Baixe ANSYS CFX Tutorials e outras Notas de estudo em PDF para Engenharia Química, somente na Docsity! ANSYS CFX Tutorials ANSYS CFX Release 11.0 December 2006 ANSYS, Inc. Southpointe 275 Technology Drive Canonsburg, PA 15317 ansysinfo@ansys.com http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494 Page vANSYS CFX Tutorials Table of Contents Copyright and Trademark Information Disclaimer Notice U.S. Government Rights Third-Party Software Introduction to the ANSYS CFX Tutorials Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Setting the Working Directory . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 Changing the Display Colors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3 Before You Begin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Tutorial 1 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6 Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .12 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .15 Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31 Before You Begin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32 Tutorial 1a Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32 Table of Contents: Tutorial 2: Flow in a Static Mixer (Refined Mesh) Page vi ANSYS CFX Tutorials Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .33 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .34 Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .41 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .43 Tutorial 2: Flow in a Static Mixer (Refined Mesh) Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .59 Tutorial 2 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .60 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .60 Defining a Simulation using General Mode in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .61 Obtaining a Solution Using Interpolation with ANSYS CFX-Solver . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .66 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .68 Tutorial 3: Flow in a Process Injection Mixing Pipe Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .77 Tutorial 3 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .78 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .78 Defining a Simulation using General Mode in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .79 Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .87 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .88 Tutorial 4: Flow from a Circular Vent Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .93 Tutorial 4 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .94 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .95 Defining a Steady-State Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .95 Obtaining a Solution to the Steady-State Problem . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .99 Defining a Transient Simulation in ANSYS CFX-Pre. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100 Obtaining a Solution to the Transient Problem . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 104 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105 Tutorial 5: Flow Around a Blunt Body Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109 Tutorial 5 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111 Table of Contents: Tutorial 6: Buoyant Flow in a Partitioned Cavity ANSYS CFX Tutorials Page vii Obtaining a Solution Using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 116 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119 Tutorial 6: Buoyant Flow in a Partitioned Cavity Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127 Tutorial 6 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 129 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135 Tutorial 7: Free Surface Flow Over a Bump Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Tutorial 7 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 148 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149 Using a Supercritical Outlet Condition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 154 Tutorial 8: Supersonic Flow Over a Wing Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155 Tutorial 8 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162 Tutorial 9: Flow Through a Butterfly Valve Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165 Tutorial 9 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 166 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 180 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 180 Tutorial 10: Table of Contents: Tutorial 19: Cavitation Around a Hydrofoil Page x ANSYS CFX Tutorials Tutorial 18 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 300 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301 Using Eddy Dissipation and P1 Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301 Defining a Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 302 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 307 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 308 Laminar Flamelet and Discrete Transfer Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311 Further Postprocessing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 316 Tutorial 19: Cavitation Around a Hydrofoil Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 317 Tutorial 19 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 318 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319 Creating an Initial Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319 Obtaining an Initial Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 323 Viewing the Results of the Initial Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324 Preparing a Simulation with Cavitation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 326 Obtaining a Cavitation Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328 Viewing the Results of the Cavitation Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328 Tutorial 20: Fluid Structure Interaction and Mesh Deformation Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 331 Tutorial 20 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 332 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 333 Using CEL Expressions to Govern Mesh Deformation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 334 Using a Junction Box Routine to Govern Mesh Deformation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 343 Tutorial 21: Oscillating Plate with Two-Way Fluid-Structure Interaction Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 353 Tutorial 21 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354 Setting up the Solid Physics in Simulation (ANSYS Workbench) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 355 Setting up the Fluid Physics and ANSYS Multi-field Settings in ANSYS CFX-Pre. . . . . . . . . . . . . . . . . . . . . . . . . 358 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 364 Viewing Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 365 Tutorial 22: Table of Contents: Tutorial 23: Aerodynamic & Structural Performance of a Centrifugal Compressor ANSYS CFX Tutorials Page xi Optimizing Flow in a Static Mixer Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 369 Tutorial 22 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 370 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 370 Creating the Project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 371 Creating the Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 372 Creating the Mesh. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 377 Overview of ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 380 Setting the Output Parameter in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 386 Running Design Studies in DesignXplorer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 387 Tutorial 23: Aerodynamic & Structural Performance of a Centrifugal Compressor Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395 Tutorial 23 Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 396 Overview of the Problem to Solve. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 397 Reviewing the Centrifugal Compressor Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 397 Creating the Mesh in ANSYS TurboGrid . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 398 Defining the Aerodynamic Simulation in ANSYS CFX-Pre . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 401 Obtaining a Solution using ANSYS CFX-Solver Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 403 Viewing the Results in ANSYS CFX-Post . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 404 Importing Geometry into DesignModeler . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 405 Simulating Structural Stresses Due to Pressure Loads . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 406 Simulating Structural Stresses Due to Rotation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 407 Table of Contents: Tutorial 23: Aerodynamic & Structural Performance of a Centrifugal Compressor Page xii ANSYS CFX Tutorials Page 3 ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS CFX Tutorials Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode Introduction This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a mixing vessel; the water exits through an outlet pipe. A general workflow is established for analyzing the flow of fluid into and out of a mixer. This tutorial includes: • Before You Begin (p. 4) • Tutorial 1 Features (p. 4) • Overview of the Problem to Solve (p. 5) • Defining a Simulation in ANSYS CFX-Pre (p. 6) • Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 12) • Viewing the Results in ANSYS CFX-Post (p. 15) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) To learn how to perform these tasks in Workbench, see Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench (p. 31 in "ANSYS CFX Tutorials"). Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Before You Begin Page 4 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Before You Begin Create a working directory for your files. Once this is done, copy the sample files used in this tutorial to your working directory from the installation folder for your software (<CFXROOT>/examples/ (for example, C:\Program Files\ANSYS Inc\v110\CFX\examples)) to avoid overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 7). Sample files used by this tutorial are: • StaticMixerMesh.gtm • StaticMixer.pre Tutorial 1 Features This tutorial addresses the following features of ANSYS CFX. In this tutorial you will learn about: • Using Quick Setup mode in ANSYS CFX-Pre to set up a problem. • Modifying the outline plot in ANSYS CFX-Post. • Using streamlines in ANSYS CFX-Post to trace the flow field from a point. • Viewing temperature using colored planes and contours in ANSYS CFX-Post. • Creating an animation and saving it to an MPEG file. Component Feature Details ANSYS CFX-Pre User Mode Quick Setup Wizard Simulation Type Steady State Fluid Type General Fluid Domain Type Single Domain Turbulence Model k-Epsilon Heat Transfer Thermal Energy Boundary Conditions Inlet (Subsonic) Outlet (Subsonic) Wall: No-Slip Wall: Adiabatic Timestep Physical Time Scale ANSYS CFX-Post Plots Animation Contour Outline Plot (Wireframe) Point Slice Plane Streamline Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Overview of the Problem to Solve ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 5 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overview of the Problem to Solve This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a mixing vessel; the water exits through an outlet pipe. A general workflow is established for analyzing the flow of fluid into and out of a mixer. Water enters through both pipes at the same rate but at different temperatures. The first entry is at a rate of 2 m/s and a temperature of 315 K and the second entry is at a rate of 2 m/s at a temperature of 285 K. The radius of the mixer is 2 m. Your goal in this tutorial is to understand how to use ANSYS CFX to determine the speed and temperature of the water when it exits the static mixer. Figure 1 Static Mixer with 2 Inlet Pipes and 1 Outlet Pipe 2 m/s 285 K 2 m/s 315 K r=2m Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-Pre Page 8 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 2. Under File type, select CFX Mesh (*gtm *cfx). 3. From your working directory, select StaticMixerMesh.gtm. 4. Click Open. The mesh loads. 5. Click Next. Using the Viewer Now that the mesh is loaded, take a moment to explore how you can use the viewer toolbar to zoom in or out and to rotate the object in the viewer. Using the Zoom Tools There are several icons available for controlling the level of zoom in the viewer. 1. Click Zoom Box 2. Click and drag a rectangular box over the geometry. 3. Release the mouse button to zoom in on the selection. The geometry zoom changes to display the selection at a greater resolution. 4. Click Fit View to re-center and re-scale the geometry. Rotating the geometry If you need to rotate an object or to view it from a new angle, you can use the viewer toolbar. 1. Click Rotate on the viewer toolbar. 2. Click and drag within the geometry repeatedly to test the rotation of the geometry. The geometry rotates based on the direction of movement. Notice how the mouse cursor changes depending on where you are in the viewer: 3. Right-click a blank area in the viewer and select Predefined Camera > View Towards-X). 4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z Up). A clearer view of the mesh is displayed. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 9 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Defining Model Data You need to define the type of flow and the physical models to use in the fluid domain. You will specify the flow as steady state with turbulence and heat transfer. Turbulence is modeled using the - turbulence model and heat transfer using the thermal energy model. The - turbulence model is a commonly used model and is suitable for a wide range of applications. The thermal energy model neglects high speed energy effects and is therefore suitable for low speed flow applications. Procedure 1. Ensure that Physics Definition is displayed. 2. Under Model Data, set Reference Pressure to 1 [atm]. All other pressure settings are relative to this reference pressure. 3. Set Heat Transfer to Thermal Energy. 4. Set Turbulence to k-Epsilon. 5. Click Next. Defining Boundaries The CFD model requires the definition of conditions on the boundaries of the domain. Procedure 1. Ensure that Boundary Definition is displayed. 2. Delete Inlet and Outlet from the list by right-clicking each and selecting Delete. 3. Right-click in the blank area where Inlet and Outlet were listed, then select New. 4. Set Name to in1. 5. Click OK. The boundary is created and, when selected, properties related to the boundary are displayed. Setting Boundary Data Once boundaries are created, you need to create associated data. Based on Figure 1, you will define the first inlet boundary condition’s velocity and temperature. Procedure 1. Ensure that Boundary Data is displayed. 2. Set Boundary Type to Inlet. 3. Set Location to in1. Setting Flow Specification Once boundary data is defined, the boundary needs to have the flow specification assigned. Procedure 1. Ensure that Flow Specification is displayed. 2. Set Option to Normal Speed. 3. Set Normal Speed to 2 [m s^-1]. k ε k ε Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Defining a Simulation in ANSYS CFX-Pre Page 10 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Setting Temperature Specification Once flow specification is defined, the boundary needs to have temperature assigned. Procedure 1. Ensure that Temperature Specification is displayed. 2. Set Static Temperature to 315 [K]. Reviewing the Boundary Condition Definitions Defining the boundary condition for in1 required several steps. Here the settings are reviewed for accuracy. Based on Figure 1, the first inlet boundary condition consists of a velocity of 2 m/s and a temperature of 315 K at one of the side inlets. Procedure 1. Review the boundary in1 settings for accuracy. They should be as follows: Creating the Second Inlet Boundary Definition Based on Figure 1, you know the second inlet boundary condition consists of a velocity of 2 m/s and a temperature of 285 K at one of the side inlets. You will define that now. Procedure 1. Under Boundary Definition, right-click in the selector area and select New. 2. Create a new boundary named in2 with these settings: Creating the Outlet Boundary Definition Now that the second inlet boundary has been created, the same concepts can be applied to building the outlet boundary. 1. Create a new boundary named out with these settings: Tab Setting Value Boundary Data Boundary Type Inlet Location in1 Flow Specification Option Normal Speed Normal Speed 2 [m s^-1] Temperature Specification Static Temperature 315 [K] Tab Setting Value Boundary Data Boundary Type Inlet Location in2 Flow Specification Option Normal Speed Normal Speed 2 [m s^-1] Temperature Specification Static Temperature 285 [K] Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Obtaining a Solution Using ANSYS ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 13 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Two windows are displayed when ANSYS CFX-Solver Manager runs. There is an adjustable split between the windows, which is oriented either horizontally or vertically depending on the aspect ratio of the entire ANSYS CFX-Solver Manager window (also adjustable). One window shows the convergence history plots and the other displays text output from ANSYS CFX-Solver. The text lists physical properties, boundary conditions and various other parameters used or calculated in creating the model. All the text is written to the output file automatically (in this case, StaticMixer_001.out). Start the Run The Define Run dialog box allows configuration of a run for processing by ANSYS CFX-Solver. When ANSYS CFX-Solver Manager is launched automatically from ANSYS CFX-Pre, all of the information required to perform a new serial run (on a single processor) is entered automatically. You do not need to alter the information in the Define Run dialog box. This is a very quick way to launch into ANSYS CFX-Solver without having to define settings and values. Procedure 1. Ensure that the Define Run dialog box is displayed. 2. Click Start Run. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Obtaining a Solution Using ANSYS Page 14 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS CFX-Solver launches and a split screen appears and displays the results of the run graphically and as text. The panes continue to build as ANSYS CFX-Solver Manager operates. Note: Once the second iteration appears, data begins to plot. Plotting may take a long time depending on the amount of data to process. Let the process run. Move from ANSYS CFX-Solver to ANSYS CFX-Post Once ANSYS CFX-Solver has finished, you can use ANSYS CFX-Post to review the finished results. Procedure 1. When ANSYS CFX-Solver is finished, click Yes to post-process the results. After a short pause, ANSYS CFX-Post starts and ANSYS CFX-Solver Manager closes. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 15 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Viewing the Results in ANSYS CFX-Post When ANSYS CFX-Post starts, the viewer and Outline workspace are displayed. The viewer displays an outline of the geometry and other graphic objects. You can use the mouse or the toolbar icons to manipulate the view, exactly as in ANSYS CFX-Pre. Workflow Overview This tutorial describes the following workflow for viewing results in ANSYS CFX-Post: 1. Setting the Edge Angle for a Wireframe Object (p. 16) 2. Creating a Point for the Origin of the Streamline (p. 17) 3. Creating a Streamline Originating from a Point (p. 18) 4. Rearranging the Point (p. 19) 5. Configuring a Default Legend (p. 19) 6. Creating a Slice Plane (p. 20) 7. Defining Slice Plane Geometry (p. 21) 8. Configuring Slice Plane Views (p. 21) 9. Rendering Slice Planes (p. 22) 10. Coloring the Slice Plane (p. 23) 11. Moving the Slice Plane (p. 23) 12. Adding Contours (p. 24) 13. Working with Animations (p. 25) 14. Showing the Animation Dialog Box (p. 25) Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post Page 18 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Creating a Streamline Originating from a Point Where applicable, streamlines can trace the flow direction forwards (downstream) and/or backwards (upstream). Procedure 1. From the main menu, select Insert > Streamline. You can also use the toolbars to create a variety of objects. Later modules and tutorials will explore this further. 