[分享]Frequently Asked Questions about STAR-CD

NASA · 发表于 2005-9-15 07:43

马上注册，结交更多好友，享用更多功能，让你轻松玩转社区。

您需要登录才可以下载或查看，没有账号？我要加入

x

What does the STAR in STAR-CD and STAR-HPC stand for?

How much memory do pro*am and STAR use?

What is the reference pressure?

How does the value of the reference pressure influence the analysis?

What happens to the reference pressure when there are multiple fluid streams?

What is the temperature datum?

How do velocity, density, temperature and the pressure field interact at INLET boundaries?

How do the various options for PRESSURE boundaries work?

How do velocity, density, temperature and the pressure field interact at PRESSURE boundaries?

What are the allowable boundary condition combinations in STAR?

How is the Intensity/Length Scale option for boundaries and initialization different from the KE/ED option?

What are good engineering practices for estimating turbulence values at boundaries?

How do I estimate my near wall cell thickness to get the correct y+ value for wall function turbulence modeling?

How do I judge whether a problem is converged?

In the SIMPLE algorithm what influences convergence?

What parameters are required to set up a buoyancy problem?

What are good practices to achieve convergence quickly?

How do I get convergence details in the .info file?

What do the various parameters in the .info file mean?

What are the units of the various fluid properties?

How can I calculate averaged quantities using PROSTAR?

How can I compute the mass flow rate in PROSTAR?

What are some recommended procedures for working with tetrahedral meshes?

NASA · 发表于 2005-9-15 07:44

· What does the STAR in STAR-CD and STAR-HPC stand for?
Simulation of Turbulence in Arbitrary Regions.
A little known historical fact is that other names were considered for the code before the name STAR-CD was chosen:
<UL type=disc>
<UL type=circle>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level2 lfo1; tab-stops: list 72.0pt">Regionwise Arbitrary Turbulence Simulation </LI>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level2 lfo1; tab-stops: list 72.0pt">Fully Arbitrary Regionwise Turbulence Simulation </LI></UL></UL>
 
