Element Trees: Extrude and Revolve

The Element Tree for Extruded Features

The element tree for extrude features is documented in the header file ProExtrude.h. The functions ProFeatureTypeGet() and ProFeatureSubtypeGet() return an Extrude feature. The types of Extrude features are:

•

Protrusion

•

Cut

•

Surface

•

Surface Trim

•

Thin Protrusion

•

Thin Cut

•

Sheetmetal Cut

•

Sheetmetal Unattached Wall

Refer to the section Production Applications: Sheetmetal for element details on sheetmetal features.

The extrude element tree contains toggles to switch between different feature types. An extruded feature tree also contains subtrees supporting the section and depth parameters for the feature.

You can use Intent Datums such as Intent Point, Intent Axis, and Intent Plane for depth reference in extrude features.

The following figure shows the element tree for extruded features.

The Element Tree for Extruded Feature

The elements are assigned values depending on the type of extrusion you want to create.

The following table lists the common elements for all types of extrusions and their permissible values:

Element ID

Value

PRO_E_FEATURE_TYPE

Feature type, not required for creation: PRO_FEAT_PROTRUSION

PRO_FEAT_CUT

PRO_FEAT_DATUM_SURFN

PRO_E_FEATURE_FORM

Mandatory = PRO_EXTRUDE

PRO_E_EXT_SURF_CUT_SOLID_TYPE

Mandatory

Of type ProExtFeatType

= PRO_EXT_FEAT_TYPE_SOLID

for Solid feature type

= PRO_EXT_FEAT_TYPE_SURFACE

for Surface feature type

PRO_E_REMOVE_MATERIAL

Material Removal

Of type ProExtRemMaterial

= PRO_EXT_MATERIAL_ADD

for a Protruded feature

= PRO_EXT_MATERIAL_REMOVE

for a Cut feature

PRO_E_STD_SECTION

Standard section elements

PRO_E_BODY

Compound Element. Specifies the body options.

PRO_E_STD_DIRECTION*

Direction of creation.

Of type ProExtDirection

= PRO_EXT_CR_IN_SIDE_ONE

for depth in side one

= PRO_EXT_CR_IN_SIDE_TWO

for depth in side two

PRO_E_STD_MATRLSIDE*

Direction of material affected with respect to the sketch. Required for all cuts, all thin features, and for solid protrusions with open sections.

PRO_E_STD_EXT_DEPTH

Compound Element. Specifies the depth type and value for the extrude feature.

PRO_E_EXT_DEPTH_TO

Compound Element. Specifies the depth type and value for Side 1, that is, extrusion in the first direction from the sketch plane.

PRO_E_EXT_DEPTH_TO_TYPE

Mandatory element. Specifies the type of depth for Side 1. The depth type is specified using the enumerated data type ProExtDepthToType. The valid values are:

•

PRO_EXT_DEPTH_TO_BLIND—Extrudes a section from the sketching plane to the specified depth value.

•

PRO_EXT_DEPTH_TO_NEXT—Extrudes a section from the sketching plane to the first surface that it reaches.

•

PRO_EXT_DEPTH_TO_ALL—Extrudes a section from the sketching plane to the last surface it reaches.

•

PRO_EXT_DEPTH_TO_UNTIL—Extrudes a section to intersect with a selected surface.

•

PRO_EXT_DEPTH_TO_REF—Extrudes a section to a selected point, curve, plane, or surface.

•

PRO_EXT_DEPTH_SYMMETRIC—Extrudes a section on each side of the sketching plane by half of the specified depth value in each direction.

