foamscience / assignment-basic-flow-equations

Assignment for the "Basic Equations, advective and diffusive transport" lecture

Goals

Table of Contents

Basic-level skills

In the lecture, we have introduced end results of some advective/diffusive OpenFOAM simulations. This Basic-Level section tries to get you to produce similar resuls on your own.

1. Clone our (Steady-State) introductory case from here (to your run directory):

git clone https://github.com/FOAM-School/res-eng-openfoam-intro diff-adv

2. Increase cells count to 20 in the x-direction (check constant/polyMesh/blockMeshDict)

3. In system/fvSchemes, replace steadyState with Euler to approximate the time derivative using Euler's forward scheme.

4. Changing ddtSchemes.default entry to Euler is not enough! we need to adjust the numerical methods featured in system/fvSolution and some settings in system/controlDict as well:

   a. For the T variable, select an appropriate numerical solver (other than smoothSolver) with a decent preconditioner. Make it so the solver's tolerance is 1e-7 and no max iteration count is specified.

   b. Adjust system/controlDict settings so that we simulate the flow for 1.5 seconds, with an initial tiemstep of 0.001 seconds. The solver should write results to disk every 10 timesteps.

Now you should be able to run a sample simulation and check the results with ParaView.

5. To explore the advective case, there are some changes that should be made:

   a. The boundary condition on T at the outlet patch should be zeroGradient.

   b. The diffusion coefficient in constant/transportProperties should be null.

   c. The 0/U file should reflect an initial velocity of (0.5 0 0) in the whole domain.

   Run the case in that state; you should notice some oscillatory behaviour around 0.25 seconds.

6. From the previous question, we know that the advective term is causing instabilities. To fix the situation, we can, for example, select a more "reliable" divergence schemes: In system/fvSchemes, pick limitedLinear 0.2 as the scheme used for divSchemes.div(phi, T) entry.

   The 0.2 value represents "by how much we limit the linear scheme". a value of 1 will result in no limitation.

   Run the simulation again and see for yourself if there is a stability gain.

7. Now to the diffusion case.

   a. Make the velocity null initially and assign 0.1 to the diffusion coefficient.

   b. The Laplacian term is approximated with linear uncorrected which is fine because we don't need any corrections for such simple meshes. Correcting operator approximations should be selected only in meshes with significant non-orthogonality angles. Run the simulation and check if it runs smooth.

Intermediate-level skills

The general transport equation is the elementary block of most OpenFOAM solvers; However, the equation we described in the lecture was the one used in the scalarTransportFoam from the Foam-Extend package. Recent Mainline OpenFOAM solvers add an interesting feature, called fvOptions.

1. Take a look at the equation at scalarTransportFoam.C, line 64 from OpenFOAM7 source code. How its transport equation is different from what we described in the lecture?

fvOptions is a framework to include "user-defined" source terms into solved equation without re-compiling the solver. We sacrificed this framework when we chose to work with Foam-Extend-4 in this course. Because, it needs some programming experience, we will discuss it in Part 2 of this course.

2. Go back to our adv-diff case (from the basic-level section) and:

   a. Change the preconditioner for the numerical solver (Try diagonal, DILU, ... etc) and note the number of iterations per timestep required for convergence.

   b. Get the case into that "pure-advective" state (null diffusivity) then write a Shell script (Or a perl/Python script) that:

   • Copies the case to a new directory multiple times
   • Changes fvSchemes.divSchemes.div(phi,T) in each new case. Use the following (Gauss) schemes: linear, limitedLinear, filteredLinear and QUICK. (You need to figure out how these schemes are used first).
   • Builds and checks the mesh
   • Runs the simulation

Hints for those who are new to Shell scripting:

• A shell script is a just a group of shell commands
• Execute help for in a BASH shell to figure out how looping is supposed to work.
• cp -r copies a directory
• sed is the most basic tool for "search-and-replace" operations on Unix files
• Then you can run OpenFOAM commands the usual way.

At this point, we lack the necessary post-processing skills to make anything useful from this script, but we'll learn those skills in no time! For now, you can figure out which scheme works best by going opening each case in ParaView and inspecting how the scheme performed.

Advanced-level skills

No advanced-level questions until you complete the whole module.