5 STUDENT USER MANUAL - Mechanical and Mechatronics
Contents
1. In the help page search for keywords rotation modes and select CF X Mesh Help to find more information on changing the view Click the X button on the PipeBend DesignModeler tab to close the DesignModeler page You can click No to quit without saving changes Introduction to the CF X Post GUI The tasks associated with CFD simulation in Workbench are referred to as Ad vanced CFD Tasks For historical reasons there are differences in the GUI and Help files for the three CFX 5 components We will use CFX Post to look at the completed simulation of flow through a pipe bend to get a feel for these interfaces In the Workbench file area click on the filename PipeBend_001 Under Advanced CFD Tasks choose Open in CFX Post to open the results file PipeBend_001 res All of the pertinent CFD model data mesh flow at tributes and boundary condition information for this problem is stored in this file A new page for CFX Post will open There are three major areas on the screen Command menus and buttons at the top selector and edit panels on the left and Viewer window Wireframe models of the pipe inlet and outlet should be in the Viewer To see the pipe bend click the O Domain 1 Default object on in the Objects panel The mouse button action for controlling the view is similar to that in De signModeler There is a significant difference in that the rotat2. edit panel set e Locations Y Plane 1 e Variable Y Velocity e Hybrid on e Projection V None e Reduction 10 e O Visibility on and click Apply The vector plot should appear in the Viewer window and the vector object should be listed in the Object database panel Under the View Control branch in the Object tree turn DEFAULT LEGEND off and back on to remove and then replace the scale legend 7 To visualize the pressure field create a contour plot Remove the vector plot click O Vector 1 and O Plane 1 off in the Object tree Choose Cre ate Object Contour from the top menu row In the New Contour panel accept Name Contour 1 and click OK In the Contour Contour 1 edit panel set e Locations V Plane 1 e Variable Y Pressure e Hybrid on e Colour Scale Y Linear e Colour Map Y Rainbow e of Contours 10 e O Visibility on and click Apply The fringe plot should appear in the Viewer window Go to the Render tab in the Contour edit panel turn O Draw Faces off and click Apply to see a line contour plot of the pressure field Does this pressure field make sense to you 8 On line help is av
3. the fluid library which has many common fluids The Materials panel manages the fluid library There are provisions for selecting pre defined fluids defining new fluids and creating duplicates or copies of existing fluids The properties of fluids can be general functions of temperature and pressure for liquids or gases The CFX Expression Language CEL is used to input for mulae for specifying equations of state and other applications such as boundary variable profiles initialization and post processing CEL allows expressions with standard arithmetic operators mathematical functions standard CFX variables and user defined variables All values must have consistent units and variables in CEL expressions must result in consistent units Full details of CEL including the names of the standard CFX variables are included in the CFX 5 Reference Material Guide For low speed flows of gases and liquids it is adequate to use constant property fluids It is easiest to build up a new constant property fluid from a comparable fluid from the existing CFX fluid library as a template For example to define constant property air at 20 C make a duplicate copy of air at 25 C and then edit this copy Boundary Throughout each domain mass and momentum conservation balances are ap plied over each element These are universal relationships which will not distin guish one flow field from another To a large extent a particular f
4. 1 7 1 Objects Three types of objects can be created geometrical flow visualization and viewer augmentations Geometrical objects include Point a point in the domain Often used to probe flow properties within the domain Line a straight line between two points on the line Intermediate points on the line can be set at intesections with mesh faces referred to as a cut line or uniformly spread along the line referred to as a sample line Plane a flat plane in the domain Like a line object a plane object can be either a cut plane or a sample plane 22 STUDENT USER MANUAL Isosurface the surface along which some scalar field property has a constant value Polyline a piecewise continuous straight line between a series of points The line can be derived from the intersection of a boundary and another geo metrical object or as a contour line and User Surface a surface derived in a manner similar to a polyline object The definition of each of these objects involves choosing from a range of options for each atttribute including location line colour etc The object edit panels outline the possible options for each attribute of the object See the on line help for further information on each of these objects and their generation Flow visualization objects allows exploration of the velocity pressure tem perature fields For each flow property calculated at a node there are two fields hybrid and conservative At interior n
5. In the CFX 5 Solver Finished 1 8 COMMANDS FOR DUCT BEND EXAMPLE 35 5 Post processing The most interesting step is the analysis of the results To illustrate this step the commands listed in the next paragraph step through the following tasks load the results from the res file for post processing create a vector plot on one of the symmetry boundary planes save an image of the plot create a vorticity variable create a fringe plot of the vorticity field create a line and export the velocity data along the line export the inner wall pressure and wall shear stress distribution probe the velocity field and save the visualization state To accomplish these tasks click the CFX Post tab in bottom left corner and then Choose File Load Results and select the Ductbend_001 res results file Choose Create Object Vector accept Name Vector 1 and click OK to define a vector object and open an edit panel In the panel set x Locations FRONT SURFACE x Variable V Velocity Hybrid on Projection V None Reduction 1 plots vector at every mesh point Visibility on and click Apply The vector plot should appear in the Viewer window and the vector object is listed in the Object database panel Under the View Control branch in the Object tree turn O DEFAULT LEGEND off and back on to remove and then
6. Move the mouse cursor down to create a vertical line Look for the V constraint symbol and click the left mouse button b Switch to the Dimensions toolbox to size the inner entrance wall length i Select the General tool ii Select a point near the centre of the line Then move the cursor to the right Click to complete a dimension which is labelled V2 iii In the Details View change the value of V2 to 0 10 m c To join the inner entrance wall and the inner wall bend switch to the Constraints toolbox i Select the Coincident tool ii Select the upper end of the entrance inner wall with a left mouse button click The square end marker should be yellow iii Select the square end marker of the arc that lies on the X axis with a left mouse button click The inner entrance wall should join the inner wall bend 4 To draw a line across the inflow entrance a Use the Line tool in the Draw toolbox b Place the cursor over the bottom end point of the entrance inner wall and notice that a P constraint symbol appears Left mouse 2Notice that the drawing instruction steps are provided in the lower left corner COMMANDS FOR DUCT BEND EXAMPLE 27 button click to select this point and then move the cursor to the left and click while the H constraint symbol is visible c Use the General tool in the Dimensions toolbox
7. atm ti Buoyancy Option Non Buoyant and Domain Motion Option Y Fluid Models Stationary sub panel set o Heat Transfer Model Option Y o Turbulence Model Option v None 9 k Epsilon Scalable 9 None None 9 and 32 STUDENT USER MANUAL x on the Initialization sub panel ensure that O Domain Initialization is off and then click Ok to close the panel Notice that the Domain Ductbend is now listed in the Physics database tree If you double click on this object in the list then the Edit panel will reappear e Click the Create a Boundary Condition button to open a definition panel Fill in Name INFLOW SURFACE and click OK In the Edit Boundary Inflow surface in Domain Ductbend panel x under the Basic Settings tab set o Boundary Type Y Inlet and o Location Y inflow surface x and under the Boundary Details tab set o Flow Regime Option VY Subsonic o Mass and Momentum Option Y Normal Speed o Normal Speed Y 3 WV ms 1 o Turbulence Option Y Intensity and Length Scale o Fractional Intensity 0 05 o Eddy Length Scale 0 00
8. tetrahedral prismatic and hexahedral These notes present a basic methodology for devel oping simple geometries for tetrahedral meshes To develop expertise for more complex geometries work through the sequence of tutorials in given in CFX Mesh 2 1 Help 1 4 1 Basic Concepts and Definitions Vertex Occupies a point in space Often other geometric entities like edges connect at vertices Edge A curve in space An open edge has beginning and end vertices at distinct points in space A straight line segment is an open edge A closed edge has beginning and end vertices at the same point is space A circle is a closed edge Face An enclosed surface The surface area inside a circle is a planar face and the outer shell of a sphere is a non planar face An open face has all of its edges at different locations in space A rectangle makes an open face A closed face has two edges at the same location in space The cylindrical surface of a pipe is a closed face Solid The basic unit of three dimensional geometry modelling e is a space completely enclosed in three dimensions by a set of faces volume e the surface faces of the solid are the the external surface of the flow domain and e holes in the solid represent physical solid bodies in the flow domain such as airfoils etc Part One or more solids that form a flow domain Multiple Solids May be used in each part e the solid volumes cannot overlap e the solids must join at common
