Auto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial

Size: px
Start display at page:

Download "Auto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial"

Transcription

1 Auto Injector Syringe A Fluent Dynamic Mesh 1DOF Tutorial ANSYS, Inc. June 26, 2015

2 Prerequisites This tutorial is written with the assumption that You have attended the Introduction to ANSYS Fluent training course including Design Modeler, Meshing, Fluent and CFD-Post. You are familiar with basic geometry creation/import into ANSYS Design Modeler and operations to split geometry. You are familiar with assigning size functions and mesh generation in ANSYS Meshing. You are familiar with the ANSYS Fluent navigation pane and menu structure. The focus of the current tutorial is on the auto-injector application and not on the mechanics of the setup. Some steps in the setup and solution procedure will not be shown explicitly. Workbench project is attached (note that the included project was saved in R16.0, the current release version of the product). The UDF and this presentation are included in the user_files folder in the Workbench project ANSYS, Inc. June 26, 2015

3 Problem Description Axisymmetric Auto-injector Outlet Plunger with virtual spring Barrel Axis Wall Needle Wall Skin (Porous Zone) Needle Tip The 2D geometry is created in Design modeler with appropriate dimensions. The geometry is decomposed to allow hex meshing ANSYS, Inc. June 26, 2015

4 Mesh 4 elements across the cross section of the needle Spacing of 5e-4m along the syringe barrel Needle penetrates into the skin. Needle zone is separated from skin by a wall/wall-shadow in Fluent ANSYS, Inc. June 26, 2015

5 Named Selections Labels on the left ANSYS, Inc. June 26, 2015

6 Fluent General Settings o This is a transient problem o The flow is laminar o No other special models are enabled o Enable UDS transport Define > User Defined > Scalars. UDS will allow tracking of convective and diffusive transport of drug into skin ANSYS, Inc. June 26, 2015

7 Material Properties o Create Water material o Enable compressible liquid property for the water. This helps numerically stabilize pressure spikes that can happen when plunger moves and helps convergence. o Enter appropriate diffusion coefficient of scalar in liquid o Set the diffusion coefficient to zero if convective transport dominates ANSYS, Inc. June 26, 2015

8 Porous Zone Settings for Skin o Fluid resistance in the skin depth direction is higher than along skin direction. Measured data can be entered for more accurate results ANSYS, Inc. June 26, 2015

9 Solution Settings (Fluent Defaults) Second-order discretization can improve the accuracy of the solution ANSYS, Inc. June 26, 2015

10 Setting Monitors to Track Solution o Surface monitors can be created to track mass flow rate of drug through fluid outlet, plunger location etc ANSYS, Inc. June 26, 2015

11 Writing Backup and Solution Files Enable solution backup Write CFD-Post files for later processing ANSYS, Inc. June 26, 2015

12 Compiling and Hooking the UDF o Plunger motion is defined via User Define Function (UDF) called rigid_body.c. The UDF has two functions defined: o Fixed plunger motion o Plunger motion controlled by spring and fluid forces o A C-compiler is needed to compile the UDF (see Customer Portal for details) ANSYS, Inc. June 26, 2015

13 Initializing the Solution o Initialize the solution with quiescent conditions o Patch the User Scalar (UDS) representing the drug into the barrel and needle ANSYS, Inc. June 26, 2015

14 Dynamic Mesh Settings o o o o o So far we have described the general settings for the application The most critical part of this application is setting up the dynamic mesh algorithm to track the plunger motion The following section outlines the settings specific to three situations: (a) prescribed motion (b) spring activated fluid controlled motion of the plunger using Fluent 6DOF approach with solution stabilization and implicit update (c) spring activated fluid controlled motion of the plunger using explicit UDF approach (see APPENDIX) A Smoothing algorithm is used to modify the mesh in the barrel volume as the plunger moves For more details, please review material related to Moving Dynamic Mesh (MDM) algorithm on the Customer Portal ANSYS, Inc. June 26, 2015

15 ANSYS, Inc. June 26, 2015 Fixed Plunger Movement

16 Dynamic Mesh Settings Diffusion based smoothing is activated, this parameter controls mesh distribution as plunger moves ANSYS, Inc. June 26, 2015 Define barrel_wall_stationary as a stationary zone

17 Dynamic Mesh Settings Hook the function plunger_fixed to the plunger_wall boundary zone under motion attributes tab. Explicitly define the skin and needle as stationary ANSYS, Inc. June 26, 2015

18 Dynamic Mesh Settings Deforming zones are defined as a plane to make sure they do not distort as plunger moves ANSYS, Inc. June 26, 2015

