When using one of the Reynolds Stress turbulence models the CFX Solver can sometimes fail in the first few iterations. What's the best way to initialize a simulation when using these models? |
<br>The Reynolds Stress models (which include: k epsilon EARSM, BSL, BSL EARSM, BSL Reynolds Stress, SSG Reynolds Stress, LRR Reynolds Stress, QI Reynolds Stress and Omega Reynolds Stress)... |
Why does the user receive the following error message when trying to run the CEsetup?
Workbench was installed on the machine prior to running the CE setup.
ERROR MESSAGE
RSM
Exception occurred while initializing the installation:
System.IO.FileNotFoundException: File or assembly name Ansys, or one of its
dependencies, was not found.
OK
After the user clicked okay, it uninstalled itself. |
In this particular case, it turned out to be a bad IIS installation.<br>Reinstalling IIS should resolve the problem.
|
Remote Solution Web Server WebPage shows text only, as if it were a notepad document rather than a web-based menu system.
Also, when you go to the webpage, it seems to be already logged in and you can not click on 'Log out'
What could be the problem? |
This is an IIS/.net installation order problem.<br> IIS has to be installed first. Then .net is to be installed.<br> If not, the user will have to... |
How can I avoid extinction occurring in my combusting flow calculations so that i just get a cold flow solution? |
<br>Most combustion models have flame extinction options that prevent reaction occurring if conditions are not right for combustion. It is therefore important to choose initial conditions... |
We've been running quite some time with the standard CFX version where our real gas properties are prescribed in a RGP file.
This ran fine in CFX5.7.1. Now we started to use CFX10 using the same files and suddenly CFX cannot calculate the temperature field anymore (and hence density, and all temperature related variables). |
<br>A change in thedefault interpolation of tabulated thermodynamic data from 5.7 to 10 caused a lack of proper data for critical and triple point values to be crucial. The RGP data is... |
SYMPTOM:
When trying to create a User Function in CFX-Pre, the Argument Units widget appears to be disabled and I can't type anything into it. The Result Units widget works fine.
PROBLEM:
This is a minor bug in the CFX-Pre GUI initialization file. |
WORKAROUND:<br>You can edit the file 'CFXPreGui.ccl' in your CFX installation (located in the /etc directory). Simply change the following section:<br><br> ... |
.: I would make a contour plot that dissects a region. Is it possible to put contour plots onto slice planes? |
Yes, this is possible. Assuming you are using the latest CFX-10, all you need to do is create the plane (or planes) that you want, but turn off the visibility and click 'apply'. Then... |
SYMPTOM:
A multi-domain case that contains Fluid, Solid and Porous Domains fails in the solver with the following error:
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine DEF_ALGM_ZIF |
PROBLEM:
This error is generated because one or more Domain Interfaces are defined with an invalid Connection Type. For Fluid-Porous, Solid-Porous and Porous-Porous Domain Interfaces the Connection Type must be GGI. However, when these types of Domain Interfaces are generated automatically by CFX-Pre, for example when the Definition File is written, those found with matching grids are incorrectly given an Automatic (1:1) Connection Type. |
WORKAROUND:<br>Check all Porous Domain Interfaces and modify those with an incorrect Connection Type by editing the CCL. Note that modifying the Connection Type in the GUI may still produce... |
Q
I have set up a problem in which the flow is buoyant and a gravity vector is specified. I would like to know whether this setting in the domain will automatically apply gravity to my particles, or whether some other setting is required.
A
To apply gravity to the particles you need to do two things:
1. define the flow as buoyant with a gravity vector, e.g.
DOMAIN: Domain 1
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = 0 [m s^-2]
Gravity Z Component = -9.8 [m s^-2]
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Option = Automatic
END
END
DOMAIN MOTION:
Option = Stationary
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
2. set the buoyancy for the particle phase, e.g.
FLUID: Aluminium
FLUID MODELS:
FLUID BUOYANCY MODEL:
Option = Density Difference
END
MORPHOLOGY:
Option = Dispersed Particle Transport Solid
PARTICLE DIAMETER DISTRIBUTION:
Diameter = 0.001 [m]
Option = Specified Diameter
ENDEND
END
END |
Q<br>I have set up a problem in which the flow is buoyant and a gravity vector is specified. I would like to know whether this setting in the domain will automatically apply gravity to my... |
Q
I have doubts about specifying sources of 'additional variable'. For example, I have to implement following equation
D(phi)/Dt = S_phi
where phi is dimensionless. Therefore units of source term S_phi are s^-1. However when I implemented additional variable as
ADDITIONAL VARIABLE: ICVariance
Option = Definition
Units = [ ]
Variable Type = Specific
END
the units of sources need to be implemented are [kg m-3 s-1]. Do I need to multiply the source terms Rpi and RDi with density? And what is the difference between specification of 'additional Variable' Volumetric or Specific.