9. a line object and open an edit panel Use Method Two Points set Point 1 to 0 0 0 1 0 01 set Point 2 to 0 0 0 025 0 01 notice that we put the line in the middle of the domain to avoid boundary effects set the number of samples to 25 and click Apply to see the line make sure that the visibility of the contour plot etc is turned off Choose File Export to open the Export panel where you can set File uvelocity dat select Line 1 from the Locator list set O Export Geometry Information on select Ctrl key plus click Velocity u and Velocity v from the Select Variable s list and click Save to write the data to a file in a space separated format that can be imported into a conventional spreadsheet program for plotting or further analysis Notice that this file includes x y and z values Choose Create Object Plane accept Name Plane 1 and click OK to define a plane object and open an edit panel Use Method Y XY Plane with Z 0 m and click Apply set O Visibility off to avoid clutter in the view Choose Create Object Polyline accept Name Polyline 1 and click OK to define a polyline object In the edit panel use Method V Boundary Intersection with Boundary List V INNER WALL and Intersects With W P
10. d Select a point near the centre of the line Then move the cursor down Click to complete a dimension which is labelled H3 e In the Details View change the value of H3 to 0 075 m Repeat the procedure used for the entrance inner wall to draw the exit inner wall a Draw a horizontal line in the upper right XY quadrant near the end point of the inner wall bend b Set the length of the line to 0 20 m with the General tool from the Dimensions toolbox c Join the exit inner wall to the inner wall bend with the Coincident tool from the Constraints toolbox Draw the outer entrance wall with the Line tool Start at the outer left end point of the inflow edge look for the P constraint symbol and draw a vertical line that is coincident C with the X axis Draw the outer bend wall with the Arc by Center at the origin make the start point at approximately 20 above the X axis in the upper left quadrant and make the end point coincident C with the Y axis Use the Coincident constraint tool to join the start point of the arc to the end point of the outer entrance wall Draw the outer exit wall with the Line tool Draw a horizontal H line coincident C with the Y axis above its final desired location Use the Coincident constraint tool to join this line to the end of the outer bend wall Use the Equal Length
11. get a list of possible variables expressions locators functions and constants that can be input into a new expression There are two type of functions Functions CFX Post functions for performing operations on scalar fields and Functions CEL functions for conventional mathematical operations and Create Variable allows the calculation of new field variables New variables can be defined in terms of defined expressions or by entering new expressions directly into the variable definition For example calculating local pressure coefficients based on the maximum speed in the domain backstep i e Cp p Pref ZPV max can be done with the expression Pressure 0 Pa 0 5 Density maxVal sqrt Velocity u 2 Velocity v 2 backstep 2 for a variable called Cp 1 7 3 Controls A set of controls can be used to save a particular post processing setup or state so that it can be repeated This is useful when comparing different simulations to see the impact of a design change on flow properties Common controls include Camera The image size orientation perspective etc in the Viewer window is associated with a Camera viewer imagine that the user moves a camera around in space to create a two dimensional image of a three dimensional object in the camera s viewer Camera views can be saved deleted and refreshed with the buttons on the right top of the Viewer window Note that the camera does not determine which graphics
12. last step is to remove unnecessary files created by CFX 5 This step is necessary to ensure that you do not exceed your disk quota At the end of each session delete all files except e agdb cmdat cmdb wbdb def and _ res files If you no longer need your results but would like to be able to replicate them then you should delete all files except e def files After removing all unnecessary files use the WinZip utility to compress the contents of your directory
13. point of rotation can be changed by clicking the left button while the cursor is on the pipe bend surface this may take some experimentation A small red sphere indicates the centre of rotation With the mouse cursor in a corner of the Model View press and hold the left mouse button get a roll action in which there is 2D rotation about an axis perpendicular to the Model View window Move the cursor to either the left or right of the Model View and hold the left button to get a yaw action in which there is 2D rotation about the horizontal axis Move the cursor to either the top or bottom of the Model View and hold the left button to get a pitch action in which there is 2D rotation about the vertical axis Rotate zoom and pan actions can be achieved directly by pressing the middle mouse key alone with the Shift key and with the Ctrl key respec tively 4 STUDENT USER MANUAL 8 10 The Tree View on the left shows the geometric entities that were used to generate the cylinder Expand the 1 Part 1 Body entity and click on Solid to see some properties of the cylinder in the Details View The pipe bend was generated from two entities a Sketch1 which can be found in the Plane4 entity Click on Sketch1 to highlight the circle that the pipe bend is based upon with yellow b Sketch2 which can be found in the YZPlane entity Click on the Sketch2 to highlight the path that is swept out by Sketch1 to gener ate the pipe bend
14. region with no mass flow through the faces and with negligible shear stresses and negligible heat fluxes This condition is often used to simulate a two dimensional flow field with a three dimensional flow solver and to minimize mesh size requirements by taking advantage of natural symmetry planes in the flow domain Since it is crucial that each surface element face have a boundary condition attached to it CFX Pre automatically provides a default boundary condition for each domain Once all boundary surfaces have been attached to explicit boundary conditions the default boundary condition object is deleted This allows the user to identify surfaces which still require explict boundary conditions For the flow solver to successfully provide a simulated flow field the spec ified boundary conditions should be realizable i e they should correspond to conditions in a laboratory setup In particular ensure that the inlet and outlet boundary conditions are consistent and that they take advantage of the known information Table 1 1 lists several common inlet outlet condition combinations CFX PRE PHYSICAL MODELLING 17 Inlet Sets Outlet Sets Solution Predicts velocity static pressure inflow static pressure total pressure velocity outflow pressure inflow velocity total pressure static pressure system mass flow Table 1 1 Common boundary condition combinations along with the global flow quantity which
15. surfaces or faces and GEOMETRY AND MESH SPECIFICATION 9 e the faces where two solids join can be thin surfaces Thin Surface A thin solid body in a flow like a guide vane or baffle can be modelled as an infinitely thin surface with no slip walls on both sides Units To keep things simple and to minimize errors use metric units through out Advanced Concepts See the Geometry section of the CFX Mesh Help for fur ther information on geometry modelling requirements To develop improved skill follow the tutorials given in CFX Mesh Help Tutorials 1 4 2 Geometry Creation The basic procedure for creating a three dimensional solid geometry is to make a 2D sketch of an enclosed area possibly with holes on a flat plane The resulting 2D sketch is a profile which is swept through space to create a 3D solid feature This process can be repeated to either remove portions of the 3D solid or to add portions to the solid Each sketch is made on a Plane e There are three default planes XYPlane XZPlane and YZPlane which coincide with the three planes of the Cartesian coordinate system e Each plane has a local X Y coordinate system and normal vector the plane s local Z axis e New planes can be defined based on existing planes faces point and edge point and normal direction three points origin local X axis and another point in plane and coordinates of the origin and normal and e Plane transforms such as translations and rotat
