The curve used to loft the hub/shroud surface may be constructed in one of two ways, as determined by the Curve Type setting. The available Curve Type options are:

Set File Name to the name of the blade set file. To open a file selector, click Browse  .

The blade file must contain data points that define the blade profile (or rib) curves and should have the file extension .curve or .crv.

The profile points must be listed line by line, in free-format ASCII style in a closed-loop surrounding the blade.

A minimum of two profiles are required in the blade file: one which lies close to the hub surface and one which lies close to the shroud surface. The profile is not required to lie exactly on the surface. If it lies between the hub and shroud surfaces, it must be within 8% of the span from the surface. If a profile lies outside of the passage, its distance from the surface has no maximum limit.

Profiles can be used to define tips. For details, see The Hub Tip and Shroud Tip Objects. Profiles are allowed, and sometimes required, beyond a tip.

The profiles must be listed in the file in order from hub to shroud. Individual profile datasets are separated by a line beginning with the "#" character. Any text following the "#" character is used as the name associated with the subsequent profile.

For example:

# Hub Profile
0.0  0.0  1.0 le
1.0  0.0  1.0
1.0  1.0  1.0 te
0.0  1.0  1.0
0.0  0.0  1.0
# Intermediate Blade Profile
0.0  0.0  2.0 le
1.0  0.0  2.0
1.0  1.0  2.0 te
0.0  1.0  2.0
0.0  0.0  2.0
# Shroud Tip Profile
0.0  0.0  2.75 le
1.0  0.0 2.75
1.0  1.0 2.75 te
0.0  1.0 2.75
0.0  0.0 2.75
# Shroud Profile
0.0  0.0  3.0 le
1.0  0.0  3.0
1.0  1.0  3.0 te
0.0  1.0  3.0
0.0  0.0  3.0

There is no restriction on the number of profiles or the number of data points in a profile dataset. However, as noted above, a minimum of two profiles is required.

Set Coordinates, Angle Units, and Length Units according to the data in the blade file.

The Method setting allows two preset methods, and one general method, for controlling the settings that govern the geometric representation of blade surfaces (that is, the Lofting, Curve Type, and Surface Type settings, described shortly).

The available Method options are:

The following rules are followed by Ansys TurboGrid for selecting the geometric representation method:

The direction in which lofting occurs is set by the Lofting setting. The available Lofting options are:

Figure 10.4: Spanwise Lofting versus Streamwise Lofting shows how spanwise lofting and streamwise lofting differ.

Figure 10.4: Spanwise Lofting versus Streamwise Lofting

The appropriate lofting setting depends on how the geometry was produced. For example, BladeModeler can produce blades via streamwise or spanwise lofting. The appropriate setting is stored in the BladeGen.inf file. As another example, a flank-milled blade should be generated and interpreted using two blade profiles (one at (or near) the hub and one at (or near) the shroud) with streamwise lofting.

The set of curves that are used to loft the blade surface may be constructed in one of two ways, as determined by the Curve Type setting. The available Curve Type options are:

The manner in which the set of curves is lofted is controlled by the Surface Type setting. The available Surface Type options are:

The Cut-off or square option is an option that, when not using ATM3D, may be used to create a flat leading/trailing edge between two edge curves. See Figure 10.5: "Cut-off or square" Trailing Edge for an example of a trailing edge that uses the Cut-off or square option; note that the trailing edge is defined by a pair of trailing-edge curves.

Figure 10.5: "Cut-off or square" Trailing Edge

The Cut-off or square option is intended for use on blade profiles that have discontinuities in slope at the edges. Use of this option on rounded or blunt leading/trailing edges may result in edge curves that are not placed in optimal locations (that is, further adjustments may be necessary).

A "cut-off or square" edge having the same axial and radial coordinates at both cut-off points will have lines of rotation that coincide. In this case, TurboGrid considers the edge to be "cut-off". If the cut-off points do not have the same axial and radial coordinates, TurboGrid considers the edge to be "square", whether or not the edge appears, in a blade-to-blade view, to be orthogonal to the camberline.

Select Hub Blend and/or Shroud Blend as appropriate to specify which blends to generate using the rolling ball process. Specify the applicable Rolling Ball Radius values to be used in generating the blade blends.

A specified blade blend can optionally be rendered into a high-fidelity geometric representation, or true blend, for meshing with high-fidelity geometry. If you intend to mesh with high-fidelity geometry, see the description for the Blend Style setting in Defining Geometry from Generated CAD: CAD From Profile Points in the TurboGrid User's Guide.

Figure 10.6: Approximate Blend versus True Blend shows how an approximate blend differs from a true blend; an approximate blend meets the hub/shroud at a small angle whereas a true blend meets the hub/shroud asymptotically. The small angle is required to support ATM topology; no such requirement exists for ATM3D topology.

Figure 10.6: Approximate Blend versus True Blend

A true blend is considered to be a type of complex blade end. As a result, when you specify a true blend:

For details, see Blade CAD Rotation Axis.

For details, see Generated CAD Definition.

Set Tip Option to one of the following:

For details, see Blade CAD Rotation Axis.

For details, see Generated CAD Definition.

For a blade without blends, you can rotate the blade from its data-defined orientation by a specified blade stagger angle about the defined blade CAD rotation axis.

Set Option to one of the following:

For details, see Blade CAD Rotation Axis.

For details, see Generated CAD Definition.

Specify the X, Y, and Z coordinates of two points, From and To, that define a vector along the rotation axis of the first (as given by the profile point data) blade instance. The right-hand rule, as applied to that vector, determines the sense of positive rotation.