19 Explanation of the UDF Pre-defined plunger velocity Setting x-direction plunger velocity to the pre-defined fixed value DEFINE_CG_MOTION is the Fluent macro for defining motion of rigid bodies. For more details, please refer the UDF manual on the ANSYS customer portal ANSYS, Inc. June 26, 2015

20 Preview the mesh motion o Mesh motion preview helps ensure that the re-meshing algorithm works without problems without actually solving for the flow. o Pre-viewing mesh motion is a good practice while setting up any type of moving boundary problem ANSYS, Inc. June 26, 2015

21 Running the Calculation o Time step size is based on plunger speed of ~ m/s and the minimum mesh element size in the Layering region ~ 5e-4 m o Time step size of 0.05 s allows the plunger to move a distance equal to about ½ the mesh element size in one time step o Maximum number of iterations per time step set to ensure convergence in every step. The problem typically converges in far less than the set number of iterations ANSYS, Inc. June 26, 2015

22 Calculation Monitors ANSYS, Inc. June 26, 2015

23 Drug Injection into Skin (Post processing is done on the saved solution files in CFD-Post) ANSYS, Inc. June 26, 2015

24 ANSYS, Inc. June 26, 2015 Plunger Motion Controlled by Spring and Opposing Fluid Force (using inbuilt 6DOF model)

25 6DOF UDF Explained o 6DOF model in Fluent calculates fluid forces on plunger and calculates plunger velocity Mass properties of plunger Restrict plunger motion in all directions except x Spring Compression Spring Force applied as external force ANSYS, Inc. June 26, 2015

26 Activating 6DOF Model in Fluent ANSYS, Inc. June 26, 2015 o Implicit update allows us to use much higher time steps. Implicit update adjusts the position of the moving boundary several times within a time step as controlled by the update interval. See next few slides for solution stabilization

27 Hook the 6DOF UDF to Control Plunger Motion Hook the 6DOF UDF Indicate that this is a 6DOF object ANSYS, Inc. June 26, 2015

28 Instability Mechanism For a Schematic 6DOF Case Initialized Fluid Solution First Coupling iteration Fluid P Forces passed to Plunger Displacements passed to Fluid Fluid P Initial pressure on plunger The plunger moves due fluid pressure Pressure decreases in Fluid due to increase in volume (Plunger has moved too much) Forces passed to Plunger Second Coupling iteration... Fluid P Displacements passed to Fluid Plunger Pressure in Fluid increases more due to reduced volume The plunger moves in the opposite direction ANSYS, Inc. June 26, 2015

29 Solution Stabilization Solution Stabilization is available in Fluent to stabilize these types of cases. The option can be found in the Dynamic Mesh settings on the Solver Options panel The solution stabilization changes a coefficient used for the pressure update at the current non-linear iteration. This coefficient changes the pressure convergence behavior close to the moving wall. It does however not change the converged solution For the volume-based option, the stabilization is a function of the cell volumes attached to the selected System Coupling/6DOF region For the coefficient-based option, the stabilization is a function of the linear matrix coefficients in the continuity equation The following text command activates stabilization for 6DOF cases: (rpsetvar 'dynamesh/sdof-solver-options? #t) ANSYS, Inc. June 26, 2015

30 Solution Stabilization From a physical point of view, the stabilization slows down the pressure response in Fluent at the deforming wall This means that the pressure doesn t increase/decrease as fast in Fluent when a new displacement is received This damped pressure response allows us to move towards the equilibrium, between fluid force and structural deformation, in a controlled way, rather than oscillating around it The stabilization has no effect on converged results A higher Scale Factor results in more stabilization (i.e. a slower pressure response) The appropriate value is case specific e.g. for the volume-based method Scale Factors between 0.01 and 1e5 have been used If you have small cell volumes you will need a larger Scale Factor How do we find the correct Scale Factor? ANSYS, Inc. June 26, 2015

31 Solution Stabilization Each graph illustrates pressure convergence on the FSI surface within 1 time step using different scale factors for the volume-based stabilization Scale Factor = 0 Baseline, case diverges Scale Factor = 2 Does not diverge but still oscillates too much around equilibrium (converged value) Scale Factor = 10 Very stable but over-damped. Not fully converged after 7 implicit mesh updates Scale Factor = 3 Good response. Well converged after 5 implicit mesh updates ANSYS, Inc. June 26, 2015

32 Activate Solution Stabilization for Plunger ANSYS, Inc. June 26, 2015

33 Case Modification o Case modification strategy is used to ramp up the time step size and ramp down the stabilization factor as the solution runs. o See next slide for more details of this panel ANSYS, Inc. June 26, 2015

34 Case Modification Run 2 time steps with time step size of (stabilization factor = 0.005) Run 2 time steps with time step size of 0.01 (stabilization factor = 0.005) ANSYS, Inc. June 26, 2015 Run 1500 time steps with solution stabilization factor reduced to (time step = 0.01 s)