16. two purposes 1 2 to ensure that your Windows XP NEXUS operating system is operational and to introduce the look and feel of the software 1 1 1 Windows XP NEXUS The CFD software is available on the workstations in the all Engineering Com puting labs Fulcrum E2 1313 Wheel E2 1308 Lever E2 1302 Wedge E2 1302B Helix RCH 108 and GAFF CPH 2367 and the Mechanical Engi neering 4th year computing room E2 2354 The workstations use the Windows XP operating system on Waterloo NEXUS You should be familiar with tech niques to create new folders or directories to delete files to move through the folder directory system with Windows Explorer to open programs through the Start menu on the Desktop toolbar to move resize and close windows and to manage disk space usage with tools like WinZip 1 1 2 Introduction to Workbench The ANSYS Workbench environment provides an interface to manage the files and databases associated with the individual software components These files and databases are organized into a particular project To get a feel for this environment and the GUIs associated with the software components we will look at a pre prepared project on flow through a pipe bend l 2 Create a working directory called CFDTest on your N drive Use a web browser to visit the UW ACE ME 566 course page uwace uwaterloo ca Under the Lessons tab and open the Student User Manual folder Click on the link to P
17. 50 9 Ok pi Create Output Files and Monitor Points Results Full Ok Output Boundary Flows on and choose tab panel set to close the panel and create the new boundary object button to open the ini Turbulence Eddy Dissipation is on You Ok button to open the panel 30 of the average residence time of button to open the All All 2 Click the Write a Solver File name Ductbend def and Operation Y 1 8 4 Solver Manager The CFX Solver window will open after CFX Pre closes In the Define Run panel set e Definition File and vi to open the panel Accept the defau Start Solver Manager Click ductbend def run you would enter the name of the most current results file e Type of Run Y e Run Mode and then click and Full Serial Start Run lt file OK NOTE If restarting a partially converged After a few minutes execution should begin Diagnostics will scroll on the ter minal output panel and the equation RMS residuals will be plotted as a function of time step After the first cally Execution should stop Normally window click OK few time steps the residuals should fall monotoni after 29 time steps
18. 75 w m and then click Ok to close the panel and create the new boundary ob ject Notice that incoming arrows appear on the inlet surface in the Viewer window and the boundary object is listed in the Physics database tree Clicking on Boundary INFLOW SURFACE object in the Physics database causes the inflow surface mesh to be outlined with green in the Viewer window e Click the Create a Boundary Condition button to open the definition panel Fill in Name OUTFLOW SURFACE and click OK In the Edit Boundary Outflow surface in Domain Ductbend panel x under the Basic Settings tab set o Boundary Type Y Outlet and o Location Y outflow surface x and under the Boundary Details tab set o Flow Regime Option VY Subsonic o Mass and Momentum Option Y Average Static Pressure o Relative Pressure 0 V Pa and then click Ok to close the panel and create the new boundary object e Click the Create a Boundary Condition button to open the definition COMMANDS FOR DUCT BEND EXAMPLE 33 FRONT SURFACE panel Fill in Name and click OK In the Edit Bound ary Front Surface in Domain Ductbend panel x under the tab set B
19. Basic Settings Pure Substance Steady State click the the Create Material panel fill in Name is set and then click button to open the Simulation Ok tab in the database panel to open up a list of available Create New Object icon In Water nominal tab and set Constant Property Liquids Thermodynamic State on and Thermodynamic State Material Properties General Material u Value 1000 M kgm 3 gt Ok Domains tab and set Dynamic Viscosity on and Dynamic Viscosity and click and click OK to Liquid 0 001 M kgm 1s71 OK button A small Create Domain definition panel will Ductbend to define the domain object An Edit Domain Ductbend panel will open with several tabbed sub panels On the on the O O o Turbulent Wall Functions Option V o Reaction or Combustion Model Option o Thermal Radiation Model Option Y General Options Location V Assembly Es sub panel set Domain Type V Fluid Domain pi Fluids List Y Water nominal Particle Tracking off Reference Pressure 1 M
20. Geometry Specification To ensure that reasonable flow patterns are simulated in the bend it is necessary to add short entrance and exit lengths of duct to simulate the actual flow through the bend when it is situated in a duct The domain geometry is shown in Figure 1 2 The CFD simulation code is fully three dimensional so even though we are primarily interested in flow in the plane shown in Figure 1 2 the geometry THE CFD MODEL SPECIFICATION T Fig 1 2 Geometry of the duct bend model model must have a width into the page A thin slice is used The width of the slice is set to 0 02 m Specification of Simulation Type For this application a steady flow is ap propriate Specification of Fluid Properties For this application the fluid is water which can be treated as a simple liquid with nominal constant properties p 1000 kgm 3 u 0 001 Pa Specification of Flow Models For this analysis it is reasonable to assume the following flow features e incompressible flow e fully turbulent flow the Reynolds number is approximately 225 000 e the turbulent momentum stresses can be modelled with the standard k model OU OU A C k a Z where the turbulent viscosity 4 is proportional to the fluid density the velocity scale of the turbulent eddies and the length scale of the eddies The scales of the turbulent eddying motion are estimated from two field variables which are calculated as part
21. ME 566 Computational Fluid Dynamics for Fluids Engineering Design CFX 5 STUDENT USER MANUAL Gordon D Stubley Department of Mechanical Engineering University of Waterloo G D Stubley 2004 2005 2005 Contents 1 Student User Manual 1 1 Getting Started 1 1 1 Windows XP NEXUS 1 1 2 Introduction to Workbench 1 2 The Problem 1 3 The CFD Model Specification 1 4 Geometry and Mesh Specification 1 4 1 Basic Concepts and Definitions 1 4 2 Geometry Creation 1 4 3 CFX Mesh Mesh Generation 1 5 CFX Pre Physical Modelling 1 5 1 Domain 1 5 2 Initialization 1 5 3 Output Control 1 5 4 Simulation Type 1 5 5 Solver Control 1 6 CFX Solver Manager Solver Operation 1 6 1 Monitoring the Solver Run 1 7 CFX Post Visualization and Analysis of Results 1 7 1 Objects 1 7 2 Tools 1 7 3 Controls 1 8 Commands for Duct Bend Example 1 8 1 Geometry Model 1 8 2 Mesh Generation 1 8 3 Pre processing 1 8 4 Solver Manager 1 8 5 Post processing 1 8 6 Clean Up DHAWAN NNF 1 Student User Manual In these notes the basic steps in a CFD solution will be illustrated using the professional software ANSYS Workbench Version 9 0 Service Pack 1 which includes the components DesignModeler CF X Mesh and CFX 5 Version 5 7 1 Service Pack 1 all trademarks of ANSYS These notes include an introduc tory tutorial and a mini user s guide They are not meant to replace a detailed user s guide For full information on these components refer to the on line he
22. ailable in pdf file format Help Context sensitive help is also available Position the mouse pointer in the Object Selector panel and 6 STUDENT USER MANUAL 10m 0 07m E m 22kgs Fig 1 1 Geometry of short radius duct bend press lt F1 gt to bring up the help page for that panel 9 This should give a sense of the operation of the CFX GUI Feel free to experiment with other object types and scalar fields When you have fin ished return to the Workbench Project page Exit by File Close Project and choose No do not save any items 10 Clean up by deleting the CFXTest directory 1 2 The Problem Consider the analysis problem of estimating the pressure drop of flow through the short radius duct bend shown in Figure 1 1 The duct bend has a width of 1 m and is made of galvanized steel with an average surface roughness height of 0 10 mm Water flows through the bend with a mass flow rate of m 225 kgs7 1 1 3 The CFD Model Specification The first phase in the CFD solution is a planning stage in which the complete CFD model of the duct bend is specified This specification includes Physical Model Specification The steel walls of the bend and other duct pieces are assumed to be rigid and joints in the duct work are assumed to be smooth The galvanized steel is assumed to have a uniform surface roughness height The width of the bend is sufficient that the flow can be considered to be two dimensional Domain
23. asic Settings o Boundary Type Y Symmetry o Location and then click Ok Click the Create a Boundary Condition panel Fill in Name BACK SURFACE front surface and and click to close the panel and create the new boundary object button to open the definition OK In the Edit Bound ary Back surface in Domain Ductbend panel x under the Basic Settings tab set o Boundary Type Y Symmetry back surface o Location V and then click Ok and Click the Create a Boundary Condition to close the panel and create the new boundary object button to open the definition panel Fill in Name INNER WALL and click OK In the Edit Bound ary Inner wall in Domain Ductbend panel x under the Basic Settings tab set Wall inner wall and o Boundary Type V 9 o Location V pi x and under the Boundary Details o Wall Influence on Flow Option Y o O Wall Velocity off tab set No Slip b o Wall Roughness Option Rough Wall 0 0001 o Roughness Height vim gt and then click Ok Click the Create a Boundary Condition panel Fill in Name OUTER WALL and c Outer wall
24. ccurs Outlet an outlet region is a surface over which mass leaves the flow domain For each element face on an outlet region one of the following must be specified e fluid velocity speed and direction e mass flow rate or e static pressure A specified static pressure value can be set to a specific face applied as a constant over the outflow region or treated as the average over the outflow region No information is required to model the turbulence in the fluid flow at an outflow Opening a region where fluid can enter or leave the flow domain Pressure and flow direction must be specified for an opening region If the opening region will have fluid entering leaving close to normal to the faces i e a window opening then the specified pressure value is the total pressure on inflow faces and the static pressure on outflow faces a mixed type of pressure If the opening region will have fluid flow nearly tangent to the faces i e the far field flow over an airfoil surface then the specified pressure is a constant static pressure over the faces For turbulent flows the turbulence intensity must also be set Wall a solid wall through which no mass can flow The wall can be stationary translating sliding or rotating If the flow field is turbulent then the wall can be either smooth or rough Depending upon which of these options are chosen suitable values must be input i e the size of the roughness elements etc Symmetry a
