Element Trees: Edit Menu Features

Use the function ProFeatureCreate() to create a Mirror Feature based on element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation of section Element Trees: Principles of Feature Creation.

Redefining a Mirror Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine a Mirror Feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing a Mirror Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of a Mirror Feature and to retrieve the element tree description of a Mirror Feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section Element Trees: Principles of Feature Creation.

Move Feature

The Move feature can be used to create and move a copy of an existing surface or curve rather than moving the original. Using the Move feature saves time because it enables you to create simple patterns with surfaces and curves.

The Move feature is available for both part and assembly modes. You can apply this feature in different modes:

•

Translate mode—Translate surfaces, datum curves, and axes in a direction perpendicular to a reference plane. You can also translate along a linear edge, axis, perpendicular to plane, two points, or coordinate system.

•

Rotate mode—Rotate surfaces, datum curves, and axes about an existing axis, linear edge, perpendicular to plane, two points, or coordinate system.

To move a surface or curve relative to its original position, define a move reference. In the Translate mode, the move reference is typically a plane or edge that is perpendicular to the direction in which you want to translate the moved feature. In Rotate mode, the move reference is typically an axis or edge about which you want to rotate the moved feature. In this mode, the moved object moves about the direction reference.

Following types of move references exists in Translate mode:

•

Linear curve

•

Linear edge

•

Axis

•

Axis of a coordinate system

•

Plane

•

Two points

Note

The direction reference is always perpendicular to the direction in which you want to move.

Following types of move references exists in Rotate mode:

•

Linear curve

•

Edge

•

Axis

•

Axis of a coordinate system

•

Two points

Note

You can flip the direction of the move in the Rotate mode.

Creo TOOLKIT supports Move features where the initial selection of items was of geometry (curves and /or surfaces). Creo TOOLKIT does not support the element tree for Move features where the initial selection was of one or more features. Move features made from other features will have subfeatures listed under the Move entry in the Creo Parametric model tree, while Move features made from geometry will not include any sub-features.

The Feature Element Tree for Move feature in

The element tree for a Move feature is documented in the header file ProMove.h, and has a simple structure. The following figure demonstrates the feature element tree structure:

Feature Element Tree for Move Feature

The move element tree contains no non-standard element types. The following list details special information about some of the elements in this tree:

•

PRO_E_FEATURE_TYPE—Must be PRO_FEAT_SRF_MDL.

•

PRO_E_STD_FEATURE_NAME—Specifies the feature name.

•

PRO_E_SRF_TR_SURF_SELECTION—Specifies whether to move or copy the selected geometry. Curves, composite curves, axes and quilts are eligible to for this element.

•

PRO_E_MOVE_NO_COPY—Specifies an option to control copy of the original geometry.

•

Provides the ability to transform geometry with or without a copy.

•

PRO_E_MOVE_WITH_COPY—Specifies whether to hide or display the original geometry after copy.

•

PRO_E_MOVE_GEOM_TRF_ARR—Contains an array of movements applied to the selected entities. This can be a combination of translational and rotational transformations.

•

PRO_E_DIRECTION_COMPOUND—Specifies the direction reference for the translation or rotational movement. This compound element is a standard Creo Parametric element subtree and is described in ProDirection.h.

Creating a Move Feature

Function Introduced

Use the function ProFeatureCreate() to create a Move Feature based on element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation of section Element Trees: Principles of Feature Creation.

Redefining a Move Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine a Move Feature based on the changes made in the element tree. For more information aboutProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing a Move Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of a Move Feature and to retrieve the element tree description of a Move Feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section Element Trees: Principles of Feature Creation.

Fill Feature

Creo TOOLKIT enables you to create and redefine flat surface features called fill features. A fill feature is simply a flat surface feature that is defined by its boundaries and is used to thicken surfaces.

Note

All fill features must consist of a flat, closed-loop sketched feature.

The Feature Element Tree for Fill feature in Creo Parametric

The element tree for a Fill feature is documented in the header file ProFlatSrf.h, and has a simple structure.

