Solid Edge Wiki - Articles

Bounded Surface command

Tue, 16 Apr 2013 01:01:24 +0000

Creates a construction surface using boundary elements you define. The boundary elements can be curves or edges and they must define a closed area (1). You can also specify whether any adjacent faces (2) are used to control tangency on the new bounded surface (3).

The curve/edge set must form a closed loop.
Adjacent faces can be used to control tangency on the new bounded surface.
The preparation of edges/curves to be utilized may require the use of the derived curve and split curve commands.
The keypoint curve command can be used to generate a boundary curve.

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Construct a bounded surface

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Bounded Surface command bar

Swept Surface command

Sun, 14 Apr 2013 21:44:01 +0000

Constructs a surface by extruding one or more cross sections (1) along a path you define (2).

You can define up to three paths and many cross sections. After you define the third path, the command automatically proceeds to the cross section step.

The cross sections can be open or closed and can be planar or non-planar. You can place them anywhere along the path. For predictable results, it is best if the cross sections intersect all paths. The sweep paths can be either tangent or non-tangent.

When you create a swept surface using a closed sketch, you can use the Open Ends and Close Ends options on the command bar to specify whether the ends of the swept surface are open or closed. When you set the Close Ends option, faces are added to the ends of the feature to create a closed volume.

You can select wireframe elements from multiple Parasolid bodies or sketches and the elements will remain associative.

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Construct a swept surface

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Pattern features

Sat, 13 Apr 2013 16:31:12 +0000

You construct a pattern feature by copying a parent element in a rectangular, circular, region fill, along a curve, or mirror arrangement.

When patterning part features, the parent element for a pattern can contain more than one part feature. For example, you can pattern sketch-based features, such as a protrusion (1), and a hole (2), and treatment features, such as a round (3), in one operation.

The parent element is included in the occurrence count for rectangular patterns, circular patterns, and patterns along curves. For example, if you construct a 4 by 3 rectangular pattern of holes (four holes in the x direction and three holes in the y direction) the resulting pattern feature contains the parent feature and eleven copies.

Patterning treatment features
You can pattern a treatment feature by itself or along with a sketch-based feature. For example, you can mirror the round feature (1) about the reference plane (2) to add a round to edge (3). This operation succeeds because the parent edges are symmetric about the reference plane.

Mirroring features
You can mirror one or more features, faces, or the entire part with the Mirror command. The mirror plane can be a reference plane or a planar face.

When mirroring faces or features in a solid model, if the mirrored faces touch the solid model, they are combined with the solid model, unless you set the Detach option on QuickBar. When you set the Detach option, the faces or features are mirrored as a construction body.

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Pattern Along Curve command

Sat, 13 Apr 2013 16:17:42 +0000

Constructs a pattern of elements along a specified curve. You can control how the pattern follows the curve by customizing parameters such as start point and transformation type, as well as occurrence count, spacing, and orientation. You can select features, assembly features, edges, surfaces, or design bodies as the parent elements to pattern.

You can pattern the elements along any 2D or 3D curve or model edge. For example, you can pattern a feature (A) along a set of sketch elements (B ).

In an assembly, you can pattern assembly features along a curve, which allows you to modify two or more parts in one operation.

The Select option on the command bar allows you to specify what types of elements you want to pattern. To pattern one or more surfaces or edges (model topology) that are part of a surface or solid body, you can set the Single or Chain option. To pattern one or more features, such as a cutout or protrusion, set the Feature option. To pattern a surface or solid body, set the Body option.

Note:
When constructing and editing pattern features, you cannot have more than one element type in a single pattern. For example, you cannot pattern a hole feature, a design body, and a curve in one operation.

Selecting the elements and curve
The first step in constructing a pattern along a curve is selecting the elements to be patterned. You can select features before or after starting the command. You can select the features in the graphic window or in PathFinder.
When patterning other elements, such as edges, surfaces and curves, or design bodies, you must start the command, set the Select option on the command bar, then select the elements you want to pattern in the graphic window.

The Select option allows you to specify what types of elements you want to pattern. To pattern one or more surfaces or edges (model topology) that are part of a surface or solid body, you can set the Single or Chain option. To pattern one or more features, such as a cutout or protrusion, set the Feature option. To pattern a surface or solid body, set the Body option.

The name in PathFinder indicates whether you constructed a pattern using features, design bodies, or model topology (surfaces or edges).

After you select the elements, you can select any 2D or 3D curve or edge to pattern them along. Use the Select option to choose Single or Chain, and click the curve or edge.

Configuring the pattern
You can control the number and spacing of occurrences with the Pattern Type, Count, and Spacing options. When the Pattern Type is set to Fit, the pattern operation places the number of occurrences specified by the Count option, equally spaced. When the Pattern Type is set to Fill, the pattern operation places as many occurrences as will fit on the curve, with the distance specified by the Spacing option between each occurrence. When set to Fixed, the pattern operation places occurrences using both the Count and Spacing options.
After you have configured the number and spacing of occurrences, select the anchor point. The anchor point is the point where the pattern will begin. Use the dynamic arrow on the anchor point to select the direction in which the pattern will go. You can use the Offset option to select a distance by which the pattern is offset from the anchor point.