2. Click OK. This accepts the default name. 3. Under Definition, in Start From, ensure that Point 1 is set. Tip: To create streamlines originating from more than one location, click the ellipsis icon to the right of the Start From box. This displays the Location Selector dialog box, where you can use the <Ctrl> and <Shift> keys to pick multiple locators. 4. Click the Color tab. 5. Set Mode to Variable. 6. Set Variable to Total Temperature. 7. Set Range to Local. 8. Click Apply. The streamline shows the path of a zero mass particle from Point 1. The temperature is initially high near the hot inlet, but as the fluid mixes the temperature drops. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 19 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Rearranging the Point Once created, a point can be rearranged manually or by setting specific coordinates. Tip: In this module, you may choose to display various views and zooms from the Predefined Camera option in the shortcut menu (such as Isometric View (Z up) or View Towards -X) and by using Zoom Box if you prefer to change the display. Procedure 1. In Outline, under User Locations and Plots double-click Point 1. Properties for the selected user location are displayed. 2. Under Point, set these coordinates: -1, -2.9, 1. 3. Click Apply. The point is moved and the streamline redrawn. 4. In the selection tools, click Single Select. While in this mode, the normal behavior of the left mouse button is disabled. 5. In the viewer, drag Point 1 (appears as a yellow addition sign) to a new location within the mixer. The point position is updated in the details view and the streamline is redrawn at the new location. The point moves normal in relation to the viewing direction. 6. Click Rotate . Tip: You can also click in the viewer area, and press the space bar to toggle between Select and Viewing Mode. A way to pick objects from Viewing Mode is to hold down <Ctrl> + <Shift> while clicking on an object with the left mouse button. 7. Under Point, reset these coordinates: -1, -1, 1. 8. Click Apply. The point appears at its original location. 9. Right-click a blank area in the viewer and select Predefined Camera > View Towards -X. Configuring a Default Legend You can modify the appearance of the default legend. The default legend appears whenever a plot is created that is colored by a variable. The streamline color is based on temperature; therefore, the legend shows the temperature range. The color pattern on the legend’s color bar is banded in accordance with the bands in the plot1. 1. An exception occurs when one or more bands in a contour plot represent values beyond the legend’s range. In this case, such bands are colored using a color that is extrapolated slightly past the range of colors shown in the legend. This can happen only when a user-specified range is used for the legend. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post Page 20 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The default legend displays values for the last eligible plot that was opened in the details view. To maintain a legend definition during an ANSYS CFX-Post session, you can create a new legend by clicking Legend . Because there are many settings that can be customized for the legend, this module allows you the freedom to experiment with them. In the last steps you will set up a legend, based on the default legend, with a minor modification to the position. Tip: When editing values, you can restore the values that were present when you began editing by clicking Reset. To restore the factory-default values, click Default. Procedure 1. Double click Default Legend View 1. The Definition tab of the default legend is displayed. 2. Apply the following settings 3. Click Apply. The appearance and position of the legend changes based on the settings specified. 4. Modify various settings in Definition and click Apply after each change. 5. Select Appearance. 6. Modify a variety of settings in the Appearance and click Apply after each change. 7. Click Defaults. 8. Click Apply. 9. Under Outline, in User Locations and Plots, clear the check boxes for Point 1 and Streamline 1. Since both are no longer visible, the associated legend no longer appears. Creating a Slice Plane Defining a slice plane allows you to obtain a cross–section of the geometry. In ANSYS CFX-Post you often view results by coloring a graphic object. The graphic object could be an isosurface, a vector plot, or in this case, a plane. The object can be a fixed color or it can vary based on the value of a variable. You already have some objects defined by default (listed in the Outline). You can view results on the boundaries of the static mixer by coloring each boundary object by a variable. To view results within the geometry (that is, on non-default locators), you will create new objects. You can use the following methods to define a plane: • Three Points: creates a plane from three specified points. Tab Setting Value Definition Title Mode User Specified Title Streamline Temp. Horizontal (Selected) Location > Y Justification Bottom Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 23 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The line segments show where the slice plane intersects with mesh element faces. The end points of each line segment are located where the plane intersects mesh element edges. 9. Right-click a blank area in the viewer and select Predefined Camera > View Towards -Z. The image shown below can be used for comparison with tutorial 2 (in the section Creating a Slice Plane (p. 68)), where a refined mesh is used. Coloring the Slice Plane The Color panel is used to determine how the object faces are colored. Procedure 1. Apply the following settings to Slice 2. Click Apply. Hot water (red) enters from one inlet and cold water (blue) from the other. Moving the Slice Plane The plane can be moved to different locations. Tab Setting Value Color Mode Variable* *. You can specify the variable (in this case, temperature) used to color the graphic element. The Constant mode allows you to color the plane with a fixed color. Variable Temperature Render Draw Faces (Selected) Draw Lines (Cleared) Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post Page 24 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu. 2. Click the Geometry tab. Review the settings in Definition under Point and under Normal. 3. Click Single Select . 4. Click and drag the plane to a new location that intersects the domain. As you drag the mouse, the viewer updates automatically. Note that Point updates with new settings. 5. Set Point settings to 0,0,1. 6. Click Apply. 7. Click Rotate . 8. Turn off visibility for Slice by clearing the check box next to Slice in the Outline. Adding Contours Contours connect all points of equal value for a scalar variable (for example, Temperature) and help to visualize variable values and gradients. Colored bands fill the spaces between contour lines. Each band is colored by the average color of its two bounding contour lines (even if the latter are not displayed). Procedure 1. Select Insert > Contour from the main menu or click Contour . The New Contour dialog box is displayed. 2. Set Name to Slice Contour. 3. Click OK. 4. Apply the following settings 5. Click Apply. Important: The colors of 3D graphics object faces are slightly altered when lighting is on. To view colors with highest accuracy, clear Lighting under Draw Faces on the Render tab and click Apply. Tab Setting Value Geometry Locations Slice Variable Temperature Render Draw Faces (Selected) Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 25 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The graphic element faces are visible, producing a contour plot as shown. Note: Make sure that the checkbox next to Slice in the Outline is cleared. Working with Animations Animations build transitions between views for development of video files. Workflow Overview This tutorial follows the general workflow for creating a keyframe animation: 1. Showing the Animation Dialog Box (p. 25) 2. Creating the First Keyframe (p. 26) 3. Creating the Second Keyframe (p. 26) 4. Viewing the Animation (p. 27) 5. Modifying the Animation (p. 28) 6. Saving to MPEG (p. 29) Showing the Animation Dialog Box The Animation dialog box is used to define keyframes and to export to a video file. Procedure 1. Select Tools > Animation or click Animation . The Animation dialog box can be repositioned as required. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post Page 28 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Modifying the Animation To make the plane sweep through the whole geometry, you will set the starting position of the plane to be at the top of the mixer. You will also modify the Range properties of the plane so that it shows the temperature variation better. As the animation is played, you can see the hot and cold water entering the mixer. Near the bottom of the mixer (where the water flows out) you can see that the temperature is quite uniform. The new temperature range lets you view the mixing process more accurately than the global range used in the first animation. Procedure 1. Apply the following settings to Slice 2. Click Apply. The slice plane moves to the top of the static mixer. Note: Do not double click in the next step. 3. In the Animation dialog box, single click (do not double-click) KeyframeNo1 to select it. If you had double-clicked KeyFrameNo1, the plane and viewer states would have been redefined according to the stored settings for KeyFrameNo1. If this happens, click Undo and try again to select the keyframe. 4. Click Set Keyframe . The image in the Viewer replaces the one previously associated with KeyframeNo1. 5. Double-click KeyframeNo2. The object properties for the slice plane are updated according to the settings in KeyFrameNo2. 6. Apply the following settings to Slice 7. Click Apply. 8. In the Animation dialog box, single-click KeyframeNo2. 