35 Initialize and Run Calculation o Initialization is performed as discussed in the fixed plunger movement case. o Calculation is started with an initial time step of 5e-5 o Calculation activities are programmed to ramp up the time step as discussed in previous slides. o Programmed calculation activities also control the overall length of simulation. o Solution typically converges every time step long before the maximum specified iterations/ time step is reached ANSYS, Inc. June 26, 2015

36 Solution Monitors ANSYS, Inc. June 26, 2015

37 Drug Distribution Contours ANSYS, Inc. June 26, 2015

38 APPENDIX-A Plunger Motion Controlled by Spring and Opposing Fluid Force (explicit 1DOF UDF) ANSYS, Inc. June 26, 2015

39 UDF for Flow Controlled Motion Explained o Fluid forces calculated using appropriate macro o Plunger velocity calculated each time-step using: V new = Vold + F m t where F is the total force including the spring force and m is the mass of the plunger o In addition to fluid forces, plunger motion is controlled by a spring. Spring stiffness, spring length, and spring start position are inputs to the UDF as shown below. o Motion is stopped when the plunger reaches the maximum allowable displacement ANSYS, Inc. June 26, 2015

40 UDF explained - 2 Fluent Macro to control rigid body motion Write data to file Stop plunger motion ANSYS, Inc. June 26, 2015

41 UDF Explained - 3 Macro to compute fluid forces Spring displacement Spring force dv = dt * force / mass V new = V old + dv Total force = externally applied force + spring force + fluid force Apply calculated velocity as new velocity ANSYS, Inc. June 26, 2015

42 Hooking Spring driven plunger function in the Dynamic mesh panel o No other changes ANSYS, Inc. June 26, 2015

43 Initialize and Run the Calculation o o Time step size is based on some trial and error. 1e-5 is found to be stable for this problem. Maximum number of iterations per time step set to ensure convergence in every step. The problem typically converges in far less than the set number of iterations. o Note that this section with the explicitly written UDF is included for completeness. The inbuilt 6DOF model in Fluent performs the same calculation as a black box. There are also some additional stabilization features that can be activated to speed up calculation when using the 6DOF model. See 6DOF section for details ANSYS, Inc. June 26, 2015

Simulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial

Simulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial Simulating Sinkage & Trim for Planing Boat Hulls A Fluent Dynamic Mesh 6DOF Tutorial 1 Introduction Workshop Description This workshop describes how to perform a transient 2DOF simulation of a planing

More information

Use 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution.

Use 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution. Introduction The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a moving deforming mesh (MDM) case along with the six degree of freedom (6DOF) solver and

More information

Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing

Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Introduction The purpose of this tutorial is to demonstrate how to simulate a ball check valve with small displacement

More information

Calculate a solution using the pressure-based coupled solver.

Calculate a solution using the pressure-based coupled solver. Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings

More information

This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following:

This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Tutorial 22. Modeling Solidification Introduction This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Define a

More information

Tutorial: Hydrodynamics of Bubble Column Reactors

Tutorial: Hydrodynamics of Bubble Column Reactors Tutorial: Introduction The purpose of this tutorial is to provide guidelines and recommendations for solving a gas-liquid bubble column problem using the multiphase mixture model, including advice on solver

More information

Using the Eulerian Multiphase Model for Granular Flow

Using the Eulerian Multiphase Model for Granular Flow Tutorial 21. Using the Eulerian Multiphase Model for Granular Flow Introduction Mixing tanks are used to maintain solid particles or droplets of heavy fluids in suspension. Mixing may be required to enhance

More information

The purpose of this tutorial is to illustrate how to set up and solve a problem using the. Moving Deforming Mesh (MDM) using the layering algorithm.

The purpose of this tutorial is to illustrate how to set up and solve a problem using the. Moving Deforming Mesh (MDM) using the layering algorithm. Tutorial: Introduction The purpose of this tutorial is to illustrate how to set up and solve a problem using the following two features in FLUENT. Moving Deforming Mesh (MDM) using the layering algorithm.

