Sweep Feature
The element tree for the sweep feature is documented in the header file ProSweep.h, and is shown in the following figure.
Figure 63. Element Tree for Sweep Feature
The following table describes the elements in the element tree for sweeps:
Element ID | Data Type | Description |
|---|---|---|
PRO_E_FEATURE_FORM | PRO_VALUE_TYPE_INT | Specifies the feature form. The valid value is PRO_SWEEP defined in the enumerated data type ProFeatFormType in ProFeatForm.h. |
PRO_E_SWEEP_TYPE | PRO_VALUE_TYPE_INT | Specifies the type of sweep. The valid value is PRO_SWEEP_TYPE_MULTI_TRAJ defined in the enumerated data type ProSweepType. |
PRO_E_SWEEP_FRAME_COMP | Compound | This compound element specifies the trajectories and orientation of the section plane. For more information on this element, refer to the section Element Tree for PRO_E_SWEEP_FRAME_ COMP. |
PRO_E_SWEEP_PROF_COMP | Compound | This compound element defines the sweep type and holds the sketch related elements for the sweep cross section. |
PRO_E_SWP_SEC_TYPE | PRO_VALUE_TYPE_INT | Specifies the type of sweep. The valid value is PRO_SWEEP_CONST_SECTION defined in the enumerated data type ProSweepSecType. The option specifies a constant section sweep. |
PRO_E_SWEEP_SECTION | Compound | This compound element contains the sketch for the sweep cross section. |
PRO_E_SKETCHER | PRO_VALUE_TYPE_POINTER | Specifies a sketcher pointer. The user defined sketch can be directly retrieved from this element. |
PRO_E_SWP_ATTR | Compound | This compound element defines the sweep attributes. The element is available only for surface sweeps. |
PRO_E_END_SRF_ATTR | PRO_VALUE_TYPE_INT | Specifies the option to keep the end of sweep feature open or capped. The enumerated data type ProSweepEndSrfAttr contains the valid values for this element: • PRO_SWEEP_END_SRF_OPEN • PRO_SWEEP_END_SRF_CAPPED |
PRO_E_STD_FEATURE_NAME | PRO_VALUE_TYPE_WSTRING | Specifies the name of the feature. The default value is SWEEP. |
PRO_E_EXT_SURF_CUT_SOLID_TYPE | PRO_VALUE_TYPE_INT | Specifies a solid or surface feature type. The enumerated data type ProSweepFeatType contains the following valid values for this element: • PRO_SWEEP_FEAT_TYPE_SOLID • PRO_SWEEP_FEAT_TYPE_SURFACE |
PRO_E_REMOVE_MATERIAL | PRO_VALUE_TYPE_INT | Specifies whether to extrude or remove the material along the sweep. The enumerated data type ProSweepRemMaterial contains the following valid values for this element: • PRO_SWEEP_MATERIAL_ADD • PRO_SWEEP_MATERIAL_REMOVE |
PRO_E_FEAT_FORM_IS_THIN | PRO_VALUE_TYPE_INT | Specifies whether to create a thin section. The enumerated data type ProSweepFeatForm contains the following valid values for this element: • PRO_SWEEP_FEAT_FORM_NO_THIN • PRO_SWEEP_FEAT_FORM_THIN |
PRO_E_STD_MATRLSIDE | PRO_VALUE_TYPE_INT | Specifies the direction in which material will be added with respect to the sketch. This element is mandatory for all cuts and thin features. The enumerated data type ProSweepMatlSide contains the following valid values for this element: • PRO_SWEEP_MATERIAL_SIDE_ONE • PRO_SWEEP_MATERIAL_SIDE_TWO • PRO_SWEEP_MATERIAL_BOTH_SIDES |
PRO_E_THICKNESS | PRO_VALUE_TYPE_DOUBLE | Specifies the thickness for the thin feature. This element is mandatory for thin features. |
PRO_E_TRIM_QUILT | PRO_VALUE_TYPE_SELECTION | Specifies the selection of quilt to be trimmed. |
PRO_E_TRIM_QLT_SIDE | PRO_VALUE_TYPE_INT | Specifies the side of the quilt to be trimmed. This element is relevant when the element PRO_E_STD_MATRLSIDE has its value as PRO_SWEEP_MATERIAL_BOTH_SIDES. The enumerated data type ProSweepTrimQltSide contains the following valid values for this element: • PRO_SWEEP_TRIMQLT_SIDE_ONE • PRO_SWEEP_TRIMQLT_SIDE_TWO |
PRO_E_BODY | Compound element | Compound element for body options. |
PRO_E_BODY_USE | PRO_VALUE_TYPE_INT | Mandatory. Specifies the body to add geometry to. Defined by the enumerated data type ProBodyUseOpts and the valid values follow: • PRO_BODY_USE_NEW— Feature stores its geometry in the new body. • PRO_BODY_USE_SELECTED—Feature adds its geometry to single selected body. |
PRO_E_BODY_SELECT | PRO_VALUE_TYPE_SELECTION | Specifies the reference to the selected bodies. Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_SELECTED. |
For elements specific to sheetmetal, refer to the section Production Applications: Sheetmetal.