Cashco, Inc., desired to determine whether or not a Computational Fluid Dynamic (CFD) model could accurately predict the fluid flow through a Ranger QCT Control Valve. The control valve itself was created by Cashco and modeled using Pro/ENGINEERÒ Revision 19 solid geometry. ANSYS Revision 5.4 was used to create the finite element mesh, apply loads, solve, and evaluate the results of the fluid analysis. Two result quantities were of primary interest to Cashco, the Flow Coefficient (C_v) and the Pressure Recovery Factor (F_L). The results of the fluid analysis showed that ANSYS predicted the Flow Coefficient and Pressure Recovery Factor to within 10% and 2% of their experimental values, respectively.

Cv is the flow coefficient
F_L is the pressure recovery factor.
P₁ is the upstream pressure of the fluid, in PSI, measured one pipe diameter upstream of the valve.
P₂ is the downstream pressure of the fluid, in PSI, measured ten pipe diameters downstream of the value.
P_vc is the pressure of the fluid at the vena contracta, in PSI.
Q is the fluid flow rate, in GPM.
S_g is the specific gravity of the fluid.

The goal of this analysis was to determine if ANSYS could predict the pressure distribution of water flowing through a Ranger QCT Control valve (rotary globe). The geometry was provided to DRD in the form of Pro/ENGINEER part and assembly files. The fluid geometry was created by DRD Technology also using Pro/ENGINEER Revision 19. DRD created a technique whereby the fluid flow paths in the control valve were transformed into solid geometry. This technique involves exporting IGES files representing the assembly from Pro/ENGINEER and then importing those IGES files back into Pro/ENGINEER. Prior to importing the IGES files, a simple block representing the fluid is imported first. Then, each IGES file is subsequently imported as a cut that removes a segment of the fluid. The removed segments of the geometry are voids in the flow field that represent the solid parts. Once the fluid flow geometry was completed, an IGES file was exported from Pro/ENGINEER and then imported into ANSYSÒ . Figure 1 shows a cut-away view of the control valve.

The valve assembly itself was composed of solid parts. For the fluid analysis, however, the solid parts are not required. It is the open void between the solid parts that must be meshed for the fluid analysis. Therefore, the assembly must be "inverted", whereby, the fluid void becomes a solid volume and any solid parts in the flow become voids. The analysis assumes the fluid flow was isothermal and steady state. The water temperature was 60° F (values for density and viscosity for the fluid were determined based on this temperature and assumed to be constant).

The following section outlines the procedure used to create the finite element model of the fluid flow environment. This procedure assumes the solid geometry was originally created in Pro/ENGINEER and the flow field will be meshed with tetrahedron shaped elements.

Geometry Setup (Pro/ENGINEER):

• Remove all small features from every part in the assembly (in part mode).
• Remove all interference that exists between the parts in the assembly.
• All parts must share common (mating) surfaces.

Geometry Creation (Pro/ENGINEER):

• Create a simple geometric shape (e.g., a block) around the assembly that requires fluid analysis (assembly mode). Create a datum coordinate system for the new part (make certain the new coordinate system is in a logical location; it will be used for the IGES transfer process).
• Export IGES files of every part in the assembly (choose to export all parts as individual files). Use the newly created coordinate system. Exit assembly mode.
• Create a new part starting with default datum planes. Set the part accuracy to 0.0001.
• Import the simple geometry shape (block) IGES file using its assigned coordinate system. Pro/ENGINEER should immediately create a solid from the IGES file import. If it does not, create a solid protrusion using the quilted surface.
• Import all other IGES files in a logical order. If each part is imported as a solid, the options will be to create a protrusion, a cut, or a surface – choose cut. If the IGES file is not imported as a solid, Pro/ENGINEER will automatically create it as a surface model. Use the surface quilt to create a solid cut (if the surface is not continuous, redefine the part to zip the gaps).

Once all of the IGES files have been imported into the new part, the remaining geometry is of the flow field.

