FLUENT V5 - How to calculate mixing or blending time with the Multiple Reference Frame model
Given is a simulation of a stirred tank using multiple reference frames. Now, the blend time is to be calculated. How to do? After a fluid flow simulation for a stirred tank has been done, often the flow field is to be used for a transient simulation of the transport of a (dissolved) tracer species. This is the numerical simulation of a well-known experimental method to determine the so-called blending or mixing time: The tracer is added locally at time t=0, and from then on the tracer concentration is followed over time by appropriate probes at one or several locations in the tank. The blending time is then defined as the time after which the measured concentration(s) for the last time enter(s) a certain range around the equilibrium concentration. If this is to be done in FLUENT5.x, some important points should be noticed, as described in the second Resolution (press [>>]). The blend time is defined as the time from the addition of a trace pulse until a certain degree of homogeneity in the stirred mixture is reached. This is essentially the instruction how to proceed: 1.: Switch off the calculation of all equations (flow, turbulence, energy,...) under Solve--Controls--Solution. 2.: Switch on multiple species (no volume reactions) under Define--Models--Species. 3.: Define two different fluid materials (species) that have exactly the same properties as the fluid that the fluid flow simulation has been performed with. 4.: Create a "mixture" material that consists of these to components. Choose this "mixture" material to be active under Define--Models--Species. 5.: Under Define--Models--Solver, switch on unsteady calculation, choose 2nd order implicit unsteady formulation. 6.: Under Solve--Controls--Solution, verify that only the trace species equation is on, set its underrelaxation factor to 1.0 and choose the second order convection discretisation scheme for it(!). 7.: Mark a small part of the domain using Adapt--Region, enter coordinates, press "Mark" (NOT "Adapt"). 8.: Patch a mass fraction for the tracer species of 0.2 into the whole domain (all fluid zones). Then, patch a mass fraction (for the same trace species) of 0.8 only into the mark register from the previous step. 9.: Define several "probe positions" by creating Point Surfaces (Surface--Point) at various locations. Define Surface Monitors for these "probes"; plot and write (to a file) the (average of the) tracer species mass fraction once every time step. 10.: Run the unsteady simulation. Set the time step size so that the fluid crosses no more than ONE cell per time step everywhere in the domain. Each time step should converge (constant monitors, species residual around 10^-5 or less) within 10 to 20 iterations. If it doesn't, reduce the time step size. (This is very important!). The time-dependent trace concentrations at the various probe locations will be monitored (and written to their respective files). The blend time can now be defined as the time it takes for the concentration at any (or all of the) probe(s) to enter a certain deviation margin around the terminal concentration, which will be reached after infinite blending.gf NOTE: If you re-patch the same initial conditions and run a new tracer transport solution, very strange things may (will!) happen due to a bug in Fluent6 (6.0.20). Please see Solution 514 for details. Preparing and setting up the solution in FLUENT 5.x 1. First, do a simple fluid flow simulation for the stirred tank as usual. You may use fixed velocity data, multiple reference frames or sliding meshes to accound for the impeller in the simulation. (For particular comments on numerical tracer experiments in the latter two cases, please see below.) 2. As the very first step of the set-up of the numerical tracer experiment, go to Solve--Controls--Solution and switch off the solution of fluid flow and turbulence. Make sure this is done at first. 3. Create a second fluid material that has identical properties to the one you used as the stirred liquid, but with a different name. Switch on Multiple Species (Define--Models--Species), without reactions or any other model. Then create a mixture material that consists of the two liquid materials you used/created for this analysis. Activate this mixture material in the Species panel. (Don't forget this! -- After this step, you can switch off the Energy transport model, which will have been enabled by FLUENT when you enabled multiple [non-reacting] species.) 4. Enable transient simulations (Define--Models--Solver: unsteady). Choose second order time discretisation. Also, go to Solve--Controls--Solution again and enable second order discretisation for the species transport equation. (You may use QUICK if this is available.) 5. Mark a small part of the tank volume using any of the tools in the Adapt menu. Don't really adapt (if you pressed the "Adapt" button, just reply "No" in the confirmation box that will appear). Then use Solve--Initialize--Patch to patch a certain tracer concentration in the newly created register. 6. For the transient simulation, you have to choose a proper time step size. Use the so-called Courant criterion: The time step should be sufficiently small, so that in no cell the flow goes longer than across one cell within every time step. In addition, every time step should converge in 20 iterations maximum. Convergence should be monitored using surface monitors plotting the tracer concentration on a Point Surface (generate using Surface--Point in the menu). It will probably not become constant before the scaled residuals go down to approx. 1.e-5 or less. Too small time steps (e.g. in parts of the volume where there are very small flow velocities) usually do very little harm. Interpreting Visualised Results - Tracer Transport in Rotating Zones If you started from a flow field that was calculated using multiple reference frames or sliding meshes, and if you then visualise the tracer transport by a nice animation, you will find that the rotational movement of the tracer "blob" will go against the direction of the impeller rotation, when the tracer enters the rotating frame of reference / moving mesh zone. This is necessary - the tracer transport simulation must be done in the same numerical way as the fluid flow simulation is. (This is an inherent constrain of the finite volume technique.) For this, in the inner frame of reference / moving zone relative velocities must be used, as they are seen by an observers who rotates at the same speed as the shaft (and impeller[s]) does. (Only by this, mass conservation of the trace is guaranteed.) In spite of the apparently unrealistic simulation approach, resulting blending times have been proven to agree very well with reality. Using the absolute frame of reference If this is really desired, it is even possible to do the complete simulation in the absolute frame of reference. This will cause the tracer "blob" to rotate in the same direction throughout the computational domain. But by this, it will collide severely with the impeller blades, not penetrating them (which would be necessary for mass conservation), but disappearing out of the calculation as it is pushed against the blade surface by the flow. This will lead to severe tracer loss, so that the monitored tracer concentration will never reach the expected equilibrium value. (The extent of this loss depends on many factors, amongst them the size of the impeller.) If you really want to do the tracer transport simulation in the absolute frame of reference for the whole computational domain, proceed as follows: Before you start the unsteady simulation, create three custom field functions. Each of them should be defined to be identical to one of the velocity components (U, V, W). Now use "Solve--Initialize--Patch" to patch each of the velocity components in the complete domain (all fluid cell zones) using the corresponding custom field function. (Enable the button "Use Custom Field Function".) This should apparently exchange the current flow field by itself, i.e. change nothing. But as the custom field function will give the absolute velocities (NOT relative the any rotating frame of reference), this operation feeds the absolute velocity information into the solver's data fields, so that these data will be used for the transient tracer transport simulation. --- Remember to switch of the solution of the Flow (and turbulence) equation at the very beginning! |
||
|