Good time!

Help me please! I would like to understand how cfx Calculat Equations. So I understand cfx clculat it in Integration Point. And we have one Integration Point in one element. Is it write?

Do cfx clculat value of variable in real nods of mesh?

Thanks for any help. And I will be very gratitude if you give me more information. I am really need you help!!

CFx has in its tutorial a good explanation about it. Go to Help and check it!

Transport Equations In this section, the instantaneous equation of mass, momentum, and energy conservation are presented. For turbulent flows, the instantaneous equations are averaged leading to additional terms. These terms, together with models for them, are discussed in Turbulence and Wall Function Theory.

The instantaneous equations of mass, momentum and energy conservation can be written as follows in a stationary frame:

The Continuity Equation Equation 77.

The Momentum Equations Equation 78.

Where the stress tensor, , is related to the strain rate by

Equation 79.

The Total Energy Equation Equation 80.

Where is the total enthalpy, related to the static enthalpy by:

Equation 81.

The term represents the work due to viscous stresses and is called the viscous work term.

The term represents the work due to external momentum sources and is currently neglected.

The Thermal Energy Equation An alternative form of the energy equation, which is suitable for low-speed flows, is also available. To derive it, an equation is required for the mechanical energy .

Equation 82.

The mechanical energy equation is derived by taking the dot product of with the momentum equation Equation 78:

Equation 83.

Subtracting this equation from the total energy equation Equation 80 yields the thermal energy equation:

Equation 84.

The term is always negative and is called the viscous dissipation. Finally, the static enthalpy is related to the internal energy by:

Equation 85.

So Equation 84 can be simplified to:

Equation 86.

The term is currently neglected, although it may be non-zero for variable-density flows. This is the thermal energy equation solved by ANSYS CFX.

Please note the following guidelines regarding use of the thermal energy equation:

Although the thermal energy equation solves for , this variable is still called static enthalpy in ANSYS CFX-Post.

The thermal energy equation is meant to be used for flows which are low speed and close to constant density

The thermal energy equation is particularly suited for liquids, since compressibility effects are minor. In addition, the total energy equation may experience robustness problems due to the pressure transient and the contribution to enthalpy.

For materials which have variable specific heats (e.g., set as a CEL expression or using an RGP table or Redlich Kwong equation of state) the solver includes the contribution in the enthalpy tables. This is inconsistent, because the variable is actually internal energy. For this reason, the thermal energy equation should not be used in this situation, particularly for subcooled liquids.

Equations of State In ANSYS CFX, the flow solver calculates pressure and static enthalpy. Finding density requires that you select the thermal equation of state and finding temperature requires that you select the constitutive relation. The selection of these two relationships is not necessarily independent and is also a modeling choice.

The thermal equation of state is described as a function of both temperature and pressure:

Equation 87.

The specific heat capacity, , may also be described as a function of temperature and pressure:

Equation 88.

For an Ideal Gas, the density is defined by the Ideal Gas Law and, in this case, can be a function of only temperature:

Equation 89.

Important When or are also functions of an algebraic additional variable, in addition to temperature and pressure, then changes of that additional variable are neglected in the enthalpy and entropy functions. However, if that additional variable is itself only dependent on pressure and temperature, then the effects will be correctly accounted for.

Ideal Gas Equation of state For an Ideal Gas, the relationship is described by the Ideal Gas Law:

Equation 90.

where is the molecular weight of the gas, and is the universal gas constant.

Real Gas and Liquid Equations of State In the current version of ANSYS CFX the Redlich Kwong equation of state is available as a built-in option for simulating real gases. It is also available through several pre-supplied CFX-TASCflow RGP files. The Vukalovich Virial equation of state is also available but currently only by using CFX-TASCflow RGP tables.

Redlich Kwong Gas Properties The Redlich-Kwong equation of state was first published in 1949 and is considered one of the most accurate two parameter corresponding states equations of state. This equation of state is quite useful from an engineering standpoint because it only requires that the user know the fluid critical temperature and pressure. More recently, Aungier (1995) [96] has modified the Redlich-Kwong equation of state so that it provides much better accuracy near the critical point. The Aungier form of this equation of state is used by ANSYS CFX and is given by:

Equation 91.

This form differs from the original by the additional parameter , which is added to improve the behavior of isotherms near the critical point, as well as the form of . The parameters , , and in Equation 91 are given by:

Equation 92. Equation 93. Equation 94. Equation 95.

