Messages

46

Fluent / Re: What are the requirements for an axisymmetric analysis?

« on: May 13, 2012, 11:22:18 AM »

Axisymmetric indicates that the domain is axisymmetric about the x axis. When Axisymmetric is enabled, the 2D axisymmetric form of the governing equations is solved instead of the 2D Cartesian form. (This option is available only when you start the 2D version of the solver.)

It is important to note that while the assumption of axisymmetry implies that there are no circumferential gradients in the flow, there may still be non-zero swirl velocities.

For axisymmetric, the axial direction should be x and radial is positive y. Even if the y starts with -1e-32, it will fail.

Do a Mesh->Check to make sure you don't get

Checking for nodes that lie below the x-axis.
WARNING: Invalid axisymmetric mesh: 6 nodes lie below the x-axis.

and
WARNING: Mesh check failed.

If you do,

Use Mesh->Translate and move the geometry so ymin is +ve.

Be sure to change the zone type of the axis of rotation to "axis" and not symmetry, using the Boundary Conditions task page.

47

Fluent / Re: VOF to model draining tank, swirling fluid, vortex?

« on: May 13, 2012, 11:18:41 AM »

Use pressure inlet to maintain the tank pressure (otherwise the assumption of incompressibility in FLUENT is violated, and one gets pockets of gas in the liquid). Use a custom Field Function to set
up an initial swirl velocity.
Use velocity inlet as the boundary condition, with the direction vector pointing out of the tank, and with the volume fraction of liquid equal to unity.

48

Fluent / Re: Converge a VOF mold filling simulation

« on: May 13, 2012, 11:11:36 AM »

Converging VOF solutions may be challenging when the ratio of viscosity of the two fluids is far from 1.0.

Mold filling is a typical example of this problem. The injected material may have a viscosity a few orders of magnitude greater than that of the fluid being displaced (air, for example).

Suggested strategies are provided in the resolution below.
1) Increase the air viscosity such that ratio is about 1e+3 to 1e+4. This is an approximation and should be done with a great care.

Due to high viscosity and density of mold as compared to air, the effect of this change in property of air would not significantly affect the mold flow which is of primary interest. The improvement of convergence is significant while the approximation typically results in negligible loss of fidelity.

2) Mark one or two cells at the inlet and patch the fill material VOF to 1.0 in these cells. This provides the fill material with an easy entry to the mold and will help the simulation get off to a stable start.

3) If step 2 does not resolve the convergence problem at the start, then try enabling "Solve VOF every iteration" from the Multiphase Model panel and keep this enabled for a few time steps. Once the case shows good convergence, disable this selection.

4) A low time step is necessary at the start of the simulation. This can be increased gradually to a value where solution does not go unstable.

5) Set PISO for pressure - velocity coupling. Use PRESTO! for pressure discretization.

6) With PISO scheme, higher URFs can be used. However, for this class of problems, momentum URF should be less than 0.5. A value 0.2 to 0.4 can be selected based on the stability of solution.

49

Fluent / Re: UDF to compute the internal circulation in a bubble using VOF

« on: May 13, 2012, 11:08:19 AM »

Here you go:

1) Get the converged solution
2) The define on demand function below computes the velocity of the centroid of the bubble (and also the coordinates of the centroid).
3) The velocity vectors are modified depending upon this velocities.
Note: If you save this case file after executing the udf, then you will lose the actual velocity data. So make sure you have the original data securely saved.
**************************************************************************
* Udf to compute the velocity of the centroid of the bubble
* change the absolute velocity field to velocity field relative to
* the centroid of the bubble
* Written by Suman Basu of Fluent India
**************************************************************************/

#include "udf.h"

