solution techniques 2 l.
Skip this Video
Loading SlideShow in 5 Seconds..
Solution Techniques - 2 PowerPoint Presentation
Download Presentation
Solution Techniques - 2

Loading in 2 Seconds...

play fullscreen
1 / 30

Solution Techniques - 2 - PowerPoint PPT Presentation

  • Uploaded on

Solution Techniques - 2. Solver Options. As discussed in the last lecture Fluent has an unsteady solver and steady solver options The unsteady solver is used for dynamic simulations where you are integrating in time

I am the owner, or an agent authorized to act on behalf of the owner, of the copyrighted work described.
Download Presentation

PowerPoint Slideshow about 'Solution Techniques - 2' - Antony

An Image/Link below is provided (as is) to download presentation

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.

- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -
Presentation Transcript
solver options
Solver Options
  • As discussed in the last lecture Fluent has an unsteady solver and steady solver options
  • The unsteady solver is used for dynamic simulations where you are integrating in time
  • The steady solver is designed to get to get a steady flow or time averaged steady flow solution
solver options3
Solver Options
  • Both steady and unsteady can be used with the segregated solver or the coupled solver.
  • The segregated solver solves the equation set sequentially
  • The coupled solver solves the equation set in one go. This is the more “modern” solver but consumes more memory
my experiences
My experiences
  • The segregated solver is the default option. For most purposes this is good enough. Ive never had to use the coupled solver
  • I am of the view that you should think more about the possible transient aspects of the problem and worry about steady vs unsteady rather than segregated vs coupled
  • Inevitably any iterative/numerical solution procedure will only give a solution which is “converged” relative to some criteria
  • The solution may be converged if:
    • All discretized transport equations are obeyed to a specified tolerance defined by Fluent’s residuals (but these may be too large)
    • The solution no longer changes with more iterations (but the problem may be stuck)
    • Overall balances close (for a steady flow simulation)
  • Convergence is not the same as accuracy. The solution is accurate if it matches experimental data (which you obviously need to make the judgement)
  • Thus there are qualitative and quantitative aspects to convergence.
convergence residual plots
Convergence - Residual Plots
  • Fluent keeps track of the residuals throughout the iteration. The default value of these is 1.0e-3.(except for enthalpy - 1.0e-6 and species transport 1.0e-5) You should plot these.
    • Solve-> Monitors -> Residuals -> Plot
  • The residual plots show when the residuals have reached a specified tolerance
  • They can show which equations are having convergence problems, though this is sometimes difficult and there are other ways finding this out - see multigrid verbose
  • The residuals measure the imbalance on conservation equations
convergence residual plots8
Convergence - Residual Plots
  • Residuals are not the full story
  • For some flow problems the default values are too large
  • In my cyclone studies the solution appears to be converged on some grids but the pressure profile is unrealistic, This can only be resolved by a transient solution and even then the change in the residuals during the iteration is not much.
  • Some problems will display no apparent change in residuals but the solution may be doing the right thing from other criteria - my gravity sluice
  • Some flow problems display periodic convergence behaviour - don’t jump the gun!!!
  • You can also monitor Lift, drag or momentum or variables at points surfaces or boundaries
    • Solve -> Monitors -> Force
    • Solve -> Monitors -> Surface
  • When these values stop changing the solution may be converged
  • Check overall heat and mass balances if the problem has a defined flow volume
accelerating convergence
Accelerating convergence
  • My opinion is that if the solution is converging then leave it alone
  • Remember the equation set is non-linear
  • All numerical approaches to solving non-linear equations estimate a new solution estimate using some gradient of the solution at the current solution estimate.
  • If the gradient is large then the new estimate may be worse than the old estimate and the solution may diverge. This will tend to happen at the beginning of the iteration.
  • Accelerating convergence generally increases the likelyhood of divergence happening
under relaxation
  • If you really must fiddle then you can:
    • Increase under relaxation factors
    • under-relaxation factors slow down the rate at which the solution changes during the iteration
    • and in transient solutions increase the Courant number:
    • Courant number is the ratio of a time step to a cell residence time
courant number
Courant number
  • This specifies a maximum internal time step the solver may take during the time integration and is not the same as the time step of the simulation
  • The time step of the integration is used to calculate a final time in a numerical integration.
  • A numerical integration will take steps in time ti. which are less than ts.
  • The Courant number specifies a maximum value of ti.
supply initial conditions from a previous solution
Supply Initial Conditions from a previous solution
  • This is a good approach if the new solution is close to a previous solution and is useful if you need a family of solutions over a range of flows
  • You can also start with a solution using a simpler turbulence model or a solution which is otherwise a subset of the problem