The following figure demonstrates the feature element tree structure:

Feature Element Tree for Fill Feature

The fill element tree contains no non-standard element types. The following list details special information about some of the elements in this tree:

•

PRO_E_FEATURE_TYPE—It should be PRO_FEAT_DATUM_SURF.

•

PRO_E_FEATURE_FORM—Specifies feature form and should be of PRO_FLAT type only.

•

PRO_E_STD_SECTION—Specifies a sketched section. Refer to the section Creating Features Containing Sections for details on how to create features that contain sketched sections.

•

PRO_E_BODY—Compound element for body options.

○

PRO_E_BODY_USE—Mandatory. The valid values are :

◆

PRO_BODY_USE_NEW—New body created and newly created geometry is added to the new body. Always marks first wall.

◆

PRO_BODY_USE_SELECTED—Feature adds it's geometry to single selected body.

○

PRO_E_BODY_SELECTED—Reference to the selected bodies. Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_SELECTED, ignored otherwise. Single reference allowed.

•

PRO_E_SMT_NEW_BODY_LINKED—Specifies if the sheetmetal body is linked to a part. Mandatory if PRO_E_BODY_USE is set to PRO_BODY_USE_NEW.

The element tree for the Fill feature also supports access to Flat Sheetmetal Wall features. Refer to the section Production Applications: Sheetmetal for element details.

Creating a Fill Feature

Function Introduced

Use the function ProFeatureCreate() to create a Fill Feature based on element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation of section Element Trees: Principles of Feature Creation.

Redefining a Fill Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine a Fill Feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing a Fill Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of a Fill Feature and to retrieve the element tree description of a Fill Feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section Element Trees: Principles of Feature Creation.

Intersect Feature

Refer to the section Intersect Datum Curves Element Trees: Datum Curves for details about this feature.

Merge Feature

The Merge Feature is created by merging two or more selected quilts. In case of more than two quilts, every input quilt should have at least one of its edges adjacent to the edge of any other input quilt, and the surfaces must not overlap.

You can merge a number of input quilts by joining two adjacent quilts one after another, that is, by aligning the edges of one quilt to the edges of the other. The first quilt selected for the merge operation becomes the primary reference quilt. The second adjacent quilt is joined to the primary quilt, forming the main body or a newly formed primary quilt. The third quilt is, then, joined to the main body. This process continues until all the input quilts are joined together.

Note

•

For a successful merge, the selected quilts must be ordered based upon their adjacency.

•

The merge operation fails in case of intersecting quilts, and quilts that are not adjacent to any other input quilt. In either case, remove the problematic quilt to complete the merge.

You can also select the input quilts for the merge operation using region selection. In case of region selection, only box selection is available and the quilts to be selected must be completely inside the region. The selected quilts are ordered based on the feature number of the quilt’s parent feature.

You can merge only two quilts by intersecting. You can specify which portion of the quilt to include in the merge feature by selecting the sides for each of the quilts.

A merged quilt consists of two or more original quilts that provide the geometry, and a merge feature that contains the information for the surface joining. The input quilts are retained, even if you delete the Merge feature.

Note

In Assembly mode, you can merge only assembly-level quilts. If you want to create component-level merge features, you must first activate the component, and then merge the quilts in the component. Surface merge is available only for surfaces that belong to the same component.

Feature Element Tree for Merge feature in Creo Parametric

The element tree for the Merge feature is documented in the header file ProMerge.h, and has a simple structure. The following figure demonstrates the feature element tree structure:

Feature Element Tree for Merge Feature

The following list details special information about the elements in this tree:

•

PRO_E_FEATURE_TYPE—Specifies the feature type; must be PRO_FEAT_DATUM_QUILT.

•

PRO_E_SRF_MRG_QUILT_ARR—Specifies an array of the following compound element. The array must have atleast two elements to create the Merge feature.