9. Click Set Keyframe to save the new settings to KeyframeNo2. Tab Setting Value Geometry Point 0, 0, 1.99 Color Variable Temperature Range User Specified Min 295 [K] Max 305 [K] Tab Setting Value Color Variable Temperature Range User Specified Min 295 [K] Max 305 [K] Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 29 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Saving to MPEG By defining the geometry and then saving to MPEG, the results can be saved to a video file. Procedure 1. Click More Animation Options to view the additional options. The Loop and Bounce radio buttons determine what happens when the animation reaches the last keyframe. When Loop is selected, the animation repeats itself the number of times defined by Repeat. When Bounce is selected, every other cycle is played in reverse order, starting with the second. 2. Click Save MPEG. 3. Click Browse next to Save MPEG. 4. Under File name type: StaticMixer.mpg 5. If required, set the path location to a different folder. 6. Click Save. The MPEG file name (including path) is set. At this point, the animation has not yet been produced. 7. Click Previous Keyframe . Wait a moment as the display updates the keyframe display. 8. Click Play the animation . 9. If prompted to overwrite an existing movie click Overwrite. The animation plays and builds an MPEG file. 10. Click the Options button at the bottom of the Animation dialog box. In Advanced, you can see that a Frame Rate of 24 frames per second was used to create the animation. The animation you produced contains a total of 22 frames, so it takes just under 1 second to play in a media player. 11. Click Cancel to close the dialog box. 12. Close the Animation dialog box. 13. Review the animation in third–party software as required. Exiting ANSYS CFX-Post When finished with ANSYS CFX-Post exit the current window: 1. When you are finished, select File > Quit to exit ANSYS CFX-Post. 2. Click Quit if prompted to save. Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode: Viewing the Results in ANSYS CFX-Post Page 30 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Overview of the Problem to Solve ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 33 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overview of the Problem to Solve This tutorial simulates a static mixer consisting of two inlet pipes delivering water into a mixing vessel; the water exits through an outlet pipe. A general workflow is established for analyzing the flow of fluid into and out of a mixer. Water enters through both pipes at the same rate but at different temperatures. The first entry is at a rate of 2 m/s and a temperature of 315 K and the second entry is at a rate of 2 m/s at a temperature of 285 K. The radius of the mixer is 2 m. Your goal in this tutorial is to understand how to use ANSYS CFX to determine the speed and temperature of the water when it exits the static mixer. Figure 1 Static Mixer with 2 Inlet Pipes and 1 Outlet Pipe 2 m/s 285 K 2 m/s 315 K r=2m Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre Page 34 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Defining a Simulation in ANSYS CFX-Pre Because you are starting with an existing mesh, you can immediately use ANSYS CFX-Pre to define the simulation. This is how ANSYS CFX-Pre will look with the imported mesh: In the image above, the left pane of ANSYS CFX-Pre displays the Outline. When you double-click on items in the Outline, the Outline editor opens and can be used to create, modify, and view objects. Note: In this documentation, the details view can also be referenced by the name of the object being edited, followed by the word “details view” (for example, if you double-click the Wireframe object, the Wireframe details view appears). Synopsis of Quick Setup Mode Quick Setup mode provides a simple wizard–like interface for setting up simple cases. This is useful for getting familiar with the basic elements of a CFD problem setup. This section describes using Quick Setup mode to develop a simulation in ANSYS CFX-Pre. Workflow Overview This tutorial follows the general workflow for Quick Setup mode: 1. Creating a New Simulation (p. 35) 2. Setting the Physics Definition (p. 35) 3. Importing a Mesh (p. 36) 4. Defining Model Data (p. 37) 5. Defining Boundaries (p. 37) Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 35 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 6. Setting Boundary Data (p. 37) 7. Setting Flow Specification (p. 37) 8. Setting Temperature Specification (p. 38) 9. Reviewing the Boundary Condition Definitions (p. 38) 10. Creating the Second Inlet Boundary Definition (p. 38) 11. Creating the Outlet Boundary Definition (p. 39) 12. Moving to General Mode (p. 39) 13. Writing the Solver (.def) File (p. 40) Playing a Session File If you want to skip past these instructions and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the appropriate session file. For details, see Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 40). After you have played the session file, proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41). Creating a New Simulation Before importing and working with a mesh, a simulation needs to be started using Quick Setup mode. Procedure 1. If required, launch ANSYS Workbench. 2. Click Empty Project. The Project page appears displaying an unsaved project. 3. Select File > Save or click Save . 4. If required, set the path location to the working folder you created for this tutorial. 5. Under File name, type: StaticMixer 6. Click Save. 7. On the left-hand task bar under Advanced CFD, click Start CFX-Pre. 8. Select File > New Simulation. 9. Select Quick Setup in the New Simulation File dialog box and click OK. 10. Select File > Save Simulation As. 11. Under File name, type: StaticMixer 12. Click Save. Setting the Physics Definition You need to specify the fluids used in a simulation. A variety of fluids are already defined as library materials. For this tutorial you will use a prepared fluid, Water, which is defined to be water at 25°C. Procedure 1. Ensure that Simulation Definition is displayed at the top of the Details view. 2. Under Fluid select Water. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre Page 38 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Procedure 1. Ensure that Flow Specification is displayed. 2. Set Option to Normal Speed. 3. Set Normal Speed to 2 [m s^-1]. Setting Temperature Specification Once flow specification is defined, the boundary needs to have temperature assigned. Procedure 1. Ensure that Temperature Specification is displayed. 2. Set Static Temperature to 315 [K]. Reviewing the Boundary Condition Definitions Defining the boundary condition for in1 required several steps. Here the settings are reviewed for accuracy. Based on Figure 1, the first inlet boundary condition consists of a velocity of 2 m/s and a temperature of 315 K at one of the side inlets. Procedure 1. Review the boundary in1 settings for accuracy. They should be as follows: Creating the Second Inlet Boundary Definition Based on Figure 1, you know the second inlet boundary condition consists of a velocity of 2 m/s and a temperature of 285 K at one of the side inlets. You will define that now. Procedure 1. Under Boundary Definition, right-click in the selector area and select New. 2. Create a new boundary named in2 with these settings: Tab Setting Value Boundary Data Boundary Type Inlet Location in1 Flow Specification Option Normal Speed Normal Speed 2 [m s^-1] Temperature Specification Static Temperature 315 [K] Tab Setting Value Boundary Data Boundary Type Inlet Location in2 Flow Specification Option Normal Speed Normal Speed 2 [m s^-1] Temperature Specification Static Temperature 285 [K] Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 39 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Creating the Outlet Boundary Definition Now that the second inlet boundary has been created, the same concepts can be applied to building the outlet boundary. 1. Create a new boundary named out with these settings: 2. Click Next. Moving to General Mode There are no further boundary conditions that need to be set. All 2D exterior regions that have not been assigned to a boundary condition are automatically assigned to the default boundary condition. Procedure 1. Set Operation to Enter General Mode and click Finish. The three boundary conditions are displayed in the viewer as sets of arrows at the boundary surfaces. Inlet boundary arrows are directed into the domain. Outlet boundary arrows are directed out of the domain. Setting Solver Control Solver Control parameters control aspects of the numerical solution generation process. While an upwind advection scheme is less accurate than other advection schemes, it is also more robust. This advection scheme is suitable for obtaining an initial set of results, but in general should not be used to obtain final accurate results. The time scale can be calculated automatically by the solver or set manually. TheAutomatic option tends to be conservative, leading to reliable, but often slow, convergence. It is often possible to accelerate convergence by applying a time scale factor or by choosing a manual value that is more aggressive than the Automatic option. In this tutorial, you will select a physical time scale, leading to convergence that is twice as fast as the Automatic option. Procedure 1. Click Solver Control . 2. On the Basic Settings tab, set Advection Scheme > Option to Upwind. 3. Set Convergence Control > Fluid Timescale Control > Timescale Control to Physical Timescale and set the physical timescale value to 2 [s]. 4. Click OK. Tab Setting Value Boundary Data Boundary Type Outlet Location out Flow Specification Option Average Static Pressure Relative Pressure 0 [Pa] Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Defining a Simulation in ANSYS CFX-Pre Page 40 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Writing the Solver (.def) File The simulation file, StaticMixer.cfx, contains the simulation definition in a format that can be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, and modify the simulation definition. The simulation file differs from the definition file in that it can be saved at any time while defining the simulation. Procedure 1. Click Write Solver File . The Write Solver File dialog box is displayed. 