In the expression for , the standard Redlich Kwong exponent of has been replaced by a general exponent . Optimum values of depend on the pure substance. Aungier (1995) [96] presented values for twelve experimental data sets to which he provided a best fit polynomial for the temperature exponent in terms of the acentric factor, :

Equation 96.

The acentric factor must be supplied when running the Redlich Kwong model and is tabulated for many common fluids in Poling et al [84]. If you do not know the acentric factor, or it is not printed in a common reference, it can be estimated using knowledge of the critical point and the vapor pressure curve with this formula:

Equation 97.

where the vapor pressure, , is calculated at . In addition to the critical point pressure, this formula requires knowledge of the vapor pressure as a function of temperature.

In order to provide a full description of the gas properties, the flow solver must also calculate enthalpy and entropy. These are evaluated using slight variations on the general relationships for enthalpy and entropy which were presented in the previous section on variable definitions. The variations depend on the zero pressure, ideal gas, specific heat capacity and derivatives of the equation of state. The zero pressure specific heat capacity must be supplied to ANSYS CFX while the derivatives are analytically evaluated from Equation 91.

Internal energy is calculated as a function of temperature and volume (,) by integrating from the reference state (,) along path 'amnc' (see diagram below) to the required state (,) using the following differential relationship:

Equation 98.

First the energy change is calculated at constant temperature from the reference volume to infinite volume (ideal gas state), then the energy change is evaluated at constant volume using the ideal gas . The final integration, also at constant temperature, subtracts the energy change from infinite volume to the required volume. In integral form, the energy change along this path is:

Equation 99.

Once the internal energy is known, then enthalpy is evaluated from internal energy:

The entropy change is similarly evaluated:

Equation 100.

where is the zero pressure ideal gas specific heat capacity. By default ANSYS CFX uses a 4th order polynomial for this and requires that coefficients of that polynomial are available. These coefficients are tabulated in various references including Poling et al [84].

In addition, a suitable reference state must be selected to carry out the integrations. The selection of this state is arbitrary, and can be set by the user, but by default, ANSYS CFX uses the normal boiling temperature (which is provided) as the reference temperature and the reference pressure is set to the value of the vapor pressure evaluated using Equation 106 at the normal boiling point. The reference enthalpy and entropy are set to zero at this point by default, but can also be overridden if desired.

Other properties, such as the specific heat capacity at constant volume, can be evaluated from the internal energy as:

Equation 101.

where is the ideal gas portion of the internal energy:

Equation 102.

specific heat capacity at constant pressure, , is calculated from using:

Equation 103.

where and are the volume expansivity and isothermal compressibility, respectively. These two values are functions of derivatives of the equation of state and are given by:

Equation 104. Equation 105.

Redlich Kwong Saturated Vapor Properties When running calculations with liquid condensing out of the vapor (equilibrium phase change or Eulerian thermal phase change model) or dry calculations, the flow solver needs to know the form of the vapor pressure curve. Pressure and temperature are not independent in the saturation dome so vapor saturation properties are evaluated by first assuming an equation which gives the dependence of vapor pressure on temperature, and then substituting that into the equation of state.

For materials that use the Redlich Kwong equation of state ANSYS CFX approximates the vapor pressure curve using a form given by Aungier (2000) [65]:

Equation 106.

Vapor saturation properties are calculated by evaluating the equation of state and constitutive relations along the saturation curve.

Redlich Kwong Liquid Properties It is possible to derive liquid densities directly from the Redlich Kwong equation, however, this is not desirable because the Redlich Kwong equation is very inaccurate in the compressed liquid regime.

Instead, when you select to use the Redlich Kwong equation of state for a liquid, the properties are assumed to vary along the vapor pressure curve as a function of saturation temperature. These properties are approximate and should only be used when the amount of liquid in your calculation will be small. For example, they work well with the equilibrium condensation model or non-equilibrium small droplet phase change model.

To derive the liquid enthalpy and entropy, such that they are completely consistent with the gas phase, requires all the same data as is provided for the gas phase: the critical point data, the acentric factor and the zero pressure specific heat coefficients.

To calculate saturated liquid densities, an alternative equation of state originally published by Yamada and Gunn (1973), is used by ANSYS CFX that gives liquid specific volume as a function of temperature:

Equation 107.

This equation is convenient because it only requires knowledge of the critical volume and temperature as well as the acentric factor. The valid temperature range for the liquid equation of state is 0.4 < < 0.99. The solver will clip the temperature used in this equation to that range.