PRO_E_EXT_DEPTH_TO_REF

Specifies the reference element for Side 1, when the depth type is PRO_EXT_DEPTH_TO_REF or PRO_EXT_DEPTH_TO_UNTIL. The valid reference types are:

•

PRO_SURFACE

•

PRO_AXIS

•

PRO_EDGE

•

PRO_CURVE

•

PRO_POINT

•

PRO_EDGE_START

•

PRO_EDGE_END

•

PRO_CRV_START

•

PRO_CRV_END

•

PRO_BODY

PRO_E_EXT_DEPTH_TO_REF_TRF

Specifies the options available for the depth type PRO_EXT_DEPTH_TO_REF for Side 1. The depth type is specified using the enumerated data type ProExtDepthRefOpt. The valid values are:

•

PRO_EXT_DEPTH_REF_NONE—Extrudes a section to a selected point, curve, plane, or surface.

•

PRO_EXT_DEPTH_REF_OFFS—Extrudes a section to an offset of the selected point, curve, plane, or surface.

•

PRO_EXT_DEPTH_REF_TRNSLT—Extrudes a section to a translation of the selected point, curve, plane, or surface.

PRO_E_EXT_DEPTH_TO_REF_TRF_VAL

Specifies the offset or translation value for Side 1, when the depth type is PRO_EXT_DEPTH_TO_REF, and the option type is PRO_EXT_DEPTH_REF_OFFS or PRO_EXT_DEPTH_REF_TRNSLT.

PRO_E_EXT_DEPTH_TO_VALUE

Specifies the value of depth for Side 1, when the depth type is PRO_EXT_DEPTH_TO_BLIND or PRO_EXT_DEPTH_SYMMETRIC.

PRO_E_EXT_DEPTH_FROM

Compound Element. Specifies the depth type and value for Side 2, that is, extrusion in the second direction from the sketch plane.

PRO_E_EXT_DEPTH_FROM_TYPE

Mandatory element. Specifies the type of depth for Side 2. The depth type is specified using the enumerated data type ProExtDepthFromType. The valid values are:

•

PRO_EXT_DEPTH_FROM_BLIND—Extrudes a section from the sketching plane to the specified depth value.

•

PRO_EXT_DEPTH_FROM_NEXT—Extrudes a section from the sketching plane to the first surface that it reaches.

•

PRO_EXT_DEPTH_FROM_ALL—Extrudes a section from the sketching plane to the last surface it reaches.

•

PRO_EXT_DEPTH_FROM_UNTIL—Extrudes a section to intersect with a selected surface.

•

PRO_EXT_DEPTH_FROM_REF—Extrudes a section to a selected point, curve, plane, or surface.

•

PRO_EXT_DEPTH_FROM_NONE—Extrudes a section only on Side 1 from the sketch plane, no extrusion on Side 2.

PRO_E_EXT_DEPTH_FROM_REF

Specifies the reference element for Side 2, when the depth type is PRO_EXT_DEPTH_FROM_REF or PRO_EXT_DEPTH_FROM_UNTIL. The valid reference types are:

•

PRO_SURFACE

•

PRO_AXIS

•

PRO_EDGE

•

PRO_CURVE

•

PRO_POINT

•

PRO_EDGE_START

•

PRO_EDGE_END

•

PRO_CRV_START

•

PRO_CRV_END

•

PRO_BODY

PRO_E_EXT_DEPTH_FROM_REF_TRF

Specifies the options available for the depth type PRO_EXT_DEPTH_FROM_REF for Side 2. The depth type is specified using the enumerated data type ProExtDepthRefOpt. The valid values are:

•

PRO_EXT_DEPTH_REF_NONE—Extrudes a section to a selected point, curve, plane, or surface.

•

PRO_EXT_DEPTH_REF_OFFS—Extrudes a section to an offset of the selected point, curve, plane, or surface.

•

PRO_EXT_DEPTH_REF_TRNSLT—Extrudes a section to a translation of the selected point, curve, plane, or surface.

PRO_E_EXT_DEPTH_FROM_REF_TRF_VAL

Specifies the offset or translation value for Side 2, when the depth type is PRO_EXT_DEPTH_FROM_REF, and the option type is PRO_EXT_DEPTH_REF_OFFS or PRO_EXT_DEPTH_REF_TRNSLT.

PRO_E_EXT_DEPTH_FROM_VALUE

Specifies the value of depth for Side 2, when the depth type is PRO_EXT_DEPTH_FROM_BLIND.

