Conjugate Heat Transfer Simulation for an Aluminium Hollow Pipe

OBJECTIVE

The objective of this study is to set up a transient state flow simulation through a hollow pipe and understand the dependency of grid size on simulation time and results. Apart from this, the effect of supercycling stage interval on the simulation time will also be assessed in the study. The project includes the key results for three simulations setups based on the three different grid sizes and supercycling stage interval as per the table given below

Case Grid Size SuperCycling Stage Interval
Baseline dx = 0.004 m; dy = 0.004 m; dz = 0.004 m 0.05
Case 1 dx = 0.004 m; dy = 0.004 m; dz = 0.004 m 0.03
Case 2 dx = 0.0025 m; dy = 0.0025 m; dz = 0.0025 m 0.03
Case 3 dx = 0.0015 m; dy = 0.0015 m; dz = 0.0015 m 0.03
Case 4 dx = 0.0025 m; dy = 0.0025 m; dz = 0.0025 m 0.02
Case 5 dx = 0.0025 m; dy = 0.0025 m; dz = 0.0025 m 0.01

The report includes the following steps taken to setup the conjugate heat transfer simulation:

1. Preprocessing

    1.1. Geometry Creation

    1.2. Diagnosis

    1.3. Boundary Flagging

    1.4. Case Setup

2. Solving

3. Post Processing

   3.1. Mesh

   3.2. Plots (Velocity, Inlet and Outlet Temperature, Mean Regional Temperature)

   3.3. Contours (Velocity, Temperature)

   3.4. Total Simulation Time vs  Supercycling Stage Interval

   3.5. Animation

 

PROCEDURE:

The procedure followed for setting up the simulation is provided below

1. Preprocessing

  1.1. Geometry Creation

        a. The geometry was created using following steps: Goto Geometry>Create>Shape> Click on cylinder button

        i. Enter Center 1: 0,0,0

        ii. Enter Center 2: 0,0,0.2

        iii. Radius 1 and Radius 2: 0.015- This will create a solid pipe

        iv. Click on create and repeat the process with new Radius 1 and Radius 2: 0.02- This                will add the thickness to the pipe

        v. Now select the Inlet and outlet faces traingles and delete those

        vi. Goto create>traingles>loft edges>Select the concentric circles and click on create-              This will create the thickness

        vii. Goto Repair>patch>list of edges> select the inner circle on both the inlet stream                and outlet stream side to create the traingles at these areas

 

                                     Fig. 1: Geometry (All dimension are in m)

                                        Fig. 2: Geometry (Section View)

c. A section cut was performed on the geomerty to inspect it again as shown in Fig.2. 

d. Checked the normal orientation on surface and made sure the normals are pointing towards the fluid regime. In case it was poiting in the reverse direction, Goto Transform>Normal>Propagate Change from a single triangle>select any any traingle and click on apply

 

1.2. Diagnosis: The diagnosis tool helps in identifying the different problems in the                    geometry. 

      The Diagnosis tool looks for the following geometric issues

     a. Intersection: Highlights number of triangles with piercing inbetween adjacent two                 triangles

     b. Nonmanifold Vertices: Checks for number vertex which are being shared between two           triangles

     c. Open Edge: This highlights the number of edges of a triangle which not shared by any           other triangle

     d. Normal Orientation: This highlights the number of traingles whose normal vector is               not pointing towards the interior of fluid domain

     e. Isolated Triangles: This checks for the number of triangle surrounded by any                         neighbouring triangles that have different boundary ID number

    Goto Diagnostics Dock>Find>

       

Since all the problem traingles are green ticked, there were no issues in the geometry

1.3. Boundary Flagging:

         a. Goto Boundary>Flag>Create a New Boundary>Create Multiple Boundary>Enter 4 in               "Number of Multiple Boundaries"

        b. Select the triangles the assigned it to the respective boundaries

The figure below represent the boundaries flagged

         

 1.4. Case Setup: 

      a. Clicked on "Begin case Setup" and entered the value provided below

  

Settings Values to be Entered
Application General Flow
Material Select Air (predefined mixture) and Tick onto Species and Solid Simulation
Gas simulation>No Change
Solid Simulation>Click on Predefined Solid> select Aluminum>Add Selected
Global Transport Paramters>No  Change
Species> Gas> add O2 and N2, Solid>Add Aluminum
Simulation Parameters Run Paramters> Transient
Simulation Time Parameter>
Start Time: 0.5 s
Initial time step: 1.0e-7 s
Minimum time step: 1.0e-7 s
Maximum time step: 0.5s
Solver Parameters> No Change
Boundary Conditions  OuterWall
Boundary Type>Wall, Wall Motion Type>Stationary, Select Slip from the list
Temperature Boundary Condition> Select Heat Flux from the list & Assign the Flux value as -10000.0 W/m^2

Thickness
Boundary Type>Wall, Wall Motion Type>Stationary, Select Slip from the list
Temperature Boundary Condition> select Zero Normal Gradient

