The Style Feature - CADquest

The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

The Style Feature

Introduction

The Style feature is used to create and manipulate
interactive curves and surfaces. Click Insert, Style
or click the icon shown above. A single Style
feature can contain multiple curves and surfaces,
and the model may contain multiple Style features.
The Style feature is listed in the model tree similar
to parametric features. When you are creating a
Style feature, the model tree is split as shown
below. The Style portion of the model tree lists the
entities in the current Style feature.

Click Insert, Style

The Style feature is
listed in the model
tree

The Style Tree lists
the entities in the
current Style feature

Each type of Style
entity has a unique
icon here

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

The Style Feature

The Style feature is different from other Pro/ENGINEER features in the following ways:

• The Style feature consists of sub-features such as curves and surfaces. These sub-
features are not driven by dimensions like other Pro/ENGINEER features.

• The Style feature has its own ‘local regeneration’ that is used during the creation of
the feature.

• The Style feature has its own ‘resolve mode’ that is used when a style entity fails the
‘local regeneration’ listed above.

• The Style feature uses ‘soft point technology’ that allows multiple attachment options
when creating and editing style curves.

• The relationships between Style sub-features is not dependent on the order in which
these entities were created. In other words, the parent-child relationships between
Style entities can be changed without first reordering the entities.

• When you are creating a Style feature, the model tree is split as shown on the
previous page. The Style portion of the model tree lists the entities in the current
Style feature. Each type of Style entity has a unique icon in the Style portion of the
model tree.

• The Style feature allows you to ‘trace’ over imported images placed on a base surface.

• The Style feature can be created in part models and in assembly models.

For designs where the Style feature is required, the model is usually built with a combination of
standard parametric features and the Style feature. Sometimes this is referred to as ‘hybrid
modeling’, because the model is partially parametric and partially unconstrained.

Benefits to using the hybrid modeling method are:

• Using parametric features as a base for the Style feature provides the ability to create
symmetric, parametrically modifiable models.

• You have control over the size of the model.

• You have a chance of being able to manufacture the product.

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

Uses for Style

Use the Style feature when:
• The geometry is not defined by dimensions.
• The geometry requires greater flexibility than that offered using parametric features.
• The design intent is governed by visual or aesthetic requirements.
• You need to create high quality surfaces with curvature-continuous boundary
conditions.
• You need greater flexibility when defining the tangency conditions between surfaces.
• You have 3D scanner data for the geometry and need to reverse-engineer it into
Pro/ENGINEER.
• You have a photograph of the geometry and need to reverse-engineer it into
Pro/ENGINEER.

The Style feature can be used to:
• Create 2D or 3D unconstrained freeform curves.
• Create curves on surface (COS) by sketching directly on the base surface.
• Create curves on surface (COS) using the ‘drop tool’ to project style curves onto the
base surface.
• Create freeform surfaces using style curves as boundary entities.
• Create regular parametric features such as extrude, revolve, and sweep, using style
curves as reference entities.
• Create regular parametric surface operations such as merge, trim, and offset (replace),
using style surfaces as reference entities.

By combining the use of regular parametric features with the Style feature, you can:
• Create a parametric ‘skeleton’ to ‘layout’ the design. This could include sketches,
datum planes, points, and coordinate systems, as well as surface quilts and/or solid
geometry.
• Create Style features that reference the parametric geometry.
• Create robust models that have parametric control over the styling features.

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

Styling User Interface

While you are creating a Style feature, the user interface is slightly different than regular
Pro/ENGINEER. The graphics window can be changed to a four-view layout, and two sets of
styling icons are added to the default user interface as shown below. The model tree is split into
two sections, the lower section lists the entities in the current Style feature. New menus are
added to the top menubar, and many menus have limited commands when you are creating a
Style feature. For example, you cannot Save the model while you are creating a Style feature.

Toggle surface display on/off
Toggle curve display on/off
Toggle trace sketches on/off
Four-view layout
Curve analysis
Section analyses
Offset curve or surface analysis
Shaded curvature analysis
Reflection analysis
Draft analysis
Slope analysis
Surface knots analysis
Access saved analyses
Hide all saved analyses
Delete all saved curve analyses
Delete all saved section analyses
Delete all saved surface knots analyses

COPYRIGHT  2010 CADQUEST INC. Select mode
Set active plane
Create style curve
Edit style curve
Drop curve onto surface
Create style surface
Connect surfaces
Trim surfaces
Edit style surface
Done / Quit

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

Views and Planes

When working with the Style feature, several new concepts apply. These include the window
layout and the Active Plane.