However, these acronyms were, for unknown reasons, deemed unacceptable.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How much memory do pro*am and STAR use?
pro*am: Approximately 100 Mb per 500k cells.
STAR: Approximately 45 Mb per 100k hexahedral cells. Approximately 50 Mb per 100k trimmed cells mesh. Approximately 75 Mb per 100k tetrahedral cells.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What is the reference pressure?
The reference pressure is used to maximize the precision of calculated pressure gradients.
All pressure values stored in the .pst file and in internal arrays are stored relative to the reference pressure for each material type.
All input requested by the user interface for pressures will be relative to the reference pressure.
Calculations within the code that are dependent on absolute pressures use the stored relative pressure added to the reference pressure.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How does the value of the reference pressure influence the analysis?
o Models that contain no pressure boundaries:
Any fluid stream in a steady state analysis that contains no pressure boundaries will "pin" the pressure field such that the relative pressure at the pressure reference cell is identically zero. i.e. the absolute pressure at the pressure reference cell will be the reference pressure.
o Models that contain pressure boundaries:
Any fluid stream in a steady state analysis that does contain a pressure boundary or any transient analysis will not "pin" the pressure at the reference cell. However the pressure at the reference cell and all other cells is still stored relative to the reference pressure. i.e. the absolute pressure at the pressure reference cell will be the stored relative pressure plus the reference pressure.
<UL type=disc>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level1 lfo1; tab-stops: list 36.0pt">Back to FAQ list </LI></UL>
<UL type=disc>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level1 lfo1; tab-stops: list 36.0pt">
<HR align=center width="100%" SIZE=2>
</LI></UL>
· What happens to the reference pressure when there are multiple fluid streams?
If the fluid streams pass mass it is convenient that the value of the pressure reference be the same for each stream. 
For example, an explicit multiple reference frame problem is set up using separate material types. However, these separate fluid streams actually can pass mass back and forth. Using the same pressure reference value makes the continuity of the pressure field visible even when loading relative pressures. If the pressure reference values are different then continuity of the pressure field can only be observed by loading absolute pressures.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What is the temperature datum?
As with pressure, temperature is stored relative to a reference value. T-Datum is that value. However, unlike pressure, all references to temperature in the user interface are in absolute units (K). The only time the user is likely to encounter a relative temperature is in the user subroutines. The user should examine the "nom.inc" file to find out if the temperature arrays or values used in a user subroutine are absolute or relative.
The value of the temperature datum is also used during ISOBARIC analyses. In an isobaric analysis the user is supplying a Bulk Modulus for the variation of density with temperature and a baseline density. The code assumes that the baseline density exists at the datum temperature.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How do velocity, density, temperature and the pressure field interact at INLET boundaries?
o Incompressible flows: 
As rho is constant and equal to the fluid density, the value of rho specified at the inlet is ignored. The temperature value at the inlet is kept constant, which results in a constant mass flow entering the inlet.
o Compressible flows:
Two possible situations arise, namely subsonic flow and supersonic flow. The use of the fixed mass/fixed velocity switch in the inlet region definition only affects the inlet condition when it is subsonic.
§ Subsonic flow:
§ Flow switch set to "Fixed Mass Flow" (default):
This means that a constant mass flow will be maintained at the inlet. This is achieved as follows - the temperature value is kept constant at the specified value. The density value is evaluated at every iteration (using the Ideal Gas Law) and allowed to change if it differs from the supplied region value. This can happen if the inlet value for rho has been incorrectly estimated or the resulting flow field has a variable density.
The velocity is then adjusted based on the new values to conserve the mass flow. An additional option called the "Fixed Angle" determines whether the normal component of velocity is adjusted (Fixed Angle=Off) or whether all three components are adjusted but the original vector direction is maintained (Fixed Angle=On). 
§ Flow switch set to "Fixed Velocity":
This means that the specified inlet velocity will remain fixed. In this case temperature is again fixed at the given boundary value. Density is allowed to change based on the Ideal Gas Law and for the same reasons given above. The mass flow is then adjusted based on continuity.
<UL type=disc>
<UL type=circle>
<UL type=square>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level3 lfo1; tab-stops: list 108.0pt">Supersonic Flow: </LI></UL></UL></UL>
For supersonic flow, the the specified density and velocity values at the inlet remain unchanged.
<UL type=disc>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level1 lfo1; tab-stops: list 36.0pt">Back to FAQ list </LI></UL>

NASA · 发表于 2005-9-15 07:44

· How do the various options for PRESSURE boundaries work?
o OPTION: STATIC/PIEZO - The static option requires that the static pressure is fixed to the specified value over the entire region. The piezo option allows the value of the static pressure to vary over the region. This variation will only occur if a global body force has been applied to the fluid stream, and if the density of the fluid is allowed to vary as a function of pressure (and temperature if desired). The variation that occurs results in a local pressure that is the applied static pressure plus a rho*g*h term. The height is the distance from the body force reference location.
<UL type=disc>
<UL type=circle>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level2 lfo1; tab-stops: list 72.0pt">ENVIRONMENTAL: ON/OFF - Turning this option on changes the behavior of the pressure boundary. The boundary behaves as before for any cell where there is outflow. When there is inflow the static pressure is reduced by 0.5*rho*U2. This can be thought of as an entrance loss. It is useful when running models with large plenums simulating an external ambient environment. </LI></UL></UL>
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How do velocity, density, temperature and the pressure field interact at PRESSURE boundaries?
The velocity and density are calculated from the applied/resultant flow field. The temperature will be equal to the applied temperature in the case of inflow. The temperature will be the result of upstream conditions in the case of outflow.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What are the allowable boundary condition combinations in STAR?
The following table contains a summary of the allowable inlet, outlet and pressure combinations for a steady state, incompressible flow in STAR. Most combinations will also work for compressible and transient flows.
<TABLE cellPadding=0 align=right border=0>