More information

Using Multiple Rotating Reference Frames

Using Multiple Rotating Reference Frames Tutorial 10. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive

More information

Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling

Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling Tutorial: Modeling Domains with Embedded Reference Frames: Part 2 Sliding Mesh Modeling Introduction The motion of rotating components is often complicated by the fact that the rotational axis about which

More information

Shape optimisation using breakthrough technologies

Shape optimisation using breakthrough technologies Shape optimisation using breakthrough technologies Compiled by Mike Slack Ansys Technical Services 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Introduction Shape optimisation technologies

More information

OpenFOAM and Third Party Structural Solver for Fluid Structure Interaction Simulations

OpenFOAM and Third Party Structural Solver for Fluid Structure Interaction Simulations OpenFOAM and Third Party Structural Solver for Fluid Structure Interaction Simulations Robert L. Campbell rlc138@arl.psu.edu Fluids and Structural Mechanics Office Applied Research Laboratory The Pennsylvania

More information

Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model

Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model Introduction The purpose of this tutorial is to demonstrate setup and solution procedure of liquid chemical

More information

Simulation of Laminar Pipe Flows

Simulation of Laminar Pipe Flows Simulation of Laminar Pipe Flows 57:020 Mechanics of Fluids and Transport Processes CFD PRELAB 1 By Timur Dogan, Michael Conger, Maysam Mousaviraad, Tao Xing and Fred Stern IIHR-Hydroscience & Engineering

More information

Modeling Flow Through Porous Media

Modeling Flow Through Porous Media Tutorial 7. Modeling Flow Through Porous Media Introduction Many industrial applications involve the modeling of flow through porous media, such as filters, catalyst beds, and packing. This tutorial illustrates

More information

Appendix: To be performed during the lab session

Appendix: To be performed during the lab session Appendix: To be performed during the lab session Flow over a Cylinder Two Dimensional Case Using ANSYS Workbench Simple Mesh Latest revision: September 18, 2014 The primary objective of this Tutorial is

More information

The Level Set Method THE LEVEL SET METHOD THE LEVEL SET METHOD 203

The Level Set Method THE LEVEL SET METHOD THE LEVEL SET METHOD 203 The Level Set Method Fluid flow with moving interfaces or boundaries occur in a number of different applications, such as fluid-structure interaction, multiphase flows, and flexible membranes moving in

More information

Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications. Laz Foley, ANSYS Inc.

Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications. Laz Foley, ANSYS Inc. Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications Laz Foley, ANSYS Inc. Outline FSI Classifications FSI Solutions FSI Modeling Approaches ANSYS Workbench for FSI System

More information

Solution Recording and Playback: Vortex Shedding

Solution Recording and Playback: Vortex Shedding STAR-CCM+ User Guide 6663 Solution Recording and Playback: Vortex Shedding This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.

More information

Using Multiple Rotating Reference Frames

Using Multiple Rotating Reference Frames Tutorial 9. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive

More information

Compressible Flow in a Nozzle

Compressible Flow in a Nozzle SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a

More information

Mesh Morphing and the Adjoint Solver in ANSYS R14.0. Simon Pereira Laz Foley

Mesh Morphing and the Adjoint Solver in ANSYS R14.0. Simon Pereira Laz Foley Mesh Morphing and the Adjoint Solver in ANSYS R14.0 Simon Pereira Laz Foley 1 Agenda Fluent Morphing-Optimization Feature RBF Morph with ANSYS DesignXplorer Adjoint Solver What does an adjoint solver do,

More information

Using a Single Rotating Reference Frame

Using a Single Rotating Reference Frame Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is

More information

Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders

Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.

More information

Tutorial: Riser Simulation Using Dense Discrete Phase Model

Tutorial: Riser Simulation Using Dense Discrete Phase Model Introduction The purpose of this tutorial is to demonstrate the setup of a dense discrete phase model (DDPM) with the example of 2D riser. DDPM is used for the secondary phase that has a particle size

More information

Supersonic Flow Over a Wedge

Supersonic Flow Over a Wedge SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 2 Supersonic Flow Over a Wedge Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification A uniform supersonic stream encounters a wedge

More information

Using the Discrete Ordinates Radiation Model

Using the Discrete Ordinates Radiation Model Tutorial 6. Using the Discrete Ordinates Radiation Model Introduction This tutorial illustrates the set up and solution of flow and thermal modelling of a headlamp. The discrete ordinates (DO) radiation

More information

Coupled Simulation of Flow and Body Motion Using Overset Grids. Eberhard Schreck & Milovan Perić

Coupled Simulation of Flow and Body Motion Using Overset Grids. Eberhard Schreck & Milovan Perić Coupled Simulation of Flow and Body Motion Using Overset Grids Eberhard Schreck & Milovan Perić Contents Dynamic Fluid-Body Interaction (DFBI) model in STAR-CCM+ Overset grids method in STAR-CCM+ Advantages

More information

Tutorial 2. Modeling Periodic Flow and Heat Transfer

Tutorial 2. Modeling Periodic Flow and Heat Transfer Tutorial 2. Modeling Periodic Flow and Heat Transfer Introduction: Many industrial applications, such as steam generation in a boiler or air cooling in the coil of an air conditioner, can be modeled as

More information

Tutorial 17. Using the Mixture and Eulerian Multiphase Models

Tutorial 17. Using the Mixture and Eulerian Multiphase Models Tutorial 17. Using the Mixture and Eulerian Multiphase Models Introduction: This tutorial examines the flow of water and air in a tee junction. First you will solve the problem using the less computationally-intensive

More information

Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing

Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,

More information

Problem description. The FCBI-C element is used in the fluid part of the model.

