OpenFOAM/C3/Using-Template-files-in-PyFoam/English

Tutorial 21: C2

Title : Using Template files in PyFoam Script : Anmol Sahoo, Rahul Joshi Narration : Rahul Joshi

Keywords : OpenFOAM, PyFoam, Python, Template, supersonic flow, wedge

Visual Cue	Narration
Show slide : Title	Hello and welcome to the Spoken Tutorial on Using Template files in PyFoam.
Show Slide : Learning Objective	In this tutorial we will: Understand the function of PyFoam Utilities Create and use template files Use PyFoamFromTemplate.py for solving the supersonic flow over wedge We can run this for different wedge angles using template files.
Show Slide : System requirement	To record this tutorial I am using Ubuntu Linux Operating System 14.04 OpenFOAM 2.3.0 PyFoam-0.6.5
Show slide : Prerequisite	To practice this tutorial the user should have : Basic Knowledge of using Linux terminal Experience of running and analyzing OpenFOAM cases If not, please refer to the spoken tutorial series on Linux and OpenFOAM.
Show slide : Template Files	What are template files? Template files are used to generate OpenFOAM files like blockMeshDict or controlDict Template files can be programmed, hence we can procedurally generate data.
Show slide : Syntax of Template files	A template file should be an OpenFOAM file, with the following - Any line beginning with $$ is a Python program line. It will be executed by Python Any variable can be substituted in the file by using the syntax | -varname - |
Show slide : Using a template file	The following steps should be followed to use a template file : First copy an existing file After this create a template file Then run PyFoamFromTemplate.py
Show slide : Creating a template file	Template file will be created for blockMeshDict. We will use the supersonic flow over a wedge as an example case. The case file is available in the rhoCentralFoam solver.
Type run/tutorials/compres sible/rhoCentralFoam	Open the terminal. Type the path for the rhoCentralFoam inside compressible solvers.
Type cp -r Wedge5M15 /home/fossee/OpenFO AM/	Now copy the Wedge5M15 case directory into OpenFOAM directory by typing cp -r Wedge5M15 /home/fossee/OpenFOAM/ and press Enter.
Cd OpenFOAM/Wedge5 M15	On the terminal, type the path for Wedge5M15 folder inside OpenFOAM directory.
Type cd constant/polyMesh/bl ockMeshDict	Type the path for blockMeshDict file inside polyMesh directory inside constant.
Type gedit blockMeshDict	Open the blockMeshDict file in any editor of your choice.
Point to the vertices section	We can see the vertices section.
Show slide : vertices to be changed	We need to calculate the co-ordinates of the end points of the slope. Based on the angle, change the following lines ( 0.3048 0.081670913853 -0.005) ( 0.3048 0.081670913853 0.005)
On the terminal type cp -r blockMeshDict > blockMeshDict.templ ate	Switch back to the terminal Copy your blockMeshDict file into a file called blockMeshDict.template, type the following- cp -r blockMeshDict > blockMeshDict.template
gedit blockMeshDict.template	Open the blockMeshDict.template file using gedit
Show slide : Template file syntax	Add the following lines above convertToMeters $$import math $$thetaDegrees = 10.0 $$thetaRadians = math . radians ( thetaDegrees ) $$y_coord = 0.3048* math . tan ( thetaRadians ) Any line preceded with $$ is a Python line, and will be interpreted and executed by Python
Show slide : Template file syntax	Modify the vertices entry as ( 0.3048 |-y_coord-| -0.005) ( 0.3048 |-y_coord-| 0.005)
	Python variables assigned in the template file, should be substituted at any location in the file. To do so, use | −varname− | in the file.
Highlight or point to the changes	We can see the changes made into this file.
	Now, let's create a blank file
Type gedit templateFileConst	On the terminal, type gedit templateFileConst and press Enter.
templateFileConst	Create a dummy entry inside it by typing dummy 1.0; A dummy entry is mandatory. An external dict has to be provided with any constant that is to be used in the template file.
Press Ctrl+S and close	Save and close the both the files
cd ../../	Now go 2 levels back to your case file.
Switch back to slides	Let me switch back to slides
Show slide : Running PyFoam command	We have to run the template command now. pyFoamFromTemplate.py --template-file=./blockMeshDict.template --output=./blockMeshDict --values-dictionary=templateFileConst --allow-exec-instead-of-assignment
Type this command in terminal >> press Enter	Type this command in terminal and press Enter
Type cd constant/polyMesh	Now again go inisde the polyMesh folder inside constant
Point to blockMeshDict and a python file	We can see that 2 new files are generated the blockMeshDict.template file is replaced by blockMeshDict and .py file is also generated.
Point to the Python file.	Do not edit the Python file.
On the terminal type gedit blockMeshDict	In the terminal, open the blockMeshDict file by typing -
	gedit blockMeshDict and press Enter.
Point to wedge angle	We had changed the wedge angle from 15 deg to 10 deg.
Point to end points	The end points of the slope have also changed.
Show slide :Running the case file	We can now run the case file by executing the OpenFOAM commands blockMesh rhoCentralFoam visualize the results using Paraview.
Show slide : Assignment	As an assignment, use the following wedge angles and run the template commands. - 0deg, 5 deg, 20 deg, 25 deg
Show slide : Summary	Let us summarize. In this tutorial, we learnt about PyFoam Template We also learnt to- check the installation of script for using template and using the PyFoamFromTemplate.py command
Show Slide Forum to answer questions	Please post your timed queries in this forum.
Show Slide Forum to answer questions	Please post your general queries on OpenFOAM in this forum.
Show Slide Textbook Companion	The FOSSEE team coordinates the TBC project.
Show Slide Acknowledgement	The Spoken Tutorial Project is funded by NMEICT, MHRD, Govt. of India For more details , visit this website.
Thank You	This is Rahul Joshi from IIT Bombay signing off. Thanks for watching

Contributors and Content Editors

Nancyvarkey, Viraj20feb