Saturated liquid enthalpy is calculated using knowledge of the gas saturation enthalpy and the following equation:

Equation 108.

where the enthalpy of vaporization, , is given by the following expression taken from Poling et al [84]:

Equation 109.

Saturated liquid entropy can easily be derived using the second law and the gas saturation entropy:

Equation 110.

Prediction of liquid specific heat capacity with the Redlich Kwong equation has a similar problem to the liquid density, so ANSYS CFX uses an alternative form presented by Aungier (2000):

Equation 111.

which requires knowledge of the zero pressure heat capacity coefficients, as well as the acentric factor. For the saturated liquid it is assumed that .

Vukalovich Virial The virial equation of state used in ANSYS CFX was developed by Vukalovich and is given by:

Equation 112.

This equation of state is known to be valid over pressure and temperature ranges of 0.01 bar to 100 bar and 273.15 K to 1000 K.

IAPWS Equation of State The IAPWS-IF97 database represents an accurate equation of state for water and steam properties. The database is fully described elsewhere [125], but a summary will be provided in this section. The IAPWS database uses formulations for five distinct thermodynamic regions for water and steam, namely:

subcooled water (1)

supercritical water/steam (2)

superheated steam (3)

saturation data (4)

high temperature steam (5)

Figure 1. Regions and Equations of IAPWS-IF97

Region 5 has not been implemented in ANSYS CFX because it represents a thermodynamic space at very high temperatures (1073.15 - 2273.15 K) and reasonably low pressures (0-10 MPa) that can be adequately described using other property databases already in ANSYS CFX (i.e., Ideal Gas EOS with NASA specific heat and enthalpy). Furthermore, since this region is not defined for pressures up to 100 MPa, as is the case for regions 1, 2 and 3, problems arise in filling out the pressure-temperature space in the tables when temperatures exceed 1073.15 K and pressures exceed 10 MPa. The database implemented in ANSYS CFX therefore covers temperatures ranging from 273.15 to 1073.15 K and pressures ranging from 611 Pa to 100 MPa.

The reference state for the IAPWS library is the triple point of water. Internal energy, entropy and enthalpy are all set to zero at this point.

Tref = 273.16 K, Pref = 611.657 Pa, uliquid = 0 J/kg, sliquid = 0 J/kg/K, hliquid = 0 J/kg

In ANSYS CFX, the analytical equation of state is used to transfer properties into tabular form, which can be evaluated efficiently in a CFD calculation. These IAPWS tables are defined in terms of pressure and temperature, which are then inverted to evaluate states in terms of other property combinations (such as pressure/enthalpy or entropy/enthalpy). When developing the IAPWS database for ANSYS CFX, therefore, properties must be evaluated as functions of pressure and temperature. For the most part, this involves a straightforward implementation of the equations described in the IAPWS theory [125]. Region 4 involves saturation data which only uses pressure or temperature information.

However, some difficulties are encountered when evaluating the properties around Region 3 (near the critical point), where the EOS is defined explicitly in terms of density and temperature. In this region, the density must be evaluated using Newton-Raphson iteration. This algorithm is further complicated in that the EOS is applicable on both the subcooled liquid and superheated vapor side leading up to critical conditions. Therefore, depending on the pressure-temperature state, one may be evaluating a subcooled liquid or a superheated vapor with the same EOS. To apply the Newton-Raphson scheme in a reliable way, one must detect on which side of the saturation dome the pressure-temperature state applies, and apply an appropriate initial guess. Such an iteration scheme, including logic for an initial guess, has been implemented in CFX so that table generation around the critical region is possible.

Metastable Superheated Liquid/Supercooled Vapor States The IAPWS library also extends to metastable states, so that this equation of state is available for nonequilibrium phase change models such as the Droplet Condensation Model. The EOS for regions 1 and 3 in Figure 1 are stated to have reasonable accuracy for metastable states close to the saturation line d liquid states [125]. However, the term "reasonable" is not quantified, and therefore the degree to which the extrapolation of the EOS can be applied is unknown.

In region 2, an additional set of equations have been developed for supercooled vapor conditions under 10 MPa. These equations have been tuned to match the saturation data. Above 10 MPa, the EOS for the superheated region can safely be extrapolated into supercooled conditions, but it does not match smoothly with the specialized supercooled equations below 10 MPa.