Problem description. The FCBI-C element is used in the fluid part of the model. Problem description This tutorial illustrates the use of ADINA for analyzing the fluid-structure interaction (FSI) behavior of a flexible splitter behind a 2D cylinder and the surrounding fluid in a channel.

More information

Simulation and Validation of Turbulent Pipe Flows

Simulation and Validation of Turbulent Pipe Flows Simulation and Validation of Turbulent Pipe Flows ENGR:2510 Mechanics of Fluids and Transport Processes CFD LAB 1 (ANSYS 17.1; Last Updated: Oct. 10, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim,

More information

Modeling Evaporating Liquid Spray

Modeling Evaporating Liquid Spray Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the

More information

Simulation of Flow Development in a Pipe

Simulation of Flow Development in a Pipe Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common

More information

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they

More information

Flow in an Intake Manifold

Flow in an Intake Manifold Tutorial 2. Flow in an Intake Manifold Introduction The purpose of this tutorial is to model turbulent flow in a simple intake manifold geometry. An intake manifold is a system of passages which carry

More information

RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent

RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order

More information

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to

More information

Cold Flow Simulation Inside an SI Engine

Cold Flow Simulation Inside an SI Engine Tutorial 12. Cold Flow Simulation Inside an SI Engine Introduction The purpose of this tutorial is to illustrate the case setup and solution of the two dimensional, four stroke spark ignition (SI) engine

More information

Tutorial: Heat and Mass Transfer with the Mixture Model

Tutorial: Heat and Mass Transfer with the Mixture Model Tutorial: Heat and Mass Transfer with the Mixture Model Purpose The purpose of this tutorial is to demonstrate the use of mixture model in FLUENT 6.0 to solve a mixture multiphase problem involving heat

More information

Lecture 6 Static Data Transfers. Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent Release. Release 14.5

Lecture 6 Static Data Transfers. Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent Release. Release 14.5 Lecture 6 Static Data Transfers 14. 5 Release Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent 1 2011 ANSYS, Inc. January 4, 2013 Outline Direct Project Schematic Connections Details on

More information

Verification of Laminar and Validation of Turbulent Pipe Flows

Verification of Laminar and Validation of Turbulent Pipe Flows 1 Verification of Laminar and Validation of Turbulent Pipe Flows 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 1 (ANSYS 18.1; Last Updated: Aug. 1, 2017) By Timur Dogan, Michael Conger, Dong-Hwan

More information

Marine Hydrodynamics Solver in OpenFOAM

Marine Hydrodynamics Solver in OpenFOAM Marine Hydrodynamics Solver in OpenFOAM p. 1/14 Marine Hydrodynamics Solver in OpenFOAM Hrvoje Jasak and Henrik Rusche h.jasak@wikki.co.uk, h.rusche@wikki.co.uk Wikki, United Kingdom and Germany 4 December

More information

2008 International ANSYS Conference

2008 International ANSYS Conference 2008 International ANSYS Conference FEM AND FSI SIMULATIONS OF IMPACT LOADS ON GRP SUBSEA COMPOSITE COVERS Kjetil Rognlien, MSc Technical Consultant EDR AS, Norway 2008 ANSYS, Inc. All rights reserved.

More information

Modeling Evaporating Liquid Spray

Modeling Evaporating Liquid Spray Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow

More information

FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016

FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 Note: These instructions are based on an older version of FLUENT, and some of the instructions

More information

Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent

Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent Workshop Transient 1-way FSI Load Mapping using ACT Extension 15. 0 Release Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent 1 2014 ANSYS, Inc. Workshop Description: This example considers

More information

Ryian Hunter MAE 598

Ryian Hunter MAE 598 Setup: The initial geometry was produced using the engineering schematics provided in the project assignment document using the ANSYS DesignModeler application taking advantage of system symmetry. Fig.

More information

equivalent stress to the yield stess.

equivalent stress to the yield stess. Example 10.2-1 [Ansys Workbench/Thermal Stress and User Defined Result] A 50m long deck sitting on superstructures that sit on top of substructures is modeled by a box shape of size 20 x 5 x 50 m 3. It

More information

Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent

Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent MEGR 7090-003, Computational Fluid Dynamics :1 7 Spring 2015 Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent Rahul R Upadhyay Master of Science, Dept of Mechanical

More information

Lecture 5 Two-way FSI Solving and Post Processing. Solving FSI Applications Using ANSYS Mechanical and ANSYS CFX Release. Release 14.