• The window layout can be a single view, like regular Pro/ENGINEER, and can be
changed to a four-view layout as shown below.

• When creating planar Style curves, the points are projected onto the Active Plane,
which can be any planar surface and is displayed with a grid-like appearance.

Window Layout

To toggle between the single view layout and the four-view layout, click View, Show All Views,
or click the icon shown above. The four-view layout is useful when defining unconstrained style
curves.

• When using the single view layout, use View, Show Next View to toggle between the
default, top, front, and right side views.

• When using the four-view layout, each pane can be resized by dragging the horizontal
or vertical sashes that separate the panes. You can resize all four panes at the same
time by dragging the splitter at the intersection of the two sashes as shown below.

• Double click the sash or splitter to reset the panes to their default size.

Click here to resize
the window panes

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

Active Plane
When creating planar Style curves, the points are projected onto the Active Plane. Set the Active
Plane by clicking the icon shown below, then select the appropriate planar surface in the model.
You can create a datum plane ‘on the fly’ for the Active Plane using the other icon shown below.
These ‘internal’ datums created ‘on the fly’ are automatically hidden by the system when you
complete the Style feature.

Change the Active Plane

Create an internal datum plane
‘on the fly’ for the Active Plane

Active Plane Orientation

The Active Plane Orientation is a special model orientation maintained by the system, and
adjusts the view so that the active plane is parallel to the screen. To reorient the model to the
Active Plane Orientation, click View, Orientation, Active Plane Orientation or click Active
Plane Orientation in the right mouse button popup menu as shown below.

COPYRIGHT  2010 CADQUEST INC. Click Active Plane Orientation in
the right mouse button popup menu
Set the Active Plane here

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

Active Plane Grid

The Active Plane is displayed with a grid-like appearance to help distinguish it from other planes
in the model as shown below. Using the Styling Preferences dialog box (see page 21), the active
plane grid spacing can be changed, and the visibility of the active plane grid can be toggled on
and off.

The Active Plane is
displayed with a

grid-like appearance

Default Orientation
When using the four-view layout, each windowpane has its own ‘default’ orientation as shown
below. For experienced Pro/ENGINEER users, this may seem odd that the ‘default’ orientation is
not isometric or trimetric. Use the right mouse button popup menu to set the view to the default
orientation as shown below.

TOP

FRONT RIGHT Use the right mouse
button popup menu to
set the view to the
default orientation

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Page 13
The Edit Menu

The Edit menu has additional commands when
creating a Style feature as listed and shown below.

Regenerate All Regenerate all the entities in the
current Style feature. Examine
the Regenerate icon to
determine the need for
regeneration. See the next page.

Copy Make an exact copy of the
selected curve or curves. The
copied curve(s) can be
repositioned by dragging in 3D
space or by entering values.

Copy Proportional Make a proportional copy of the
selected curve or curves. The scaling
of the curve(s) is accomplished by
dragging the endpoints of the
curve(s) in 3D space.

Move Move the selected curve or curves by
dragging them in 3D space.

Convert Convert the selected curve or curves
from one type to another.

Unlink Break the references (parent-child
relationship) between the selected
entity and its reference entities.

Delete Delete the selected entities in the

current Style feature. You can also
press the < Delete > key on the
keyboard to delete style entities.
Confirmation is required to delete
any style entity.

Definition Redefine the selected entities in the
current Style feature.

Resolve Access the Resolve dialog box to
repair Style entities that have failed
regeneration.

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

Regenerating Style Features

The Style feature has its own internal regeneration routine that is different from regular
Pro/ENGINEER features. By default, the system is in ‘auto-regenerate’ mode, where the curves
and surfaces that you create in the Style feature are regenerated in real-time as you create and edit
the geometry. You can disable this auto-regeneration using the Styling, Preferences command,
see page 21.

While you are working with a Style feature, the system displays the regenerate icon as shown
above. This icon has three forms, green, yellow, and red, similar to a traffic control signal.

When the icon is green, the entities in the current style feature are fully regenerated.
There is no need to regenerate the feature.

