Download Computational Hydraulics, Lecture Notes- Physics - 1 and more Study notes Physics in PDF only on Docsity!
STAR-CCM+ SPRING 2011
- Notes on the software
- Assigned exercise (hand-in deadline: Friday 25th^ February, 10 am)
1. NOTES ON THE SOFTWARE
1.1 About STAR-CCM+
STAR-CCM+ is a general-purpose CFD solver. It comes as an integrated product providing solid-modelling, meshing, solving and post-processing capabilities.
1.2 Running STAR-CCM+ in the Pariser Computer Cluster
Save files initially in the c:\work folder, not your P-drive or a pen drive. STAR-CCM+ generates a single simulation file (.sim), which can subsequently be transferred elsewhere for archiving.
Start STAR-CCM+ from the Start menu: All Programs > EPS > MACE > Star CCM+ 5.04.006 > Star CCM+ 5.04. If this is the first time that STAR-CCM+ has been run on a particular cluster PC then it will take (a considerable) time to download the software.
1.3 Main Steps in a Simulation
- Start server process (File > New Simulation)
- Create a model geometry: 1.1 Create a solid model (Geometry > 3D CAD Models); 1.2 Create a geometry part ((right-click the CAD model) > New geometry part) 1.3 Create a Region ((right-click the geometry part) > Set region)
- Define a fluid continuum: 2.1 Set up (Continua (right-click) > New > Physics Continuum) 2.2 Choose model equations (Continua > Physics > Models (right click))
- Define boundary types (Regions > Body > Boundaries)
- Generate a mesh: 4.1 Set up (Continua (right-click) > New > Mesh Continuum) 4.2 Choose mesh type (Continua > Mesh > Models (right click)) 4.3 Generate (button on toolbar)
- Set inlet boundary values (Regions > Body > Boundaries)
- Set stopping criteria
- Set up reports/monitors/scenes
- Run
- Analysis and plotting
Use the residuals plot to check convergence. Check that any force monitors have reached a steady value. Watch the Output window for any “interesting” warnings.
1.4 Choice of Model Equations
To get the full range of turbulence models (and have better control over other choices):
- uncheck the “Auto-select recommended physics models” box when setting models.
For the type of incompressible, high-Reynolds-number flow calculations in this course:
- choose the segregated not the coupled solver (and use the solver properties to change under-relaxation factors if necessary);
- specify constant density rather than ideal gas (otherwise you will have to solve for enthalpy in order to find temperature);
- use the standard k - turbulence model.
1.5 Choice of Mesh Models
I recommend:
- Surface Remesher
- Polyhedral Mesher
- Prism Layer Mesher The last of these puts thin prismatic cells near any solid boundaries. For this to work, you must define the appropriate boundaries as walls before generating a mesh.
The mesh base size is used throughout by default unless you explicitly override it for a particular boundary, so set it to a reasonable value (or you will get far too many cells!). Then use the mesh properties of individual boundaries to refine the mesh near them.
1.6 Convergence Criteria
The default stopping criterion for STAR-CCM+ is the number of iterations. This is not an adequate measure of convergence. For this coursework use the following stopping criteria:
- monitors for mean-flow variables (continuity; x -, y -, and z -momentum)
- set a minimum value of 10–4^ for normalised residuals;
- use boolean AND; (i.e. this condition must be met for convergence);
- maximum steps (the default stopping criterion);
- increase the number of iterations if necessary;
- use boolean OR.
1.7 Force Coefficients
A drag coefficient is defined as
U A
F
cD (^) 2 2 0
where F is the force on an object (in the direction of the approach flow), is density, U 0 is approach flow velocity, A is the projected area of the body normal to the flow.
To ask the code to compute this:
- Create: (Reports (right click) > New Report > Force Coefficient)
2. ASSIGNED EXERCISE: Air Flow Around Buildings
Use the inbuilt solid-modelling capabilities to create the building complex shown. Taking the origin at ground level where the two south faces of the main blocks meet, the fluid domain can be generated by subtracting the bodies making up the building complex from an outer cuboid with limits –50 < x < 50 –50 < y < 50 0 < z < 40 All dimensions are in metres. x and y directions correspond to east and north, respectively.
Consider incident air flow from the north. You should assign boundaries: inlet on the north side of the domain; on this boundary set a velocity of 10 m s–1, turbulent intensity 0.05, turbulent length scale 0.1 m; pressure outlet on the south side of the domain; symmetry planes on east, west and top of the domain; wall on the building surface and the bottom boundary. (In order to set different distinct mesh sizes and calculate forces on the appropriate parts, create separate boundaries of type wall for the building faces and for the bottom boundary).
Generate a polyhedral mesh (base size 5 m) with a prism sublayer (thickness 0.25 m). Override this on the building surfaces only, by setting the mesh surface size there explicitly (minimum 0.1 m; target 0.5 m).
Initialise flow properties (Continua > Physics > Initial Conditions) with the same values as at inflow.
Compute the flow, making sure that there are sufficient iterations for convergence to a tolerance of 1.0× 10 –4^ in the mean-flow equations. Increase the maximum number of iterations and restart the solver if necessary.
Submit the following in a report (without any additional explanation!) (1) A limited screen dump showing the feature tree for the 3D-Cad modeller.
(2) A statement of how many cells, faces and vertices are used. This is output at the end of mesh generation. (It can also be found under Representations > Volume Mesh > Finite Volume Regions > …)
(3) The graph of residuals history.
(4) Suitable plots for the following:
2 3 4 2
4
10
10
6
8
2
12
NORTH
EAST
z
- building geometry;
- mesh;
- velocity vectors on one horizontal and one vertical (north-south) plane;
- streamlines (starting from an upstream horizontal line);
- shaded pressure distribution on the buildings and ground.
(5) The summary report for the calculation (File > Summary Report). Unless you want to wipe out all of your printer credit you should omit the materials database at the end!
Use your own judgement in deciding which plots to employ to illustrate the main features of the results. These should be formatted carefully in order to convey useful information – not just a smudge of lines or vectors. Unless there is a good reason to the contrary, a plot of a plane should be viewed perpendicular to that plane.
** You will be penalised if the total page count for items 1-4 exceeds 6 pages **