Lecture 5 Two-way FSI Solving and Post Processing. Solving FSI Applications Using ANSYS Mechanical and ANSYS CFX Release. Release 14. Lecture 5 Two-way FSI Solving and Post Processing 14. 5 Release Solving FSI Applications Using ANSYS Mechanical and ANSYS CFX 1 2011 ANSYS, Inc. July 26, 2013 Outline Solution Process Here we discuss starting

More information

Thank you for downloading one of our ANSYS whitepapers we hope you enjoy it.

Thank you for downloading one of our ANSYS whitepapers we hope you enjoy it. Thank you! Thank you for downloading one of our ANSYS whitepapers we hope you enjoy it. Have questions? Need more information? Please don t hesitate to contact us! We have plenty more where this came from.

More information

Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes

Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School

More information

Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert)

Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert) Middle East Technical University Mechanical Engineering Department ME 485 CFD with Finite Volume Method Fall 2017 (Dr. Sert) ANSYS Fluent Tutorial Developing Laminar Flow in a 2D Channel 1 How to use This

More information

ANSYS FLUENT. Lecture 3. Basic Overview of Using the FLUENT User Interface L3-1. Customer Training Material

ANSYS FLUENT. Lecture 3. Basic Overview of Using the FLUENT User Interface L3-1. Customer Training Material Lecture 3 Basic Overview of Using the FLUENT User Interface Introduction to ANSYS FLUENT L3-1 Parallel Processing FLUENT can readily be run across many processors in parallel. This will greatly speed up

More information

µ = Pa s m 3 The Reynolds number based on hydraulic diameter, D h = 2W h/(w + h) = 3.2 mm for the main inlet duct is = 359

µ = Pa s m 3 The Reynolds number based on hydraulic diameter, D h = 2W h/(w + h) = 3.2 mm for the main inlet duct is = 359 Laminar Mixer Tutorial for STAR-CCM+ ME 448/548 March 30, 2014 Gerald Recktenwald gerry@pdx.edu 1 Overview Imagine that you are part of a team developing a medical diagnostic device. The device has a millimeter

More information

Metafor FE Software. 2. Operator split. 4. Rezoning methods 5. Contact with friction

Metafor FE Software. 2. Operator split. 4. Rezoning methods 5. Contact with friction ALE simulations ua sus using Metafor eao 1. Introduction 2. Operator split 3. Convection schemes 4. Rezoning methods 5. Contact with friction 1 Introduction EULERIAN FORMALISM Undistorted mesh Ideal for

More information

Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil

Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -

More information

Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow

Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Introduction This tutorial illustrates the setup and solution of the two-dimensional turbulent fluid flow and heat

More information

Swapnil Nimse Project 1 Challenge #2

Swapnil Nimse Project 1 Challenge #2 Swapnil Nimse Project 1 Challenge #2 Project Overview: Using Ansys-Fluent, analyze dependency of the steady-state temperature at different parts of the system on the flow velocity at the inlet and buoyancy-driven

More information

A B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number

A B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number Individual task Objective To derive the drag coefficient for a 2D object, defined as where D (N/m) is the aerodynamic drag force (per unit length in the third direction) acting on the object. The object

More information

Module D: Laminar Flow over a Flat Plate

Module D: Laminar Flow over a Flat Plate Module D: Laminar Flow over a Flat Plate Summary... Problem Statement Geometry and Mesh Creation Problem Setup Solution. Results Validation......... Mesh Refinement.. Summary This ANSYS FLUENT tutorial

More information

Facundo DEL PIN / Iñaki ÇALDICHOURY / Rodrigo PAZ / / Livermore Software Technology Corporation

Facundo DEL PIN / Iñaki ÇALDICHOURY / Rodrigo PAZ / / Livermore Software Technology Corporation LS-DYNA R R7 : Strong Fluid Structure Interaction (FSI) capabilities and associated meshing tools for the incompressible CFD solver (ICFD), applications and examples Facundo DEL PIN / Iñaki ÇALDICHOURY

More information

Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT

Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT Workbench Tutorial Minor Losses, Page 1 Tutorial Minor Losses using Pointwise and FLUENT Introduction This tutorial provides instructions for meshing two internal flows. Pointwise software will be used

More information

2008 International ANSYS Conference Strongly Coupled FSI Simulation Moving Compressible Pressure Pulse through a Tube

2008 International ANSYS Conference Strongly Coupled FSI Simulation Moving Compressible Pressure Pulse through a Tube 2008 International ANSYS Conference Strongly Coupled FSI Simulation Moving Compressible Pressure Pulse through a Tube Daniel L. Cler, US Army RDECOM/ ARDEC/ WSEC/ Benet Labs 1 Overview Background Problem