Setting transformation type
You can customize the transformation and rotation of the pattern to better capture your design intent. You can specify that occurrences be placed in the pattern linearly, keeping the same orientations throughout the pattern. Or, you can specify a transformation that will change the orientations of the occurrences depending on the input curve or a specified plane.
The reference point is the point in the pattern at which transformation begins. By default, the reference point is the anchor point (A). To select a difference reference point, click the Reference Point button on the command bar and click a new point on the pattern (B ). The pattern transforms to the new position (c).

A linear transformation orients occurrences based on the orientation of the elements being patterned.

A full transformation orients occurrences based on the input curves.

A transformation from plane projects the initial occurrence and a target occurrence onto a plane, where a measured angle defines occurrence orientation.

You can also use the Rotation Type control to specify whether the input feature position or input curve position determines occurrence placement.

Controlling pattern occurrences
You can suppress occurrences in patterns along curves with the Suppress Occurrence button. After you click the Suppress Occurrence button, click the occurrence points for the occurrences you want to suppress. You can suppress individual occurrences, or you can use a fence to suppress adjacent multiple occurrences.
You can insert occurrences in patterns along curves with the Insert Occurrence button. After you click the Insert Occurrence button, click a keypoint to insert an occurrence. Use the Offset option to control its offset.

Patterning assembly features
In the Assembly environment, you can pattern assembly features, such as holes, cutouts, and revolved cutouts. You can specify which parts are included in the pattern feature. If you add parts to a pattern feature which were not in the parent feature, a message is displayed to instruct you the parts must also be added to the parent feature.
For more detailed information on constructing assembly-based features, see the following Help topic: Assembly-Based Features.

Note:
You can only pattern assembly features that were created within the current assembly. You cannot pattern assembly-driven part features.

Guidelines for creating pattern features

You can pattern multiple elements in one operation.
If the Fast option fails, click the Smart option on the command bar.
You can suppress individual feature occurrences in a pattern along a curve.
You can insert individual feature occurrences into a pattern along a curve.

Pattern Along Curve command bar

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Construct a pattern along a curve

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Pattern Parts command

Sat, 13 Apr 2013 14:50:03 +0000

Copies one or more assembly components into a pattern.

You can select the following types of components to define a pattern of parts:

Parts in the active assembly.
Subassemblies in the active assembly.
Patterns of parts in the active assembly.

The parts are not positioned using assembly relationships. They are positioned using a pattern feature in a selected part or in an assembly sketch.

Positioning the components to be patterned
Before creating a pattern of parts, you should properly position one copy of the components you want to pattern. For example, to pattern a bolt, use the Place Part command to place the bolt into one of the bolt holes in the part.

Note:
If the pattern feature on the part was constructed using the Fast Pattern option, you should position the first bolt in the parent feature of the pattern. For example, if you used a hole feature to create the part pattern, position the first bolt in the hole feature, not one of the holes in the pattern feature.

Selecting the components to be patterned
After you have positioned the components you want to pattern, use the Pattern Parts command to select them. The Select Parts step on the Pattern Parts command bar allows you to select the components you want to pattern. You can pattern multiple components in one operation. You can select parts in the active assembly, entire subassemblies, and existing patterns of parts.

Defining the pattern
After you have selected the components you want to pattern, the Define Pattern step on the command bar allows you to select the part that contains the pattern feature you want to use. You can also select an assembly sketch if the assembly sketch contains a 2D pattern profile.

Next, you must select the pattern feature on the part or assembly sketch. The part you use as a pattern reference does not have to be the part in which you positioned the original components. You can select pattern features that were constructed with the following commands:

Rectangular Pattern
Circular Pattern
Pattern Along Curve
Hole

When the pattern feature highlights in the assembly window, select a reference position on the pattern feature. In most cases you should select the feature into which you placed the original copy of the part to be patterned.

When you click the Finish button on the command bar, the original part is copied to each position in the pattern.

Modifying the feature pattern
If you change the design of the part containing the feature pattern, the part pattern in the assembly updates. For example, if you increase the number of holes in the feature pattern, additional bolts are added to the part pattern in the assembly.

Deleting and suppressing patterned parts
When you delete the original part in a pattern, all the patterned parts are also deleted. You cannot delete the individual Pattern Items in a pattern of parts, but you can suppress them. For example, you may have a pattern of 24 bolts where design considerations require one bolt to be shorter than the rest.

After you have placed the pattern of bolts, you can suppress the Pattern Item for that bolt in PathFinder. You can then use the Assemble command to place a shorter bolt in that location.

When you suppress a Pattern Item, the quantity value in an assembly report or a parts list in a drawing is adjusted accordingly. For example, if you suppress one Pattern Item in pattern of 24 bolts, the quantity value in the parts list would be 23 bolts.

Controlling occurrence properties of patterned parts
You can control the occurrence properties of the individual parts in a pattern of parts. When creating a pattern of parts, the parent part's occurrence properties are applied to all of the patterned parts when you set the Patterned Parts Inherit Parent Part Occurrence Properties By Default option on the Assembly Tab on the Options dialog box.
After you create a pattern of parts, you can change the occurrence properties of individual parts in the pattern. For example, you may want to hide one of the patterned parts in the drawing, but still display it in the assembly. You can select the part in PathFinder or the graphics window, then use the Occurrence Properties command on the shortcut menu to set the occurrence property Display in Drawing Views to No for that part.