25. cility for creating and naming composite 2D surface regions When the mesher is initialized all of the primitive 2D surfaces are assigned to the Default 2D Region As surfaces are assigned to new user defined regions they are removed from the Default 2D Region However the Default 2D Region must contain at least one surface These region names and the their corresponding surface meshes are passed on to CFX Pre Mesh Features The mesh is composed of two dimensional triangular elements on the surfaces and tetrahedral and prism elements in the body of the solid Figure 1 3 shows the element shapes The properties of the mesh are controlled by the settings of the following features Default Body Spacing Set the maximum length scale of the tetrahedral ele ments throughout the volume of the body Some of the actual tetrahedral elements may be smaller due to the action of other mesh features or in order to fit the tetrahedral elements into the body shape Default Face Spacing Set the length scale of the triangular elements on the surfaces e For simple meshes it is sufficient to set Face Spacing Type Y Volume Spacing 12 STUDENT USER MANUAL e For surfaces such as an airfoil in a large flow domain it might be desir able to set the triangular mesh length scale smaller than the default body spacing In this case a new Face Spacing can be defined and assigned to the airfoil surface Besides setting the triangular element l
26. ct the Sketching tab and 2 Click on the Z coordinate of the triad in the lower right corner of the Model View Select the Draw toolbox and 26 STUDENT USER MANUAL 1 With the Arc by Center tool sketch the inner wall bend shape a Place the cursor over the origin watch for the P constraint symbol and left mouse button click b Move the cursor to the left along the X axis With the C constraint visible click the left mouse button to put the start point of the arc on the X axis c Sweep the cursor clockwise until the C constraint appears at the Y axis Click the left mouse button 2 Switch to the Dimensions toolbox to size the inner wall bend radius a Select the Radius tool b Select a point on the arc Then move the cursor to the inside of the arc near the origin Click to complete a dimension which is labelled R1 c In the Details View notice that R1 is shown under the Dimensions title d Change the value of R1 to 0 025 m Notice the arc radius changes automatically If the dimension is poorly placed on your sketch you can use the Move tool to correct the placement 3 Switch back to the Draw toolbox to sketch the inner entrance wall a With the Line tool selected place the cursor in the lower left quadrant of the XY plane near the arc Click the left mouse button
27. emove operations Tools Freeze This will form a new solid body as a component of a new part and 3 Select all solids and choose Tools Form New Part When the solid model is completed an agdb file is created and saved in order to store the geometry database 1 4 3 CFX Mesh Mesh Generation The mesh generation phase can be broken down into the following steps 1 Read in or update the agdb file with the solid body geometry database 2 Set the properties of the mesh 3 Cover the surfaces of the solid body with a surface mesh of triangular or quadrilateral elements and 4 Fill the interior of the solid body with a volume mesh of tetrahedral hex ahedral or prism elements that are based on the surface meshes and that GEOMETRY AND MESH SPECIFICATION 11 Anisotropic Triangular Element Isotropic Triangular Element Tetrahedral Element Triangular Prism Element Fig 1 3 Shape of common two and three dimensional elements grow inwards from each surface mesh A gtm file containing all of the mesh information and region information is written at the end of this step The following comments and guidelines are for generating meshes for two dimensional flow simulation in relatively simple rectangular geometries Regions The geometry database contains a list of primitive faces and edges that are formed in the generation processes It is often cumbersome to work directly with these primitive entities Therefore there is a fa
28. ength scale the following properties must be set for the new face spac ing Radius of Influence The distance from the region that has a tetra hedral mesh length scale equal to that of the surface triangular elements Expansion Factor The rate at which the tetrahedral mesh length scale increases outside the radius of influence This value controls how smoothly the mesh length scale increases from the face region to the default body spacing far from from the face e For complex surfaces the face spacing type should set so that the ge ometry of the surface is well represented by the mesh relative error or angular resolution Controls are used to locally decrease the mesh length scale in the region around a point line or triangular plane surface The spacing in the vicinity of a control is set by three factors Length Scale fixes the size of the tetrahedral mesh elements Radius of Influence sets the distance from the control that has a mesh of the specified length scale and Expansion Factor controls how smoothly the mesh length scale increases to the default body spacing far from the control For line and triangle controls the spacing can be varied over the control i e from one end point of the line to the other end point Extruded Periodic Pair In cases where the flow is two dimensional it is desir able to have a single mesh element in the cross stream direction In these cases the surface meshes on two surfaces will need
29. es of the local tur bulent boundary layer Other properties include Number of Inflated Layers specifies the number of prism elements across the thickness of the inflated layer and Expansion Factor specifies how the prism height increases with each in flated layer above the wall surface This factor must be between 1 05 and 1 35 Stretch The default body mesh length scale is isotropic The vertex angles in the isotropic tetrahedral elements are close to 60 In geometries that are not roughly square in extent it may be desirable make the mesh length scale longer or shorter in one particular direction This is achieved by stretching the geometry in a given direction meshing the modified geometry with an isotropic mesh and then returning the geometry along with the mesh to its original size This means that if the y direction is stretched by a factor of 0 25 without stretching in the other two directions then the mesh size in the y direction will be roughly 4 times that of the other directions Take care to ensure that the resulting tetrahedral elements do not get too squashed For this reason the stretch factors should be between 0 2 and 5 at the very most more moderate stretch factors are desirable Note stretch parameters are ignored in extruded meshes Proximity flags set the behaviour of the mesh spacing when edges and sur faces become close together For simple rectangular geometries set Edge Proximity V No and Surface Proximit
30. esh The commands listed below will generate a discrete mesh in the flow domain name the surfaces faces of the solid geometry to ease boundary condition specification specify the properties of the mesh in the interior of the flow domain and close to solid walls preview the surface mesh to check for anomalies and create the geometry file with volume mesh information Choose the Generate CFX Mesh DesignModeler Task Notice the three pri mary areas Model View Tree View and Details View The surfaces faces of the solid are labeled as regions for ease of attach ing the boundary conditions To attach a region entity at the inflow see Figure 1 4 1 Right mouse click over Regions in the Tree View and select Insert Y Composite 2D Region to create a new region entity 2 Left click over the new entity s name Composite 2D Region 1 and edit the region name to inflow surface 3 In the Model View put the mouse cursor over the inlet surface area and left mouse click The inlet surface area should turn green and 4 In the Details View click on Location Y Apply Repeat to create a region entity called outflow surface Notice that if you left mouse button click on inflow surface or the outflow surface in the Tree View that the resulting region in the Model View turns green Create a region entity called inner wall This region is composed of three primitive surfaces To select a set of surfaces
31. esh on the duct wireframe model x To see the mesh on an individual region click the named regions in the Composite Regions tree Click through each region in the tree x Expand the inner wall region to see the three primitive faces that make up the region Each primitive face has a name of the form Fz By face x of body y where only the leading letter F or B is shown x The back surface was imported into CFX Pre attached to the De fault 2D Region If you would like to correct this naming anomaly click Create New Object icon on the right of the Region panel A small Create Object panel will open Fill in Name back surface assuming that this is the missing surface and click OK to open the Region Editor panel will open up where you set o Combination Alias o Dimension Y All Select Default 2D Region to put into the Region List panel list and o Click Ok to close panel 2 e Click the Type panel Check that Option V e Click materials To define a new material COMMANDS FOR DUCT BEND EXAMPLE 31 Define the Simulation Type Materials open a panel with two tabs Click the x Option V Material Group Y and then click Click the open Fill in Name Click the Option Y expand Equation of State Option Y Density expand Transport Properties