<TR>
<TD colSpan=2>
(Nomenclature)</TD></TR>
<TR>
<TD >
+I</TD>
<TD >
Positive inlet (flow in)</TD></TR>
<TR>
<TD >
-I</TD>
<TD >
Negative Inlet (flow out)</TD></TR>
<TR>
<TD >
Os</TD>
<TD >
Outlet (flow split)</TD></TR>
<TR>
<TD >
Of</TD>
<TD >
Outlet (fixed mass flow)</TD></TR>
<TR >
<TD >
P </TD>
<TD >
Pressure</TD></TR></TABLE>
<TABLE cellPadding=0 border=1>

<TR>
<TD >
Flow In</TD>
<TD >
Flow Out#1</TD>
<TD >
Flow Out#2</TD>
<TD >
Comments</TD></TR>
<TR>
<TD >
+I</TD>
<TD >
Os</TD>
<TD >
Os</TD>
<TD >
Not recommended for subsonic compressible transient flow </TD></TR>
<TR>
<TD >
+I</TD>
<TD >
P</TD>
<TD >
P</TD>
<TD >
 </TD></TR>
<TR>
<TD >
+I</TD>
<TD >
P</TD>
<TD >
Of</TD>
<TD >
 </TD></TR>
<TR>
<TD >
+I</TD>
<TD >
P</TD>
<TD >
-I</TD>
<TD >
 </TD></TR>
<TR>
<TD >
+I</TD>
<TD >
-I</TD>
<TD >
-I</TD>
<TD >
Must be within 5% of continuity </TD></TR>
<TR>
<TD >
+I</TD>
<TD >
-I</TD>
<TD >
Os</TD>
<TD >
Flow split must equal 1 </TD></TR>
<TR>
<TD >
P</TD>
<TD >
P</TD>
<TD >
P</TD>
<TD >
 </TD></TR>
<TR>
<TD >
P</TD>
<TD >
Of</TD>
<TD >
Of</TD>
<TD >
 </TD></TR>
<TR>
<TD >
P</TD>
<TD >
-I</TD>
<TD >
-I</TD>
<TD >
 </TD></TR>
<TR>
<TD >
P</TD>
<TD >
P</TD>
<TD >
Of</TD>
<TD >
 </TD></TR>
<TR >
<TD >
P</TD>
<TD >
-I</TD>
<TD >
Of</TD>
<TD >
 </TD></TR></TABLE>
 
All other combinations are not allowed in STAR and will result in an error message in the .info file when STAR is run.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How is the Intensity/Length Scale option for boundaries and initialization different from the KE/ED option?
The K-Epsilon turbulence model and all models derived from it calculate a turbulent kinetic energy and a turbulence dissipation rate. Nowhere in those calculations is a length scale used. However, estimating the values of K and epsilon is not easily done directly. Usually an engineer will assume that the time varying velocity components that will be represented as turbulence are some fixed percentage of the steady-state velocity. This percentage is referred to as the turbulent intensity. It is much more intuitive a value than K. To derive a value for epsilon the engineer needs to assume some characteristic length of the smallest turbulent eddies present in the inflow. A relationship between K, epsilon and a length scale is part of the general derivation of the K-epsilon turbulence model. 
While the length scale is used by the engineer to relate the free-stream velocity, turbulent kinetic energy and turbulence dissipation rate, it is never actually used by the code at any stage in the calculations. The intensity/length scale option merely automates the engineering calculation that is normally followed to when estimating turbulent boundary conditions. The intensity/length scale option has the added benefit of varying K and epsilon in response to inflow velocities at boundaries where the velocity is not constant. This is probably more physical than fixing K and epsilon while the inlet velocity changes. 
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What are good engineering practices for estimating turbulence values at boundaries?
In general the engineer should be trying to create a model where any inflow or outflow boundary is not convecting a significant amount of turbulence into the domain. A more intuitive way to assess this is to look at the resultant turbulent viscosity at an inlet relative to the molecular velocity of the fluid in question.If the values of the turbulent viscosity are more than one or two orders of magnitude greater than the molecular viscosity, then the engineer should thoroughly review the assumptions and/or data used to calculate turbulence at the boundaries.Back to FAQ list