○

PRO_E_SRF_MRG_QUILT_CMPD—Specifies the set of references and sides to be used for the merge operation. The set consists of the following two elements:

◆

PRO_E_SRF_MRG_QUILT_REF—Specifies the quilt of the type PRO_QUILT selected for the merge operation. This is a mandatory element.

◆

PRO_E_SRF_MRG_QUILT_SIDE—Specifies the side of the selected quilt that should be included in the merge feature in case of intersecting quilts. This element is ignored when the quilt array PRO_E_SRF_MRG_QUILT_ARR contains more than two elements.

•

PRO_E_SRF_MRG_TYPE—Specifies the merge type and can have following merge type options:

○

PRO_SRF_MRG_JOIN—For joining quilts.

○

PRO_SRF_MRG_INTSCT—For merging two quilts at the intersection. This is the default option.

The merge type must be PRO_SRF_MRG_JOIN when the quilt array PRO_E_SRF_MRG_QUILT_ARR contains more than two elements.

•

PRO_E_STD_FEATURE_NAME—Specifies the merge feature name.

Creating a Merge Feature

Function Introduced

Use the function ProFeatureCreate() to create a Merge Feature based on element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation of section Element Trees: Principles of Feature Creation.

Redefining a Merge Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine a Merge Feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing a Merge Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of a Merge Feature and to retrieve the element tree description of a Merge Feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section Element Trees: Principles of Feature Creation.

Pattern Feature

Refer to the section Element Trees: Patterns for details about this feature.

Wrap Feature

Refer to the section Wrap Datum Curves in the section Element Trees: Datum Curves for details about this feature.

Trim Feature

Trim feature is applied to remove portions of an existing surface feature. A trim feature is similar to a solid cut. Following are the existing types of feature creation for the trimming of a surface or a quilt.

•

Use Quilts—Cuts a piece from a surface using an intersecting quilt. Creo Parametric consumes the quilt that is used to trim a surface and allows you to keep either or both sides of the trimmed surface. You can trim quilts in the following ways:

○

By adding a cut or slot as you do to remove material from solid features

○

By trimming the quilt at its intersection with another quilt or to its own silhouette edge as it appears in a certain view

○

By filleting corners of the quilt

○

By trimming along a datum curve lying on the quilt

•

Use Curves—Trims a surface using selected curves and edges.

The rules for defining a surface trim using a datum curve are as follows:

○

You can use a continuous chain of datum curves, inner surface edges, or solid model edges to trim a quilt.

○

Datum curves used for trimming must lie on the quilt to be trimmed and should not extend beyond the boundaries of this quilt.

○

If the curve does not extend to the boundaries of the quilt, the system calculates the shortest distance to the quilt boundary and continues the trim in this direction.

•

Silhouette—Trims a surface at its silhouette edge from a specified direction.

The Feature Element Tree for Trim feature in

The element tree for a Trim feature is documented in the header file ProTrim.h, and has a simple structure. The following figure demonstrates the feature element tree structure:

Feature Element Tree for Trim Feature

The trim element tree contains no non-standard element types. The following list details special information about some of the elements in this tree:

•

PRO_E_FEATURE_TYPE—It should be PRO_FEAT_CUT.

•

PRO_E_FEATURE_FORM—Specifies feature form and is a mandatory element applicable only for use quilt and thin types. It has PRO_USE_SURFS and PRO_NOTYPE as their valid values.

•

PRO_E_SRF_TRIM_TYPE—Specifies trim type identity and is a non-redefinable mandatory element. The trim type determines the required structure for the remaining elements in the element tree. Each type requires different mandatory elements. The different trim types are as follows:

○

PRO_SURF_TRIM_USE_CRV—use curves to trim the quilt.

○

PRO_SURF_TRIM_USE_QLT—use another quilt to trim the given quilt.

○

PRO_SURF_TRIM_THIN

○

PRO_SURF_TRIM_SILH—trim quilt using silhouette edges.

•

PRO_E_TRIM_QUILT—Specifies trimmed quilt and should be of type PRO_SURFACE or PRO_QUILT only.