The Blade CAD Rotation Axis specification appears on each tab of the object editor as a convenience because it is needed by multiple CAD features (for example, to help define the shape and position of the button part of a partial tip, and to define the rotation axis when applying a blade stagger angle).

The Generated CAD Definition settings are only available if, in the geometry browser (in the Geometry workspace), Input Mode is still set to Profile Points. These settings are provided as a convenience to allow you to specify the blade CAD feature settings, change the input mode to CAD From Profile Points and generate the geometry, all from the Blade CAD Features object editor. Once the input mode is set to CAD From Profile Points, the Generated CAD Definition settings are not displayed in the Blade CAD Features object editor and you must go to the geometry browser to make changes to the name of the Parasolid file.

The blade CAD feature settings are independent of the geometry except during generation of the CAD definition, at which time the CAD definition is updated according to the current blade CAD feature settings.

To change the specified CAD file to be used for the blade CAD features (and rest of the geometry), you can click the Browse   icon to select a CAD file using a browser: the Set CAD File dialog box.

Clicking the Apply And Generate CAD button applies the blade CAD feature settings and then generates (or regenerates) the CAD geometry.

After the blade CAD feature settings have been applied, one or more objects appear in the Mesh workspace tree, in the Geometry branch, under the applicable blade.

Generation (or regeneration) of the CAD geometry involves running Ansys BladeEditor temporarily in the background to generate a Parasolid file and associated TurboGrid Initialization file, then loading those two files into TurboGrid, resulting in new/updated CAD objects and (in accordance with the contents of the TurboGrid Initialization file) new/updated topological entities in the Geometry workspace tree.

The resulting CAD geometry not only includes the blade CAD features but the entire geometry, including the blade and passage.

While working, you might want to reduce the number of times that the CAD geometry is generated because of the significant processing time required.

Clicking the Apply button applies the blade CAD feature settings without generating (or regenerating) the CAD geometry.

After the blade CAD feature settings have been applied, one or more objects appear in the Mesh workspace tree, in the Geometry branch, under the applicable blade.

To generate (or regenerate) the CAD geometry at any later time, even after saving a state file and then loading that state file into a new session of TurboGrid, you can select File > Update Geometry from the main menu or you can click the Apply And Generate CAD button.

The leading edge curve appears green in the viewer window and each point on the curve (one for each blade profile, or rib, curve) is marked with an octahedron symbol. The points are listed from hub to shroud. Edit the individual leading edge point locations to create the correct leading edge curve for the blade.

The quality of the mesh is dependent on the accuracy of the leading edge curve. In most cases, the initial placement of leading edge points is adequate. However there are some cases when some points may need to be moved.

Any change to the leading edge changes the blade surfaces, which changes the periodic surfaces as well as the hub and shroud surfaces. In order to avoid the delays associated with recreating the entire geometry after any modification to the leading edge, another step is required. The blade must be saved after the modifications to the leading edge are complete. For details, see Save Blade As Command. The saved blade file contains data in the fourth field to designate the leading edge points. To complete the leading edge modification, the blade object must be updated with this new blade file. For details, see The Blade Set Object and Blade Objects.

There are several steps required to edit the location of a point on the leading edge curve.

Picking Mode can also be used to select and translate leading edge points in the viewer. For details, see Selecting and Dragging Objects while in Viewing Mode. After moving the leading edge point, it will snap to the nearest point on the current profile curve.

If the leading edge points were designated in the blade file, it may not be necessary to adjust them since, in that case, the leading edge curve may already be acceptable. For details, see Coordinate System and Blade File Definition.

If a leading or trailing edge point has been moved, the Save & Load button appears. Clicking this button causes the modified blade profile data to be saved to a profile file (you will be prompted for the name), then reloaded (from the same file) in order for the new geometry to take effect. The blade and trailing edge objects also have this feature.

The Automatically generate required intermediate points option is available only before the hub, shroud, and blade are loaded. It is on by default. This option causes a set of intermediate points to be generated between the low hub point and low shroud point upon loading the geometry. TurboGrid aims to add an appropriate number of points, placed at locations that follow the leading or trailing edge of the blade.

The inlet/outlet curve consists of a set of points that guide the meridional shape of the inlet end of the passage mesh as a function of the local spanwise direction. By default, a set of points is automatically generated (see Automatically generate required intermediate points).

The inlet/outlet curve can be defined by creating, modifying, or deleting points in the list of points. There must be a point at both the hub and shroud while additional points are optional. The points are connected linearly and must be listed in order from hub to shroud, or they will be ignored.

A point can be selected by clicking on it in the list of points or by picking it in the viewer window. For details on picking points in the viewer, see Selecting and Dragging Objects while in Viewing Mode. The available icons become active when a point is selected. Alternatively, you can right-click an existing point in the list of points to see the same options. Each icon and its function is described in the following table:

You can modify the location of the selected point by:

Set Method to one of the available options:

Regardless of the method used to modify the location of the selected point, the location is restricted. The low hub point snaps to the line of intersection between the hub and low periodic surfaces. The low shroud point snaps to the line of intersection between the shroud and low periodic surfaces. Use the OUTLINE object as a guide when dragging the points. Any other points between the hub and shroud snap to the low periodic surface and are not constrained in the spanwise or streamwise directions. Inlet points cannot be moved further downstream on the low periodic surface than a position level with the leading edge of the blade. After you have clicked Apply, or dragged a point, the Selected Point setting will show the actual position to which the point has moved.

The visibility of the inlet or outlet points is controlled by the Point Visibility check box.

You can select and move points in the following ways:

You can move the passage interface upstream or downstream by decreasing or increasing the Hub and Shroud values, which control where the interface meets the hub and shroud, respectively.