Numerical Testing to Delineate Metastable Regions In order to make the IAPWS database as robust as possible, numerical testing has been done to determine approximate metastable vapor/liquid spinodal lines. Figure 2 is given to demonstrate these spinodal lines which are essentially boundaries up to which metastable conditions can exist. These would be defined similar to saturation curves as functions of either temperature or pressure. The IAPWS database tables are always generated up to these limits regardless of what flow models are specified (i.e., equilibrium or non-equilibrium) and thus allow nonequilibrium phase change models to be applied.

Figure 2. Spinodal Limits Built Into Tables

Numerical Discretization Analytical solutions to the Navier-Stokes equations exist for only the simplest of flows under ideal conditions. To obtain solutions for real flows, a numerical approach must be adopted whereby the equations are replaced by algebraic approximations which may be solved using a numerical method.

ANSYS CFX-Solver Theory Guide | Discretization and Solution Theory | Numerical Discretization | Numerical Discretization Prev Up / Home The Coupled System of Equations Next

Discretization of the Governing Equations This approach involves discretizing the spatial domain into finite control volumes using a mesh. The governing equations are integrated over each control volume, such that the relevant quantity (mass, momentum, energy, etc.) is conserved in a discrete sense for each control volume.

The figure below shows a typical mesh with unit depth (so that it is two-dimensional), on which one surface of the control volume is represented by the shaded area.

Figure 1. Control Volume Surface

It is clear that each node is surrounded by a set of surfaces that define the control volume. All the solution variables and fluid properties are stored at the element nodes.

Consider the mean form of the conservation equations for mass, momentum and a passive scalar, expressed in Cartesian coordinates:

Equation 1. Equation 2. Equation 3.

These equations are integrated over a control volume, and Gauss' Divergence Theorem is applied to convert some volume integrals to surface integrals. If control volumes do not deform in time, then the time derivatives can be moved outside of the volume integrals and the equations become:

Equation 4. Equation 5. Equation 6.

where V and s respectively denote volume and surface regions of integration, and dnj are the differential Cartesian components of the outward normal surface vector. The volume integrals represent source or accumulation terms, and the surface integrals represent the summation of the fluxes. Note that changes to these equations due to control volume deformation are presented below. For details, see Mesh Deformation.

The first step in the numerical solution of these exact differential equations is to create a coupled system of linearized algebraic equations. This is done by converting each term into a discrete form. Consider, for example, an isolated mesh element like the one shown below.

Figure 2. Mesh Element

Volumetric (i.e., source or accumulation) terms are converted into their discrete form by approximating specific values in each sector and then integrating those values over all sectors that contribute to a control volume. Surface flow terms are converted into their discrete form by first approximating fluxes at integration points, ipn, which are located at the center of each surface segment in a 3D element surrounding the control volume. Flows are then evaluated by integrating the fluxes over the surface segments that contribute to a control volume.

Many discrete approximations developed for CFD are based on series expansion approximations of continuous functions (such as the Taylor series). The order-accuracy of the approximation is determined by the exponent on the mesh spacing or timestep factor of the largest term in the truncated part of the series expansion. This is often the first term excluded from the approximation. Increasing the order-accuracy of an approximation generally implies that errors are reduced more quickly with mesh or timestep size refinement. Unfortunately, in addition to increasing the computational load, high-order approximations are also generally less robust (i.e., less numerically stable) than their low-order counterparts.

The discrete form of the integral equations becomes:

where V is the control volume, is the timestep, is the discrete outward surface vector, the subscript ip denotes evaluation at an integration point, and summations are over all the integration points of the control volume. Note that the First Order Backward Euler scheme has been assumed in this equation, although a second order scheme is also available as discussed below. The superscript o refers to the old time level. The discrete mass flow through a surface of the control volume, denoted by , is given by:

Equation 10.

Pressure- Velocity Coupling ANSYS CFX uses a co-located (non-staggered) grid layout such that the control volumes are identical for all transport equations. As discussed by Patankar [118], however, naïve co-located methods lead to a decoupled (checkerboard) pressure field. Rhie and Chow [2] proposed an alternative discretization for the mass flows to avoid the decoupling, and this discretization was modified by Majumdar [119] to remove the dependence of the steady-state solution on the timestep.

A similar strategy is adopted in ANSYS CFX. By applying a momentum-like equation to each integration point, the following expression for the advecting (mass-carrying) velocity at each integration point is obtained:

Equation 11. Equation 12. Equation 13.

= approximation to central coefficient of momentum equation, excluding the transient term

Equation 14.

The overbars indicate averaging of adjacent vertex values to the integration point, while the o superscript denotes values at the previous timestep.