DEFINE_ON_DEMAND(move_with_bubble)
{
int phase_domain_index;
real vel_sum[ND_ND],co_ord1[ND_ND],co_ord[ND_ND],volume,average_velocity[ND_ND],x[ND_ND];
cell_t cell;
Thread *cell_thread;
Domain *subdomain,*mixture_domain=Get_Domain(1);
NV_S(vel_sum,=,0.);
NV_S(co_ord,=,0.);
volume=0.;
NV_S( average_velocity,=,0.);
NV_S(co_ord1,=,0.);
/* loop over all subdomains (phases) in the superdomain (mixture) */
sub_domain_loop(subdomain, mixture_domain, phase_domain_index)
{
/* loop if secondary phase */
if (DOMAIN_ID(subdomain) == 3)
/* loop over all cell threads in the secondary phase domain */
{
thread_loop_c (cell_thread,subdomain)
{
/* loop over all cells in secondary phase cell threads */
begin_c_loop(cell,cell_thread)
{
C_CENTROID(x,cell,cell_thread);
co_ord[0]+=C_VOF(cell,cell_thread)*C_VOLUME(cell,cell_thread)*x[0];
co_ord[1]+=C_VOF(cell,cell_thread)*C_VOLUME(cell,cell_thread)*x[1];
vel_sum[0]+= C_VOF(cell,cell_thread)*C_VOLUME(cell,cell_thread)*C_U(cell,cell_thread);
vel_sum[1]+= C_VOF(cell,cell_thread)*C_VOLUME(cell,cell_thread)*C_V(cell,cell_thread);
volume+=C_VOF(cell,cell_thread)*C_VOLUME(cell,cell_thread);
}
end_c_loop(cell,cell_thread)
}
}
}
NV_VS(co_ord1,=,co_ord,/,volume);
NV_VS(average_velocity,=,vel_sum,/,volume);
Message("Centroid[0]=%f\nCentroid[1]=%f\n",co_ord1[0],co_ord1[1]);
Message("V_Centroid[0]=%f\nV_Centroid[1]=%f\n",average_velocity[0],average_velocity[1]);

thread_loop_c (cell_thread,mixture_domain)
{
begin_c_loop(cell,cell_thread)
{
C_U(cell,cell_thread)=C_U(cell,cell_thread)-average_velocity[0];
C_V(cell,cell_thread)=C_V(cell,cell_thread)-average_velocity[1];
}
end_c_loop(cell,cell_thread)
}

}

50

Fluent / Re: How to plot the velocity vectors inside one particular phase in VOF simulation?

« on: May 13, 2012, 11:05:19 AM »

FLUENT solves single momentum equation for mixture only and resulting velocity field is shared among the phases. Hence, the vectors are plotted for all the phases at the same time.
Following steps can be used to show the velocity vectors for a particular phase in a two phase system.
1. Create a Custom field function (CFF), vx_phase1 = X velocity * Volume fraction of particular phase using Define --> Custom Field Function panel.

As Volume fraction will be 1 inside the phase and zero outside, vx_phase1 will have same value as vx inside phase and zero value outside.

2. Similarly, create the two more CFFs: vy_phase1 and vz_phase2.

3. Now, draw the custom vectors using vx_phase1, vy_phase1 and vz_phase1 as X and Y component of the custom vectors.

Please note that at the interface where volume fraction is between 0 and 1, the vectors may not be accurate.

51

Fluent / Re: VOF Courant number and Global Courant number in FLUENT

« on: May 13, 2012, 11:01:55 AM »

When ANSYS FLUENT performs a time-dependent VOF calculation, the time step used for the volume fraction calculation will not be the same as the time step used for the rest of the transport equations. ANSYS FLUENT will refine the time step for VOF automatically, based on your input for the maximum Courant Number(C) allowed near the free surface. In Variable time stepping method, FLUENT will refine the time step for transport equations, based on your input for the Global courant number (CFLglobal). In fixed time stepping method, Global courant number varies and it is printed in the Fluent console window at every time step.

Courant number:

The Courant number(C) is a dimensionless number that compares the time step in the VOF calculation to the characteristic time of transit of a fluid element across a control volume:

C = ∆t / ∆tchar (1)

Where ∆t is the time step size used for the VOF calculations, and ∆tchar is the Characteristic time.

In the region near the fluid interface, ANSYS FLUENT calculates the ratio of cell volume over the net outgoing volume flow rate from each cell, which represents the time it would take for the fluid to empty out of the cell. The smallest such time is used as the characteristic time, i.e.,

∆tchar = Min[cell volume/Σ(volume flow rate on each cell face) ]
= Min (∆xcell/νfluid) (2)

Based upon this characteristic time and your input for the maximum allowed Courant Number (C) in the Multiphase models panel, a time step (∆t )is computed for use in the VOF calculation.

