Introduction to CFX. Workshop 1 Mixing T-Junction презентация

Workshop 1 Mixing T-Junction

Welcome! This introductory tutorial models mixing of hot and cold water streams The workshop starts from an existing mesh and applies boundary conditions to model a cold main inlet and a hot side inlet Analysis goals for this type of problem could be to determine: how well do the fluids mix? what are the pressure drops? Note: It’s a good idea to identify the quantities of interest from the start. You can use these to monitor the progress of the solution

Pre-processing Goals Launch CFX-Pre from Workbench Use pre-defined materials Define the fluid models in a domain Create and edit objects in CFX-Pre Define boundary conditions Set up monitor points using simple expressions

Start in Workbench The first step is to start Workbench: From the windows Start menu, select Programs > Ansys 12.0 > Workbench When Workbench opens, select File > Save and save the project as MixingTee.wbprj

Start a CFX case Next, expand the Component Systems toolbox and drag a CFX analysis into the top left area of the Project Schematic Double-click on Setup to launch CFX When CFX-Pre opens, right-click on Mesh in the Outline tree and select Import Mesh > ANSYS Meshing Select the file fluidtee.cmdb and click Open

CFX-Pre GUI Overview Outline Tree New objects appear here as they are created Double-click to edit existing object New objects are often inserted by right-clicking in the Outline tree Message Window Warnings, errors and messages appear here

CFX-Pre Mesh and Regions A domain named ‘Default Domain’ is automatically created from all 3-D regions in the mesh file(s) A boundary named ‘Default Domain Default’ is automatically created from all 2-D regions for each domain

CFX-Pre – Domain settings The first step is to change the domain name to something more meaningful. Right-click on Default Domain in the Outline tree Select Rename The domain name can now be edited Change the domain name to junction

CFX-Pre – Domain settings (continued) Double-click on the renamed domain junction

CFX-Pre – Domain settings (continued) Click the Fluid Models tab In the Heat Transfer section, change Option to Thermal Energy Heat Transfer will be modelled. This model is suitable for incompressible flows Leave all other settings as they are The k-Epsilon turbulence model will be used, which is the default Click OK to apply the new settings and close the domain form

Boundary Conditions

CFX-Pre – Inlet boundary conditions Now that the domain exists, boundary conditions can be added Right-click on the junction domain Select Insert > Boundary

CFX-Pre – Inlet boundary conditions (contd.) Leave the Boundary Type field set to Inlet Set Location to inlet y The available locations can be found in the drop-down menu of the extended “…” menu

CFX-Pre – Inlet boundary conditions (contd.) This inlet will have a normal speed of 5 m/s and temperature of 10°C. Click the Boundary Details tab Enter a value of 5 for Normal Speed. The default units are [m s^-1] Enter a value of 10 for Static Temperature. Use the drop-down menu to the right of the field to change the units to C (Celcius) Click OK to apply the boundary and close the form

CFX-Pre – Inlet boundary conditions (contd.)

CFX-Pre – Inlet boundary conditions (contd.) This inlet will have an inlet speed of 3 m/s and temperature of 90°C. Click the Boundary Details tab Enter a Normal Speed of 3 [m s^-1] Set the Static Temperature to 90 [C] (make sure the units are correct!) Click OK

CFX-Pre – Outlet boundary conditions

CFX-Pre – Wall boundary conditions The default boundary condition (junction Default in this case) comprises of all the 2-D regions not yet assigned a boundary condition. Right-click junction Default, select Rename and change the boundary name to wall

CCL at a Glance Right-click on inlety and select Edit in Command Editor Close the Command Editor after taking a quick look at the CCL definition of the Inlet boundary condition

Initialisation Automatic: This will use a previous solution if provided, otherwise the solver will generate an initial guess based on the boundary conditions Automatic with Value: This will use a previous solution if provided, otherwise the value you specify will be used

Solver Control Double-click on Solver Control from the Outline tree The solver will stop after Max. Iterations regardless of the convergence level Advection Scheme and Timescale Control will be discussed later Residuals are a measure of how well the posed equations have been solved. In this case the solver will stop when the RMS (Root Mean Squared) residuals have reached 1.E-4. Tighter convergence is achieved with lower residuals. Click Close

CFX-Pre – Monitor points Double-click Output Control from the Outline tree On the Output Control form, select the Monitor tab Check the Monitor Options box Click the New icon Set the Name to p inlety and click OK

CFX-Pre – Monitor points (continued) An expression will be used to define the monitor point. Set Option to Expression Enter the expression: areaAve(Pressure)@inlety in the Expression Value field The expression calculates the area weighted average of pressure at the boundary inlety. Note that expressions and expression language will be covered in more detail elsewhere.