PRO_E_STD_FEATURE_NAME

Default given by application depending

on the feature type. Can be modified by the user.

PRO_E_EXT_COMP_DRFT_ANG

Draft Compound Element that allows you to add a draft on the extrude feature.

PRO_E_EXT_DRFT_ANG

Draft of type ProExtDrftAng.

•

PRO_EXT_DRFT_ANG_NO_DRAFT—To create extruded features without a draft.

•

PRO_EXT_DRFT_ANG_DRAFT—To create extruded features with a draft.

PRO_E_EXT_DRFT_ANG_VAL

The draft angle. The draft angle can have value between [-89.9, 89.9].

PRO_E_FEAT_THIN

Compound element. It specifies how to close a thin feature when one or more surfaces can be used to cap, that is, close the feature and attach it to the solid geometry. Here the sketch is an open sketch.

PRO_E_FEAT_THIN_STRT

Compound element. It specifies the options for the first end point of the thin feature.

PRO_E_FEAT_THIN_STRT_OPT

Specifies how to cap the first end point of the thin feature using the enumerated data type ProFeatThinOpt. The valid values are:

•

PRO_FEAT_THIN_IGNORE—Caps the feature as a free end. When you specify this value, the feature is created with a free end even if a reference edge or surface is available to cap the feature.

•

PRO_FEAT_THIN_DEFAULT—Caps the feature to the specified edge or surface.

PRO_E_FEAT_THIN_STRT_REF

Specifies the edge or surface that must be used to cap and attach the first end point of the feature to the solid geometry.

PRO_E_FEAT_THIN_END

Compound element. It specifies the options for the second end point of the feature.

PRO_E_FEAT_THIN_END_OPT

Specifies how to cap the second end point of the thin feature using the enumerated data type ProFeatThinOpt. The valid values are:

•

PRO_FEAT_THIN_IGNORE—Caps the feature as a free end. When you specify this value, the feature is created with a free end even if a reference edge or surface is available to cap the feature.

•

PRO_FEAT_THIN_DEFAULT—Caps the feature to the specified edge or surface.

PRO_E_FEAT_THIN_END_REF

Specifies the edge or surface that must be used to cap and attach the second end point to the solid geometry.

PRO_E_SMT_NEW_BODY_LINKED

Specifies if the sheetmetal body is linked to a part.

Elements identified with ‘*’ depend on the definition of the standard section. These elements are not assigned values until the standard section has been completely allocated (which typically happens during redefine of the feature). Values assigned to these elements while the section is not complete are ignored.

The following table lists the elements needed to create extruded features, in addition to those already discussed:

Feature Type

Element ID

Comment

Solid

PRO_E_EXT_COMP_DRFT_ANG

Compound element to specify draft options.

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Mandatory. Specifies the body to add geometry to.

The valid values are:

•

PRO_BODY_USE_NEW—The geometry in the feature is stored in the new body.

•

PRO_BODY_USE_SELECTED—The geometry in the feature is stored in the single selected body.

PRO_E_BODY_SELECTED

Specifies the reference to the selected body.

Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_SELECTED

Note

Only single reference is allowed.

Thin

PRO_E_THICKNESS

Mandatory >= 0.0

Of type PRO_VALUE_TYPE_DOUBLE

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Mandatory. The valid values for PRO_BODY_USE_NEW and PRO_BODY_USE_SELECTED are same as Solid.

PRO_E_BODY_SELECTED

Same as Solid.

PRO_E_FEAT_FORM_IS_THIN

Of Type ProExtFeatForm

= PRO_EXT_FEAT_FORM_NO_THIN for a feature not having Thin

= PRO_EXT_FEAT_FORM_THIN for a Thin feature

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProExtMatlSide

PRO_E_FEAT_THIN

Compound element to specify options to cap and attach thin features to solid geometry.

Solid Cut

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Mandatory. Specifies the body features that cuts the geometry.

