsā box. For this coursework use the following model physics:
- 3-dimensional
- steady
- gas (constant density)
- segregated flow solver
- turbulent; standard k - model with wall functions
- passive scalar (you will then need to go to the Passive Scalars node, add a new passive scalar and rename it as āconcentrationā.)
1.4 Mesh
For this coursework use the following mesh models:
- Surface Remesher
- Polyhedral Mesher
- Prism Layer Mesher (boundaries to be used as walls must be set beforehand)
1.5 Convergence Criteria
For this coursework use the following stopping criteria:
- monitors for mean-flow variables: continuity; x -, y -, z -momentum (tolerance 10ā4).
- monitor for passive scalar (tolerance 10ā3).
It is your responsibility to make sure that the calculation has genuinely converged, not just reached the default criterion of maximum steps. The number of steps is cumulative: increase the maximum number to be allowed if necessary. Make sure that your additional monitors all have a Boolean condition of AND: i.e., convergence is not obtained until all are satisfied.
1.6 Reports
Reports are used to analyse data on one or more bodies or parts. Examples include forces (or force coefficients), area or volume averages, maximum and minimum values.
You will usually have to define:
- the parts on which the report is to be applied;
- the directions (for forces, projected areas, etc);
- other parameters (e.g. reference density, velocity, area in force coefficients).
If the flow has already been computed, run a report by right clicking and choosing Run Report. The result will appear in the output window.
The right-click options also allow reports to be used during the calculation as monitors. These appear with the default monitors (equation residuals) and can be used to check progress.
2. ASSIGNED EXERCISE
The object of the exercise is to compute flow and dispersion around the power-station complex shown. Detailed dimensions are given in the Appendix. Primary quantitative outputs will be the force on cooling tower 1 (CT1) and maximum ground-level concentration (glc) from the roof-level release.
2.1 Set-Up
Geometry
Construct the geometry using the built-in CAD system. The fluid domain may be created by subtracting all individual components (simultaneously) from an outer cuboid which extends 100 m in each cardinal direction from the point O (see the Appendix) and to a height of 60 m. For the purpose of this exercise the cooling towers may be treated as solid blocks (even if they would obviously not then function as cooling towers!). For consistency, please adhere to the coordinate system in the Appendix.
Generate solid bodies by extruding or revolving individual sketches without merging. Then use Boolean operations to combine or subtract the bodies. To isolate forces on individual buildings it is recommended that you create separate part surfaces for each building. (Multiple faces can be selected and combined using CTRL-click.) These are best named before subtracting from the outer block.
A separate surface for the roof-level release may be created by imprinting a block with the correct face area onto the required block. (The block used to imprint may then be deleted).
Boundary Conditions
Set the southern boundary as an inlet, the northern boundary as a constant-pressure outlet and the western, eastern and top boundaries as symmetry planes (to simulate far-field conditions). The section of the roof of R1 used for emission should also be defined as a velocity inlet. The ground boundary should be treated as rough (with Nikuradse roughness 0.25 m), but all other walls treated as smooth.
On the south boundary, use your own Field Functions for the inflow mean velocity U , turbulent kinetic energy k and turbulent dissipation rate. The mathematical forms to be used are typical of rough-wall boundary layers, such as the atmospheric boundary layer:
ln( ) 0
z
u z z U
k = C ā 1 /^2 u^2 (which is constant)
z z
u
Here, take z 0 = 0.1 m and calculate u ^ so as to give U = 10 m sā1^ at z = 10 m. The turbulence
parameters are C ^ = 0.09 and = 0.41. Note that, as the coding of field functions is similar to
the C family of programming languages, the coordinates are numbered 0, 1, 2 and not 1, 2, 3! In particular, z can be obtained as $Position_2. Turbulence on the inlet boundary is then specified in terms of k and (via Field Functions), rather than the default turbulence intensity and viscosity ratio. The passive scalar should have a value 0 at inlet.
The emission section in the roof should have a uniform inflow velocity 0.5 m sā1, with turbulence intensity 0.1 (i.e. 10%) and turbulent viscosity ratio 1000. The passive scalar should be set to 1 here (all concentrations are then fractions of the concentration at release).
Mesh
For a full CFD investigation it would be necessary to do a detailed set of calculations with different meshes. However, for the purpose of this exercise use:
- base size 5 m, surface growth rate 1.1 and prism-layer thickness 1 m;
- customised surface size (1.0 m target, 0.25 m minimum) and prism-layer thickness 0.25 m on all buildings (the surface size also applying in the emission region).
APPENDIX: BUILDING DIMENSIONS
Elevation
R
8 m
12 m
x
z
dome
radius 6 m
CT
R
CT
10 m
O
Plan
CT1 CT
R1 O R
rooftop
emission
(2 m x 2 m)
14 m
16 m
8 m
x
y
12 m
24 m 20 m
Apart from the rooftop emission, R1 and R2 are similar, as are CT and CT2.
Individual cooling towers may be formed by rotating splines defined by the three control points shown.
5 m
8 m
4 m
10 m
10 m
CT
N