•

PRO_E_STD_USEQLT_QLT—Specifies trimming quilts and trimming planes. It should have PRO_SURFACE, PRO_QUILT and PRO_DATUM_PLANE values only. It is applicable for use quilt and thin types only.

•

PRO_E_STD_CURVE_COLLECTION_APPL—Specifies the trimming curves and is applicable for use curve only.

•

PRO_E_TRIM_SILH_PLANE—Specifies silhouette plane and can be of type PRO_SURFACE or PRO_DATUM_PLANE only.

•

PRO_E_MATERIAL_SIDE—Specifies material side options and has the following values:

○

PRO_TRIM_MATL_SIDE_ONE

○

PRO_TRIM_MATL_SIDE_TWO

○

PRO_TRIM_MATL_BOTH_SIDES

•

PRO_E_PRIMARY_QLTSIDE—Specifies the primary quilt side options and they are listed as follows:

○

PRO_TRIM_PRIM_QLT_SIDE_ONE

○

PRO_TRIM_PRIM_QLT_SIDE_TWO

•

PRO_E_STD_USEQLT_SIDE—Specifies thickness direction options for thin trims and can only be as follows:

○

PRO_TRIM_STD_QUILT_SIDE_ONE

○

PRO_TRIM_STD_QUILT_SIDE_TWO

○

PRO_TRIM_STD_QUILT_BOTH_SIDES

•

PRO_E_KEEP_TRIM_SURF_OPT—Specifies to keep trimming surface option and is valid only when the trimming quilt is a surface or quilt. It has the following values:

○

PRO_KEEP_TRIM_SURF_OPT_NO

○

PRO_KEEP_TRIM_SURF_OPT_YES

•

PRO_E_THICKNESS—Specifies thickness for thin trims.

•

PRO_E_SRF_OFFS_METHOD—Specifies the types of offset for thin trims and are as follows:

○

PRO_TRIM_SRF_OFFS_METH_NORMTOSURF—The surface or quilt is thickened in a direction normal to the surface.

○

PRO_TRIM_SRF_OFFS_METH_AUTOSCALE—The surface or quilt is thickened by automatically determining scaling coordinate system and fit along all three axes.

○

PRO_TRIM_SRF_OFFS_METH_MANUALSCALE—The surface or quilt is thickened by specifying the scaling coordinate system and control fitting motion.

•

PRO_E_SRF_OFFS_CTRLFIT—Specifies the control fit and is applicable for thin trims only. It offsets the surface by creating a best-fit offset that is scaled with respect to a selected coordinate system. It allows you to define the axis for translation. It consists of the following elements:

○

PRO_E_SRF_OFFS_SCALINGCSYS specifies the control fit coordinate system and should have a value of PRO_CSYS.

○

PRO_E_SRF_OFFS_AXISES specifies the control fit axes having the following values:

◆

PRO_TRIM_OFFS_TRF_NONE

◆

PRO_TRIM_OFFS_TRF_X

◆

PRO_TRIM_OFFS_TRF_Y

◆

PRO_TRIM_OFFS_TRF_Z

◆

PRO_TRIM_OFFS_TRF_XY

◆

PRO_TRIM_OFFS_TRF_YZ

◆

PRO_TRIM_OFFS_TRF_ZX

◆

PRO_TRIM_OFFS_TRF_ALL

•

PRO_E_SRF_OFFS_HANDLINGS—Specifies an array of PRO_E_SRF_OFFS_HANDLING and is applicable for thin trims only.

•

PRO_E_SRF_OFFS_HANDLING—Specifies special handling item and consists of PRO_E_SRF_OFFS_REF_SEL which are special handling faces which should be from the trimming quilt.