The part will be displayed in the assembly and counted in an assembly report, but will be hidden in the drawing and not counted in a parts list in the drawing.

Replacing patterned parts
You can use the Replace Part command to replace the original part, but not the patterned parts. When you replace the original part, all the patterned parts are also replaced.

Patterned parts and assembly relationships
Although the parts in a pattern are not positioned using assembly relationships, they do change position if a relationship controlling the original part is modified. For example, if you edit the offset value of the original part, all the patterned parts also update.

Defining patterns productively
You can create patterns of parts that contain part patterns you defined earlier. For example, you can create a part pattern of socket head screws, then use that part pattern to construct another pattern.

Assembly patterns and alternate assemblies
The Pattern Parts command is available when the Apply Edits to All Members option on the Alternate Assemblies tab is set (you are working globally) or cleared (you are working locally).

You can only modify the inputs for a pattern of parts when the Apply Edits to All Members option is set (you are working globally). For example, if an assembly pattern of parts originally included a bolt and nut, you cannot modify the pattern to add a washer to the pattern unless you are working globally.

For more information, see the Alternate Assemblies Impact on Solid Edge Functionality Help topic.

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Pattern Parts command bar

Pattern command (3D features)

Sat, 13 Apr 2013 14:44:18 +0000

Note:
In the Assembly environment, this command is named Pattern Assembly Feature.

Constructs a rectangular or circular pattern of selected elements. You can select part features, assembly features, edges, surfaces, or design bodies as the parent elements to pattern. For example, you can construct a hole feature, then construct a rectangular pattern of holes using the hole feature as the parent element of the pattern.

In an assembly, you can pattern assembly features, which allows you to modify two or more parts in one operation.

You can suppress individual pattern members to define gaps in a pattern to avoid other features.

Patterning elements other than features is useful when constructing models that use freeform surfaces. For example, you can construct a lofted surface, then construct a circular pattern of the lofted surface.

Steps
The basic steps for defining a pattern feature are:

Select the geometry to pattern.
Draw the pattern profile or select an existing pattern sketch.
Select the parts to be modified by the pattern (assembly documents only).

When constructing a pattern, you can also specify whether the pattern is a fast pattern or a smart pattern using the Fast and Smart options on the command bar. You can set these options at any point while creating or editing a pattern.

For more information on smart and fast patterns, see the following Help topics:

Selecting the elements to pattern
The first step in constructing a pattern is selecting the parent elements. In a part or sheet metal document, you can pattern features, edges, curves, surfaces, or the entire design body. In an assembly document, you can pattern assembly features.

The Select option allows you to specify what types of elements you want to pattern. To pattern one or more surfaces or edges (model topology) that are part of a surface or solid body, you can set the Single or Chain option. To pattern one or more features, such as a cutout or protrusion, set the Feature option. To pattern a curve, surface, or solid body, set the Body option.

The name in PathFinder indicates whether you constructed a pattern using features, design bodies, or model topology (surfaces or edges).

Patterning part and sheet metal features
You can select part and sheet metal features before or after starting the Pattern command. You can select the features in the graphic window or in PathFinder. You can select profile-based features or treatment features, but special rules apply when patterning a treatment feature by itself.
Patterning treatment features
You can pattern treatment features by themselves or in conjunction with a profile-based feature. To pattern a treatment feature by itself, the part geometry must allow it.
Patterning edges, curves, surfaces, and design bodies
When patterning other elements, such as edges, surfaces and curves, or design bodies, you must start the Pattern command, set the Select option on the command bar, then select the elements you want to pattern in the graphic window.
Patterning assembly features
In the Assembly environment, you can pattern assembly features that remove material, such as holes, cutouts, and revolved cutouts. If the assembly is a weldment assembly, you can also pattern assembly features that add material, such as fillet welds, groove welds, and protrusion features.
The Select option, available during the Select Features Step, allows you to specify whether you can select material removal features, or material addition features. The Feature option allows you to select material removal features; the Body option allows you to select material addition features.
You can also specify which parts are included in the pattern feature. If you add parts to a pattern feature which were not in the parent feature, a message is displayed to instruct you the parts must also be added to the parent feature.

For more detailed information on constructing assembly-based features, see Assembly-Based Features.

Note:
You can only pattern assembly features that were created within the current assembly. You cannot pattern assembly-driven part features.

Drawing the pattern profile or selecting an existing sketch
You can draw a new pattern profile or select an existing pattern profile from a sketch. If you draw a new profile, you must first specify a plane to draw it on.

Pattern profiles (A) do not have to be drawn such that they are aligned with the parent feature (B ). This makes it possible to reuse pattern profiles.

When working with large or complex patterns, however, you may find it easier to construct the pattern if you draw the pattern profile so that it is aligned with the parent elements.

Note:
You can only reuse pattern profiles that were drawn as sketches.

Controlling the pattern profile
A Pattern profile is the same as any other profile in Solid Edge. You must apply relationships and dimensions so it will behave predictably. You can also use the Variable Table to define variables between pattern profile dimensions and other dimensions on the model.

Specifying the pattern type
You can create rectangular and circular patterns with the Pattern command. With the profile window open, select the pattern type by clicking the Rectangular Pattern or Circular Pattern button on the Features tab. You can also draw lines, arcs, and other elements as construction geometry to help you define the pattern profile.