Inlet
Boundary Type> Inflow
Pressure BC>Zero Normal Gradient
Velocity BC>Specified Value, Assign Vz=0.37m/s*
Temperature BC>Specified Value, Assign Temperature Value>300K
Species BC> Add Air with Total Mass Fraction as 1, i.e., O2:0.23, N2:77

Outlet
Boundary Type-OUTFLOW
Pressure Boundary Condition>Specified Value, Enter a value of 101325.0 Pa
Velocity Boundary Condition>Zero Normal Gradient (NE)
Temperature Backflow>300k
Species Backflow>Air

InterfaceBoundary
Boundary Type> Interface
Velocity Boundary Condition> Stationary
Forward Boundary>region>Fluid
Velocity BC>Law of Wall
Temperature BC>Law of Wall
Backward Boundary>Region>Solid
Velocity BC>Slip
Temperature BC>Specified Value

Assign Region Solid to OuterWall and Thickness, & Region Fluid to Inlet and Outlet
Initial Conditions & Events
Regions and Initialization
Regions and Initialization
Add region>"Fluid"
Stream ID: 0
Temperature: 300k
Enter Pressure value:101325.0Pa
Species: Add Air

Add region>"Solid"
Stream ID: 1, Tick on the Solid
Temperature: 300k
Species: Add Aluminum
Physical Models

Physical Model> Tick on Supercycling
Turbulence Modeling-RNG-K Eplison is selected
Supercycling: Use the Settings as per the following:


Note: The output coordinate should be within the thickness layer in the geometry

For the case setups used the following interval values
Case 1 :Supercyling Interval: 0.03

Case 2 :Supercyling Interval: 0.03

Case 3 :Supercyling Interval: 0.03

Case 4 :Supercyling Interval: 0.02

Case 5 :Supercyling Interval: 0.01

Grid Controls Enter the grid values for (dx, dy, dz) as per the case Baseline
Baseline: dx = 0.004 m; dy = 0.004 m; dz = 0.004 m

For Case 1,2,3 use the following grid size
Case 1
dx = 0.004 m; dy = 0.004 m; dz = 0.004 m
Case 2
dx = 0.0025 m; dy = 0.0025 m; dz = 0.0025 m
Case 3
dx = 0.0015 m; dy = 0.0015 m; dz = 0.0015 m

For Case 4 & 5 used base grid size equivalent to case 2
Output/Post Processing Post Variable Selection>
Goto to the Combustion/Turbulence tab and tick on y+, No other change
Output Files Time Interval for writing 3D output data files: 0.01 s
Time Interval for writing text output: 1e-07 s
Time Interval for restarting output: 0.1 s

After this all the input files was imported to a seperate folder. Converge creates .txt  files which contains all the values entered while setting up the case for respective settings done above. These input files will be processed by converge using Message Passing Interface (MPI) standard

2. Solving:

For running the simulation, Cygwin tool was used instead of converge studio interface. Cygwin is a POSIX-compatible API which is based on command prompt is used to run the simulation

Steps:

a. Navigated to the folder location containing the input files

b. Entered the command> mpiexec.exe -n 2 converge.exe logfile & : This allows converge to run two processors (selection on number of processor cores present as per the system configuration, can use multiple cores if available) for the parallel processing and load balancing

c. Entered the command> taif -f logfile

d. After the simulation is over. Went back to converge studio>Post-Processing 3D

e. Enter Case Name>"Test", Change the File Type to Paraview VTK in-line binary format

d. Enter the address for the output files>Select all files>Select all Cell Variables>click on Convert

e. After the conversion of the post files to the binary output, open the Test.vtm (group file) file in Paraview

 

 

3. POST-PROCESSING:

After opening the group file in paraview, clicked on apply to load the results. Created slice, glyphs and other plots as required

  3.1. Meshing:

                                               Fig: Cell Count (Case 1, 2 & 3)

 

                                            Fig: Case 1 Mesh View

                                            Fig: Case 2 Mesh View

                                            Fig: Case 3 Mesh View

3.2. Plots

Velocity Plots

                                        Fig: Case 1: Inlet and Outlet Velocity Plots

                                           

Inlet and Outlet Temperature Plots

                                         Fig:  Baseline: Inlet and Outlet Temperature Plots

                                            Fig:  Case 1: Inlet and Outlet Temperature Plots

                                               Fig:  Case 2: Inlet and Outlet Temperature Plots

                                                   

                                                Fig:  Case 3: Inlet and Outlet Temperature Plots

                                                Fig:  Case 4: Inlet and Outlet Temperature Plots

                                                Fig:  Case 5: Inlet and Outlet Temperature Plots

 

 

Mean Regionwise Temperature Plots

                             Fig:  Baseline: Region 0 and Region 1 Temperature Plots

 

                            Fig:  Case 1: Region 0 and Region 1 Temperature Plots                           

                              Fig:  Case 2: Region 0 and Region 1 Temperature Plots

                             Fig:  Case 3: Region 0 and Region 1 Temperature Plots

                             Fig:  Case 4: Region 0 and Region 1 Temperature Plots

 