A list of elements required for different types of trims:

Trim type	Element Id
Quilt Type	PRO_E_FEATURE_TYPE
	PRO_E_FEATURE_FORM
	PRO_E_SRF_TRIM_TYPE
	PRO_E_STD_FEATURE_NAME
	PRO_E_SURF_TRIM_TYPE
	PRO_E_TRIM_QUILT
	PRO_E_STD_USEQLT_QLT
	PRO_E_MATERIAL_SIDE
	PRO_E_PRIMARY_QLTSIDE
	PRO_E_KEEP_TRIM_SURF_OPT
Use Curve	PRO_E_FEATURE_TYPE
	PRO_E_SRF_TRIM_TYPE
	PRO_E_STD_FEATURE_NAME
	PRO_E_SURF_TRIM_TYPE
	PRO_E_TRIM_QUILT
	PRO_E_STD_CURVE_COLLECTION_APPL
	PRO_E_MATERIAL_SIDE
	PRO_E_PRIMARY_QLTSIDE
Thin	PRO_E_FEATURE_TYPE
	PRO_E_FEATURE_FORM
	PRO_E_SRF_TRIM_TYPE
	PRO_E_STD_FEATURE_NAME
	PRO_E_SURF_TRIM_TYPE
	PRO_E_TRIM_QUILT
	PRO_E_STD_USEQLT_QLT
	PRO_E_STD_USEQLT_SIDE
	PRO_E_KEEP_TRIM_SURF_OPT
	PRO_E_THICKNESS
	PRO_E_SRF_OFFS_METHOD
	PRO_E_SRF_OFFS_CTRLFIT
	PRO_E_SRF_OFFS_HANDLINGS
Silhouette	PRO_E_FEATURE_TYPE
	PRO_E_SRF_TRIM_TYPE
	PRO_E_STD_FEATURE_NAME
	PRO_E_SURF_TRIM_TYPE
	PRO_E_TRIM_QUILT
	PRO_E_TRIM_SILH_PLANE
	PRO_E_MATERIAL_SIDE
	PRO_E_PRIMARY_QLTSIDE
	PRO_E_KEEP_TRIM_SURF_OPT

Creating a Trim Feature

Function Introduced

Use the function ProFeatureCreate() to create a Trim Feature based on element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creationof section Element Trees: Principles of Feature Creation.

Redefining a Trim Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine a Trim Feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing a Trim Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of a Trim Feature and to retrieve the element tree description of a Trim Feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section Element Trees: Principles of Feature Creation.

Offset Feature

Refer to the section Offset Datum Curves in the section Element Trees: Datum Curves for details about this feature.

Thicken Feature

The Thicken feature is available for both part and for assembly modes and can be defined with respect to coordinate systems, axes, and surfaces. You can apply this feature to check the thickness of a part in the model. This feature also forms the basis for model analysis and thickness check. The result of the thickness analysis is as follows:

•

The thickness is between the design range.

•

The thickness exceeds the maximum design value.

•

The thickness is below the minimum design value.

Thicken features use predetermined surface features or quilt geometry to add or remove thin material sections in the design. The surface features or quilt geometry provide greater flexibility within the design and enable you to transform the geometry to better meet the design needs.

The Feature Element Tree for Thicken feature in Creo Parametric

The element tree for a Thicken feature is documented in the header file ProThicken.h, and has a simple structure. The following figure demonstrates the feature element tree structure:

Feature Element Tree for Thicken Feature

The Thicken element tree contains no non-standard element types. The following list details special information about some of the elements in this tree:

•

PRO_E_FEATURE_TYPE—PRO_FEAT_PROTRUSION or PRO_FEAT_CUT.

•

PRO_E_FEATURE_FORM—Must be PRO_E_SURFS.

•

PRO_E_FEAT_FORM_ALWAYS_THIN—Must be PRO_THIN.

•

PRO_SRF_OFFS_METHOD—Offset method that can be enumerated as follows:

○

PRO_OFFS_METH_NORMTOSURF— Specifies the offset of the thickened surface normal to the original surface.

○

PRO_OFFS_METH_AUTOSCALE— Specifies autoscale and translates the thickened surface with respect to an automatically determined coordinate system.

○

PRO_OFFS_METH_MANUALSCALE— Specifies manual scale.