32. etween the mesh points element nodes has to be approximated to form the discrete equations These approxi mations are classified as the discretization scheme The discretization scheme for approximating advective transport flows listed in order of increasing accuracy options are e Upwind a constant profile between nodes e Specified Blend Factor a blend of upwind and high resolution and e High Resolution a linear profile between nodes In choosing a discretization scheme accuracy is obviously an important consid eration Increasing the accuracy of the discretization often slows convergence sometimes to the extent that the solution algorithm does not converge The choice of time step size for the flow evolution plays a big role in establish ing the rate of convergence Good results are usually obtained when the physical time step size is set to approximately 30 of the average residence time or cycle time of a fluid parcel in the flow domain This residence time is referred to as the global time scale The initial guesses for the velocity pressure turbulent kinetic energy and dissipation rate nodal values will not necessarily satisfy the discrete algebraic equations for each node If the initial nodal values are substituted into the dis crete equations there will be an imbalance in each equation which is known as the equation residual As the nodal values change to approach the final solution the residuals for each nodal equati
33. exit wall the same length as the inner exit wall and Draw a line from the end of the outer exit wall to the end of the inner exit wall to form the outflow edge Make sure that the end points are coincident P tool Put the center constraint tool to make the outer The sketch should now be an enclosed contour on the XYPlane e To create the three dimensional solid body 1 Switch to the Tree View by selecting the Modeling tab bi 2 Click on the In the Extrude button to create the Extrudel feature Details View Check Base Object Select Operation v Add Material Select Direction v NONE Normal Set FD1 Depth gt 0 0 02 Select As Thin Surface Y No Sketch and 28 STUDENT USER MANUAL Select Merge Topology Y Yes 3 Click on the Generate button to create a Solid Use the isometric view in the Model View to check that you have a three dimensional solid grey body Choose File Save As and set File name Ductbend agdb in the Save As window Click Save to close window Return to the Project page by clicking on the Ductbend Project tab at the top left corner of the window 1 8 2 Mesh Generation The second phase uses CFX M
34. ie He ee U Mom 0 00 2 2E 02 V Mom 0 00 3 6E 08 W Mom 0 00 9 5E 20 P Mass 0 00 2 8E 03 A a i i i K TurbKE 0 00 1 8E 01 Se eee See a a EES E Diss K 0 00 1 6E 01 patahan OUTER LOOP ITERATION 2 Equation Rate RMS Res Sam as a a oat a p U Mom 6 37 1 4E 01 V Mom 199 99 9 1E 03 W Mom 199 99 2 8E 11 P Mass 0 82 2 3E 03 has RS ea prs K TurbKE 0 21 3 7E 02 a pone acess sas s E Diss K 0 24 3 8E 02 D a a ta Table 1 3 Typical convergence diagnostics For each field variable equation set the following information time step Rate the convergence rate Rate RMS res current time step RMS res previous time step which should typically be 0 95 or less is output each RMS Res the root mean square of the nodal normalized residuals Max Res the maximum nodal normalized residual in the flow domain and Linear Solution after each equation set is linearized an estimate of the solu tion of the resulting linear equation set is obtained and statistics on this solution are reported CFX POST VISUALIZATION AND ANALYSIS OF RESULTS 21 Work Units a measure of the effort required to obtain the solution esti mate Residual Reduction the amount that the linear solver has reduced the RMS residual of the li
35. in Domain Ductbend panel Basic Settings tab set Wall outer wall x under the and o Boundary Type Y p o Location V gt x and under the Boundary Details o Wall Influence on Flow Option Y o O Wall Velocity off lick to close the panel and create the new boundary object button to open the definition OK In the Edit Boundary tab set No Slip b o Wall Roughness Option Rough Wall 0 0001 o Roughness Height Yim pj 34 STUDENT USER MANUAL and then click Click on the tialization panel Make sure that can accept V Click on the Under the x Advection Scheme Option V Physical Timescale Ok Define the Global Initial Conditions Automatic initialization for all properties and click Define the Solver Control Criteria Basic Settings tab set Upwind Timescale Control Vv Physical Timescale 0 04 M vA a fluid parcel inside the flow domain and then click Click the panel In the x Option V Output Variable Operators on and choose and then click Max No Iterations MAX 1 0e 3 Residual Type V Residual Target
36. ion action is not context sensitive 2D rotation about an axis perpindicular to the screen is achieved by pressing the Ctrl key with the left button while in rotation mode The coordinate system triad is shown in the lower right corner Unlike in DesignModeler the triad cannot be used to change the view The view can be changed with the view buttons at the top of the Viewer window Use the X to select an orthographic view towards x along the x axis Now look at some results Each visualization is created by defining a new visualization object and then editing the properties of the object To make a vector plot along the centre plane of the pipe bend GETTING STARTED 5 a Choose Create Object Plane from the top menu row or click on the Create Plane button In the New Plane panel accept Name Plane 1 and click Ok to open a Plane edit panel in the lower left In the edit panel set e Domains Y All Domains the default e Method Y YZ Plane X 0 O Visibility on and click Apply To see this plane click the Domain 1 Default object off in the Objects panel Faas Choose Create Object Vector from the top menu row or use the cor responding button on the second row In the New Vector panel accept Name Vector 1 and click OK to open a Vector edit panel In the
37. ions can be used to modify the base definition of the plane The creation of a sketch is similar to the creation of a drawing with modern computer drawing software e A sketch is a set of edges on a plane A plane can contain more than one sketch e The sketching toolbox contains tools for drawing a variety of common two dimensional shapes e Dimensions are used to set the lengths and angles of edges e Constraints are used to control how points and shapes are related in a sketch Common constraints include Coincident C The selected point or end of edge is coincident with another shape For example the end point of a new line segment can be constrained to lie on the line extending from an existing line segment Note that the two line segments need not touch Coincident Point P The selected points are coincident in space Vertical V The line is parallel to the local plane s Y axis Horizontal H The line is parallel to the local plane s X axis Tangent T The line or arc is locally tangent to the existing line or arc Perpendicular L The line is perpendicular to the existing line and 10 STUDENT USER MANUAL Parallel The line is parallel to the existing line As a sketch is drawn the symbols for each relevant constraint will appear If the mouse button is clicked while a constraint symbol is on the sketch then the constraint will be applied Note that near the X and Y axes it is often difficult to distingui
38. ions can significantly impact the efficiency of the iterative solution algorithm If there are condition difficulties then values or expressions with CEL can be used to provide intial conditions that e match the initial conditions to the dominant inlet boundary conditions and e align the flow roughly with the major flow paths from inlet regions to outlet regions 1 5 3 Output Control For many cases especially those with a strong emphasis on fluid mechanics it is necessary to output additional fields to the res output data file For example it is often worthwhile to output the turbulent stress fields throughout the flow do main wall shear stresses on all boundary walls and gradient operations applied to all primary solution variables 1 5 4 Simulation Type The numerical formulations for steady and transient flows differ slightly The focus is on steady flow simulations however transient evolution with no transient accuracy is used in the iterative solution algorithm Each iteration is treated as a step forward in time 1 5 5 Solver Control The numerical methods operation used in the equation set solver are largely fixed however some aspects of the numerical methods must be explicitly set by the user 1 the choice of discretization scheme 2 the time step size for the flow evolution and 3 the criteria for stopping the iterative process CFX SOLVER MANAGER SOLVER OPERATION 19 The variation of velocity pressure etc b