A
Looking at the transient term and source only, for specific AVs the transport equation is
d(rho.phi)/dt = S_phi (1)
and for volumetric AVs it is
d(phi)/dt = S_phi (2)
It might be expected that a dimensionless specific AV should have units of kg^-1, and a dimensionless volumetric AV, m^-3. However, dimensionless AVs are exactly that (dimensionless) and have dimensions [ ]. From (1) and (2) we therefore see that for dimensionless, specific AVs sources are in units of kg m^-3 s^-1, whilst for volumetric AVs, they are s^-1.
So, to return to your original question, you should multiply your source terms by density. |
Q<br>I have doubts about specifying sources of ¿additional variable¿. For example, I have to implement following equation<br><br>D(phi)/Dt =... |
Q
I would like to define a problem with static pressures at the inlet and outlet, but the Help Manual suggests that this does not appear to a sensible thing to do.
A
The advice in the manual is sound; setting static pressures at the inlet and outlet may well give convergence problems. You may however find that it is possible to converge such a set-up, in which case there is nothing physically wrong with the model.
If you can specify the inlet condition in terms of a total pressure (i.e. static pressure + rho.U^2/2) then convergence behaviour is likely to be much better.
A useful trick may be to use a total pressure inlet, but set the inlet total pressure using CFX Expression Language (CEL) to be your required static pressure plus rho.U^2/2. Please note that this definition of total pressure is valid only for fluids of constant density, e.g. liquids and low-speed gas flows.
Below is the CCL/CEL that is needed to do this:
LIBRARY:
CEL:
EXPRESSIONS:
pstat in = 5 [Pa]
vel in = massFlow()@INLET /
(Water.density * area()@INLET)
ptot in = pstat in + 0.5*Water.density*vel in^2
END
END
END
FLOW:
DOMAIN: Domain 1
BOUNDARY: INLET
Boundary Type = INLET
Location = INLET
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
ENDFLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Total Pressure
Relative Pressure = ptot in
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
END
END
In this case pstat in is the required inlet static pressure, which the user should specify. vel in is the inlet velocity, calculated as part of the solution from the current mass flow at the inlet, the inlet area and the density. Finally, the inlet total pressure, ptot in, is calculated from the sum of the specified inlet static pressure an |
Q<br>I would like to define a problem with static pressures at the inlet and outlet, but the Help Manual suggests that this does not appear to a sensible thing to... |
Q
I am trying to solve two-phase flow equations together with transport equations for two additional variables. The continuity equations have a source term, which depends on the additional variable. I know I have to set velocity components when I set the source term, but it makes no sense to me. How am I supposed to choose values for velocity components? Can I just set something arbitrarily or shall I choose initial values/values at the inlet?
A
I presume that when you say the continuity equations have a source term you mean that you are setting something under Fluid Sources on a subdomain.
If this is the case then the velocity must be that which is associated with the mass being transferred. If you add mass to a phase, then it must have properties associated with it, such as temperature, velocity, composition. For a sink term (i.e. removing mass from a phase) you are presented with Sink Option, which allows you to specify how the value of temperature or mass fraction is to be specified (this is useful for example if you have a multicomponent mixture in which not all components are evaporating at the same rate). For source terms however you have to specify the values explicitly. If you are transferring mass from the other phase, then it may be appropriate to set the velocities equal to those of the other phase, e.g. if your phases are Air at 25 C and Water, you might have a source term as follows:
FLOW:
DOMAIN:Domain 1
SUBDOMAIN:Subdomain 1
Coord Frame = Coord 0
Location = Assembly
FLUID:Air at 25 C
SOURCES:
EQUATION SOURCE:continuity
Option = Fluid Mass Source
Source = 0.1 [kg m^-3 s^-1]
VARIABLE:velOption = Cartesian Vector Components
xValue = Water.Velocity u
yValue = Water.Velocity v
zValue = Water.Velocity u
END
END
END
END
END
END
END
To sum up, you can't create mass out of nothing, |
Q<br>I am trying to solve two-phase flow equations together with transport equations for two additional variables. The continuity equations have a source term, which depends on the... |
How can I set a defined pressure drop in a subdomain? |
<br>You need to set momentum sinks in the subdomain to represent the pressure loss. The units of the momentum sink are N/m^3, which is equivalent to N/m^2/m = Pa/m i.e. pressure gradient,... |
Q
How within CFX-Post can one perform a circumferential average along a circular line of specified radius and at a specified height in a mixing vessel.