Note

If you change the offset method for a particular feature, all children of this feature fail.

Creating a Thicken Feature

Function Introduced

Use the function ProFeatureCreate() to create a Thicken Feature based on element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation of section Element Trees: Principles of Feature Creation.

Redefining a Thicken Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine a Thicken Feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing a Thicken Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of a Thicken Feature and to retrieve the element tree description of a Thicken Feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section . Element Trees: Principles of Feature Creation

Solidify Feature

Solidify features are used to create complex geometry that would be difficult to create using regular solid features.

Solidify features use predetermined surface features or quilt geometry and convert them into solid geometry. You can use Solidify features to add, remove, or replace solid material in the designs. The quilt geometry provides greater flexibility within the design, and the Solidify feature enables the designer to transform the geometry to meet design needs.

The attributes of the Solidify feature are:

•

Patch—Replaces a portion of the surface with quilt. The quilt boundary must lie on the surface.

•

Add Material—Fills a quilt with solid material.

•

Remove Material—Removes material from inside or outside a quilt.

Note

add material and remove material attributes are always available. Patch is available only if the selected quilt boundaries lie on solid geometry.

The Feature Element Tree for Solidify Feature in Creo Parametric

The element tree for a Solidify feature is documented in the header file ProSolidify.h, and has a simple structure. The following figure demonstrates the feature element tree structure:

Feature Element Tree for Solidify Feature

The solidify element tree contains no non-standard element types. The following list details special information about some of the elements in this tree:

•

PRO_E_STD_FEATURE_TYPE—Must be one of the following types—

○

Protrusion—PRO_FEAT_PROTRUSION

○

Cut—PRO_FEAT_CUT

○

Patch—PRO_FEAT_PATCH

•

PRO_E_FEATURE_FORM— Must be of the following types:

○

PRO_USE_SURFS— Represents protrusion (PRO_FEAT_PROTRUSION) and cut (PRO_FEAT_CUT).

○

PRO_NOTYPE— Represents patch (PRO_FEAT_PATCH).

•

PRO_E_PATCH_QUILT— Specifies the reference quilt and is a mandatory element. A valid quilt or surface satisfies any of the following contexts:

Quilt is open

•

CASE 1

○

All boundaries lie on solid surfaces.

○

Solid geometry does not intersect quilt.

○

Solid geometry and quilt form closed empty volume.

•

CASE 2

○

All boundaries lie on solid surfaces.

○

Solid geometry intersects quilt.

•

CASE 3

○

All one sided edges are inside solid geometry.

•

CASE 4

○

All one sided edges are outside solid geometry.

○

Solid geometry intersects quilt.

•

CASE 5

○

Solid geometry and quilt form closed empty volume.

○

At least, one sided edge intersects geometry.

•

CASE 6

○

Quilt intersects geometry.

○

None of the one sided edges intersect geometry.

•

CASE 7

○

Solid geometry does not intersect quilt.

Quilt is closed

•

CASE 1

○

Solid geometry does not intersect quilt.

•

CASE 2

○

Quilt completely buried inside Material.

•

CASE 3

○

Solid geometry partly intersects quilt.

Creating a Solidify Feature

Function Introduced

Use the function ProFeatureCreate() to create a Solidify Feature based on element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation of section Element Trees: Principles of Feature Creation.

Redefining a Solidify Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine a Solidify Feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing a Solidify Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of a Solidify Feature and to retrieve the element tree description of a Solidify Feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section Element Trees: Principles of Feature Creation.

Remove Feature

Use the Remove feature to remove geometry without disturbing the feature history. It allows you to modify existing imported geometry or delete some geometry from a part (not necessarily formed by a single feature) without having to reroute and refine a number of features.

You can select one of the following items for removal:

•

Surfaces, surface sets, or intent surfaces

•

One closed loop chain of one-sided edges from a single quilt

Geometry removal results in neighboring surfaces being extended or trimmed to converge and close the void. The extended geometry is attached as a solid or surface to the selected surfaces. In case of a one-sided edge chain selected as the reference, the extended geometry can be attached to the selected quilt, or created as a new quilt.