When the icon is yellow, some or all of the entities in the current style feature need to be
regenerated. Click the regenerate icon to regenerate the entities in the current style
feature. After the entities successfully regenerate, the icon changes to green.

When the icon is red, some or all of the entities in the current style feature have failed to
successfully regenerate. Using the Resolve dialog box, shown below, you can fix the
failure or delete the failed entities. See pages 276-277 for details about resolving Style
failures.

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

The View Menu

The View menu has additional commands when creating a Style feature as listed and shown
below.

Show All Views Toggle the window between the single-view layout
Show Next View and the four-view layout.
Orientation, Active Plane Orientation
When using the single-view layout, toggle between
the top, front, right, and default views.

Orient the model such that the active plane is
parallel to the screen.

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

The Styling Menu

The Styling menu is active when creating a Style feature and is shown below.

The Styling menu
is used when creating
a Style feature

Preferences Access the Styling Preferences dialog box to set preferences for grid
display and spacing, surface mesh display and spacing, and other styling
Set Active Plane items.
Internal Plane
Set the active plane for curve creation and editing.
Trace Sketch
Snap Create an internal datum plane ‘on the fly’ to use as the active plane.
Curve These internal planes become part of the Style feature and are hidden by
Circle the system when you complete the Style feature.

Access the Trace Sketch dialog box to add images to planar surfaces. You
then trace over the image while creating style curves.

Toggle ‘snapping’ on/off. You can also activate snapping using the SHIFT
key while selecting locations for style entities.

Create a style curve.

Create a style circle.

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Arc Create a style arc.

Drop Curve Drop a style curve onto a surface or quilt. This command creates a ‘COS’
or ‘curve on surface’.

COS By Intersect Create a ‘curve on surface’ using the intersection of two entities.

Offset Curve Offset a curve on the same surface or in a perpendicular direction.

Curve from Datum Convert edges, curves, and sketches that are created outside of the Style
feature to style curves.

Curve from Surface Create a style curve using the iso-line of an existing surface.

Curve Edit Edit a style curve by dragging points or tangents.

Surface Create a style surface.

Surface Connect Change the connections between style surfaces.

Surface Trim Remove portions of style surfaces using style curves to define the area to
be removed.

Surface Edit Directly edit style surfaces.

The Analysis Menu

The Analysis menu is used frequently when creating a Style feature and is shown below. Many
of the Geometry analysis commands are used to determine the quality of style curves and
surfaces as they are being created and edited. The use of Saved Analysis is critical to producing
high quality style curves and surfaces.

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

The Info Menu

The Info menu has two additional commands when creating a Style feature as listed and shown
below.

Entity Display information about the selected style curve or surface.
Current Feature Display information about each entity in the current Style feature.

Use these two
commands to display
information about the
current Style feature
and its entities

Page 18 The Information Window

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

Shortcut Menus

There are a variety of right mouse button popup menus that provide shortcuts to common styling
commands. Some of these shortcut menus are shown below.

The main popup menu has shortcuts
for creating and editing curves and
surfaces

Other useful shortcuts are found in
the main popup menu

For curve endpoints, the popup
menu has shortcuts to commands
that are commonly used

For curve tangents, the popup menu
has shortcuts to commands that are
commonly used

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

Keyboard Shortcuts

In addition to the standard Pro/ENGINEER keyboard shortcuts, the following keyboard shortcuts
are used when working with the Style feature:

ALT Drag the curve point normal to the original active plane of the curve.
CTRL
SHIFT Copy and move the selected geometry. Press and hold < Ctrl >, then select
CTRL+SHIFT and drag to create a copy of the style entity.

SHIFT+ALT Activate curve snapping. Press and hold < Shift > while dragging a style
CTRL+ALT curve point to snap it to other geometry.

Move the selected geometry without making a copy. Press and hold
< Ctrl > and < Shift >, then select and drag the entity to move it to a new
location in 3D space.

Extend the curve point using the same curvature.

Drag the curve point in a horizontal and/or vertical direction relative to the
screen.

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

Styling Preferences

The Styling Preferences dialog box is used to set various options as shown below. Click
Styling, Preferences to access this dialog box.

• Set the spacing of the active plane grid by entering a number in the dialog box as
shown below.

• You can toggle on and off the display of the active plane grid by adding or removing
the appropriate checkmark in the dialog box as shown below.