• Add cuts to the new part geometry to intersect the simple block with the previous cuts from the IGES imports (if the block does not intersect with the cuts, the model will not be continuous and ANSYS will be unable to create a single volume).
• Simplify the model, removing areas of the flow field that are not important to the analysis.
• Once the model is continuously connected and simplified as much as possible, export the part as an IGES file.

Refer to Figure 2 for a visual description of the fluid flow geometry near the valve created in Pro/ENGINEER.

• Import the IGES file into ANSYS (choose the Alternate IGES option, set the global tolerance for merging to the IGES file).
• Once the import procedure is complete, check for exterior lines. A volume may be created if there are no exterior lines. If exterior lines do exist, gaps remain in the model that must be repaired prior to volume creation.
• Create the volume.

Finite Element Model Creation (ANSYS):

• Select a shell and solid (structural) element types – SHELL63 and SOLID45.
• Choose an appropriate elements size for different areas in the model (e.g., set a global element size to a smaller value where the mesh requires refinement for good flow field resolution) and mesh all the areas in the model with triangular shaped SHELL63s.
• Once all areas are meshed, change the element type to the SOLID45 and mesh the volume (use tetrahedron shaped elements).
• Once the volume is meshed satisfactorily, clear all the shell elements from all areas and delete the shell element type.
• Change the SOLID45 to a FLUID142.

Once all the elements have been changed from SOLID45s to FLUID142s the finite element model is complete and ready for boundary condition application. The analyzed model contained approximately 377,000 elements, 71,000 nodes, and 425,000 DOF’s (degrees-of-freedom). This mesh also included refinement in the boundary layer.

All exterior surfaces (except the inflow and outflow boundaries) of the fluid domain were assumed to have no-slip conditions (velocity components in the x, y, and z directions defined as zero). The inflow boundary x-direction component (direction of flow) of velocity was set at –79.64 in/s. This corresponds to a volumetric flow rate of 854 GPM given by Cashco (based on a pipe inside diameter of 8 in). For the given fluid properties, the Reynold's number is approximately 360,000. The y and z components of velocity on the inflow boundary were set to zero. The pressure on the outflow boundary was set to 0 PSI. This is the standard ANSYS/FLOTRAN outlet condition and assumes the flow is leaving at atmospheric pressure (0 PSI gage pressure).

• Fluid flow was Newtonian.
• Fluid flow was isothermal.
• Fluid flow was steady state.
• The k-Epsilon turbulence model was used.
• Small features were not modeled.

The values for C_V and F_L are calculated as follows and shown in Table 1 (the actual calculations are shown in the Appendix).

Where the pressures P₁ and P₂ where taken at the near wall nodes, Q derived from the mass flow balance given in the ANSYS/FLOTRAN output file (.pfl), and S_g being defined by CASHCO. The pressure at the vena contracta was deduced by CASHCO based on results like those shown in Figure 4. Determining the location and aggregate value of the vena contracta is difficult and somewhat subjective, especially for devices with multiple flow paths. The technique used for this model was to use a path plot (like the path shown in Figure 4) to determine the change in pressure as the flow passed near the center of the flow streams. The pressure at the vena contracta is the lowest value of pressure downstream of where the flow is locally restricted by the valve plug. From this data, the pressure at the vena contracta was determined to be approximately –2.3 PSI (12.4 PSI absolute pressure). The method used for determining the location of the vena contracta is not necessarily valid for all valve types for any given set of flow conditions. However, it is considered to by an accurate estimation of the pressure at the vena contracta for the Ranger QCT Control Valve with the given flow conditions. It should be noted that the actual test data was based on the flow conditions being compared to choked flow conditions in order to determine the pressure recovery factor rather than by direct measure of the vena contracta pressure.

The normalized rate of change for the momentum variables ranged from 1.6e-3 to 3.5e-3, turbulence variables ranged from 3.3e-3 to 7.2e-3, and the pressure variable was 3.6e-3. Figures 5 and 6 show a cut view of the pressure and velocity of the water flowing through the valve.