39. ipeBend zip and follow the instructions to download the archive containing the working files Use WinZip to extract the files in the PipeBend archive into your working directory Open ANSYS Workbench from Start Programs Engineering ANSYS 9 0 ANSYS Workbench Open the project file Check that Open Y Workbench Project is selected before using the Browse button below the Open Workbench Projects panel area to find and selecting the file PipeBend wbdb from your working directory There are three main areas on the screen command menus buttons and tabs at the top a list of potential Project Tasks on the left and a list of the files linked to the project On line help for Workbench DesignModeler and CFX Mesh is available in web page format similar to other Windows programs Choose Help ANSYS Workbench Help to open the ANSYS Workbench Documentation Search GETTING STARTED 3 for keyword Tutorials and select CFX Mesh Help Follow the Tutorials link to see the list of available tutorials Introduction to DesignModeler CFX Mesh GUI 1 In the Workbench file area click on the filename PipeBend just to the right of the DesignModeler button DM Notice that the Project Tasks area at the left adjusts to reflect your choice Under DesignModeler Tasks choose Open to open the geometry file A new page for DesignModeler will open Go back to the Projec
40. is estimated as part of the solution for each combination Domain Models In incompressible flow fields the actual pressure level does not play any role in establishing the flow field it is pressure differences which are important The solver calculates these pressure differences with respect to a reference pressure Solution fields are in relative pressure terms but absolute pressure relative pres sure plus reference pressure is used for equation of state calculations In turbomachinery applications it is convenient to analyse the flow in a ro tating reference frame In this case the domain is in a rotating reference frame and its axis of rotation and rotation rate must be specified Fluid Models Heat Transfer Model options include None no temperature field is computed not an applicable option for ideal gases Isothermal a constant temperature field is used Thermal Energy a low speed neglecting kinetic energy effects form of the enthalpy conservation equation is computed to provide a tempera ture field and Total Energy a high speed form for conservation of energy including ki netic energy effects is computed Turbulence Model options include None laminar flow simulation k Epsilon the accepted state of the art turbulence model involves the so lution of two transport equations Shear Stress Transport a variant of the k Epsilon model that provides a higher resolution solution in near wall regions and SSG Re
41. lane 1 and then click Apply This creates a line the follows the inner wall You can follow the steps for export along a line to export the values of the pres sure total pressure and wall shear stress along this line into the data file wall dat Choose Create Object Point accept Name Point 1 and click OK to define a point object Use Method XYZ and initialize the point to 0 10 0 04 0 before clicking Apply Choose Tools Calculator to open the COMMANDS FOR DUCT BEND EXAMPLE 37 Function Calculator panel Use Function Y probe Location Y Point 1 Variable W Velocity u Gradient X Note Use the 7 to get a list of all possible variables before clicking on the Calculate button The result with units appears in the results box Move the point around to probe other regions in the flow e Choose File Save State and enter tutorial1 cst for the file name to save all of the information associated with the visualization and post processing objects you have created in this session You can load this state file File Load State to recreate these objects and images in later sessions This facility allows easy comparison of results between simulations e Return to the Project page and choose File Exit Select Yes to save high lighted files 1 8 6 Clean Up The
42. low field for a particular geometry is established by the boundary conditions on the surfaces of the domain A standard boundary condition object includes a name a type a set of surfaces and a set of parameter values In CFX Post the boundary condition object name is used to refer to the set of surfaces on which the boundary condition is applied For this reason the habit of naming each boundary condition by the name of its surfaces as defined in CFX Mesh is often followed Boundary condition types include Inlet an inlet region is a surface over which mass enters the flow domain For each element face on an inlet region one of the following must be specified e fluid speed and direction either normal to the inflow face or in a par ticular direction in Cartesian coordinates e mass flow rate and flow direction or e the total pressure 1 Pod P PV J Protal spec 2 and flow direction If the flow is turbulent then it is necessary to specify two properties of the turbulence Most commonly the intensity of the turbulence T Average of speed fluctuations 3 Mean speed 16 STUDENT USER MANUAL and one additional property of the turbulence the length scale of the turbu lence a representative average size of the turbulent eddies or eddy viscos ity ratio turbulent to molecular viscosity ratio 4 1 are specified Typical turbulence length scales are 5 to 10 of the width of the domain through which the mass flow o
43. lp documentation provided with the software These notes include sections on Getting Started Instructions for a short computer session in which the soft ware graphical user interfaces GUIs are introduced The Problem A description of the example problem The CFD Specification A complete description of the CFD model imple mented in the software Software Components A description of the concepts and operation involved in the five software components DesignModeler CFX Mesh CF X Pre CFX Solver and CFX Post and Commands for the Example Problem A complete step by step list of in structions for solving the model problem The following font format conventions are used to indicate the various com mands that should be invoked Menu Sub Menu Sub Sub Menu Item chosen from the menu hierarchy at the top of a main panel or window Button Tab Command Option activated by clicking on a button or tab Link description Click on the description to move by a link to the next step page Name value Enter the value in the named box Name Y selection Choose the selection s from the named list Name Panel or window name Name On off switch box and Name On off switch circle radio button Many of the features available in these software components will not be explored in intro ductory CFD courses 2 STUDENT USER MANUAL 1 1 Getting Started This working session has
44. nd Particle Tracks If particle paths an advanced feature were calculated as part of the simulation then these paths can be drawn Again see the on line help for further information on each of these objects and their generation Common Viewer augmentation objects include Legend a scale legend to associate property values with colours Text a piece of text Clip Plane a flat plane that is used to reduce the portion of the domain shown in the viewer and CFX POST VISUALIZATION AND ANALYSIS OF RESULTS 23 Instancing Transformation for repeating views to show full geometries when periodic or symmetry conditions have been used to model a portion of a domain 1 7 2 Tools Common post processing tools include File Export allows the export of portions of the results in a space separated tabular form This is useful for exporting data to programs like Excel for graphing etc File Print allows the export and printing of the graphical image in the viewer window Images saved in encapsulated postscript eps or portable network graphics png formats can be easily inserted into reports and presentations Tools Calculator is a powerful tool for carrying out a wide range of mathemat ical calculations including a range of integration and averaging calculations Create Expression allows the input of CEL expressions To learn the expres sion syntax right mouse click in the Definition box within the Expression Editor panel to
45. near equation set and Status an indicator of the linear solver performance OK residual reduction criteria met ok residual reduction criteria not met but converging F solution diverging residual increased dramatically and solver terminates due to floating point number overflow error Some of the above information is displayed graphically in the monitor window so that the solver execution can be monitored When execution is complete the final results are written to the res file In addition all of the information pertinent to the operation of the solver is output to the out file including the CPU memory or storage requirements the physical flow model grid summary estimate of the global length speed and time scales based on the initial fields the convergence diagnostics e estimate of the global length speed and time scales based on the final fields e the fluxes of all conserved quantities through the boundary surfaces these should balance to 0 01 of the maximum fluxes and e the computational time required to obtain the solution 1 7 CFX Post Visualization and Analysis of Results To the typical user of CFD the generation of the velocity and pressure fields is not the most exciting part It is the ability to view the flow field that makes CFD such a powerful design tool CFX Post has capabilities for visualizing the results in graphics objects for using calculation tools and for controlling the post processing state
46. objects are visible Session Provides a mechanism for recording and saving a series of operations This is useful for users interested in learning power programming of CFX Post see on line help for more information 24 STUDENT USER MANUAL State Saves all information views graphical objects expressions and variable in a cst state file Loading a state file will automatically re generate all views objects expressions and variables from a previous CF X Post session 1 8 Commands for Duct Bend Example As indicated in Section 1 the following conventions will be used to indicate the various commands that should be invoked Menu Sub Menu Sub Sub Menu Item chosen from the menu hierarchy at the top of a main panel or window Button Tab Command Option activated by clicking on a button or tab Link description Click on the description to move by a link to the next step page Name value Enter the value in the named box Name Y selection Choose the selection s from the named list Name Panel or window name Name On off switch box and Name On off switch circle radio button 1 8 1 Geometry Model The first phase uses DesignModeler The commands listed below will create a solid body geometry that will represent the flow domain set up the project directory and page set up a plane for sketching on sketch in the flow path through the duct Figure 1 4 generate