NASA · 发表于 2005-9-15 07:45

<UL type=disc>
<LI class=MsoNormal style="MARGIN: 0cm 0cm 0pt; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto; mso-list: l0 level1 lfo1; tab-stops: list 36.0pt">How do I estimate my near wall cell thickness to get the correct y+ value for wall function turbulence modeling? </LI></UL>
The equations:
y+ = UT * y / V where: UT = sqrt(Tw / rho) Tw = (µlam + µturb) du/dy µturb = fµ * Cµ * rho * K**2 / E K = 1.5 (U * I)**2 E = Cµ0.75 * K1.5 / l
The picture:
<v:shapetype><v:stroke joinstyle="miter"></v:stroke><v:formulas><v:f eqn="if lineDrawn pixelLineWidth 0"></v:f><v:f eqn="sum @0 1 0"></v:f><v:f eqn="sum 0 0 @1"></v:f><v:f eqn="prod @2 1 2"></v:f><v:f eqn="prod @3 21600 pixelWidth"></v:f><v:f eqn="prod @3 21600 pixelHeight"></v:f><v:f eqn="sum @0 0 1"></v:f><v:f eqn="prod @6 1 2"></v:f><v:f eqn="prod @7 21600 pixelWidth"></v:f><v:f eqn="sum @8 21600 0"></v:f><v:f eqn="prod @7 21600 pixelHeight"></v:f><v:f eqn="sum @10 21600 0"></v:f></v:formulas><v:path connecttype="rect" gradientshapeok="t" extrusionok="f"></v:path><lock aspectratio="t" v:ext="edit"></lock></v:shapetype><v:shape><v:imagedata></v:imagedata></v:shape>
The method:
1. Work out K based on estimates for U and I. 
2. Work out E based on an estimate for l. 
3. Work out µturb. Note that µturb >> µlam such that µlam can be ignored for a rough estimation. 
4. Work out Tw based on an estimated value of du/dy for the first cell. 
5. Work out UT. If the flow is compressible, estimate rho from the ideal gas law. 
6. Work out y+. Note that the y value is based in the cell centroid location and not the cell thickness. 
 Nomenclature:
<TABLE cellPadding=0 border=1>