  • Get an approximation using lower order discretization
  • The solvers use a methodology where the grid is coarsened by merging several neighbouring control volumes into one volume and an approximate solution is obtained for the coarser grid that is applied as a starting point to your grid
  • The solver does this automatically but you can adjust the parameters
grid independence
Grid Independence
  • Finer grids are more accurate but are usually less stable
  • Check your solution with more than one grid.
  • You can generate a finer grid using an existing grid by grid adaptation. This technique will be discussed in a later lecture
boundary conditions
Boundary Conditions
  • Any solution of a set of PDE’s requires a set of boundary conditions for closure
  • From a physical perspective you need to specify boundary conditions such an an inlet flow. However boundary conditions are required at all boundaries that surround the flow domain
  • For example a wall boundary condition specifies by zero velocity at the wall by default. If you are solving mass or heat transfer then you need to specify the boundary conditions for these variables either as a flux or boundary concentration
  • Fluent by default assumes a wall boundary condition unless you specify otherwise
boundary condition types
Boundary Condition Types
  • Flow inlet and outlet boundaries
  • Wall and repeating boundaries
  • Internal cell zones
  • Internal face boundaries
  • Define -> Boundary Conditions
    • Set boundary conditions
    • Change the type of boundary condition
flow inlet and outlet boundaries
Flow inlet and outlet boundaries
  • These specify boundaries conditions across which there is a flow
    • Velocity inlet
    • Mass flow inlet
    • Pressure inlet
    • Pressure outlet
    • Outflow
    • Pressure far-field
    • Inlet vent, outlet vent, Intake fan, exhaust fan
  • These are typically used for flow problems inside vessels or channels
mass flow inlet velocity inlet b c
Mass Flow inlet & Velocity inlet b.c.
  • The simplest inlet bc is the Mass Flow inlet
  • However you can also specify a velocity inlet bc with either a constant velocity or you can specify a velocity profile such a fully developed pipe flow profile
  • You also need to specify the turbulence if the flow in a turbulent problem
  • You will need at least one outlet bc (either Outflow or Pressure Outlet)
  • Fluent calculates the Pressure
pressure inlet b c
Pressure inlet b.c.
  • Alternatively you can specify the Pressure at the inlet and Fluent will calculate the flow
  • You still need to specify the turbulence
  • can be used for compressible and incompressible flow problems
  • can also be used to define a free boundary in an external or unconfined flow
  • Must be used in conjunction with a pressure outlet b.c.
pressure outlet b c
Pressure outlet b.c.
  • Here you specify the pressure at the outlet from the flow domain
  • However this b.c has backflow parameters allows for flow reversal. In this instance the b.c behaves like a pressure inlet b.c.
outflow b c
Outflow b.c.
  • This is used to model flow exits where details of flow velocity and pressure are not known before hand.
  • Fluent extrapolates from the interior
  • You can’t use this b.c. where
    • You have a pressure inlet b.c
    • The flow contains a density variation
    • the flow enters the domain (like a flow reversal)
    • gradients in the flow direction are significant
outflow b c multiple outlets
Outflow b.c. - multiple outlets
  • If you have multiple outflows you need to specify the flow split otherwise Fluent assumes that the flow is split equally
  • If you don’t know the flow split, or your aim is to predict the split, then you can’t use this b.c
  • Although you could use outlet b.c.s to get an initial estimate and change them to a Pressure b.c to accelerate convergence
pressure far field b c
Pressure far field b.c.
  • used to model a free stream condition at infinity (or a long way away)
  • Also called a characteristic b.c
  • used typically in aerodynamic applications such as flow around wings
vent and fan b c
Vent and fan b.c.
  • These are specialised b.c.s that model flows at vents and fans - see the documentation
wall boundary conditions
Wall boundary conditions
  • Obviously to model the boundary conditions at the vessel or channel walls
  • They are also used to bound fluid & solid regions(Fluent can solve heat transfer in solids)
  • Default is to assume zero velocity.
    • But you can specify the shear stress
    • This can be used to approximate a free surface
    • can also be used to model a momentum source
  • Also need to specify wall fluxes for heat and mass transfer. This is either as a temp, concentration or flux.
  • Walls can move. Moving boundaries, sliding meshes etc will be treated in a later lecture
repeating and periodic and symmetry b c s
Repeating and periodic and symmetry b.c.s
  • These are used when the flow geometry has some symmetry that enables you simplify the flow problem by solving a portion of the domain
symmetry b c
Symmetry b.c.
  • Used when the physical geometry and the flow filed has a mirror symmetry
  • At the symmetry plane the following must be satisfied
    • zero normal velocity
    • zero normal gradients of all variables
periodic b c
Periodic b.c.
  • These must be in pairs and they have to be set up correctly in Gambit
  • They also have to be physically identical
  • Here there is a symmetry but there is a flow normal to the b.c.
  • The flow field in at one b.c equals the flow field out at the other.
other boundary conditions
Other Boundary Conditions
  • Other Boundary conditions are axis, interrior and interface boundary conditions
  • You can also specify the fluuid type and whether the domain is fluid or solid via the bc panel