The valid values are:

•

PRO_BODY_USE_ALL—The geometry in the feature is cut by all the existing bodies.

•

PRO_BODY_USE_SELECTED—The geometry in the feature is stored in the selected bodies.

PRO_E_BODY_SELECTED

Specifies the reference to the selected bodies.

Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_SELECTED

Note

Multiple references are allowed.

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProExtMatlSide

PRO_E_EXT_COMP_DRFT_ANG

Draft compound element for features that do not have feature form as Thin.

PRO_E_FEAT_FORM_IS_THIN

Of Type ProExtFeatForm

= PRO_EXT_FEAT_FORM_NO_THIN for a feature not having Thin

= PRO_EXT_FEAT_FORM_THIN for a Thin feature

Thin Cut

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Same as Solid Cut

PRO_E_BODY_SELECTED

Same as Solid Cut

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProExtMatlSide

PRO_E_THICKNESS

Mandatory >= 0.0

Of type PRO_VALUE_TYPE_DOUBLE

PRO_E_FEAT_FORM_IS_THIN

Of Type ProExtFeatForm

= PRO_EXT_FEAT_FORM_NO_THIN for a feature not having Thin

= PRO_EXT_FEAT_FORM_THIN for a Thin feature

Surface

PRO_E_SRF_END_ATTRIBUTES

Mandatory

Of type ProExtSurfEndAttr

It must be assigned at the same time or after the section is fully completed.

PRO_E_EXT_COMP_DRFT_ANG

Draft compound element for features that do not have feature form as Thin.

PRO_E_FEAT_FORM_IS_THIN

Of Type ProExtFeatForm

= PRO_EXT_FEAT_FORM_NO_THIN for a feature not having Thin

= PRO_EXT_FEAT_FORM_THIN for a Thin feature

Surface Trim

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProExtMatlSide

PRO_E_TRIM_QUILT

Mandatory

Of type Quilt

PRO_E_TRIM_QLT_SIDE

Mandatory

Of typeProExtTrimQltSide

PRO_E_FEAT_FORM_IS_THIN

Of Type ProExtFeatForm

= PRO_EXT_FEAT_FORM_NO
_THIN for a feature not having Thin

= PRO_EXT_FEAT_FORM
_THIN for a Thin feature

PRO_E_EXT_COMP_DRFT_ANG

Draft compound element for features that do not have feature form as Thin.

Thin Surface Trim

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProExtMatlSide

PRO_E_THICKNESS

Mandatory >= 0.0

Of type PRO_VALUE_TYPE_DOUBLE

PRO_E_TRIM_QUILT

Mandatory

Of type Quilt

PRO_E_TRIM_QLT_SIDE

Mandatory

Of type ProExtTrimQltSide

if PRO_E_STD_MATRLSIDE is “both”. Must be assigned at the same time as PRO_E_STD_MATRLSIDE.

PRO_E_FEAT_FORM_IS_THIN

Of Type ProExtFeatForm

= PRO_EXT_FEAT_FORM_NO
_THIN for a feature not having Thin

= PRO_EXT_FEAT_FORM_THIN for a Thin feature

Examples: Creating Extruded Features

The following examples demonstrate creation of extrude features of various forms. These examples are adapted from an example template file UgSktExtrusionTemplate.c available on the Creo Parametric load point under protoolkit/protk_appls/pt_userguide/ptu_featcreat.

•

Example 1: Creating an Extruded Feature

•

Example 2: To Create an Extruded Cut with Two-sided Thru-all Depth

•

Example 3: To Create an Extruded Thin Cut

•

Example 4: To Create an Extruded Datum Surface Feature

•

Example 5: To Create a Surface Trim Extruded Feature

Conventional Approach

Example 1: Creating an Extruded Feature

The sample code in the file UserSktExtrusionProtrusion.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create an Extruded Protrusion by the conventional approach for sketched features. The example creates an incomplete feature using ProFeatureCreate(), extracts the section from the element tree of the incomplete feature, builds the section on the section handle obtained, and, completes the feature using ProFeatureRedefine().