• If your model is complex, or your computer is slow, you may want to turn off the
automatic regeneration of the surfaces by removing the appropriate checkmarks in the
dialog box as shown below.

• Set the spacing of the surface mesh using the slider at the bottom of the dialog box as
shown below.

• Many of these preferences can be set using configuration options.

When this option is checked, the
system will attempt to connect
surfaces as they are created

Toggle on/off the display of the
active plane grid here

Set the active plane grid spacing
here

Set the automatic curve and
surface regeneration options here

Control the display of the surface
meshing here

Set the quality of the surface
meshing here

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

EXERCISE 1 – THE STYLE FEATURE

Purpose

The goal of this exercise is to become familiar with the ISDX user
interface and the Style feature.

Task 1: Working with the Style feature.

• Open the part called ‘nozzle.prt’
• In the model tree, select the feature called Style 1, then press and hold the right mouse

button and click Edit Definition in the popup menu
• Notice the changes to the user interface as shown below

Notice the Styling menu and
the two sets of styling icons

Notice the Style Tree

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

• Notice the grid displayed on the TOP datum plane indicating the Active Plane

• Set the model display to No Hidden, notice the surface is meshed

• Set the model display to Shaded, notice the surface is not meshed

• Press and hold the right mouse button and select Active Plane Orientation in the
popup menu

• Notice the other options in the right mouse button popup menu, select Default
Orientation

• Click the four-view-layout icon in the top toolbar

• Notice the four-view layout

• Resize the window panes as shown below

Click here to resize
the window panes

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

• Double click the sash to resize the window panes to their default size
• Press and hold the right mouse button and click Show All Views in the popup menu
• Notice the window returns to the single-view layout
• Press and hold the right mouse button and click Default Orientation
• Press and hold the right mouse button and click Set Active Plane in the popup menu,

then select FRONT
• Notice the grid is now displayed on FRONT indicating the Active Plane
• Press and hold the right mouse button and click Active Plane Orientation
• Notice the model is oriented with the active plane parallel to the window
• Click View, Show Next View
• Notice the system displays the model in a different orthographic orientation
• Click View, Show Next View
• Notice the system displays the model in a different orthographic orientation
• Click View, Show Next View
• Notice the system displays the model in a different orthographic orientation
• Press and hold the right mouse button and click Default Orientation
• Select this style curve

• Click Info, Entity
• Read the information then Close the Information Window
• Click Info, Current Feature
• Read the information then Close the Information Window

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

Task 2: Set the Styling Preferences.

• Click Styling, Preferences, then change the grid spacing and surface mesh quality as
shown below

Enter < 10 > for the 10
grid spacing here

Click On here

Increase the surface
mesh quality here

• Click OK in the Styling Preferences dialog box
• Notice the surface is meshed when the model display is set to Shaded
• Notice the active plane grid is more dense
• Click Styling, Preferences again
• In the Display area of the dialog box, remove the checkmark next to Grid
• In the Surface Mesh area of the dialog box, click Off When Shaded
• Click OK in the Styling Preferences dialog box

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The Style Feature Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design

Task 3: Using Query Select.
• Select the model exactly here

• Press and hold the right mouse button and select Next in the popup menu
• Notice a different style entity is highlighted
• Press and hold the right mouse button and click Pick From List in the popup menu
• In the Pick From List dialog box, select Style: 832: Surface: SF-25 then click OK

Select the Style Surface here
Click OK here

• Notice the style surface is highlighted
• Click Edit, Delete, Delete or press the < Delete > key on the keyboard
• Click Yes, Yes to delete the entity

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Pro/ENGINEER Wildfire 5.0 Introduction to Interactive Surface Design The Style Feature

• Click Edit, Undo or click the icon
• Notice the Regenerate icon is displayed as a ‘yellow light’
• Click the Regenerate icon to update the entities in the current Style feature
• Notice the Regenerate icon changes to a ‘green light’
• Click the checkmark in the right-side toolbar to complete the Style feature
• Close the window

Task 4: Work with another Style feature.

• Open the part called ‘mid-tower.prt’
• Be sure the display is set to Shaded
• In the model tree, select the feature called Style 1, then press and hold the right mouse

button and click Edit Definition in the popup menu
• Select this style curve

• Click Styling, Curve Edit Page 27

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