2. Set File name to StaticMixer.def. 3. Ensure that Start Solver Manager is selected from the drop down menu located in the top-right corner of the dialog box. 4. Click Save. 5. If you are notified the file already exists, click Overwrite. This file is provided in the tutorial directory and may exist in your tutorial folder if you have copied it there. 6. If prompted, click Yes or Save & Quit to save StaticMixer.cfx. The definition file (StaticMixer.def) and the simulation file (StaticMixer.cfx) are created. ANSYS CFX-Solver Manager automatically starts and the definition file is set in the Define Run dialog box. 7. Proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41). Playing the Session File and Starting ANSYS CFX-Solver Manager Note: This task is required only if you are starting here with the session file that was provided in the examples directory. If you have performed all the tasks in the previous steps, proceed directly to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 41). Events in ANSYS CFX-Pre can be recorded to a session file and then played back at a later date to drive ANSYS CFX-Pre. Session files have been created for each tutorial so that the problems can be set up rapidly in ANSYS CFX-Pre, if desired. Procedure 1. If required, launch ANSYS Workbench. 2. Click Empty Project. 3. Select File > Save or click Save . 4. Under File name, type: StaticMixer 5. Click Save. 6. Click Start CFX-Pre. 7. Select Session > Play Tutorial. 8. Select StaticMixer.pre. 9. Click Open. A definition file is written. 10. Click the CFX-Solver tab. 11. Select File > Define Run. 12. Under Definition File, click Browse . Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 43 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Viewing the Results in ANSYS CFX-Post When ANSYS CFX-Post starts, the viewer and Outline workspace are displayed. The viewer displays an outline of the geometry and other graphic objects. You can use the mouse or the toolbar icons to manipulate the view, exactly as in ANSYS CFX-Pre. Workflow Overview This tutorial describes the following workflow for viewing results in ANSYS CFX-Post: 1. Setting the Edge Angle for a Wireframe Object (p. 44) 2. Creating a Point for the Origin of the Streamline (p. 45) 3. Creating a Streamline Originating from a Point (p. 46) 4. Rearranging the Point (p. 47) 5. Configuring a Default Legend (p. 47) 6. Creating a Slice Plane (p. 48) 7. Defining Slice Plane Geometry (p. 49) 8. Configuring Slice Plane Views (p. 49) 9. Rendering Slice Planes (p. 50) 10. Coloring the Slice Plane (p. 51) 11. Moving the Slice Plane (p. 51) 12. Adding Contours (p. 52) 13. Working with Animations (p. 53) Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post Page 44 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Setting the Edge Angle for a Wireframe Object The outline of the geometry is called the wireframe or outline plot. By default, ANSYS CFX-Post displays only some of the surface mesh. This sometimes means that when you first load your results file, the geometry outline is not displayed clearly. You can control the amount of the surface mesh shown by editing the Wireframe object listed in the Outline. The check boxes next to each object name in the Outline control the visibility of each object. Currently only the Wireframe and Default Legend objects have visibility selected. The edge angle determines how much of the surface mesh is visible. If the angle between two adjacent faces is greater than the edge angle, then that edge is drawn. If the edge angle is set to 0°, the entire surface mesh is drawn. If the edge angle is large, then only the most significant corner edges of the geometry are drawn. For this geometry, a setting of approximately 15° lets you view the model location without displaying an excessive amount of the surface mesh. In this module you can also modify the zoom settings and view of the wireframe. Procedure 1. In the Outline, under User Locations and Plots, double-click Wireframe. Tip: While it is not necessary to change the view to set the angle, do so to explore the practical uses of this feature. 2. Right-click on a blank area anywhere in the viewer, select Predefined Camera from the shortcut menu and select Isometric View (Z up). 3. In the Wireframe details view, under Definition, click in the Edge Angle box. An embedded slider is displayed. 4. Type a value of 10 [degree]. 5. Click Apply to update the object with the new setting. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 45 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Notice that more surface mesh is displayed. 6. Drag the embedded slider to set the Edge Angle value to approximately 45 [degree]. 7. Click Apply to update the object with the new setting. Less of the outline of the geometry is displayed. 8. Type a value of 15 [degree]. 9. Click Apply to update the object with the new setting. 10. Right-click on a blank area anywhere in the viewer, select Predefined Camera from the shortcut menu and select View Towards -X. Creating a Point for the Origin of the Streamline A streamline is the path that a particle of zero mass would follow through the domain. Procedure 1. Select Insert > Location > Point from the main menu. You can also use the toolbars to create a variety of objects. Later modules and tutorials explore this further. 2. Click OK. This accepts the default name. 3. Under Definition, ensure that Method is set to XYZ. 4. Under Point, enter the following coordinates: -1, -1, 1. This is a point near the first inlet. 5. Click Apply. The point appears as a symbol in the viewer as a crosshair symbol. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post Page 48 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The default legend displays values for the last eligible plot that was opened in the details view. To maintain a legend definition during an ANSYS CFX-Post session, you can create a new legend by clicking Legend . Because there are many settings that can be customized for the legend, this module allows you the freedom to experiment with them. In the last steps you will set up a legend, based on the default legend, with a minor modification to the position. Tip: When editing values, you can restore the values that were present when you began editing by clicking Reset. To restore the factory-default values, click Default. Procedure 1. Double click Default Legend View 1. The Definition tab of the default legend is displayed. 2. Apply the following settings 3. Click Apply. The appearance and position of the legend changes based on the settings specified. 4. Modify various settings in Definition and click Apply after each change. 5. Select Appearance. 6. Modify a variety of settings in the Appearance and click Apply after each change. 7. Click Defaults. 8. Click Apply. 9. Under Outline, in User Locations and Plots, clear the check boxes for Point 1 and Streamline 1. Since both are no longer visible, the associated legend no longer appears. Creating a Slice Plane Defining a slice plane allows you to obtain a cross–section of the geometry. In ANSYS CFX-Post you often view results by coloring a graphic object. The graphic object could be an isosurface, a vector plot, or in this case, a plane. The object can be a fixed color or it can vary based on the value of a variable. You already have some objects defined by default (listed in the Outline). You can view results on the boundaries of the static mixer by coloring each boundary object by a variable. To view results within the geometry (that is, on non-default locators), you will create new objects. You can use the following methods to define a plane: • Three Points: creates a plane from three specified points. Tab Setting Value Definition Title Mode User Specified Title Streamline Temp. Horizontal (Selected) Location > Y Justification Bottom Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 49 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. • Point and Normal: defines a plane from one point on the plane and a normal vector to the plane. • YZ Plane, ZX Plane, and XY Plane: similar to Point and Normal, except that the normal is defined to be normal to the indicated plane. Procedure 1. From the main menu, select Insert > Location > Plane or click Location > Plane. 2. In the New Plane window, type: Slice 3. Click OK. The Geometry, Color, Render, and View tabs let you switch between settings. 4. Click the Geometry tab. Defining Slice Plane Geometry You need to choose the vector normal to the plane. You want the plane to lie in the x-y plane, hence its normal vector points along the z-axis. You can specify any vector that points in the z-direction, but you will choose the most obvious (0,0,1). Procedure 1. If required, under Geometry, expand Definition. 2. Under Method select Point and Normal. 3. Under Point enter 0,0,1. 4. Under Normal enter 0, 0,1. 5. Click Apply. Slice displays under User Locations and Plots. Rotate the view to see the plane. Configuring Slice Plane Views Depending on the view of the geometry, various objects may not appear because they fall in a 2D space that cannot be seen. Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up). Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post Page 50 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The slice is now visible in the viewer. 2. Click Zoom Box . 3. Click and drag a rectangular selection over the geometry. 4. Release the mouse button to zoom in on the selection. 5. Click Rotate . 6. Click and drag the mouse pointer down slightly to rotate the geometry towards you. 7. Select Isometric View (Z up) as described earlier. Rendering Slice Planes Render settings determine how the plane is drawn. Procedure 1. In the Details pane for Slice, select the Render tab. 2. Clear Draw Faces. 3. Select Draw Lines. 4. Under Draw Lines change Color Mode to User Specified. 5. Click the current color in Line Color to change to a different color. For a greater selection of colors, click the ellipsis to use the Select color dialog box. 6. Click Apply. 7. Click Zoom Box . 8. Zoom in on the geometry to view it in greater detail. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 53 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The graphic element faces are visible, producing a contour plot as shown. Working with Animations Animations build transitions between views for development of video files. Workflow Overview This tutorial follows the general workflow for creating a keyframe animation: 1. Showing the Animation Dialog Box (p. 53) 2. Creating the First Keyframe (p. 53) 3. Creating the Second Keyframe (p. 54) 4. Viewing the Animation (p. 55) 5. Modifying the Animation (p. 56) 6. Saving to MPEG (p. 57) Showing the Animation Dialog Box The Animation dialog box is used to define keyframes and to export to a video file. Procedure 1. Select Tools > Animation or click Animation . The Animation dialog box can be repositioned as required. Creating the First Keyframe Keyframes are required in order to produce an animation. You need to define the first viewer state, a second (and final) viewer state, and set the number of interpolated intermediate frames. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post Page 54 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up). 2. In the Outline, under User Locations and Plots, clear the visibility of Slice Contour and select the visibility of Slice. 3. Select Tools > Animation or click Animation . The Animation dialog box can be repositioned as required. 4. In the Animation dialog box, click New . A new keyframe named KeyframeNo1 is created. This represents the current image displayed in the viewer. Creating the Second Keyframe Keyframes are required in order to produce an animation. Procedure 1. In the Outline, under User Locations and Plots, double-click Slice. 2. On the Geometry tab, set Point coordinate values to (0,0,-1.99). 3. Click Apply. The slice plane moves to the bottom of the mixer. 4. In the Animation dialog box, click New . KeyframeNo2 is created and represents the image displayed in the Viewer. 5. Select KeyframeNo1. 6. Set # of Frames (located below the list of keyframes) to 20. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 55 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. This is the number of intermediate frames used when going from KeyframeNo1 to KeyframeNo2. This number is displayed in the Frames column for KeyframeNo1. 7. Press Enter. The Frame # column shows the frame in which each keyframe appears. KeyframeNo1 appears at frame 1 since it defines the start of the animation. KeyframeNo2 is at frame 22 since you have 20 intermediate frames (frames 2 to 21) in between KeyframeNo1 and KeyframeNo2. Viewing the Animation More keyframes could be added, but this animation has only two keyframes (which is the minimum possible). The controls previously greyed-out in the Animation dialog box are now available. The number of intermediate frames between keyframes is listed beside the keyframe having the lowest number of the pair. The number of keyframes listed beside the last keyframe is ignored. Procedure 1. Click Play the animation . The animation plays from frame 1 to frame 22. It plays relatively slowly because the slice plane must be updated for each frame. Tutorial 1a: Simulating Flow in a Static Mixer Using Workbench: Viewing the Results in ANSYS CFX-Post Page 58 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Page 59 ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS CFX Tutorials Tutorial 2: Flow in a Static Mixer (Refined Mesh) Introduction This tutorial includes: • Tutorial 2 Features (p. 60) • Overview of the Problem to Solve (p. 60) • Defining a Simulation using General Mode in ANSYS CFX-Pre (p. 61) • Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66) • Viewing the Results in ANSYS CFX-Post (p. 68) If this is the first tutorial you are working with, it is important to review the following topics before beginning: • Setting the Working Directory (p. 1) • Changing the Display Colors (p. 2) Unless you plan on running a session file, you should copy the sample files used in this tutorial from the installation folder for your software (<CFXROOT>/examples/) to your working directory. This prevents you from overwriting source files provided with your installation. If you plan to use a session file, please refer to Playing a Session File (p. 61). Sample files used by this tutorial are: • StaticMixerRefMesh.gtm • StaticMixerRef.pre • StaticMixer.def • StaticMixer_001.res Tutorial 2: Flow in a Static Mixer (Refined Mesh): Tutorial 2 Features Page 60 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorial 2 Features This tutorial addresses the following features of ANSYS CFX. In this tutorial you will learn about: • Using the General Mode of ANSYS CFX-Pre (this mode is used for more complex cases). • Rerunning a problem with a refined mesh. • Importing CCL to copy the definition of a different simulation into the current simulation. • Viewing the mesh with a Sphere volume locator and a Surface Plot. • Using a Plane Volume locator and the Mesh Calculator to analyze mesh quality. Overview of the Problem to Solve In this tutorial, you use a refined mesh to obtain a better solution to the Static Mixer problem created in Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode (p. 3). You establish a general workflow for analyzing the flow of fluid into and out of a mixer. This tutorial uses a specific problem to teach the general approach taken when working with an existing mesh. You start a new simulation in ANSYS CFX-Pre and import the refined mesh. This tutorial introduces General Mode—the mode used for most tutorials—in ANSYS CFX-Pre. The physics for this tutorial are the same as for Tutorial 1: Simulating Flow in a Static Mixer Using CFX in Standalone Mode (p. 3); therefore, you can import the physics settings used in that tutorial to save time. Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid Type General Fluid Domain Type Single Domain Turbulence Model k-Epsilon Heat Transfer Thermal Energy Boundary Conditions Inlet (Subsonic) Outlet (Subsonic) Wall: No-Slip Wall: Adiabatic Timestep Physical Time Scale ANSYS CFX-Post Plots Planevolume Slice Plane Spherevolume Other Viewing the Mesh Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 63 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Procedure 1. Select File > Import CCL. The Import CCL dialog box appears. 2. Under Import Method, select Append. Replace is useful if you have defined physics and want to update or replace them with newly imported physics. 3. Under File type, select CFX-Solver Files (*def *res). 4. Select StaticMixer.def created in Tutorial 1. If you did not work through Tutorial 1, you can copy this file from the examples directory. 5. Click Open. 6. Select the Outline tab. Tip: To select Outline you may need to click the navigation icons next to the tabs to move ‘forward’ or ‘backward’ through the various tabs. The tree view displays a summary of the current simulation in a tree structure. Some items may be recognized from Tutorial 1—for example the boundary condition objects in1, in2, and out. Viewing Domain Settings It is useful to review the options available in General Mode. Various domain settings can be set. These include: • General Options Specifies the location of the domain, coordinate frame settings and the fluids/solids that are present in the domain. You also reference pressure, buoyancy and whether the domain is stationary or rotating. Mesh motion can also be set. • Fluid Models Sets models that apply to the fluid(s) in the domain, such as heat transfer, turbulence, combustion, and radiation models. An option absent in Tutorial 1 is Turbulent Wall Functions, which is set to Scalable. Wall functions model the flow in the near-wall region. For the k-epsilon turbulence model, you should always use scalable wall functions. • Initialization Sets the initial conditions for the current domain only. This is generally used when multiple domains exist to allow setting different initial conditions in each domain, but can also be used to initialize single-domain simulations. Global initialization allows the specification of initial conditions for all domains that do not have domain-specific initialization. Procedure 1. On the Outline tree view, under Simulation, double-click Default Domain. The domain Default Domain is opened for editing. 2. Click General Options and review, but do not change, the current settings. 3. Click Fluid Models and review, but do not change, the current settings. 4. Click Initialization and review, but do not change, the current settings. 5. Click Close. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-Pre Page 64 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Viewing the Boundary Condition Setting For the k-epsilon turbulence model, you must specify the turbulent nature of the flow entering through the inlet boundary. For this simulation, the default setting of Medium (Intensity = 5%) is used. This is a sensible setting if you do not know the turbulence properties of the incoming flow. Procedure 1. Under Default Domain, double-click in1. 2. Click the Boundary Details tab and review the settings for Flow Regime, Mass and Momentum, Turbulence and Heat Transfer. 3. Click Close. Defining Solver Parameters Solver Control parameters control aspects of the numerical-solution generation process. In Tutorial 1 you set some solver control parameters, such as Advection Scheme and Timescale Control, while other parameters were set automatically by ANSYS CFX-Pre. In this tutorial, High Resolution is used for the advection scheme. This is more accurate than the Upwind Scheme used in Tutorial 1. You usually require a smaller timestep when using this model. You can also expect the solution to take a higher number of iterations to converge when using this model. Procedure 1. Select Insert > Solver > Solver Control from the main menu or click Solver Control . 2. Apply the following Basic Settings 3. Click Apply. 4. Click the Advanced Options tab. 5. Ensure that Global Dynamic Model Control is selected. 