The user is prompted to select the sketching and the orientation planes and then the reference edges for the sketch. The user is also required to enter the X and Y offsets to be applied to the sketch from the projected edges.

Example 2: To Create an Extruded Cut with Two-sided Thru-all Depth

The sample code in the file UgSktExtrusionCut.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create an extruded cut with two-sided thru-all depth.

Example 3: To Create an Extruded Thin Cut

The sample code in the file UgSktExtrusionCut.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create an extruded thin cut. Its depth is two-sided, up to a selected reference.

Example 4: To Create an Extruded Datum Surface Feature

The sample code in the file UgSktExtrusionSurfaceCapped.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create an extruded datum surface feature. Its depth is one-side blind.

Example 5: To Create a Surface Trim Extruded Feature

The sample code in the file UgSktExtrusionSurfaceTrim.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create an extruded surface trim. Its depth is one-side blind.

Direct Creation Approach

The sample code in the file UgSktExtrusionCreate.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create an extruded protrusion by the direct approach for sketched features introduced in Pro/ENGINEER Wildfire. The user is prompted to select a sketched datum curve feature that is used as a section for the created protrusion.

The Element Tree for Revolved Features

The element tree for revolved features is documented in the header file ProRevolve.h, and has a fairly simple structure. It shows that, apart from the usual elements for the tree root and feature name, a revolved feature tree contains the elements to make the feature a solid protrusion, a thin protrusion, a solid cut, a thin cut, a surface, a surface trimmed feature, or a thin surface trimmed feature.

You can use Intent Datums such as Intent Axis, Intent Plane, and Intent Point for placement references.

The following figure shows the element tree for revolved features.

Element Tree for Revolved Feature

The elements are assigned values depending on the type of revolved feature you want to create.

The following table lists the common elements for all types of revolved features and their permissible values:

Element ID

Value

PRO_E_FEATURE_TYPE

Feature type:

PRO_FEAT_PROTRUSION

PRO_FEAT_CUT

PRO_FEAT_DATUM_SURF

Not required for creation.

PRO_E_FEATURE_FORM

Mandatory= PRO_REVOLVE

PRO_E_EXT_SURF_CUT_SOLID_TYPE

Mandatory

Of type ProRevFeatType

= PRO_REV_FEAT_TYPE_SOLID

for Solid feature type

= PRO_REV_FEAT_TYPE_SURFACE

for Surface feature type

PRO_E_FEAT_FORM_IS_THIN

Feature Form

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO
_THIN

for a Solid feature

= PRO_REV_FEAT_FORM_THIN

for a Thin feature

PRO_E_REMOVE_MATERIAL

Material Removal

Of type ProRevRemMaterial

= PRO_REV_MATERIAL_ADD

for a Protruded feature

= PRO_REV_MATERIAL_REMOVE

for a Cut feature

PRO_E_STD_SECTION

Standard section elements.

PRO_E_BODY

Compound Element

PRO_E_STD_DIRECTION*

Direction of creation.

Of type ProRevDirection

= PRO_REV_CR_IN_SIDE_ONE

for angle in side one

= PRO_REV_CR_IN_SIDE_TWO

for angle in side two

PRO_E_STD_MATRLSIDE*

Direction of material affected with respect to the sketch. It is required for all cuts, all thin features, and for solid protrusions with open sections.

PRO_E_REVOLVE_AXIS_OPT

Optional, of the type ProRevAxisOptAttr. Identifies if the axis to revolve about is a part of the sketch or an external datum axis.

PRO_E_REVOLVE_AXIS

Optional. Reference to external datum axis, if PRO_E_REVOLVE_AXIS = PRO_REV_AXIS_EXT_REF.