Note:
Any lines, arcs, and circles you draw will be automatically converted to construction geometry when you close the profile window.

Rectangular patterns
You can construct rectangular patterns with the following placement options:

Fit
Fill
Fixed

Fit example
With the Fit option, you specify the number of occurrences in the x and y directions, and the height and width of the pattern. The X Spacing and Y Spacing values on the command bar are calculated automatically, are read-only, and are not required to be whole numbers.

For example, you set the Fit option and then specify an X Count of 4, a Y Count of 3, a Width of 96, and a Height of 48.

The X Spacing between each occurrence is calculated automatically by dividing the Width by 3 (the X Count minus 1), for a result of 32. The Y Spacing is calculated automatically by dividing the Height by 2 (the Y Count minus 1) for a result of 24.

Fill example
With the Fill option, you specify the x and y spacing, and the height and width of the pattern. The X Count and Y Count values on the command bar are calculated automatically, are read-only, and will always be whole numbers. The Fill option fills the area, but does not place the last row or column if the theoretical X or Y Count value is not a whole number.

For example, you set the Fill option and then specify an X spacing of 33, a Y spacing of 24, a width of 96, and a height of 48.

The X Count is calculated automatically by dividing the Width by the X Spacing, then adding 1. Since the result in this example is 3.9, which is not a whole number, there is not enough room for the fourth occurrence, so the X Count is automatically rounded down to 3.

The Y Count is calculated by dividing the Height by the Y Spacing, then adding 1. The result in this example is 3, which is a whole number, so there is room for the third occurrence.

Fixed example
With the Fixed option, you specify the number of occurrences in the x and y directions, and the x and y spacing. The Width and Height values on the command bar are calculated automatically, are read-only, and are not required to be whole numbers.

For example, you set the Fixed option and then specify an X Count of 4, a Y Count of 3, an X Spacing of 32, and a Y Spacing of 24.20.

The Width is calculated automatically by multiplying the X Spacing times 3 (the X Count minus 1), for a result of 96.
The Height is calculated by multiplying the Y Spacing times 2 (the Y Count minus 1), for a result of 48.40.

When you place dimensions on the pattern profile placed using the Fixed option, the dimensions are driven, since the height and width values are calculated from the values you enter for the spacing and number of occurrences.

Circular patterns
You can construct partial or full circular patterns.

When drawing the pattern arc or circle, you specify a center point (A), a start point (B ) and a direction (c).

The center point defines the center of the pattern arc or circle and also defines the axis of rotation for the feature you are patterning.

The start point defines the radius of the pattern circle. The physical size of the pattern circle has no impact on the pattern you are placing.

The direction controls whether the pattern occurrences are copied in a clockwise or counter-clockwise direction.
You can construct circular patterns with the following placement options:

Fit
Fill
Fixed

The Fit and Fill options are available with both partial and full circular patterns. The Fixed option is only available when placing partial circular patterns.

Fit example
With the Fit option, you specify the number of occurrences, and the radius of the pattern circle. If you specify a partial circular pattern, you also specify the sweep angle of the arc. The angular Spacing value on the command bar is calculated automatically, is read-only, and it is not required to be a whole number.
Fill example
With the Fill option, you specify the angular spacing, and the radius of the pattern circle. If you specify a partial circular pattern, you also specify the sweep angle of the arc. The Count value on the command bar is calculated automatically, is read-only, and will always be a whole number.

The Fill option fills the area, but does not place the last occurrence if the theoretical Count value is not a whole number, and the product of the angular Spacing times the Count minus 1 exceeds 360° for full circular patterns.

For example, you can create a full circular pattern with an angular Spacing of 47°, and still have a total of 8 occurrences in the pattern, since 7 times 47 equals 329. The angular spacing between the last occurrence and the parent feature will be 31°.

Fixed example
With the Fixed option, you specify the you the number of occurrences, the angular spacing, and the radius of the pattern circle. The Sweep value on the command bar is calculated automatically, is read-only, and it is not required to be a whole number.

Defining the reference point
When you draw the rectangular pattern profile, the first point you click becomes the default reference point. The reference point is shown as a bold x symbol (B ). Regardless of where you draw the pattern profile, the feature pattern is constructed relative to the reference point and the parent feature. For example, when patterning hole A, using reference point B, the pattern is constructed as shown.

You can change how the pattern is constructed by redefining the reference point. For example, you can move the reference point to the center occurrence (c).

Staggered patterns
By default, rectangular pattern members are aligned with each other along both axes. With the Rectangular Pattern Stagger Options dialog box you can stagger rows or columns by a given value.

Changing the angle of a rectangular pattern
To change the angle of a rectangular pattern, first delete the horizontal relationship (A) on the pattern rectangle, then place a dimension or relationship to control its angular orientation. For example, you can apply a parallel relationship (B ) between the pattern rectangle and a part edge.

Suppressing pattern occurrences
You can suppress pattern occurrences in rectangular and circular patterns with the Suppress Occurrence button on the command bar. With the profile window open, select the pattern profile, then click the occurrence symbols to specify which occurrences you want to suppress (A). The symbols change size and color to indicate that the corresponding occurrences are suppressed.

You can individually select occurrences to suppress, or drag the cursor to fence any number of occurrences.