The naïve discretization, given simply by averaging the adjacent vertex velocities to the integration point, is augmented by a high order pressure variation that scales with the mesh spacing. In particular, when substituted into the continuity equation, the expression

becomes a fourth derivative of pressure which scales with . This expression represents term that is spatially third-order accurate, and is sometimes also called the pressure redistribution term. This term is usually significantly smaller than the average of vertex velocities, especially as the mesh is refined to reasonable levels.

In some cases, the pressure redistribution term can produce apparently significant spurious velocity fields. This may occur when a strong pressure gradient is required to balance a body force, , such as buoyancy or porous drag. In these cases, the Rhie Chow discretization may lead to velocity wiggles at locations where the body force is discontinuous (e.g., at a free surface interface, or at the boundary of a porous region). The wiggles are greatly reduced or eliminated by redistributing the body force as follows:

Equation 15.

Transient Term For control volumes that do not deform in time, the general discrete approximation of the transient term for the nth timestep is:

Equation 16.

where values at the start and end of the timestep are assigned the superscripts n+½ and n-½, respectively.

With the First Order Backward Euler scheme, the start and end of timestep values are respectively approximated using the old and current time level solution values. The resulting discretization is:

Equation 17.

It is robust, fully implicit, bounded, conservative in time, and does not yield a timestep size limitation. This discretization is, however, only first-order accurate in time and will introduce discretization errors that tend to diffuse steep temporal gradients. This behavior is similar to the numerical diffusion experienced with the Upwind Difference Scheme for discretizing the advection term.

With the Second Order Backward Euler scheme, the start and end of timestep values are respectively approximated as:

Equation 18. Equation 19.

When these values are substituted into the general discrete approximation, Equation 16, the resulting discretization is:

Equation 20.

This scheme is also robust, implicit, conservative in time, and does not create a timestep limitation. It is second-order accurate in time, but is not bounded and may create some nonphysical solution oscillations. For quantities such as volume fractions, where boundedness is important, a modified Second Order Backward Euler scheme is used instead.

Shape Functions

Shape Functions The solution fields are stored at the mesh nodes. However, various terms in the equations require solutions or solution gradients to be approximated at integration points. Finite element shape functions are consequently used to evaluate the solution and its variation within mesh elements.

A variable varies within an element as follows:

Equation 21.

where Ni is the shape function for node i and is the value of at node i. The summation is over all nodes of an element. Key properties of shape functions include:

Equation 22. Equation 23.

The shape functions used in ANSYS CFX are linear in terms of parametric coordinates. They are used to calculate various geometric quantities as well, including ip coordinates and surface area vectors. This is possible because Equation 21 also holds for the coordinates:

Equation 24.

The trilinear shape functions for each supported mesh element are given below:

Hexahedral Element

Figure 3.

The tri-linear shape functions for the nodes are:

Equation 25.

Tetrahedral Element

Figure 4.

The tri-linear shape functions for the nodes are:

Equation 26.

Wedge Element

Figure 5.

The tri-linear shape functions for the nodes are:

Equation 27.

Pyramid Element

Figure 6.

The tri-linear shape functions for the nodes are:

Equation 28.

At this point, it is worth highlighting that these shape functions yield linear combinations of positively and negatively weighted nodal values. The significance of these positive and negative influences is identified in Discretization Errors.

Diffusion Terms Following the standard finite element approach, shape functions are used to evaluate spatial derivatives for all the diffusion terms. For example, for a derivative in the x direction at integration point ip:

Equation 29.

The summation is over all the shape functions for the element. The Cartesian derivatives of the shape functions can be expressed in terms of their local derivatives via the Jacobian transformation matrix:

Equation 30.

The shape function gradients can be evaluated at the actual location of each integration point (i.e., true tri-linear interpolation), or at the location where each ip surface intersects the element edge (i.e., linear-linear interpolation). The latter formulation improves solution robustness at the expense of locally reducing the spatial order-accuracy of the discrete approximation.

Pressure Gradient Term The surface integration of the pressure gradient in the momentum equations involves evaluating of the expression:

Equation 31.

The value of Pip is evaluated using the shape functions:

Equation 32.

As with the diffusion terms, the shape function used to interpolate P can be evaluated at the actual location of each integration point (i.e., true tri-linear interpolation), or at the location where each ip surface intersects the element edge (i.e., linear-linear interpolation). As in the discretization of the diffusion terms, the formulation improves solution robustness but reduces the local spatial order-accuracy of the discrete approximation.