PRO_E_REV_ANGLE

Compound Element

PRO_E_REV_ANGLE_TO

Compound Element

PRO_E_REV_ANGLE_TO_TYPE

Mandatory

Of type ProRevAngleToType

PRO_E_REV_ANGLE_TO_VAL

Depends on PRO_E_REV_ANGLE_TO_TYPE

Of type PRO_VALUE_TYPE_DOUBLE (in degrees)

PRO_E_REV_ANGLE_TO_REF

Depends on PRO_E_REV_ANGLE_TO_TYPE

Of type listed in the Angle Type table that follows.

PRO_E_REV_ANGLE_FROM

Compound Element

PRO_E_REV_ANGLE_FROM_TYPE

Mandatory

Of type ProRevAngleFromType

PRO_E_REV_ANGLE_FROM_VAL

Depends on PRO_E_REV_ANGLE_FROM_TYPE

Of type PRO_VALUE_TYPE_DOUBLE (in degrees)

PRO_E_REV_ANGLE_FROM_REF

Depends on PRO_E_REV_ANGLE_FROM_TYPE

Of type listed in the Angle Type table that follows.

PRO_E_STD_FEATURE_NAME

Default given by application depending

on the feature type. Can be modified by the user.

PRO_E_FEAT_THIN

Compound element. It specifies how to close a thin feature when one or more surfaces can be used to cap, that is, close the feature and attach it to solid geometry. Here the sketch is an open sketch.

PRO_E_FEAT_THIN_STRT

Compound element. It specifies the options for the first end point of the thin feature.

PRO_E_FEAT_THIN_STRT_OPT

Specifies how to cap the first end point of the thin feature using the enumerated data type ProFeatThinOpt. The valid values are:

•

PRO_FEAT_THIN_IGNORE—Caps the feature as a free end. When you specify this value, the feature is created with a free end even if a reference edge or surface is available to cap the feature.

•

PRO_FEAT_THIN_DEFAULT—Caps the feature to the specified edge or surface.

PRO_E_FEAT_THIN_STRT_REF

Specifies the edge or surface that must be used to cap and attach the first end point to the solid geometry.

PRO_E_FEAT_THIN_END

Compound element. It specifies the options for the second end point of the thin feature.

PRO_E_FEAT_THIN_END_OPT

Specifies how to cap the second end point of the thin feature using the enumerated data type ProFeatThinOpt. The valid values are:

•

PRO_FEAT_THIN_IGNORE—Caps the feature as a free end. When you specify this value, the feature is created with a free end even if a reference edge or surface is available to cap the feature.

•

PRO_FEAT_THIN_DEFAULT—Caps the feature to the specified edge or surface.

PRO_E_FEAT_THIN_END_REF

Specifies the edge or surface that must be used to cap and attach the second end point to the solid geometry.

PRO_E_SMT_NEW_BODY_LINKED

Specifies if the sheetmetal body is linked to a part.

Elements identified with ‘*’ depend on the definition of the standard section. These elements may not be assigned values until the standard section has been completely allocated (which typically happens during redefine of the feature). Values assigned to these elements while the section is not complete are ignored.

The following table lists the angle types for revolved features along with possible valid references:

Angle Type	Valid Reference Types
PRO_REV_ANGLE_TO_REF	PRO_POINT, PRO_EDGE_START, PRO_EDGE_END, PRO_CRV_START, PRO_CRV_END, PRO_SURFACE (Plane).
PRO_REV_ANGLE_FROM_REF	PRO_POINT, PRO_EDGE_START, PRO_EDGE_END, PRO_CRV_START, PRO_CRV_END, PRO_SURFACE (Plane).

The following table lists the elements needed to create revolved features, in addition to those already discussed:

Feature Type

Element ID

Comment

Solid

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Mandatory. Specifies the body to add geometry to.

The valid values are:

•

PRO_BODY_USE_NEW—The geometry in the feature is stored in the new body.

•

PRO_BODY_USE_SELECTED—The geometry in the feature is stored in the single selected body.

PRO_E_BODY_SELECTED

Specifies the reference to the selected body.

Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_SELECTED

Note

Only single reference is allowed.