This option is useful for when you need to define gaps in a large pattern, for example, to leave space for another feature.

You can also redisplay suppressed pattern occurrences with the Suppress Occurrence button. Click the button and then select the suppressed occurrences you want to redisplay.

Suppressing pattern regions
You can also suppress a region of pattern occurrences using the Suppress Region option on the command bar. To suppress a region, you must select an existing closed sketch. The closed sketch can be of any shape. You can use the Flip option on the command bar to specify whether the suppressed occurrences are inside or outside of the closed sketch.

Deleting pattern occurrences
When constructing smart patterns, you can also delete pattern occurrences. Position the cursor over the pattern occurrence you want to delete (A), then pause. When the ellipsis is displayed, click the left mouse button to display QuickPick. You can then use QuickPick to select the pattern occurrence, then press DELETE to delete it.

When you delete a pattern occurrence, the software is actually suppressing the corresponding x symbol on the pattern profile. Deleting, rather than suppressing, an occurrence can be useful when working with large or complex models, because you do not have to enter the profile window to suppress the occurrence. To restore the deleted occurrence, you can use the workflow for redisplaying suppressed occurrences.

Guidelines for creating pattern features

You can pattern multiple elements in one operation.
When patterning features, if the Fast option fails, click the Smart option on the command bar.
You can suppress individual feature occurrences in a pattern.
You can delete individual feature occurrences in a pattern.

Pattern Command Bar

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Construction Display command

Sat, 13 Apr 2013 14:30:24 +0000

Displays the Construction Display dialog box, which allows you to control the display of reference elements such as:

coordinate systems
reference planes
sketches
axes
construction surfaces
construction curves
blue dots
design bodies

You can click the Show All or Hide All buttons for the type of reference element for which you want to control the display.

You can also use the Show All and Hide All commands on the shortcut menu to control the display of reference elements.

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Boolean command

Sat, 13 Apr 2013 12:44:38 +0000

Performs a union, a difference, or an intersection operation on a part using a reference plane, construction surface, or construction solid as a tool.

For example, you can use the Boolean Feature command to create a cavity in a die. First, use the Part Copy command to insert an existing model into a new file as a construction body. Next, create a rectangular solid that represents the die, and then use the Boolean Feature command to subtract the construction body from the solid.

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Extend Surface command

Sat, 13 Apr 2013 12:36:00 +0000

Extends a surface along one or more edges you select.

The edges you select can form a continuous chain (1) or be interrupted (2).

The extend options which are available depend on whether the surface is an analytic surface or a non-analytic surface. Examples of analytic surfaces include planes, partial cylinders, cones, spheres, and tori. You create non-analytic surfaces when you sweep or extrude a b-spline curve, or when you construct lofted, swept or BlueSurf feature using b-spline curves.

When extending a non-analytic surface, you can specify whether the extension is Natural, Linear, or Reflective along certain types of edges. For example, when extending an extruded surface constructed using a b-spline curve, you can specify the Natural Extend, Linear Extend, or Reflective Extend options for the two edges which are parallel to the input b-spline curve (1, 2).

For the two edges which are perpendicular to the input b-spline curve (3, 4), only the Natural Extend option is mathematically possible. In this example, the natural extension is linear.

Additional examples are illustrated in the Extend Surface command bar topic.

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Extend a surface

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Surface construction

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Extend Surface command bar

Working with points, curves, and surfaces

Sat, 13 Apr 2013 12:27:41 +0000

You can use commands in Solid Edge to create points, curves, and surfaces. These elements are typically used to construct part features, and are often referred to as construction elements. For example, you can use a single, curved surface to replace several planar faces on a model. Using points, curves, and surfaces helps you model complex design scenarios more quickly.

You can also use these commands when working with foreign data that you have imported into Solid Edge.
For some model types, you may not use the solid modeling commands until very late in the modeling process. Complex, freeform parts often require that you begin the modeling process by defining points and curves that are used to define and control the surfaces that comprise the model. Surfaces are then generated, and in the final steps, the surfaces are stitched together to form a solid model. For more information on this type of workflow, see the Surface construction Help topic.

Note:
Construction elements that drive other features have a parent-child relationship with the features they drive. If you delete a construction element that is a parent to another feature, you can invalidate the other feature.

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General surface modeling workflow

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Curve display and edit

Sat, 13 Apr 2013 11:54:49 +0000

Displaying curves

You can use the options on the Curve command bar to control the display of a curve.
The Add/Remove Points button adds or removes edit points along the curve. When you add an edit point, the shape of the curve does not change. If the number of edit points on the curve is the same as the number of control vertex points, adding an edit point adds a corresponding control vertex point. The control vertex point moves to maintain the shape of the curve.

When you remove edit points, the control vertex points move, and the shape of the curve changes.

Note:
If there are only two edit points on the curve, you cannot remove an edit point from the curve.

See Insert or remove points on a curve.

The Show Polygon button displays the control polygon of the curve, which you can use to edit the curve.

The edit points and control vertex points are handles that you can drag to change the shape of the curve.

Note:

You can also use these points as keypoints for relationships and dimensions.

Edit Profile mode: Just like editing a sketch.
Dynamic Edit mode: Shows all of the control and edit points.

When you move a control point or edit point, the curve updates automatically; any surface that has the curve as one of its defining entities will update dynamically.