CFX-Pre – Monitor points (continued) A second monitor point will be used to monitor the pressure at the second inlet, inletz. Click the New icon Set the Name to p inletz and click OK

CFX-Pre – Monitor points (continued) An expression will be used to define the monitor point: Set Option to Expression Enter the expression areaAve(Pressure)@inletz in the Expression Value field Click OK to apply the settings and close the Output Control form The expression calculates the area weighted average of pressure at the boundary ‘inletz’. These monitor points will be utilised during the solution process in a later part of this tutorial.

Solution Goals Launch CFX-Pre from Workbench. Use pre-defined materials. Define the fluid models in a domain. Create and edit objects in CFX-Pre. Define boundary conditions. Set up monitor points using simple expressions.

Obtaining a solution Exit CFX-Pre When running in WB the CFX-Pre case will be saved automatically Save the Workbench project In Workbench, double-click Solution to launch the CFX Solver Manager

Obtaining a solution (continued) The CFX Solver Manager will start with the simulation ready to run. Click Start Run to begin the solution process

Post-processing Goals Launch CFX-Pre from Workbench. Use pre-defined materials. Define the fluid models in a domain. Create and edit objects in CFX-Pre. Define boundary conditions. Set up monitor points using simple expressions.

Launching CFD-Post Exit the CFX Solver Manager Save the project Double click Results to launch CFD-Post

CFD-Post Overview Selector Window Lists currently defined graphics objects. Object for each boundary condition are created automatically Object are edited by double-clicking or right-clicking on the object The check boxes next to each object turn the visibility on or off in the Viewer Details Window When you edit an object the Details window shows the current object status

CFD-Post – Manipulating the view When the results are loaded, CFD-Post displays the outline (wireframe) of the model The icons on the viewer toolbar control how the mouse manipulates the view

CFD-Post – Temperature contour plot In the first step, you will plot contours of temperature on the exterior walls of the model Click the Contour icon from the toolbar Click OK to accept the default name Contour 1 Set Locations to wall

CFD-Post – Temperature contour plot (contd.)

CFD-Post - Temperature contour plot (contd.) A temperature contour plot on the walls should now be visible. Try changing the view using rotate, zoom and pan. You may find it easier to use the middle mouse button in combination with <Ctrl> and <Shift> Also try clicking on the axes in the bottom right corner of the Viewer

CFD-Post Location: Points, Lines, Planes, Surfaces, Volumes Vector Plots Contour Plots Streamline Plots Particle Track (if enabled in CFX-Pre)

CFD-Post – Creating a plane at x = 0 First, hide the previously created contour plot, by un-checking the associated box in the tree view

CFD-Post – Creating a plane at x = 0 (contd.)

CFD-Post – Creating a velocity vector plot While planes can be coloured by variables, in this case the plane will be used only as a locator for a vector plot. Hide the plane by un-checking the associated box in the tree view

CFD-Post – Velocity vector plot (continued)

CFD-Post – Aligning the view Given that the vector plot is on a 2-D Y-Z plane, you might want to view the plot normal to that axis (i.e. aligned with the X axis). Click on the red x-axis in the bottom right corner of the Viewer to orientate the view

CFD-Post – Creating velocity streamlines Hide the previously created vector plot, by un-checking the associated box in the tree view

CFD-Post – Velocity streamlines (continued)

CFD-Post – Velocity streamlines (continued) Click the Symbol tab Change the Stream Type to Ribbon Click Apply Examine the streamlines from different views using rotate, zoom and pan The ribbons give a 3-D representation of the flow direction Their colour indicates the velocity magnitude Velocity streamlines may be coloured using other variables e.g. temperature

CFD-Post – Creating a velocity isosurface Hide the previously created streamlines, by un-checking the associated box in the tree view

CFD-Post – Velocity isosurface (continued) Set the Variable to Velocity (magnitude used in this context) Enter a value of 7.7 [m s^-1] in the Value field (note: there is nothing special about this value – other values can be tried) Click Apply The speed is > 7.7 m/s inside the isosurface and < 7.7 m/s outside. Isosurfaces in general are useful for showing pockets of highest velocity, temperature, turbulence, etc.

CFD-Post – Velocity isosurface (continued) By default, an isosurface is coloured by the variable used to create it (speed in this case), but a different variable can be used. Click the Colour tab Set the Mode to Temperature Set the Range to Local Click Apply