Thin

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProRevMatlSide

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Same as Solid

PRO_E_BODY_SELECTED

Same as Solid

PRO_E_THICKNESS

Mandatory >= 0.0

Of type PRO_VALUE_TYPE_DOUBLE

PRO_E_FEAT_FORM_IS_THIN

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO
_THIN for feature not having Thin

= PRO_REV_FEAT_FORM_THIN for a Thin feature

PRO_E_FEAT_THIN

Compound element to specify options to cap and attach thin features to solid geometry.

Solid Cut

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Mandatory. Specifies the body features that cuts the geometry.

The valid values are:

•

PRO_BODY_USE_ALL—The geometry in the feature is cut by all the existing bodies.

•

PRO_BODY_USE_SELECTED—The geometry in the feature is stored in the selected bodies.

PRO_E_BODY_SELECTED

Specifies the reference to the selected bodies.

Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_SELECTED

Note

Multiple references are allowed.

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProRevMatlSide

PRO_E_FEAT_FORM_IS_THIN

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO
_THIN for feature not having Thin

= PRO_REV_FEAT_FORM_THIN for a Thin feature

Thin Cut

PRO_E_BODY

Compound element

PRO_E_BODY_USE

Same as Solid Cut

PRO_E_BODY_SELECTED

Same as Solid Cut

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProRevMatlSide

PRO_E_THICKNESS

Mandatory >= 0.0

Of type PRO_VALUE_TYPE_DOUBLE

PRO_E_FEAT_FORM_IS_THIN

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO_THIN for feature not having Thin

= PRO_REV_FEAT_FORM_THIN for a Thin feature

Surface

PRO_E_SRF_END_ATTRIBUTES

Mandatory

Of type ProRevSurfEndAttr

Must be assigned at the same time or after the section is fully completed.

PRO_E_FEAT_FORM_IS_THIN

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO
_THIN for feature not having Thin

= PRO_REV_FEAT_FORM_THIN for a Thin feature

Surface Trim

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProRevMatlSide

PRO_E_TRIM_QUILT

Mandatory

Of type Quilt

PRO_E_TRIM_QLT_SIDE

Mandatory

Of type ProRevTrimQltSide if PRO_E_STD_MATRLSIDE is “both”. Must be assigned at the same time as PRO_E_STD_MATRLSIDE.

PRO_E_FEAT_FORM_IS_THIN

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO
_THIN for feature not having Thin

= PRO_REV_FEAT_FORM_THIN for a Thin feature

Thin Surface Trim

PRO_E_STD_MATRLSIDE

Mandatory

Of type ProRevMatlSide

PRO_E_THICKNESS

Mandatory >= 0.0

Of type PRO_VALUE_TYPE_DOUBLE

PRO_E_TRIM_QUILT

Mandatory

Of type Quilt

PRO_E_TRIM_QLT_SIDE

Mandatory

Of type ProRevTrimQltSide

PRO_E_FEAT_FORM_IS_THIN

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO
_THIN for feature not having Thin

= PRO_REV_FEAT_FORM_THIN for a Thin feature

Examples: Creating Revolved Features

The following examples demonstrate creation of revolved features of various forms. These examples are adapted from an example template file UgSktRevolveTemplate.c available on the Creo Parametric loadpoint under <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat.

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Example 6: To Create a Revolved Protrusion

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Example 7: To Create a Revolved Thin Cut

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Example 8: To Create a Revolved Surface

Example 6: To Create a Revolved Protrusion

The sample code in the file UgSktRevolveProtrusion.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create a revolved protrusion feature with symmetric depth.

Example 7: To Create a Revolved Thin Cut

The sample code in the file UserSktRevolveThinCut.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create a revolved thin cut, with independent angular dimensions for both sides.

Example 8: To Create a Revolved Surface

The sample code in the file UgSktRevolveSurface.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create a revolved surface. It includes all possible element assignments. By following the instructions for the feature you want to create, it is possible to remove element settings not appropriate for your use.

The Element Tree for First Features

First features (extrude and revolve solids created as the first feature in a part) require a subset of the standard element tree and some special handling for the section pointer.