<TR>
<TD width=100>
y </TD>
<TD >
Normal distance from wall</TD></TR>
<TR>
<TD >
V </TD>
<TD >
Kinematic viscosity</TD></TR>
<TR>
<TD >
Tw </TD>
<TD >
Wall shear stress</TD></TR>
<TR>
<TD >
rho </TD>
<TD >
Density</TD></TR>
<TR>
<TD >
mulam </TD>
<TD >
Laminar viscosity</TD></TR>
<TR>
<TD >
muturb</TD>
<TD >
Turbulent viscosity</TD></TR>
<TR>
<TD >
du/dy </TD>
<TD >
Velocity gradient</TD></TR>
<TR>
<TD >
fmu </TD>
<TD >
Empirical coefficient (=1.0)</TD></TR>
<TR>
<TD >
Cmu </TD>
<TD >
Coefficient (= 0.09)</TD></TR>
<TR>
<TD >
K </TD>
<TD >
Turbulent energy</TD></TR>
<TR>
<TD >
E </TD>
<TD >
Eddy dissipation</TD></TR>
<TR>
<TD >
U </TD>
<TD >
Average flow velocity</TD></TR>
<TR>
<TD >
I </TD>
<TD >
Turbulence intensity</TD></TR>
<TR >
<TD >
l </TD>
<TD >
Mixing length</TD></TR></TABLE>
 Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How do I judge whether a problem is converged?
There are several criteria that allow the user to judge convergence. It is recommended that these methods be used in combination to give a complete picture of how solution convergence.
o Reduction in global normalized residuals. This data is output in the .run and .rsi file and can be graphed. It is the most easily obtained picture of the convergence behavior of the model as a whole. Use the STARWatch facility to monitor STAR dynamically.
o Examination of engineering quantities of interest (drag, pressure drop, swirl, etc). Post processing .pst files a hundred or so iterations apart. For example, if the drag at iteration 500 is 10 percent lower than the drag at iteration 400 the solution is not yet converged, even if all global residuals have dropped below 1e-4.
o Direct comparison of flow field variables a few hundred iterations apart. Flow field data from two .pst files spaced several hundred iterations apart can be loaded simultaneously using the OPERATE commands. This data can then be manipulated to form a field variable equal to the percent change or absolute change in that variable. This tells the engineer where the solution is still changing.
o Similarly, strategically placed monitoring cells allow the user to graph the various data on a per iteration basis. When the variable values have flattened out and remain unchanged for several parts of the grid, the solution can be considered converged.
o To compare STAR convergence results with other codes, the absolute residual criteria should be disabled and a relative one used instead. The "ANORM" command allows this to be achieved by normalising all the residuals to unity at the beginning.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· In the SIMPLE algorithm what influences convergence?
The residual reduction factor determines how much the residual for a flow variable must be reduced during a single iteration. Sometimes it is helpful to reduce this value. This results in more sweeps per iteration but each iteration is closer to the final converged solution. A clue that this is necessary is if the number of sweeps for a flow variable shows large variation from iteration to iteration.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What parameters are required to set up a buoyancy problem?
o The user must specify a global Cartesian body force that represents gravity.
o The user must specify a reference location in space that defines a zero level for the rho*g*h term that will be added to the local pressures.
o The user must specify a reference density.
o The reference density, reference pressure and initial temperature must be consistent under the ideal gas law.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What are good practices to achieve convergence quickly?
o Set the reference location to be the cell centroid of the pressure reference cell.
o Make sure the the reference density is the ideal gas law result for the reference pressure and initial temperature.
o Ramp all applied temperatures and source terms such that no temperature gradients exist at iteration zero. Doing this following the previous step should result in an ideally quiescent flow field as the initial field. 
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How do I get convergence details in the .info file?
In the STARGUIde, go to the Analysis Controls->Output Controls->Monitor numeric Behavior panel. Turn on the option labelled "Print Iteration Residuals and Conservation Checks".
At the command line type "PRCHECK,,,CONV" Back to FAQ list

NASA · 发表于 2005-9-15 07:45

· What do the various parameters in the .info file mean?
o RES0 is the residual sum for the variable in question.
o The values below RES0 for each variable indicate the ratio of the current residual sum to the initial residual sum for each sweep. This value must reach that specified in the control module as the residual reduction factor.
o FVIN and FVOUT are the sum of inlet and outlet flows through INLET boundaries.
o FPIN and FPOUT are the sum of the inlet and outlet flows through PRESSURE boundaries.
o ENIN and ENOUT are the sum of the enthalpies convected in or out through all open boundaries.
o HTIN and HTOUT are the heat transfer in and out of fluid or solid materials at walls, baffles and any other solid/fluid interfaces
o QSOR is the sum of any user defined heat sources
o HDIFF is the material wise heat balance. This value should reduce to near zero for a converged solution.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What are the units of the various fluid properties?
STAR-CD is a dimensional code. All units must be SI. This means that the physical constants have the units shown below.