VOF time step , ∆t = C ∆tchar (3)

For example, if the maximum allowed Courant number is 0.25 (the default), the time step will be chosen to be at most one-fourth the minimum transit time for any cell near the interface.

Global Courant number:
The Global Courant number(CFLglobal) is a dimensionless number that compares the time step in the transport equations to the characteristic time of transit of a fluid element across a control volume:

CFLglobal = ∆tglobal / ∆tchar (4)

Where ∆t global is the global time step size used for the transport equations, and ∆tchar is the Characteristic time.

Based upon this characteristic time and your input for the maximum allowed Global Courant Number (CFLglobal) in the Variable time stepping panel, a time step (∆t global) is computed for use in the transport equation calculation.

Global time step, ∆tglobal = CFLglobal ∆tchar (5)

The Global Courant number and Courant number can be related in the following manner:

CFLglobal = C ∆tglobal / ∆t (6)

Number of VOF sub time steps = ∆tglobal / ∆t = CFLglobal / C (7)

The default value of the Global Courant number is 2, but smaller value may be required for more accurate solution and more stable numerical calculation.



Note: ∆ stands for delta.

52

Fluent / Re: VOF: How do I plot the interface between two phases?

« on: May 13, 2012, 10:55:36 AM »

In FLUENT, you can contours

In CFD-POST:

Assuming that the VOF problem involves water and air, you first create a surface at the interface using Insert->Location->Isosurface. The variable would be Water.Volume Fraction and the value is 0.5.

The isosurface can be seen in the viewer. The function calculator may be used for evaluating quantities on this surface.

A curve may be created based on the intersection on the isosurface and a boundary. Use Insert->Location->Polyline. For Method, select Boundary Intersection. Select the desired boundary surface and the isosurface. The polyline can now be used as a locater in an expression, or can be used for charting, or can be exported via a .csv file.

53

Fluent / Re: How can I access Compressive VOF scheme in Fluent 12?

« on: May 13, 2012, 10:53:19 AM »

This is a beta feature available in F12. To enable this, type the following command in the Fluent console window:

define/beta-feature-access

Type yes for the prompt

Please note that in addition to this, many other features will also be turned on.

The Compressive scheme will be available in the Volume fraction discretization drop-down list.

54

CFX / Re: How do I setup a simulation in CFX 10.0 with R134a?

« on: May 13, 2012, 10:50:23 AM »

R134 is just a material which we support with RGP files and with the Redlich Kwong equation of state.
Thus it should be fairly simple to set up a simulation using R134.

However there are a few things you should be aware of:
If you are not doing phase change or the operating range of the device is at low enough pressure (or high enough temperature) you may not need to use Redlich Kwong or an RGP file. Specifying an Ideal Gas may be good enough.


If you need to do phase change (condensation) then R-134 calculations are setup exactly the same as for steam, other than picking the different materials of course.
For R-134 though we only have the Redlich Kwong EOS. The RGP files are for R134a.

It is worth noting that if you are modelling boiling/evaporation/non-equilibrium then condensation is a bit trickier.
All the real gas properties are currently only setup for equilibrium condensation modelling.

55

CFX / Re: Error: mpirun_mpid version mismatch

« on: May 13, 2012, 10:47:32 AM »

CFX Distributed Parallel in ANSYS CFX 13 uses HP-MPI while CFX Distributed Parallel in ANSYS CFX 14 uses PCMPI. These different installations of MPI can have a conflict when installed on the same Windows machine. To avoid such a conflict, be sure to follow the installation instructions that appear during Platform MPI installation. "

The only workaround is to unset or delete MPI_ROOT. This should allow CFX-13.0 and CFX-14.0 to run independently.


To Remove this Variable

Open up Control Panel > System > Advanced > Environment Variables. The MPI_ROOT will be in the System Variables. Delete this variable.

56

Fluent / Re: How to specify velocity-inlet to interior faces types?