The following table lists the elements applicable to first feature creation (extrude or revolve):

Element ID

Value

PRO_E_FEATURE_TYPE

Feature type: PRO_FEAT_FIRST

PRO_E_FEATURE_FORM

PRO_EXTRUDE / PRO_REVOLVE

PRO_E_FEAT_FORM_IS_THIN

Feature Form

Of Type ProRevFeatForm

= PRO_REV_FEAT_FORM_NO_THIN for a Solid feature = PRO_REV_FEAT_FORM_THIN for a Thin feature

PRO_E_BODY_USE

Mandatory. Specifies the body to add geometry to.

The valid values are:

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PRO_BODY_USE_NEW—The geometry in the feature is stored in the new body.

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PRO_BODY_USE_SELECTED—The geometry in the feature is stored in the single selected body.

PRO_E_BODY_SELECT

Specifies the reference to the selected body.

Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_SELECTED

Note

Only single reference is allowed.

PRO_E_SKETCHER

Sketcher pointer. Used because the standard section requires selected references not available in an empty model.

PRO_E_STD_MATRLSIDE*

Mandatory if thin

Of type ProExtMatlSide (Extrude)

Of type ProRevMatlSide (Revolve)

PRO_E_THICKNESS

Mandatory >= 0.0 if thin

Of type PRO_VALUE_TYPE_DOUBLE

PRO_E_EXT_DEPTH_FROM

Compound Element (Extrude only)

PRO_E_EXT_DEPTH_FROM_VAL

Depth dimension (of type PRO_VALUE_TYPE_DOUBLE) (Extrude only)

PRO_E_REV_ANGLE_FROM

Compound Element (Revolve only)

PRO_E_REV_ANGLE_FROM_VAL

Angular dimension (of type PRO_VALUE_TYPE_DOUBLE)

(Revolve only)

PRO_E_STD_FEATURE_NAME

Default given by application depending on the feature type. Can be modified by the user.

Example 9: Creating the First Extruded Protrusion Feature by Conventional Approach

The sample code in the file UgSktFirstFeatureCreate.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create the first extruded protrusion using the approach for the sketched features.

The following example:

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Creates an incomplete feature using ProFeatureCreate(),

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Extracts the section from the element tree of the incomplete feature,

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Builds the section on the section handle obtained, and,

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Completes the feature using ProFeatureRedefine().

Following is the change in the approach for Pro/ENGINEER Wildfire release:

Level of PRO_E_SKETCHER in an element tree is changed.

For any Pro/ENGINEER release previous to Wildfire:

PRO_E_FEATURE_TREE -> PRO_E_STD_SECTION -> PRO_E_SKETCHER

For Pro/ENGINEER Wildfire release:

PRO_E_FEATURE_TREE -> PRO_E_SKETCHER

Value of PRO_E_SKETCHER—A new ProValue is to be allocated and then assigned to the element (rather than the old approach of reusing the value extracted from the element tree).

Example 10: Creating the First Thin Revolve Protrusion Feature by Conventional Approach

The sample code in the file UgSktFirstFeatureRevCreate.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create a thin first revolve Protrusion using the approach for sketched features.

The following example:

•

Creates an incomplete feature using ProFeatureCreate(),

•

Extracts the section from the element tree of the incomplete feature,

•

Builds the section on the section handle obtained, and,

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Completes the feature using ProFeatureRedefine().

Following is the change in the approach for Pro/ENGINEER Wildfire release:

Level of PRO_E_SKETCHER in an element tree is changed.

For any Pro/ENGINEER release previous to Wildfire:

PRO_E_FEATURE_TREE -> PRO_E_STD_SECTION -> PRO_E_SKETCHER

For Pro/ENGINEER Wildfire release:

PRO_E_FEATURE_TREE -> PRO_E_SKETCHER

Value of PRO_E_SKETCHER—A new ProValue is to be allocated and then assigned to the element (rather than the old approach of reusing the value extracted from the element tree).