<TABLE cellPadding=0 border=1>

<TR>
<TD >
TIME</TD>
<TD >
s</TD></TR>
<TR>
<TD >
VELOCITY </TD>
<TD >
m/s</TD></TR>
<TR>
<TD >
MASS </TD>
<TD >
Kg</TD></TR>
<TR>
<TD >
TEMPERATURE </TD>
<TD >
K</TD></TR>
<TR>
<TD >
DENSITY</TD>
<TD >
Kg/m3</TD></TR>
<TR>
<TD >
PRESSURE </TD>
<TD >
Kg m3/s2 (Pascals)</TD></TR>
<TR>
<TD >
CONDUCTIVITY </TD>
<TD >
Watts/mK</TD></TR>
<TR>
<TD >
SPECIFIC HEAT </TD>
<TD >
J/m3K</TD></TR>
<TR>
<TD >
VISCOSITY </TD>
<TD >
Kg/ms</TD></TR>
<TR>
<TD >
TURBULENT ENERGY </TD>
<TD >
m2/s2</TD></TR>
<TR >
<TD >
EDDY DISSIPATION</TD>
<TD >
m2/s3</TD></TR></TABLE>
Important Note:
Only geometric entities (including the position of the reference density point for buoyancy problems and any tabular XYZ data) are scaled by the scaling factor supplied during the geomerty write. All other quantities entered in pro*am are in SI units.
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How can I calculate averaged quantities using PROSTAR?
Example showing the calculation of area averaged (for boundary or wall data) pressure:
OPER GETC P 1 OPER GETC AREA 2 OPER MULT 1 2 3 CSET NEWS [SHELLS OF INTEREST] *GET PRDT RTOT 3 *GET AREA RTOT 2 *SET PRES PRDT / AREA Volume averaged quantity with cell data
Example showing the calculation of volume averaged pressure:
OPER GETC P 1 OPER GETC VOLU 2 OPER MULT 1 2 3 CSET NEWS [CELLS OF INTEREST] *GET PRDT RTOT 3 *GET VOLU RTOT 2 *SET PRES PRDT / VOLU
 Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· How can I compute the mass flow rate in PROSTAR?
Using FLUX command (when fluxes are available) 
o Select a fluid cell layer where the mass flux is to be calculated
o Apply shells of type ICTID to the faces of those fluid cells.
o Read in the mass flux (GETC FLUX ).
o Calculate the mass flux with FLUX CSET ICTID.
Using INTEGRATE command (When velocities are available)
o Identify the plane at which the flow rate is to be calculated by using the "Section Slice" button as you would normally do for a section plot.
o Select a set of cells at the location of the plane.
o Read in the vector/scalar quantity - for flux use "GETC ALL DENS". 
o Calculate the mass flow rate with "INTEGRATE CSET".
o Output is as follows:
TOT A = Area that the section cuts through the cell set TOT A* VN = Sum of Area * <st1:place w:st="on">Normal</st1:place> Velocity TOT A * S = Sum of Area * Scalar Value (density in this case) TOT A* VN* S = Sum of Area * Normal Velocity * Scalar =FLOW RATE
Back to FAQ list 
<DIV class=MsoNormal style="MARGIN: 0cm 0cm 0pt 36pt; TEXT-ALIGN: center; mso-margin-top-alt: auto; mso-margin-bottom-alt: auto" align=center>
<HR align=center width="100%" SIZE=2>
</DIV>
· What are some recommended procedures for working with tetrahedral meshes?
o Resize a local PROSTAR using prosize. Choose the tet option and set parameter MAXCUT to the expected number of fluid cells.
o Use one or two extrusion layers to improve the calculations in wall cells.
o Check tet quality:
CHECK CSET,,TETQ CSET SUBS PRANGE 4,0,0.1
o Apply the TETALIGN command to the tetrahedral cells to reorder the vertex numbering (reduces memory and time requirements for STAR).
o Use the CREORDER command to reorder the cell numbering (also reduces the time requirements for STAR).
o Use a higher oder differencing scheme, such as central differencing or MARS. If residual convergence is a problem, try reducing the under-relaxation factors for velocity and pressure to 0.5 and 0.1, respectively, and the residual tolerance for pressure to 0.01.
Back to FAQ list

账号		自动登录	找回密码
密码			我要加入

[基础理论] [分享]Frequently Asked Questions about STAR-CD

马上注册，结交更多好友，享用更多功能，让你轻松玩转社区。

回复：（oscar32）[分享]Frequently Asked Questions ...

回复：（oscar32）[分享]Frequently Asked Questions ...

回复：（oscar32）[分享]Frequently Asked Questions ...

回复：（oscar32）[分享]Frequently Asked Questions ...