The Add/Remove Points and Curve Options buttons are disabled in dynamic edit mode. These options are only available in Edit Profile mode.

Add/Remove Points

Show Polygon

Show Curvature Comb

Shape Edit

Local Edit

Close Curve

Curve Options

The Curve command bar controls how the shape of the curve changes when you make changes to the edit points and control vertex points.

The Shape Edit and Local Edit buttons control the shape of the curve when you move a point on the curve.
When you select the Shape Edit button, you affect the shape of the entire curve when you move a point on the curve.

When you select the Local Edit button, you affect the shape of the curve around the edit point.

With Local Edit, if you drag a vertex point on an unconstrained curve, no other vertex points will move. However, if you drag a vertex point on a curve that has some relationships, then other vertex points may move as well. This allows the curve to adapt to the new location of the vertex point you moved while still maintaining the relationships.

Note:
You cannot drag an edit point that is fully constrained.

You can select the Curve Options button to display the Curve Options dialog box. You can use this dialog box to change the number of degrees for the curve and to specify the relationship mode for the curve. You can set the relationship mode to:

Flexible
Rigid

In Flexible mode you can use external relationships to control the shape of the curve. For example, you can apply a dimension relationship on the curve and as you make changes to the dimensions, the shape of the curve automatically updates.

In Rigid mode you cannot use external relationships to control the shape of the curve. Instead, the curve shape remains unchanged and the curve simply rotates.

Simplifying curves
You can use the Simplify Curve command to simplify a polygon-based curve by reducing the number of edit points and control vertex points on a curve. The Simplify Curve dialog box increases or decreases a fit tolerance for the curve.

Note:
Simplifying a curve can cause the relationships placed on a curve to be deleted.

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General surface modeling workflow

Sun, 07 Apr 2013 19:37:58 +0000

1. Create control drawings.

Definition: Control Drawings are 2D drawing views defining the top, side, and end views. Typically one or two views dominate (define the majority of the shape).

Part environment: You can create control drawings directly by drawing on reference planes. Pierce points aid in connecting curves.

Draft environment: You can create control drawings in 2D, then use Copy and Paste to transfer the 2D elements from Draft into Part. Also, you can use Create 3D or import sketches.

Tip:

While drawing any sketch element in either the Part or Draft environment, use Line Color to help distinguish edges and construction edges in the control drawing.

Draw all character curves.
Do not over draw. Do not model rounds, ribs, or features best created with solid features.
Capture design intent. Add dimensions and constraints.
Create simple B-splines with few Edit Points.
Make sure view sketches register.
Build edge continuity into your sketches.

2. Use 2D geometry to develop 3D curves.

Project curves from control drawings.
You may need some construction surfaces to generate 3D curves. This is very important in reducing modeling steps.
3D curves give simplified control over edges.
Capture your design intent by using control drawings.

Without 3D curves, character edges may not be captured.
Lack of 3D edges eliminates design intent and adds more modeling.

With 3D curves, design intent is preserved and modeling is reduced.
You can easily change the shape by altering the character curves for the respective view.
Creating 3D edges guarantees an accurate design and reduces modeling steps.

Making changes to the 3D curve is simple. Edit the character curve in the control drawing.
Repeat the process until all 3D curves are created
A wireframe representation of the model should result.
All 3D curves should be touching.

3. Use 3D curves to develop surfaces.

BlueSurf command.

Inputs are guides and sections.

Swept command.
Inputs are guides and sections.
Bounded command
N-sided patch.

4. Create a solid and add appropriate solid based features.

Stitch together surfaces
Add solid-based features
Thinwall
Stiffening Rib
Hole
Round
Web network
Lip

5. Tweak.

Analyze edge continuity using:
- Curvature Comb
- Zebra Stripes
Edit character curves
Edit tangent vectors
Edit vertex mapping

What is surfacing and why use it?

Sun, 07 Apr 2013 19:22:55 +0000

The solid modeling method is typically used when modeling with solid features. The following are key features of the solid modeling approach:

It is characterized by 2D sketches/profiles used in creating extrusions, revolutions, and lofts to form solids, and blends on the edges of solids.
It most often involves the addition or subtraction of material using analytic shapes.
The model's topology is driven by faces.
Holes are used for alignment.
Feature faces are used for alignment as well as for mating with other features.
Edges are rounded for safety and strength.
Edges and faces are primarily analytic-based.

Modeling with surface-based features typically begins with a wireframe, from which surfaces are generated. Key features of surface modeling:

It is characterized by control points used to define 2D and 3D curves.
A model's topology is driven by edges and curves. Edges and faces are mainly based on splines.
Surface shapes are very important, therefore direct editability of underlying curves and edges is crucial.
Highlight lines, silhouette edges and flow lines of a model are important.

Using surfaces
The surfacing commands help you create complex parts and surface topology more easily. You can use surfaces in the following ways:

To define the projection extents when extruding a feature.
To replace existing part faces.
To divide a part into multiple parts.
To create a new surface or solid by stitching together separate surfaces.
To repair a model you imported from a third-party CAD system.

Construction surfaces are commonly used as projection extents when extruding a feature. For example, you can create a construction surface, then use the surface as input during the Extent step when constructing a protrusion.

You can use the Offset Surfaces command to offset a new surface. The options on the command bar allow you to specify whether you want to offset a single face, a chain of faces, or all the faces that make up a feature.