A
There are two ways of doing this. One would be to create a Polyline by importing From File, and then use the lengthAve option in the Function Calculator.
The other way, which does not involve creating a data file to import and which is done entirely within CFX-Post, is as follows:
1. create a new Variable called RADIUS which is the radius (e.g. sqrt(X*X+Y*Y) if the circle is to lie in the X-Y plane)
2. create a Plane on which the circle is to lie (e.g. the X-Y plane)
3. now create a Contour and plot RADIUS on this plane
4. create a Polyline using method From Contour, and choose the appropriate Contour Name (the contour created in 3.). Choose the Contour Level that you want
5. use the Function Calculator to give lengthAve on Polyline 1 of the variable in which you are interested. |
Q<br>How within CFX-Post can one perform a circumferential average along a circular line of specified radius and at a specified height in a mixing vessel.<br><br>A<br>There... |
Q
How can swirl be represented at an inlet which is very small compared to the overall domain, i.e. without meshing the inlet in detail?
A
There are three solutions to the problem you describe:
1. Explicitly mesh the swirler inlets in your model. This can be expensive computationally if the inlets are very small compared to the size of the room or if there are a large number of inlets. Care needs to be taken that the mesh is sufficiently fine to resolve any important variations in the flow.
2. Perform a detailed simulation of the inlet in isolation (i.e. in a surrounding box with pressure boundaries all around) from which the velocity profile on the pressure boundary could be exported. This could then be applied as a specified-velocity inlet boundary condition on the coarser mesh of the whole domain. Depending on the location chosen for the surface surrounding the detailed simulation there may be inflow (entrainment) into the inlet region. In this case the boundary condition should be of type Opening, to allow flow both to enter and leave the domain through the surface surrounding the inlet.
3. The third option is essentially the same as Option 2, except that rather than perform a detailed CFD simulation of the inlet to give the boundary conditions for the coarser mesh, experimental data may be used to specify the velocity profile. |
Q<br>How can swirl be represented at an inlet which is very small compared to the overall domain, i.e. without meshing the inlet in detail?<br><br>A<br>There are three... |
Q
I'm trying to plot the value of vorticity behind an impeller blade in CFX-5.7.1. I was able to output Vorticity by editing the CEL file, but I found that there is a big "jump" in vorticity values across the rotating frame interface. Is this due to vorticity being defined by velocity gradients rather than stationary frame velocity gradients? Is there a way to get consistent values of vorticity accross the interface?
A
The problem is due to the vorticity being calculated using local-frame velocities. However, there is a variable, vortstn, which is vorticity in the stationary frame. To include this, you should add the following lines to your CCL:
LIBRARY:
VARIABLE: vortstn
Output to Postprocessor = Yes
END
END
You should then find that this is available in CFX-Post. |
Q<br>I'm trying to plot the value of vorticity behind an impeller blade in CFX-5.7.1. I was able to output Vorticity by editing the CEL file, but I found that there is a big... |
Can't open DSDB file in 32bit WB 10.0 after it was saved in WB 10.0 64bit Beta. Why? |
The 64bit Workbench 10.0 Beta is saving the .dsdb file as a new version version .dsdb file.<br>Just as you can not read a WB 10.0 .dsdb into WB 9.0.
|
I need to find out the force exerted on an internal wall by the fluid.
Could you explain how the "force" is calculated? For example, for a coordinate-aligned wall, the area integration of pressure should equal the force normal to the wall? I checked but "areaInt(Pressure)@Face" does not seem to equal "force_x()@Face". |
<br><br>There are different methods to get a result for the force on a wall, internal or external. They should all give similar results, but there will be slight differences as they... |
How to freeze the motion of a rotating domain while post processing a transient rotor-stator (TRS) simulaiton? |
set the CFXPOST_IGNORE_DOMAIN_TRANSFORM environment variable (it doesn't matter to what value, it just needs to exist).<br><br>After this environment variable is created, the... |
Q: We have had an annoying problem with ICEM CFD 10.0 when creating blocks
from vertices/points or by extruding. Sometimes the block which is
created disappears from view immediately after creation. However, when
ICEM or Workbench (if ICEM is run from there) is restarted, the block is there.