Advection Term To complete the discretization of the advection term, the variable must be approximated in terms of the nodal values of . The advection schemes implemented in ANSYS CFX can be cast in the form:

Equation 33.

where is the value at the upwind node, and is the vector from the upwind node to the ip. When using a specified blend, is the average of the adjacent nodal gradients and when using high resolution scheme, is the nodal gradient of the upwind node. Particular choices for and yield different schemes.

1st Order Upwind Differencing Scheme A value of yields a first order Upwind Difference Scheme (UDS). This scheme is very robust, but it will introduce diffusive discretization errors that tend to smear steep spatial gradients as shown below:

Numerical Advection Correction Scheme (Specify Blend) By choosing a value for between 0 and 1, and by setting equal to the average of the adjacent nodal gradients, the discretization errors associated with the UDS are reduced. The quantity , called the Numerical Advection Correction, may be viewed as an anti-diffusive correction applied to the upwind scheme. The choice is formally second-order-accurate in space, and the resulting discretization will more accurately reproduce steep spatial gradients. However, it will introduce dispersive discretization errors that tend to cause non-physical oscillations in regions of rapid solution variation as shown below. This scheme is also not as robust as the UDS.

Central Difference Scheme With this scheme, the value of is set to 1 and is set equal to the local element gradient. An alternative interpretation is that is evaluated using the trilinear shape functions:

Equation 34.

The resulting scheme is also second-order-accurate, and shares both the desirable and undesirable attributes of the Numerical Advection Correction Scheme. An additional undesirable attribute is that this scheme may suffer from serious decoupling issues. While use of this scheme is not generally recommended, it has proven both useful and accurate when used with LES based turbulence models - add reference.

High Resolution Scheme The High Resolution Scheme computes locally to be as close to 1 as possible without introducing local oscillations, and sets equal to the control volume gradient at the upwind node. The recipe for is based on the boundedness principles used by Barth and Jesperson [28]. This scheme is both accurate and bounded since it only reduces to first order near discontinuities. Note that for vector quantities, such as velocity, is independently calculated for each vector component.

Compressibility Mass flow terms in the mass conservation equation involve a product of the density, which depends upon pressure and the advecting velocity. For compressible flows, the discretization of these terms is made as implicit as possible in each timestep with the use of the following Newton-Raphson linearization:

Equation 35.

Here, the superscripts k and k-1 respectively indicate the current and previous iterates. This results in an active linearization involving both the new density and velocity terms for compressible flows at any Mach number.

Mesh Deformation The integral conservation equations presented above Equation 4 must be modified when the control volumes deform in time. These modifications follow from the application of the Leibnitz Rule:

Equation 36.

where is the velocity of the control volume boundary.

As before, the differential conservation equations are integrated over a given control volume. At this juncture, the Leibnitz Rule is applied, and the integral conservation equations become:

Equation 37. Equation 38. Equation 39.

The transient term accounts for the rate of change of storage in the deforming control volume, and the advection term accounts for the net advective transport across the control volume's moving boundaries.

Erroneous sources of conserved quantities will result if the Geometric Conservation Law (GCL):

Equation 40.

is not satisfied by the discretized transient and advection terms. The GCL simply states that for each control volume, the rate of change of volume must exactly balance the net volume swept due to the motion of its boundaries. The GCL is satisfied by using the same volume recipes for both the control volume and swept volume calculations, rather than by approximating the swept volumes using the mesh velocities.

[aer]

Hi
I use IAPWS IF97 in CFX for modelling the two phase flow (steam and water) in a nozzle,
I test different table generation value , but this error is appeared ' Independent variables were clipped during table generation' for all temperature and pressure range, but solving process is continue, but when I change this bound the result is changed and also the convergence process is very slow.
How can I choose proper bounds?
I use twice more than max pressure in nozzle, and twice less than min pressure , and for temperature do same.
Could you help me please?

[ghorrocks]

The table needs to be defined to cover the highest to lowest value present in the simulation. Note that these limiting values may occur in the centre of the simulation rather than at a boundary and might not be known before hand (eg in a nozzle).

A further thing to note is that as the simulation converges it is common for the flow to go through flaw states which result in the fluid properties going outside the steady state ranges. This means you should always give some margin over the steady state max and min values to allow for this.

And finally: If your simulation is diverging then you probably have a weird flow occurring which will require wacky fluid properties. In this case you need to fix the divergence, not the table generation.