6. Click OK. Writing the Solver (.def) File Once all boundaries are created you move from ANSYS CFX-Pre into ANSYS CFX-Solver. Setting Value Advection Scheme > Option High Resolution Convergence Control > Max. Iterations* *. If your solution does not meet the convergence criteria after this number of timesteps, the ANSYS CFX-Solver will stop. 150 Convergence Control > Fluid Timescale Control > Timescale Control Physical Timescale Convergence Control > Fluid Timescale Control > Physical Timescale 0.5 [s] Tutorial 2: Flow in a Static Mixer (Refined Mesh): Defining a Simulation using General Mode in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 65 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The simulation file—StaticMixerRef.cfx—contains the simulation definition in a format that can be loaded by ANSYS CFX-Pre, allowing you to complete (if applicable), restore, and modify the simulation definition. The simulation file differs from the definition file in two important ways: • The simulation file can be saved at any time while defining the simulation. • The definition file is an encapsulated set of meshes and CCL defining a solver run, and is a subset of the data in the simulation file. Procedure 1. Click Write Solver File . The Write Solver File dialog box is displayed. 2. If required, set the path to your working directory. 3. Apply the following settings: 4. Ensure Start Solver Manager is selected and click Save. 5. If you are notified that the file already exists, click Overwrite. 6. If prompted, click Yes or Save & Quit to save StaticMixerRef.cfx. The definition file (StaticMixerRef.def) and the simulation file (StaticMixerRef.cfx) are created. ANSYS CFX-Solver Manager automatically starts and the definition file is set in the Definition File box of Define Run. 7. Proceed to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66). Playing the Session File and Starting ANSYS CFX-Solver Manager If you have performed all the tasks in the previous steps, proceed directly to Obtaining a Solution Using Interpolation with ANSYS CFX-Solver (p. 66). Two procedures are documented. Depending on your installation of ANSYS CFX follow either the standalone procedure or the ANSYS Workbench procedure. Procedure in Standalone 1. If required, launch ANSYS CFX-Pre. 2. Select Session > Play Tutorial. 3. Select StaticMixerRef.pre. 4. Click Open. A definition file is written. 5. Select File > Quit. 6. Launch ANSYS CFX-Solver Manager from CFX Launcher. 7. After ANSYS CFX-Solver starts, select File > Define Run. 8. Under Definition File, click Browse . 9. Select StaticMixerRef.def, located in the working directory. Setting Value File name StaticMixerRef.def Quit CFX–Pre* *. If using ANSYS CFX-Pre in Standalone Mode. (Selected) Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post Page 68 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. After a short pause, ANSYS CFX-Post starts. Viewing the Results in ANSYS CFX-Post In the following sections, you will explore the differences between the mesh and the results from this tutorial and tutorial 1. Creating a Slice Plane More information exists for use by ANSYS CFX-Post in this tutorial than in Tutorial 1 because the slice plane is more detailed. Once a new slice plane is created it can be compared with Tutorial 1. There are three noticeable differences between the two slice planes. • Around the edges of the mixer geometry there are several layers of narrow rectangles. This is the region where the mesh contains prismatic elements (which are created as inflation layers). The bulk of the geometry contains tetrahedral elements. • There are more lines on the plane than there were in Tutorial 1. This is because the slice plane intersects with more mesh elements. • The curves of the mixer are smoother than in Tutorial 1 because the finer mesh better represents the true geometry. Procedure 1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up). 2. From the main menu, select Insert > Location > Plane or under Location, click Plane. 3. In the Insert Plane dialog box, type Slice and click OK. The Geometry, Color, Render and View tabs let you switch between settings. 4. Apply the following settings 5. Click Apply. 6. Right-click a blank area in the viewer and select Predefined Camera > View Towards -Z. 7. Click Zoom Box . 8. Zoom in on the geometry to view it in greater detail. Tab Setting Value Geometry Domains Default Domain Definition > Method XY Plane Definition > Z 1 [m] Render Draw Faces (Cleared) Draw Lines (Selected) Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 69 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Compare the on-screen image with the equivalent picture from tutorial 1 (in the section Rendering Slice Planes (p. 22)). Coloring the Slice Plane Here, you will color the plane by temperature. Procedure 1. Apply the following settings 2. Click Apply. Loading Results from Tutorial 1 for Comparison In ANSYS CFX-Post, you may load multiple results files into the same instance for comparison. Procedure 1. To load the results file from Tutorial 1, select File > Load Results or click Load Results . 2. Be careful not to click Open until instructed to do so. In the Load Results File dialog box, select StaticMixer_001.res in the <CFXROOT>\examples directory or from your working directory if it has been copied. Tab Setting Value Color Mode* *. A mode setting of Constant would allow you to color the plane with a fixed color. Variable Variable Temperature Range Global Render Draw Faces (Selected) Draw Lines (Cleared) Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post Page 70 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 3. On the right side of the dialog box, there are two frames. Under Results file option, select Add to current results. 4. Select the Offset in Y direction check box. 5. Under Additional actions, ensure that the Clear user state before loading check box is cleared. 6. Click Open to load the results. In the tree view, there is now a second group of domains, meshes and boundary conditions with the heading StaticMixer_001. 7. Double-click the Wireframe object under User Locations and Plots. 8. In the Definition tab, set Edge Angle to 5 [degree]. 9. Click Apply. 10. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up). Both meshes are now displayed in a line along the Y axis. Notice that one mesh is of a higher resolution than the other. 11. Set Edge Angle to 30 [degree]. 12. Click Apply. Creating a Second Slice Plane Procedure 1. In the tree view, right-click the plane named Slice and select Duplicate. 2. Click OK to accept the default name Slice 1. 3. In the tree view, double-click the plane named Slice 1. 4. On the Geometry tab, set Domains to Default Domain 1. 5. On the Color tab, ensure that Range is set to Global. 6. Click Apply. 7. Double-click Slice and make sure that Range is set to Global. Comparing Slice Planes using Multiple Views Procedure 1. Select the option with the two vertical rectangles. Notice that the Viewer now has two separate views. The visibility status of each object is maintained separately for each view or figure that can be displayed in a given viewport. This allows some planes to be shown while others are hidden. Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 73 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 9. Click Apply. Viewing the Surface Mesh on the Mixer Body Procedure 1. Double-click the Default Domain Default object. 2. Apply the following settings 3. Click Apply. Viewing the Layers of Inflated Elements on a Plane You will see the layers of inflated elements on the wall of the main body of the mixer. Within the body of the mixer, there will be many lines that are drawn wherever the face of a mesh element intersects the slice plane. Procedure 1. From the main menu, select Insert > Location > Plane or under Location, click Plane. 2. In the Insert Plane dialog box, type Slice 2 and click OK. 3. Apply the following settings 4. Click Apply. 5. Turn off the visibility of all objects except Slice 2. 6. To see the plane clearly, right-click in the viewer and select Predefined Camera > View Towards -X. Viewing the Mesh Statistics You can use the Report Viewer to check the quality of your mesh. For example, you can load a .def file into ANSYS CFX-Post and check the mesh quality before running the .def file in the solver. Tab Setting Value Geometry Definition > Point -0.22, 0.4, -1.85 Definition > Radius 0.206 [m] Color Color Orange Tab Setting Value Render Draw Faces (Selected) Draw Lines (Selected) Line Width 2 Tab Setting Value Geometry Definition > Method YZ Plane Definition > X 0 [m] Render Draw Faces (Cleared) Draw Lines (Selected) Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post Page 74 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Procedure 1. Click the Report Viewer tab (located below the viewer window). A report appears. Look at the table shown in the “Mesh Report” section. 2. Double-click Report > Mesh Report in the Outline tree view. 3. In the Mesh Report details view, select Statistics > Maximum Face Angle. 4. Click Refresh Preview. Note that a new table, showing the maximum face angle for all elements in the mesh, has been added to the “Mesh Report” section of the report. The maximum face angle is reported as 148.95°. As a result of generating this mesh statistic for the report, a new variable, Maximum Face Angle, has been created and stored at every node. This variable will be used in the next section. Viewing the Mesh Elements with Largest Face Angle In this section, you will visualize the mesh elements that have a Maximum Face Angle value greater than 140°. Procedure 1. Click the 3D Viewer tab (located below the viewer window). 2. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up). 3. In the Outline tree view, select the visibility check box of Wireframe. 4. From the main menu, select Insert > Location > Volume or under Location, click Volume. 5. In the Insert Volume dialog box, type Max Face Angle Volume and click OK. 6. Apply the following settings 7. Click Apply. The volume object appears in the viewer. Tab Setting Value Geometry Definition > Method Isovolume Definition > Variable Maximum Face Angle* *. Select Maximum Face Angle from the larger list of variables available by clicking to the right of the Variable box. Definition > Mode Above Value Definition > Value 140 [degree] Inclusive† †. This includes any elements that have at least one node with a variable value greater than or equal to the given value. (Selected) Tutorial 2: Flow in a Static Mixer (Refined Mesh): Viewing the Results in ANSYS CFX-Post ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 75 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Viewing the Mesh Elements with Largest Face Angle Using a Point Next, you will create a point object to show a node that has the maximum value of Maximum Face Angle. The point object will be represented by a 3D yellow crosshair symbol. In order to avoid obscuring the point object with the volume object, you may want to turn off the visibility of the latter. Procedure 1. From the main menu, select Insert > Location > Point or under Location, click Point. 