This is extremely annoying if it happens with every second block and you
have to restart the software all the time. Do you know how to correct this?
Please note that all the parts are visible when this happens so this should not be
due to creating blocks into invisible parts.
A) This happens because the new block created changes the index of block.
That is, if the range of blocks is 2x4x6, say, Hexa shows by default, the range of 2x4x6 blocks.
This index allows you to hide some of the blocks and work on specific regions of blocks, which can be useful for a very complex geometry and blocking.
When you create a block outside this original range, i.e. extend from one side of the geometry outwards to make the range 2x4x7, Hexa keeps the original range visible and this is why you cannot see the new block.
To get around this problem, right click on Blocking, click on Index Control and click the reset button. This should then show the whole range.
Please also note that the same thing happens if you make an o-grid inside another o-grid. The block range will then be 2x4x6 - x2 (o-grid direction), but will only show one o-grid direction block and therefore the second o-grid will appear to disappear. Again, Reset will fix this problem. |
Q: We have had an annoying problem with ICEM CFD 10.0 when creating blocks<br>from vertices/points or by extruding. Sometimes the block which is<br>created disappears from view... |
Q: How can I use the CEL in CFX 10.0 to specify the
value of a parameter over a range; e.g. different temperatures for
different values of "xGlobal":
T = 10 [C] for xGlobal = 0 [m] to xGlobal = 1 [m]
T = 50 [C] for xGlobal = 1 [m] to xGlobal = 2 [m]
T = 55 [C] for xGlobal = 2 [m] to xGlobal = 3 [m]
...and so on...
A) You should use the step function for this.
The step function works as follows:
Step(x)=1, if x>0
Step(x)=0.5, if x=0
Step(x)=0, if x<0
Therefore, to write the below you would need:
xbar=x/1.0 [m]
T1=10 [K]
T2=50 [K]
T3=55 [K]
T = T1*step(1-xbar)+T2*step(2-xbar)*(step(xbar-1)+ T3*step(3-xbar)*(step(xbar-2). |
Q: How can I use the CEL in CFX 10.0 to specify the<br>value of a parameter over a range; e.g. different temperatures for<br>different values of... |
In the DOE mode, it takes ~15s to change from normal to Gaussian, for example.
To make any change, it just takes a lot of time.
It does not take any CPU power when it is "thinking." When switching to Monte Carlo simulation, it is all very fast and normal.
What is the cause of this? |
In a DOE, we generate a matrix of design points. When we are finished solving each of these design points, we fit the solution using a quadratic response surface. Monte-Carlo does not generate a... |
How to define mesh displacement as a function of the original mesh?
Mesh displacement is defined relative to the original, undeformed mesh. When the mesh displacement shall be a function of the coordinates of the original mesh, then this is not straightforward, as the original coordinates are not available to the user in CEL. |
The original coordinates can be recomputed by using an expression like:<br><br>(x-Total Mesh Displacement x)<br><br>and this expression can be used to define the mesh... |
I have installed Workbench 10 and ICEM CFD 10 on a Windows XP machine and this went fine. However when I try to proceed to Advanced Meshing in Workbench 10 I get the following pop-up:
Windows Security Alert
To help protect your computer, Windows Firewall has blocked some features of this program.
Your computer administrator can unblock this program for you.
Name: ICEM Tck/Tk Interpretor
Publisher: ICEM CFD Engineering |
ICEM Tcl/Tk Interpretor is related to the executable med.exe (part of ICEM) so allowing med.exe through the firewall will solve this problem.
|
Class 3 Error
SYMPTOM:
If a mass source is used in a multi-component flow with heat transfer, then the associated energy source term in the enthalpy equation is calculated incorrectly, giving incorrect answers.
PROBLEM:
There is a coding error in the calculation of the energy source term due to a switch to using conservative mass fractions in the mixture enthalpy |
WORKAROUND:<br>Using the expert parameter setting 'masfrn for mixture enthalpy = t' will avoid the problem in most circumstances, including the EDM/FRC combustion models, but... |