47. odes the two fields are identical For nodes on the wall there are two values for every flow property the value implied by the boundary condition and the average value in the sub element region around the node The first value is the hybrid value and the second value is the conser vative value For a node on a solid wall the hybrid velocity will be zero and the conservative velocity will typically be non zero Common flow visualization objects include Wireframe a singleton object automatically created to show the surface mesh on the flow domain The edge angle controls how much of the surface mesh is drawn An element edge is drawn if the angle between the two adjacent element faces is bigger than the edge angle For rectangular geometries and meshes an edge angle of 30 ensures that the outside edges of the domain are drawn and an edge angle of 0 ensures that all mesh edges are drawn Contour lines of a constant scalar value on a specified surface like elevation lines on a topological map The appearance of the plot is controlled by the rendering options For example with the smooth shading option turned on a fringe plot areas between contour lines are filled with colour is drawn and with no shading only the contour lines are drawn Vector the field of vectors in a region Streamline lines that are parallel to the local velocity vectors Typically stream lines are started on an inlet surface and will extend to an outlet surface a
48. of the model k the turbulent kinetic energy and the rate at which k is dissipated by molecular viscous action Specification of the Boundary Conditions The boundary conditions that model the interaction of the surroundings with the solution domain are e uniform velocity of 3 ms7 and uniform turbulence properties of tur bulence intensity of 5 and turbulence eddy length scales of 0 0075 m i e 10 of the duct height across the inlet surface e uniform static pressure across the outlet surface 8 STUDENT USER MANUAL e no slip conditions along the duct walls and the standard wall function treatment to resolve log law behaviour in the near wall region where the flow is not fully turbulent and e symmetry conditions on the front and back surfaces to ensure that the simulated flow is two dimensional The above provides a mathematically complete description of the CFD model In the next four sections information will be provided on the use of the soft ware that can implement the CFD steps of geometry modelling mesh generation physical modelling solver operation and visualization The actual software com mands to use for this example problem are given in Section 1 8 1 4 Geometry and Mesh Specification In the first steps of the CFD computer modelling the solution domain is cre ated in a digital form and then subdivided into a large number of small finite elements or volumes Common finite element types shapes include
49. on should decrease The iterative algorithm will stop when either the maximum number of itera tions is reached or when the convergence criterion is reached whichever occurs first The convergence criterion is a convergence goal for either the maximum normalized residuals or the root mean square RMS of the normalized residuals Note that the residuals are normalized to have values near one at the start of the iterative process 1 6 CFX Solver Manager Solver Operation A solver run requires a definition file to define and initialize the run Table 1 2 shows how def and res files can be used to define different runs Definition File Initial File Use def Start from simple initial fields res Continue solution for further convergence def res Restart from existing solution with new flow model Table 1 2 Input file combinations 1 6 1 Monitoring the Solver Run The solution of the algebraic equation set is the component of the code operation which takes the most computer time Fortunately because it operates in a batch 20 STUDENT USER MANUAL mode it does not take much of the user s time The operation of the solver should however be monitored and facilities are provided for this Table 1 3 shows typical solver diagnostic output listing the residual reduc tion properties for the first few time steps iterations of a solver run OUTER LOOP ITERATION 1 Equation Rate RMS Res H
50. or faces hold the Ctrl key down while clicking on the component surfaces in the Model View Repeat to create an entity called outer wall For a region called front surface use the Z view of the Model View when selecting the surface Notice that there are two parallel planes in the lower left corner of the model view The front most of these planes should be outlined in red COMMANDS FOR DUCT BEND EXAMPLE 29 e Do not set up a region for the back surface It will remain as the single surface in the Default 2D Region e In the Tree View select Options to see the mesh options in the the Details View Set Surface Meshing W Advancing Front and Meshing Strategy V Extruded 2D Mesh In the Tree View expand the Spacing entity Select the Default Body Spacing entity to open the Body Spacing Details View Set Maximum Spacing m 0 0075 e Right mouse click on the Extruded Periodic Pair entity x In the Model View select the front surface and then click Location 1 Apply in the Details View In the Model View select the back surface remember to use the loca tion planes in the lower left corner of the Model View and then click Location 2 Apply in the Details View and Set Periodic Type V Translation e In the Tree View right mouse click on Inflation and select Insert Inflated Boundary to create an Inflated Boundary entity Selec
51. replace the scale legend Under the Regions branch turn O Wireframe on Orthographic projection will work best for two dimensional views Notice that if you double click on an object in the Object tree then an edit panel opens up for that object Choose File Print and in the Print panel set x x File vectorplot png and x Format V PNG followed by Print The plot will printed to the file vectorplot png in your working directory You can import this file into other documents Choose Create Variable and in the New Variable definition window set Name Vorticity and click OK In Vorticity edit panel lower left x set Method Expression x set O Scalar on 36 STUDENT USER MANUAL e Choose Create Object Contour accept Name Contour 1 and click OK fill in Expression Velocity v Gradient X Velocity u Gradient Y and click Apply to define a fringe contour plot object and open an edit panel In the panel set Locations Y FRONT SURFACE Variable V Vorticity Visibility on and click Apply The fringe plot should appear in the Viewer window Choose Create Object Line accept Name Line 1 and click OK to de fine
52. sh between coincident and coincident point constraints and e Auto Constraints are used to automatically connect points and edges For example if one edge of a square is increased in length the opposite edge length is also increased so that the shape remains rectangular Features are created from sketches by one of the following operations Extrude Sweep the sketch in a particular direction i e to make a bar Revolve Sweep the sketch through a revolution about a particular axis of ro tation i e to make a wedge shape Sweep Sweep the sketch along a sketched path i e to make a curved bar and Skin Loft Join up a series of sketches or profiles to form the 3D feature like putting a skin over the frame of a wing Features are integrated into the existing active solid with one of the following Boolean operations Add Material Merge the new feature with the active solid Cut Material Remove the material of the new feature from the active solid Slice Material Remove a section from an active solid and Imprint Face Break a face into two parts For example this will open a hole on a cylindrical pipe wall Sometimes it is necessary to use multiple solids in a single part These solids must share at least one common face This common face might be used to model a thin surface in the flow solver In this case 1 Select active solid with the body selection filter turned on 2 Freeze the solid body to stop the Boolean merge or r
53. t page by clicking on the PipeBend Project tab at the top left of the screen Click on the PipeBend DesignModeler tab to return to the DesignModeler page There are four major areas on the page command menus and buttons at the top a Tree View and Sketch Toolbox on the left a Details View at the bottom left and a Model View window Place the mouse cursor over one of the command buttons in the top row A brief description of the button s action should appear you may need to click in the window once to make it active Visit each button with the mouse cursor to see its action One method of controlling the view is with the coordinate system triad in the lower right corner of Model View Click on the Z axis of the triad to see a back view of the pipe bend Click on the cyan sphere to select the isometric view Another method of controlling the view is with the mouse left button in conjunction with a mouse action selection From the upper row of buttons select the Pan action Holding the left mouse button down drag the mouse over the Model View to translate the view Select the Zoom action and repeat the mouse action to change the size of the view Select the Rotate action The rotate action is context sensitive in that it depends upon the position of the mouse cursor With the mouse cursor close to the pipe bend press the left mouse button to get free 3D rotation The