You can use the Stitched Surface command to stitch together Solid Edge surfaces, as well as surfaces created with another CAD system and then imported into Solid Edge.

You can also create surfaces using the Part Copy command. If the Copy As Construction option is set in the Part Copy Parameters dialog box, the part copy is created as a construction surface.

Surface construction
Solid Edge provides two distinct 3D modeling methods:

solid modeling
surface construction

The solid modeling method

A product's function is the primary concern and aesthetics are purely an afterthought.
Solid Edge is an industry leader of this modeling style and exhibits these additional characteristics:
The various modeling operations are identified as features.
A history tree of features is maintained.
All properties used in defining a feature can be edited at any time.

The surface modeling method

Many consumer products are designed using surface modeling techniques due to the market's emphasis on style and ergonomics; therefore, a model's aesthetics is the number one concern and key element in the design process. Product function is only a secondary consideration.
Like the solid modeling features, Solid Edge extends this style by making each point, curve, and surface an entity that knows how it was created, and can be edited at any time.

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BlueSurf Options Dialog Box

Sat, 30 Mar 2013 13:13:17 +0000

Standard Tab Options

Tangency Control

Specifies the options you want for controlling the shape at the ends of the feature. For example, when you are creating a BlueSurf feature that must blend smoothly with adjacent surfaces, you can set the Normal to Section option to ensure a smooth blend between the existing surfaces.

The following options are available, depending on the geometry you select for the cross section or guide curve:

Natural—There are no constraining condition enforced at the end sections. This is the default end condition and is valid for any cross section type.

Normal to Section—End cross sections that are planar support a normal to section end condition. You can control the length of the vector using the variable table or by modifying the vector handle in the graphic window. In this example, the resultant surface illustrates the graphic handles (1) that you can use to modify the surface.

Parallel to Section—End cross sections that are planar support a parallel to section end condition. You can control the length of the vector using the variable table or by modifying the vector handle in the graphic window. To see the effect of this setting, compare the following illustration of Parallel to Section with the Normal to Section example.
Tangent Interior—End cross sections defined using part edges and construction surfaces support a tangent interior condition. Tangent Interior forces the surface to be tangent to the inside faces. For example, the surface below has the Tangent Continuous option applied to cross section (1), and the Tangent Interior option applied to cross section (2). The resulting surface is constructed tangent to the planar face (3).
Tangent Continuous—End cross sections defined using part edges and construction curves support a tangent condition. The tangent vector for the surface is determined by the adjacent surfaces. You can control the length of the vector using the variable table or by modifying the vector handle in the graphic window.
Curvature Continuous—End cross sections defined using part edges and construction surfaces support a curvature continuous condition. The tangent vector for the surface is determined by the adjacent surfaces. You can control the length of the vector using the variable table or by modifying the vector handle in the graphic window.

For more information and illustrations which show you how you can control the surface shape at the ends of BlueSurf and lofted features, see the End Conditions section in the Constructing Lofted Features (ordered) or Constructing Lofted Features (synchronous) Help topics.

Start Section
Specifies the tangency control option you want for the first cross section.

End Section
Specifies the tangency control option you want for the last cross section.

Edge Guide 1
Specifies the tangency control option you want for the first guide curve. The options available for defining guide curve tangency conditions depend on the type of element you select for the guide curve. For example, if you want to be able to control the tangency of the BlueSurf feature with respect to an adjacent surface, use an edge on the surface as the guide curve rather than, for example, the sketch that was used to construct the adjacent surface.

Edge Guide 2
Specifies the tangency control option you want for the last guide curve. The options available for defining guide curve tangency conditions depend on the type of element you select for the guide curve. For example, if you want to be able to control the tangency of the BlueSurf feature with respect to an adjacent surface, use an edge on the surface as the guide curve rather than, for example, the sketch that was used to construct the adjacent surface.

End Capping

Specifies the end capping options you want. This option is available only when the cross section profiles are closed.

Open Ends
Specifies that no planar end caps are added to the feature.

Close Ends
Specifies that planar end caps are added to the feature to create a enclosed volume.

Extent type

Controls whether or not the feature closes on itself.

Open
Specifies that the feature begins with the first cross section and ends with the last cross section. The feature does not close on itself.

Closed
Specifies that the surface will close on itself. When you set this option, the first cross section is also used for the last cross section.

Curve Connectivity

Specifies how a cross section and a guide curve are connected. These options only apply to new sketches you add using the Insert sketch button on the command bar.

Use Pierce Points

Specifies that a connect relationship is used to connect the cross section and guide curve where they intersect. The position of the connect relationship is calculated using the Pierce Point option on the IntelliSketch dialog box. The Use Pierce Points option is typically used when constructing engineered surfaces, such as the surfaces for a fan or turbine blade, where engineering data or dimension-driven criteria must be maintained.

Use BlueDots
Specifies that a BlueDot is used to connect the cross section and guide curve where they intersect. When you connect a cross section and a guide curve with a BlueDot , you can use the BlueDot as a handle to dynamically modify the shape of the cross section and guide curve. The Use BlueDots option is typically used when constructing esthetic surfaces, such as the surfaces for consumer electronics product, where a more free-form approach to surface design is desired.