More information

November c Fluent Inc. November 8,

November c Fluent Inc. November 8, MIXSIM 2.1 Tutorial November 2006 c Fluent Inc. November 8, 2006 1 Copyright c 2006 by Fluent Inc. All Rights Reserved. No part of this document may be reproduced or otherwise used in any form without

More information

Modeling Unsteady Compressible Flow

Modeling Unsteady Compressible Flow Tutorial 4. Modeling Unsteady Compressible Flow Introduction In this tutorial, FLUENT s density-based implicit solver is used to predict the timedependent flow through a two-dimensional nozzle. As an initial

More information

Flow and Heat Transfer in a Mixing Elbow

Flow and Heat Transfer in a Mixing Elbow Flow and Heat Transfer in a Mixing Elbow Objectives The main objectives of the project are to learn (i) how to set up and perform flow simulations with heat transfer and mixing, (ii) post-processing and

More information

Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić

Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions Milovan Perić Contents The need to couple STAR-CCM+ with other theoretical or numerical solutions Coupling approaches: surface and volume

More information

Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM)

Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry

More information

First Steps - Ball Valve Design

First Steps - Ball Valve Design COSMOSFloWorks 2004 Tutorial 1 First Steps - Ball Valve Design This First Steps tutorial covers the flow of water through a ball valve assembly before and after some design changes. The objective is to

More information

Introduction to ANSYS SOLVER FLUENT 12-1

Introduction to ANSYS SOLVER FLUENT 12-1 Introduction to ANSYS SOLVER FLUENT 12-1 Breadth of Technologies 10-2 Simulation Driven Product Development 10-3 Windshield Defroster Optimized Design 10-4 How Does CFD Work? 10-5 Step 1. Define Your Modeling

More information

DMU Engineering Analysis Review

DMU Engineering Analysis Review DMU Engineering Analysis Review Overview Conventions What's New? Getting Started Entering DMU Engineering Analysis Review Workbench Generating an Image Visualizing Extrema Generating a Basic Analysis Report

More information

Simulation in Computer Graphics. Deformable Objects. Matthias Teschner. Computer Science Department University of Freiburg

Simulation in Computer Graphics. Deformable Objects. Matthias Teschner. Computer Science Department University of Freiburg Simulation in Computer Graphics Deformable Objects Matthias Teschner Computer Science Department University of Freiburg Outline introduction forces performance collision handling visualization University

More information

ANSYS/LS-Dyna. Workbench Using. Steven Hale Senior Engineering Manager CAE Associates, Inc. June 13, CAE Associates

ANSYS/LS-Dyna. Workbench Using. Steven Hale Senior Engineering Manager CAE Associates, Inc. June 13, CAE Associates ANSYS/LS-Dyna Customization in Workbench Using ACT Steven Hale Senior Engineering Manager CAE Associates, Inc. June 13, 2013 2013 CAE Associates CAE Associates CAE Associates is an engineering services

More information

midas NFX 2017R1 Release Note

midas NFX 2017R1 Release Note Total Solution for True Analysis-driven Design midas NFX 2017R1 Release Note 1 midas NFX R E L E A S E N O T E 2 0 1 7 R 1 Major Improvements Midas NFX is an integrated finite element analysis program

More information

Fluid-structure Interaction by the mixed SPH-FE Method with Application to Aircraft Ditching

Fluid-structure Interaction by the mixed SPH-FE Method with Application to Aircraft Ditching Fluid-structure Interaction by the mixed SPH-FE Method with Application to Aircraft Ditching Paul Groenenboom ESI Group Delft, Netherlands Martin Siemann German Aerospace Center (DLR) Stuttgart, Germany

More information

ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity

ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity Phil Stopford Duxford Air Museum 11th May 2011 2011 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Fluid Structure

More information

Chapter 5 Modeling and Simulation of Mechanism

Chapter 5 Modeling and Simulation of Mechanism Chapter 5 Modeling and Simulation of Mechanism In the present study, KED analysis of four bar planar mechanism using MATLAB program and ANSYS software has been carried out. The analysis has also been carried

More information

Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding

Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,

More information

Revolve 3D geometry to display a 360-degree image.