54. t the three surfaces of the inner wall in the Model View for the Location and set Maximum Thickness m 0 0075 e Repeat to create an Inflated Boundary of Maximum Thickness m 0 0075 on the outer wall e In the Tree View expand the Preview entity Right mouse click on Default Preview Group and select Generate This Surface Mesh An Overall Progress window should open in the lower left corner and after a short time you should see a mesh of triangles on the surfaces of the solid There will be some gaps on the front and back surfaces near the inner and outer walls where the inflated boundary meshing is used e Click the Generate a volume mesh for the current problem icon on the top row of icons buttons In the Windows file window set File name Ductbend gtm Again a progress window will open in the lower left corner When this win dow closes go to the Tree View and select Errors to ensure that no errors are reported in the Details View To close this phase select File Save As and set File name Ductbend cmdb Return to the Project page by clicking on the Ductbend Project tab at the top left corner of the window 1 8 3 Pre processing The first CFD phase is preprocessing In this phase the complete CFD model mesh fluids flow processes boundary conditions etc is defined and saved in a hierarchical database Af
55. ter opening CFX Pre the commands listed below will accomplish the following steps 30 STUDENT USER MANUAL e link the mesh gtn file to a CFX flow project e set simulation type to steady state e establish a fluid with nominal properties of water e specify the region through which the fluid will flow the fluid nominally water and the physical models fluid flow no heat transfer turbulence standard k e model with scalable wall functions e set up and attach the rough wall boundary condition the inlet boundary condition the outlet boundary condition and the symmetry boundary con ditions e set the global initial conditions e set the solver controls for discretization scheme time step type and conver gence criteria e set the output variable list and e write the complete CFD model definition to a def file To accomplish these steps execute the following commands e Highlight the mesh file Ductbend gtm in the Project page Choose Create CFD Simulation with Mesh Advanced CFD Task e After a short wait the CFX Pre page will open This page is similar to the CFX Post page There are three main areas the menus and command buttons at the top the Viewer window at the right and the database panels at the left e Select the Regions tab to see the region database Check that O Assembly entity under the Mesh Assemblies tree is on Click on the name of the entity Assembly to see the m
56. the solid body geometry To begin e Create a new folder N Ductbend to be the working directory for the project files Open ANSYS Workbench from Start Programs Engineering ANSYS 9 0 ANSYS Workbench To open a new project 1 In the Start window select Empty Project in the New panel 2 From the menu bar choose File Save As to create a project file in your working directory and 3 In the Save As window fill in File name Ductbend wbdb and click the Save button e From the menu bar choose Tools Options to change the length units options In the Options window expand the DesignModeler entity and select O Grid Defaults Meters in the tree view on the left Set Minimum Axes Length 0 5 and Major Grid Spacing 0 1 Click OK to save the options and close the window e Choose the Create DesignModeler geometry task COMMANDS FOR DUCT BEND EXAMPLE 25 ses i i i i i H i i i i i i Fig 1 4 Wireframe of the final sketch of the duct bend flow path Check that the desired length unit is Meter is selected and click Ok in the units window that appears In the Tree View select the XYPlane entity and then click the New Sketch icon to create the Sketch1 entity as a component of the XYPlane To start the sketching select the Sketching tab e To draw in the 2D sketch of the duct flow path Figure 1 4 1 Sele
57. thm 1 5 CFX Pre Physical Modelling CFX Pre is a program that builds up a database for storing all of the informa tion geometry mesh physics and numerical methods that is required by the equation solver The contents of the database is written to a def definition file at the end of the CFX Pre session The database is organized as a hierarchy of objects Each object in the hier archy is composed of sub objects and parameters There are two main objects Flow and Library The Flow object holds all of the data on the flow model and the Library object holds the property data on a set of common fluids The major components of the Flow object are organized in the following hierarchy e Flow x Domain o Fluids List o Boundary o Domain Models Domain Motion Reference Pressure o Fluid Models Heat Transfer Model Turbulence Model Turbulent Wall Functions x Initialization x Output Control x Simulation Type x Solver Control o Advection Scheme o Convergence Control o Convergence Criteria CFX Pre has functions to create new objects in the hierarchy and to edit existing objects through edit panels For most objects the edit panel provides guidance on the possible parameter settings 1 5 1 Domain Fluids List A fluid or mixture of fluids in more complex multi phase flows has to be asso ciated with each domain The fluid for a particular domain can be selected from CFX PRE PHYSICAL MODELLING 15
58. to be identical i e the face mesh on the first surface can be uniquely mapped onto the second surface In other cases where the flow is three dimensional it may still be desirable to have identical face meshes on two bounding surfaces For example this is useful in periodically repeating geometries Each Periodic Pair is defined by two surfaces and a two dimensional pla nar Periodic Type Y Translational or axisymmetric Periodic Type V Rotational mapping Inflation In boundary layer regions adjacent to solid walls it is often desirable to make a very small mesh size in the direction normal to the wall in order to resolve the large velocity shear strain rates If tetrahedral meshes are used in this region there will either be a large number of very small elements with equal spacing in all directions i e isotropic elements with vertex angles close to 60 or very thin squashed elements These choices are either inefficient or inaccurate A better element shape in this region is a triangular prism Figure 1 3 based on the surface triangular mesh The basic shape of the GEOMETRY AND MESH SPECIFICATION 13 prism element is independent of the height of the prism mesh length scale normal to the wall The layer of prism elements is an inflated boundary with Maximum Thickness that is often approximately the same as the default body mesh spacing or First Layer Thickness that is often set by the properti
59. y Y No Options are used for setting the output filename and for setting the algorithms used for generating the volume and surface meshes Volume Meshing Vv Advancing Front is the primary algorithm for gen erating meshes in 3D geometries The algorithm starts with a surface mesh and then builds a layer of tetrahedral elements over the surface based on the surface triangular elements This creates a new surface The process is repeated advancing the layers of tetrahedral elements into the interior of the volume Volume Meshing V Extruded 2D Mesh is an algorithm for generating meshes in geometries that are effectively 2D A surface mesh is ex truded through space by either translation or rotation from one face to a matching face in the periodic pair This option is useful for simulating two dimensional flows and flows in long constant area ducts The num ber of elements often 1 and mesh spacing distribution in the extruded direction can be specified Surface Meshing V Delaunay lis a fast algorithm for creating isotropic 14 STUDENT USER MANUAL surface meshes Suited to complex surface geometries with small mesh spacing Surface Meshing VW Advancing Front starts at the edges of the surface and is a similar algorithm to the volume meshing algorithm described above Since it creates regular meshes on simple rectangular type surfaces it is the recommended algori
60. ynolds Stress a second moment closure model that explicitly solves transport equations for all six components of the turbulent stress tensor and that requires significantly more computing resources than the two equation variations Turbulent Wall Functions are required to treat the transition to laminar like flow close to solid walls The wall treatments are tied to the turbulence model choice The scalable wall function method used with the k Epsilon turbulence model is a variant of the standard wall function method The 18 STUDENT USER MANUAL scalable wall function method automatically adjusts the near wall treatment with mesh spacing in the near wall region 1 5 2 Initialization The algebraic equation set that must be solved to find the velocity and pressure at each mesh point is composed of nonlinear equations All strategies for solving nonlinear equation sets involve iteration which requires an initial guess for all solution variables For a turbulent flow sufficient information must be provided so that the following field values can be set initialized at each mesh point e velocity vector 3 components e fluid pressure e turbulent kinetic energy and e dissipation rate of turbulent kinetic energy CFX Pre provides a default algorithm for calculating initial values based on interpolating boundary condition information into the interior of the domain This default algorithm is adequate for many simulations The initial condit
Download Pdf Manuals
Related Search