You can exclude contours in multi-contour surfaces from being removed. For periodic features separated by artificial edges (for example, extruded cylinders or revolved features), the feature internally references all the surfaces, even if one of them is selected.

Note

•

All surfaces that are extended or trimmed must be adjacent to the boundary defined by references.

•

If an adjacent surface does not need to be extended, it will not be copied.

•

Surfaces that are to be extended must be extendable.

•

Extended surfaces must converge to form a defined volume.

•

No new patches are created when the surfaces are extended.

•

If the modified geometry cannot be attached as a solid, it can be manually attached as a quilt.

•

Feature operations such as Suppress, Delete, Redefine, Reroute, Copy/Paste, and Pattern (limited to reference pattern if patterning by itself) are supported.

•

Transformation of this feature by itself is not applicable and allowed.

Feature Element Tree for the Remove Feature

The element tree for the Remove feature is documented in the header file ProRemoveSurf.h. The following figure demonstrates the element tree structure:

Feature Element Tree for Remove Feature

The Remove element tree contains standard element types. The following list details special information about the elements in this tree:

•

PRO_E_FEATURE_TYPE—Specifies the feature type and should always have the value PRO_FEAT_RM_SURF.

•

PRO_E_STD_FEATURE_NAME—Specifies the name of the remove feature.

•

PRO_E_RM_SURF_REF_TYPE—Specifies the reference type. This element decides the type of references that you can select for removal. It can have the following values:

○

PRO_RM_SURF_SRF_REF—Specifies that surface sets can be selected as the references.

○

PRO_RM_SURF_CRV_REF—Specifies that a chain of one-sided edges can be selected as the reference.

•

PRO_E_RM_SURF_ATTACH_TYPE—Specifies the attachment type. It can have the following values:

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FM_RM_SURF_ATTACH_SAME—Specifies that the extended geometry will be attached to the selected surfaces if PRO_E_RM_SURF_REF_TYPE is equal to PRO_RM_SURF_SRF_REF, or to the selected quilt if PRO_E_RM_SURF_REF_TYPE is equal to PRO_RM_SURF_CRV_REF.

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FM_RM_SURF_ATTACH_SEP—Specifies that the extended geometry will be created as a separate quilt if PRO_E_RM_SURF_REF_TYPE is equal to PRO_RM_SURF_CRV_REF.

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PRO_E_RM_SURF_SRF_REFS—Specifies the set of surface references. This element is required if PRO_E_RM_SURF_REF_TYPE is equal to PRO_RM_SURF_SRF_REF. It consists of the following elements:

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PRO_E_STD_SURF_COLLECTION_APPL—Specifies the surfaces selected for removal. You can select multiple surfaces. This element is required if PRO_E_RM_SURF_REF_TYPE is equal to PRO_RM_SURF_SRF_REF.

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PRO_E_STD_EXCL_CNTRS—Specifies an array of excluded contours of the type PRO_E_STD_EXCL_CNTRS_ONE_CNTR.

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PRO_E_KEEP_REMOVED_SRFS_OPT—Specifies the ProBoolean option that allows you to retain the removed surfaces as a separate quilt.

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PRO_E_RM_SURF_CRV_REFS—Specifies the set of curve references. This element is required if PRO_E_RM_SURF_REF_TYPE is equal to PRO_RM_SURF_CRV_REF. It consists of the following element:

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PRO_E_STD_CURVE_COLLECTION_APPL—Specifies the single closed loop chain of one-sided edges. This element is required if PRO_E_RM_SURF_REF_TYPE is equal to PRO_RM_SURF_CRV_REF.

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PRO_E_RM_SURF_LEAVE_OPEN_OPT—Specifies if the hole that is created after surfaces are removed must be kept open. The solids are converted to quilts and closed quilts are converted to open quilts.