Revolve 3D geometry to display a 360-degree image. Tutorial 24. Turbo Postprocessing Introduction This tutorial demonstrates the turbomachinery postprocessing capabilities of FLUENT. In this example, you will read the case and data files (without doing

More information

Coupled Analysis of FSI

Coupled Analysis of FSI Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA

More information

A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue. Alan Mueller & Oleg Voronkov

A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue. Alan Mueller & Oleg Voronkov A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue Alan Mueller & Oleg Voronkov Case description Main structural dimensions [1]: deformable jumper [2] in Mixture on

More information

Simulation of Turbulent Flow around an Airfoil

Simulation of Turbulent Flow around an Airfoil Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Pre-Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew Opyd, Dong-Hwan

More information

Introduction to ANSYS ICEM CFD

Introduction to ANSYS ICEM CFD Lecture 1 Introduction to ANSYS ICEM CFD 14.5 Release Introduction to ANSYS ICEM CFD 2012 ANSYS, Inc. April 1, 2013 1 Release 14.5 Purpose/Goals Ansys ICEM CFD is a general purpose grid generating program

More information

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1 Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 2 (ANSYS 19.1; Last Updated: Aug. 7, 2018) By Timur Dogan, Michael Conger,

More information

LS-DYNA s Linear Solver Development Phase 2: Linear Solution Sequence

LS-DYNA s Linear Solver Development Phase 2: Linear Solution Sequence LS-DYNA s Linear Solver Development Phase 2: Linear Solution Sequence Allen T. Li 1, Zhe Cui 2, Yun Huang 2 1 Ford Motor Company 2 Livermore Software Technology Corporation Abstract This paper continues

More information

Driven Cavity Example

Driven Cavity Example BMAppendixI.qxd 11/14/12 6:55 PM Page I-1 I CFD Driven Cavity Example I.1 Problem One of the classic benchmarks in CFD is the driven cavity problem. Consider steady, incompressible, viscous flow in a square

More information

Isotropic Porous Media Tutorial

Isotropic Porous Media Tutorial STAR-CCM+ User Guide 3927 Isotropic Porous Media Tutorial This tutorial models flow through the catalyst geometry described in the introductory section. In the porous region, the theoretical pressure drop

More information

Wall thickness= Inlet: Prescribed mass flux. All lengths in meters kg/m, E Pa, 0.3,

Wall thickness= Inlet: Prescribed mass flux. All lengths in meters kg/m, E Pa, 0.3, Problem description Problem 30: Analysis of fluid-structure interaction within a pipe constriction It is desired to analyze the flow and structural response within the following pipe constriction: 1 1

More information

The Spalart Allmaras turbulence model

The Spalart Allmaras turbulence model The Spalart Allmaras turbulence model The main equation The Spallart Allmaras turbulence model is a one equation model designed especially for aerospace applications; it solves a modelled transport equation

More information

Introduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.

Introduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved. Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.

More information

Modeling External Compressible Flow

Modeling External Compressible Flow Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras

More information

Multi-Axis Tabular Loads in ANSYS Workbench

Multi-Axis Tabular Loads in ANSYS Workbench Multi-Axis Tabular Loads in ANSYS Workbench 2/24/2017 1 Users of ANSYS Workbench (18) may have noticed that the they have a choice of independent variables when defining a tabular load Typical choices

More information

Directions: 1) Delete this text box 2) Insert desired picture here

Directions: 1) Delete this text box 2) Insert desired picture here Directions: 1) Delete this text box 2) Insert desired picture here Multi-Disciplinary Applications using Overset Grid Technology in STAR-CCM+ CD-adapco Dmitry Pinaev, Frank Schäfer, Eberhard Schreck Outline

More information

Appendix P. Multi-Physics Simulation Technology in NX. Christian Ruel (Maya Htt, Canada)

Appendix P. Multi-Physics Simulation Technology in NX. Christian Ruel (Maya Htt, Canada) 251 Appendix P Multi-Physics Simulation Technology in NX Christian Ruel (Maya Htt, Canada) 252 Multi-Physics Simulation Technology in NX Abstract As engineers increasingly rely on simulation models within

More information

TryItNow! Step by Step Walkthrough: Spoiler Support

TryItNow! Step by Step Walkthrough: Spoiler Support TryItNow! Step by Step Walkthrough: Spoiler Support 1 2015 ANSYS, Inc. March 28, 2016 TryItNow! Step by Step Walkthrough: Spoiler Support ANSYS designed this TryItNow! experience to give you quick access

More information

T6: Position-Based Simulation Methods in Computer Graphics. Jan Bender Miles Macklin Matthias Müller

T6: Position-Based Simulation Methods in Computer Graphics. Jan Bender Miles Macklin Matthias Müller T6: Position-Based Simulation Methods in Computer Graphics Jan Bender Miles Macklin Matthias Müller Jan Bender Organizer Professor at the Visual Computing Institute at Aachen University Research topics

More information

ALE and Fluid-Structure Interaction in LS-DYNA March 2004

ALE and Fluid-Structure Interaction in LS-DYNA March 2004 ALE and Fluid-Structure Interaction in LS-DYNA March 2004 Workshop Models 1. Taylor bar impact 2. One-dimensional advection test 3. Channel 4. Underwater explosion 5. Bar impacting water surface 6. Sloshing

More information