Sign-up for free online course on ANSYS simulations!Unable to render {include} The included page could not be found.
Unable to render {include} The included page could not be found.
Numerical Solution
Skipping to Solution Controls, deselect Premixed Combustion and PDF so that the only equations solved for are flow, swirl velocity, and turbulence as a preliminary solution. Press OK.
Go to Solution Initialization. Press Initialize; let Fluent initialize the domain as a Hybrid Initialization, taking all boundaries into account.
Go to Run Calculation. Enter 1000 under the number of iterations and run the simulation until it converges.
Now adapt a small region near the inlet with a progress variable of zero (denotes no combustion in this region, so that this region is entirely recalculated)
Go to Adapt-Region at the menus at the top of the page. Select a small region near the inlet: X from 0.1 to 0.14m, Y from 0 to 0.03m. Click "Mark", which marks 207 cells for refinement, and then click "Close".
Patch this region by going to Solution Initialization, and click "Patch". Select "Progress Variable" as the variable, and patch the region that you just marked. Close the dialogue after patching.
Now go back to Solution Controls and click "Equations". Reselect the PDF and Partially Premixed options so that all options are highlighted and will be solved for. Press OK. In Solution Methods, make sure that all solvers (Momentum, Swirl Velocity, and Turbulent Kinetic Energy) are set to a second order solver scheme.
Go to Run Calculation. Click on Data File Quantities and select any additional quantities (ie Stream Function) that you would like to export. Now press "Calculate". Allow the solution to converge (convergence criterion being that the residuals are all at least 1E-3 or smaller).