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PRO_E_RM_SURF_AUTO_SPLIT_SRF—Specifies if the extending surface for the selected shape surface must be automatically split when geometry is removed. The splitting surface is automatically selected.

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PRO_E_RM_SURF_MAINTAIN_TOPO—Specifies if the regeneration must fail when the model changes and the same solution type cannot be reconstructed. It is used to indicate if the topology in the model must be maintained.

Note

The Remove feature is available in the parametric modeling environment as well as in the flexible modeling environment. In the parametric modeling environment, a collection of surfaces or curves are used as the references. In the flexible modeling environment, a region or a collection of surfaces that include regions is used as the reference. In the flexible modeling environment with a surface collection that includes regions, the Remove feature replaces each region by the surface it belongs to. The contours that define other regions of the same surface are automatically saved as the PRO_E_STD_EXCL_CNTRS_ONE_CNTR element.

Element Details of PRO_E_STD_EXCL_CNTRS_ONE_CNTR

Each PRO_E_STD_EXCL_CNTRS_ONE_CNTR specifies one excluded contour. It consists of the following elements:

PRO_E_STD_EXCL_CNTRS_ONE_CNTR

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PRO_E_STD_EXCL_CNTR_SRF_REF—Specifies the surface reference for the excluded contour.

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PRO_E_STD_EXCL_CNTR_EDGE_REF—Specifies the edge reference for the excluded contour. This element can be any edge of the contour.

Creating the Remove Feature

Function Introduced

Use the function ProFeatureCreate() to create the Remove feature based on the element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation in the section Element Trees: Principles of Feature Creation.

Redefining the Remove Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine the Remove feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing the Remove Feature

Function Introduced

Use the function ProFeatureElemtreeExtract() to create a feature element tree that describes the contents of the Remove feature, and to retrieve the element tree description of the Remove feature. For more information about ProFeatureElemtreeExtract(), refer to the section Feature Inquiry of section Element Trees: Principles of Feature Creation.

Example 1: Creating a Remove Surface Feature

The sample code in UgRemoveSurfCreate.c located at <creo_toolkit_loadpoint>/protk_appls/pt_userguide/ptu_featcreat shows how to create a remove Surface feature.

Attach Feature

The Attach feature allows you to attach open quilts to solid or quilt geometry, if the open quilt does not intersect the solid or quilt geometry. You can select an open quilt and attach it to another quilt or solid geometry within the same model. You can also select two open quilts within the same model which do not intersect and attach them.

This feature is useful in case of UDF placement when the geometry of the UDF does not intersect the part.

Feature Element Tree for Attach Feature

The element tree for a Attach feature is documented in the header file ProFlexAttach.h and has a simple structure. The following figure demonstrates the structure of the feature element tree.

Attach Feature Element Tree

The elements in this tree are described below:

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PRO_E_FEATURE_TYPE—Specifies the feature type and should be PRO_FEAT_FLXATTACH.

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PRO_E_STD_FEATURE_NAME—Specifies the name of the feature.

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PRO_E_ATTACH_QLT_REFS—Specifies the open quilts you select for attachment.

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PRO_E_ATTACH_OPT_TYPE—Specifies the attachment type. It is given by the enumerated type ProFlexAttachOptType and is of the following types:

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PRO_FLXATT_SOLID_OPT—Specifies the solid to which the open quilts are attached.

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PRO_FLXATT_SURF_OPT—Specifies the quilt surface to which the open quilts are attached.

Creating the Attach Feature

Function Introduced

Use the function ProFeatureCreate() to create the Attach feature based on the element tree input. For more information about ProFeatureCreate(), refer to the section Overview of Feature Creation in the section Element Trees: Principles of Feature Creation.

Redefining the Attach Feature

Function Introduced

Use the function ProFeatureRedefine() to redefine the Attach feature based on the changes made in the element tree. For more information about ProFeatureRedefine(), refer to the section Feature Redefine of section Element Trees: Principles of Feature Creation.

Accessing the Attach Feature

Function Introduced