« on: May 12, 2012, 02:50:16 PM »

-Define -> Boundary Condition

-Select interior-5 under Zone

-Select wall on the right column under Type
-Click on Yes to change the type.

-two internal walls will be created, wall-5 and wall-5-shadow. ID of wall-5 will be the same as the ID of interior-5. These two new walls with be Coupled by default and the available types for them are fan, interior, porous-jump, radiator, and wall. We don't have velocity-inlet type for internal wall. In order to have types that can be applied on external zones, they need to be split.

-In text user interface (TUI), type: /grid/modify-zones/slit-face-zone wall-5. Two additional walls will be created: wall-5, and wall-###. It will print on the cortex window of Fluent to find out which zone is wall-###. These are two external zones, one is adjacent to fluid-1 and the other is facing fluid-2. To have the fluid entering the pipe, the one which is adjacent to fluid-1 needs to be changed to velocity-inlet type. To find which one is adjacent to fluid-1, you need to visit the boundary condition panel for that zone and look under 'Adjacent Cell Zone'.

-Repeat the above procedure to apply pressure-oulet to interior-6.

57

Meshing / Re: How to create a helical pipe/coil in Gambit?

« on: May 12, 2012, 01:56:47 PM »

Helical coil is often used in mixing tanks or other applications. How to quickly create such structure in Gambit is a frequently asked question.

Attached file is a journal file, which shows how to create helical pipe in Gambit 2.1. Please save that file in your gambit working directory
as "helical.jou".
(1) Open gambit and go to the File/Run Journal panel, pick up "edit and run" option and pick up the file just saved. Click "Accept" to open that
journal file.
(2) Move mouse cursor to the file text area, right click the mouse button, a drop-down panel will show and choose "Select all" option.
(3) Click "Step" option" on the screen and run journal file step by step. You will see how a helical geometry is created.

The basic procedure includes:

(1) create cylinder tank.
(2) create three vertices and create two edges using those vertices.
(3) create a flat helical face using twist sweep option.
(4) create a small circle, which will be the pipe cut plane. And move it to the right location.
(5) Sweep that small circle along with the outer edge of the flat helical face.
(6) delete the flat helical face.
(7) do splitting if necessary.

---------------------Gambit 2.1 journal file----------------------------

volume create height 3 radius1 1 radius3 1 offset 0 0 1.5 zaxis frustum
vertex create coordinates 0 0 -1
vertex create coordinates 0 0 4
vertex create coordinates 0.8 0 -1
edge create straight "vertex.3" "vertex.5"
edge create straight "vertex.3" "vertex.4"
face create rotate "edge.3" onedge "edge.4" twist 3600
face create radius 0.1 zxplane circle
face move "face.5" offset 0.8 0 -1
volume create rotate "face.5" onedge "edge.6" draft 0 extended
face delete "face.4" lowertopology
volume split "volume.1" volumes "volume.2" connected
window modify shade
window modify volume "volume.1" invisible
window modify visible
window modify noshade

58

Fluent / Re: What are the flow iterations per radiation iteration?

« on: May 12, 2012, 12:57:48 PM »

They refer to the number of Flow Iterations per Radiation Iteration. If the RTE (radiation transfer equation) has a slower rate of convergence the number of Flow Iterations per Radiation Iteration should be decreased to 1 or 2.

59

Fluent / Re: How big should be the domain for an automotive external aerodynamics calculation

« on: May 12, 2012, 12:13:13 PM »

To replicate a wind tunnel test, you are obviously limited to the physical size of the wind tunnel lateral to the car. It is suggested to have at least two body-lengths upstream of the car for the inflow boundary and three body-lengths downstream of the car for the outflow boundary. As always, more is better, but it is not always cost-effective.

To replicate the vehicle on the open road, you can use the old rule-of-thumb from the wind tunnel testing of using a solid blockage of .5%. For example, the projected area of your car should be .5% of the total area of the inflow plane.

60

Fluent / Re: Mass flow rate of a chemical species not equal to product mass fraction

« on: May 12, 2012, 12:08:23 PM »

The net mass flow rate of a species at an inlet boundary includes contributions from both convection and diffusion. The convection component is determined from your input of species concentration while the diffusion component is calculated by FLUENT.