2. Click OK to use the default name. 3. Apply the following settings 4. Click Apply. Quitting ANSYS CFX-Post Two procedures are documented. Depending on your installation of ANSYS CFX, follow either the standalone procedure or the ANSYS Workbench procedure. Procedure in Standalone 1. When you are finished, select File > Quit to exit ANSYS CFX-Post. 2. Click Quit if prompted to save. Procedure in Workbench 1. When you are finished, select File > Close to close the current file. 2. Click Close if prompted to save. 3. Return to the Project page. Select File > Close Project. 4. Select No, then close Workbench. Tab Setting Value Geometry Definition > Method Variable Maximum Definition > Location Default Domain Definition > Variable Maximum Face Angle Symbol Symbol Size 2 Tutorial 3: Flow in a Process Injection Mixing Pipe: Tutorial 3 Features Page 78 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorial 3 Features This tutorial addresses the following features of ANSYS CFX. In this tutorial you will learn about: • Applying a profile boundary condition using data stored in a file. • Visualizing the velocity on a boundary in ANSYS CFX-Pre. • Using the CFX Expression Language (CEL) to describe temperature dependent fluid properties in ANSYS CFX-Pre. • Using the k-epsilon turbulence model. • Using streamlines in ANSYS CFX-Post to track flow through the domain. Overview of the Problem to Solve In this tutorial, you establish a general workflow for analyzing the flow of fluid into and out of an injection pipe. This tutorial is important because it uses a specific problem to teach the general approach taken when working with an existing mesh. Component Feature Details ANSYS CFX-Pre User Mode General Mode Simulation Type Steady State Fluid Type General Fluid Domain Type Single Domain Turbulence Model k-Epsilon Heat Transfer Thermal Energy Boundary Conditions Boundary Profile visualization Inlet (Profile) Inlet (Subsonic) Outlet (Subsonic) Wall: No-Slip Wall: Adiabatic CEL (CFX Expression Language) Timestep Physical Time Scale ANSYS CFX-Post Plots default Locators Outline Plot (Wireframe) Slice Plane Streamline Other Changing the Color Range Expression Details View Legend Viewing the Mesh Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 79 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The injection mixing pipe, common in the process industry, is composed of two pipes: one with a larger diameter than the other. Analyzing and optimizing the mixing process is often critical for many chemical processes. CFD is useful not only in identifying problem areas (where mixing is poor), but also in testing new designs before they are implemented. The geometry for this example consists of a circular pipe of diameter 1.0 m with a 90° bend, and a smaller pipe of diameter 0.3 m which joins with the main pipe at an oblique angle. Defining a Simulation using General Mode in ANSYS CFX-Pre After having completed meshing, ANSYS CFX-Pre is used as a consistent and intuitive interface for the definition of complex CFD problems. Playing a Session File If you wish to skip past these instructions, and have ANSYS CFX-Pre set up the simulation automatically, you can select Session > Play Tutorial from the menu in ANSYS CFX-Pre, then run the appropriate session file. For details, see Playing the Session File and Starting ANSYS CFX-Solver Manager (p. 87). After you have played the session file, proceed to Obtaining a Solution Using ANSYS CFX-Solver Manager (p. 87). Workflow Overview This section provides a brief summary of the topics to follow as a general workflow: 1. Creating a New Simulation (p. 80) 2. Importing a Mesh (p. 80) 3. Setting Temperature-Dependent Material Properties (p. 81) 4. Plotting an Expression (p. 82) Figure 1 Injection Mixing Pipe φ=1.0 m φ=0.3 m 5.0 m/s 315.0 K 0.5 m/s 285.0 K Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre Page 80 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 5. Evaluating an Expression (p. 82) 6. Modify Material Properties (p. 82) 7. Creating the Domain (p. 82) 8. Creating the Side Inlet Boundary Conditions (p. 83) 9. Creating the Main Inlet Boundary Conditions (p. 84) 10. Creating the Main Outlet Boundary Condition (p. 85) 11. Setting Initial Values (p. 85) 12. Setting Solver Control (p. 85) 13. Writing the Solver (.def) File (p. 86) Creating a New Simulation Before importing and working with a mesh, a simulation needs to be started using General Mode. Note: Two procedures are documented. Depending on your installation of ANSYS CFX follow either the Standalone procedure or the Workbench procedure. Procedure in Standalone 1. If required, launch ANSYS CFX-Pre. 2. Select File > New Simulation. 3. Ensure General is selected and click OK. 4. Select File > Save Simulation As. 5. Under File name, type InjectMixer. 6. Click Save. 7. Proceed to Importing a Mesh (p. 80). Procedure in Workbench 1. If required, launch ANSYS Workbench. 2. Click Empty Project. The Project page will appear displaying an unsaved project. 3. Select File > Save or click Save . 4. If required, set the path location to your working folder. 5. Under File name, type InjectMixer. 6. Click Save. 7. Click Start CFX-Pre under Advanced CFD on the left hand task bar. 8. Select File > New Simulation. 9. Click General in the New Simulation File window and then click OK. 10. Select File > Save Simulation As. 11. Under File name, type InjectMixer. 12. Click Save. Importing a Mesh An assembly is a group of mesh regions that are topologically connected. Each assembly can contain only one mesh, but multiple assemblies are permitted. Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 83 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Both General Options and Fluid Models are changed in this module. The Initialization tab is for setting domain-specific initial conditions, which are not used in this tutorial. Instead, global initialization is used to set the starting conditions. Procedure 1. Select Insert > Domain from the main menu or click Domain . 2. In the Insert Domain dialog box, type InjectMixer. 3. Click OK. 4. Apply the following settings 5. Click Fluid Models. 6. Apply the following settings 7. Click OK. Creating the Side Inlet Boundary Conditions The side inlet boundary condition needs to be defined. Procedure 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition . 2. Set Name to side inlet. 3. Click OK. 4. Apply the following settings 5. Click OK. Tab Setting Value General Options Basic Settings > Location B1.P3 Basic Settings > Fluids List Water Domain Models > Pressure > Reference Pressure 0 [atm] Setting Value Heat Transfer > Option Thermal Energy Tab Setting Value Basic Settings Boundary Type Inlet Location side inlet Boundary Details Mass and Momentum > Option Normal Speed Normal Speed 5 [m s^-1] Heat Transfer > Option Static Temperature Static Temperature 315 [K] Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre Page 84 ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Creating the Main Inlet Boundary Conditions The main inlet boundary condition needs to be defined. This inlet is defined using a velocity profile found in the example directory. Profile data needs to be initialized before the boundary condition can be created. You will create a plot showing the velocity profile data, marked by higher velocities near the center of the inlet, and lower velocities near the inlet walls. Procedure 1. Select Tools > Initialize Profile Data. 2. Under Data File, click Browse . 3. From your working directory, select InjectMixer_velocity_profile.csv. 4. Click Open. 5. Click OK. The profile data is read into memory. 6. Select Insert > Boundary Condition from the main menu or click Boundary Condition . 7. Set name Name to main inlet. 8. Click OK. 9. Apply the following settings 10. Click Generate Values. This causes the profile values of U, V, W to be applied at the nodes on the main inlet boundary, and U, V, W entries to be made in Boundary Details. To later modify the velocity values at the main inlet and reset values to those read from the BC Profile file, revisit Basic Settings for this boundary condition and click Generate Values. 11. Apply the following settings 12. Click OK. Tab Setting Value Basic Settings Boundary Type Inlet Location main inlet Profile Boundary Conditions > Use Profile Data (Selected) Profile Boundary Setup > Profile Name main inlet Tab Setting Value Boundary Details Flow Regime > Option Subsonic Turbulence > Option Medium (Intensity = 5%) Heat Transfer > Option Static Temperature Static Temperature 285 [K] Plot Options Boundary Contour (Selected) Profile Variable W Tutorial 3: Flow in a Process Injection Mixing Pipe: Defining a Simulation using General Mode in ANSYS CFX-Pre ANSYS CFX Tutorials. ANSYS CFX Release 11.0. © 1996-2006 ANSYS Europe, Ltd. All rights reserved. Page 85 Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 13. Zoom into the main inlet to view the inlet velocity contour. Creating the Main Outlet Boundary Condition In this module you create the outlet boundary condition. All other surfaces which have not been explicitly assigned a boundary condition will remain in the InjectMixer Default object, which is shown in the tree view. This boundary condition uses a No-Slip Adiabatic Wall by default. Procedure 1. Select Insert > Boundary Condition from the main menu or click Boundary Condition . 2. Set Name to outlet. 3. Click OK. 4. Apply the following settings 5. Click OK. Setting Initial Values Procedure 1. Click Global Initialization . 2. Select Turbulence Eddy Dissipation. 3. Click OK. Setting Solver Control Procedure 1. Click Solver Control . 2. Apply the following settings Tab Setting Value Basic Settings Boundary Type Outlet Location outlet Boundary Details Flow Regime > Option Subsonic Mass and Momentum > Option Average Static Pressure Relative Pressure 0 [Pa]