                             Fig:  Case 5: Region 0 and Region 1 Temperature Plots

3.3. Total Simulation Time vs Supercycling Stage Interval

Note: Here the baseline case was run with grid size of dx=dy=dz=0.0025m for capturing the proper comparison of the simulation time which is independent of the grid size

3.4. Contours:

Case 1:

                          Fig: Velocity and Temperature Contour Plot (Case 1-Output 10)   

                          Fig: Pressure and yPlus Contour Plot (Case 1-Output 10)

Case 2:

                  Fig: Velocity and Temperature Contour Plot (Case 2-Output 10)

                  Fig: Pressure and yPlus Contour Plot (Case 2-Output 10)

Case 3:

                  Fig: Velocity and Temperature Contour Plot (Case 3-Output 10)

                  Fig: Pressure and yPlus Contour Plot (Case 3-Output 10)

 

3.5. Animation :

Case 2

Case 3

Key Conclusions

1.With the decrease in grid size the total cell increases and the simulation time as well, since more number of equations are being solved

2. The rise in the outlet temperature curve increase sharply and then slowly reaches the steady state after some time. The increase in cell count the thereby, results in more accurate capture of the temperature rise

3. Grid dependency test was conducted to obtain the optimal grid size i.e., a tradeoff between the simulation time and results. It also assists in understanding the grid size and time to achieve converged state of results, which inturn influences the grid selection decision. In our case, the grid size of dx=dy=dz=0.0025m was selected, for further assesstment of the supercycling stage interval on the total simulation time

4. Activating the yplus results in the smooth acquisition of the velocity profile near the solid interface or the inner wall

5. By reducing the supercycling stage interval, the simuation took less time and the optimal results were also obtained, which is one of the key objectives of using this concept. Lower stage interval results in more frequent update of the temperature values in the solid domain which thereby overcomes the time scale differences at a faster pace


Projects by Gaurav Samanta

Data Analysis
Gaurav Samanta · 2020-01-08 12:32:09

Objective: The objective of this project is to write a code for data analysis from an input file and perform the following operations 1. Compatibility Check: The program will ask for the file name with valid extension which if provided incorrect will terminate the prog Read more

Constraint Minimization
Gaurav Samanta · 2020-01-08 11:52:01

Objective: The objective of this project is to minimize a simple non-linear funtion using Lagrange Multiplier The target equation is: `f(x,y)=5-(x-2)^2-2(y-1)^2` & the constrain equation: `x+4y=3` Theory: In real engineering applications there is a Read more

Curve Fitting
Gaurav Samanta · 2019-12-27 19:42:51

Objective: The objective of this project is to perform a curve fitting between the temperature and Cp values given the data file   Theory:  Curve Fitting: it is a process of constructing a curve that best fits the provided data series. Curve fitting in gene Read more

Ice Breaking Challenge
Gaurav Samanta · 2019-12-27 19:01:57

Objective:  The objective of this project is to determine the minimum pressure required to break a given thickness of ice using an air cushion vehicle through Newton Raphson Method Equation: `p^3(1-beta^2)+(0.4hbeta^2-(sigmah^2)/r^2)p^2+((sigma^2h^4)/(3r^4))p-((s Read more

Objective: The objective of this report is to understand the CAD modeller features in Star CCM+ and use it to generate a 3D model of an Ahmed Body and a Convergent Divergent Nozzle in the same as per the drawing given below   Procedure & Results: Conv Read more

Air Standard Cycle
Gaurav Samanta · 2019-12-10 14:51:18

Objective: The objective of this report is to create a python based Otto Cycle simulator which can create the  PV diagram and give the thermal efficiency of the engine as output  Theory: Otto cycle is the set of processes used by the spark ignition Read more

2R Robotic Arm
Gaurav Samanta · 2019-12-10 14:33:33

 Objective: The objective of this report is to simulate the foward kinematics of a 2R robotic arm using python programming   Theory: Robotic arm manipulators are used in various industry verticals such as automotive, electronics, warehouses and logistic Read more

Solving 2nd order ODE
Gaurav Samanta · 2019-12-10 08:14:29

Objective: The objective of this report is the simulate the transient behaviour of a simple pendulum and the create the animation of its motion for a given time interval Theory: The following equation (Ordinary Differential Equation) for the position of the bob w. Read more

Flow over Bicycle
Gaurav Samanta · 2019-11-22 18:54:05

Objective:   The objective of this  study to understand the change in drag force with respect to velocity different cycling positions and drag coefficeint for constant frontal area and constant velocity.   Theory: Cyclists tend to experien Read more

Objective: The objective of this report is to understand the different steps involved in any CFD simulation and the applications of CFD in Medical, Oil & Gas and Construction Industry 1. Steps involved in a CFD Simulation  Step 1. CAD Modelling/Geometry Impor Read more


Loading...

The End