Note:
The Use BlueDots option is available only in the ordered modeling environment. The BlueDots functionality is not available in the synchronous environment.

Inserted-Sketch

Allows you to define a tolerance value for sketches you insert. The tolerance value you specify is used to control the complexity of the curve that is created.

Tolerance
Specifies the tolerance value you want to use.

Advanced Tab Options

Vertex Mapping
Vertex mapping is a technique to help create flow between section vertices; you can map a vertex or point on one cross section to a vertex or point on another cross section. Vertex mapping is useful for controlling or eliminating twists and discontinuities in a surface. If there is a vertex count mismatch between sections, equally spaced vertices are used on each section.

You can add vertex maps while creating a BlueSurf or by editing an existing BlueSurf.
Notice in the first image below that section (A) has four vertices and section (B ) has three vertices. The BlueSurf command automatically inserts vertices equally spaced on each section. Notice the surface flow is not smooth.

The result of vertex mapping.

Map Sets
Lists the sets of mapped vertices you have defined. You can add vertex map sets to create a smooth surface flow; to add a new set of mapped vertices, click the Add button, then click a point on each cross section curve.

Add
Allows you to add a new mapped vertex set.

Delete
Allows you to add a delete an existing mapped vertex set.

Reorder

Allows you to reorder cross sections that were defined out-of-sequence. This option is useful when you modify an existing feature by adding a new cross section. You cannot use the reordering capability to create a feature that intersects itself.

To reorder a cross section, select the cross section in the list, then click the Up or Down buttons to move the cross section entry in the list.

BlueDot command

Fri, 29 Mar 2013 20:00:25 +0000

Note:
BlueDots are only available in the ordered modeling environment

A BlueDot is a control point where two curves or analytics connect, or where one curve and one analytic connect, thereby providing a control point between the curves. It is a point which can edited to suit design or styling needs.

Creates a control point (1) between two sketch elements. You can connect the elements at their keypoints or at a point along the elements. The BlueDot overrides any existing associativity of the elements. This allows you to edit the location of the BlueDot or the elements it connects without regard to the order in which the elements were constructed.

After you connect the keypoints of two elements with a BlueDot, you can edit the position of the BlueDot to change the shape of the elements. Surfaces that were constructed using the elements also update.

Refer to Connect sketch elements with a BlueDot for more info on BlueDot creation.

Edit a BlueDot
To edit the position of a BlueDot, use the Select Tool to select a BlueDot (1), then click the Dynamic Edit button on the Select Tool command bar. When you edit the position of a BlueDot, you can use the OrientXpres tool (2) to restrict the movement to be parallel to a particular axis or plane. You can then drag the BlueDot to a new position (3). The wireframe elements and the surface also update.

When you use OrientXpres to restrict movement to a plane (1), you can move the BlueDot along two axes simultaneously (2).

You can also reposition the OrientXpres tool by selecting the origin of the X, Y, and Z axes, and then dragging OrientXpres to a new position.

You can use the BlueDot Edit command bar to specify whether the edit value is relative to its current position or its absolute position with respect to the global origin of the document. The global origin is the point where the three default reference planes intersect (the exact center of the design space).

When you apply a BlueDot to b-spline curves, you can also control how the curves react to the edit by setting options on the Curve 1 and Curve 2 controls on the command bar.

Note:

When you use a BlueDot to connect two elements, it affects the associative relationship of the reference planes on which the elements lie. For example, if one of the elements lies on a reference plane that was created parallel to another reference plane, the dimensional offset value for the reference plane is deleted. When you edit the position of the BlueDot, the reference plane can be moved to a new position to facilitate the repositioning of the elements.

Refer to BlueDot Edit command bar for more information.

BlueDots in Harness Design
When working in Harness Design, you cannot use the command to connect sketch elements. However, the command allows you to connect the endpoints of two or more wire paths to create a single path.

Note:

When editing a BlueDot in Harness Design, the Curve 1 and Curve 2 options are not displayed on the BlueDot Edit command bar since you can connect more than two curves.

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BlueDot Edit command bar

BlueSurf

Fri, 29 Mar 2013 19:39:02 +0000

Note:
Please refer to the Help topics BlueSurf command and BlueSurf Options dialog box for more detailed information.

BlueSurf is a surface creation command used to generate complex, but highly editable surfaces. Like loft and sweep, a BlueSurf utilizes cross sections and guide curves, and these parent curves drive the behavior of the resultant surface. Several techniques can be applied to further edit a BlueSurf.

New section and/or guides can be incorporated, providing additional control over the BlueSurf topology.
As sections and/or guides are added, the number of edit points can be increased or reduced through the concept called Edit Point Data Management.
BlueDot edit points can be moved in order to manipulate the surface; both Shape and Local Edits are available.

The first step in creating a BlueSurf is selecting cross sections. The Cross Section Step activates automatically. At least two cross sections are required.

Next, you can select Guide curves if needed. Click the Guide Curve Step and select the guide curve(s).

Click Preview and then Finish.

The example below shows the BlueSurf result of two cross-sections (C1, C2) and two guide curves (G1, G2).

A BlueSurf may also consist of a single cross-section and a single guide curve. The following example shows the BlueSurf result of using cross-section (C1) and guide curve (G1) from the previous example.

At this point, editing any of the cross-sections or guide curves modifies the shape of the BlueSurf. If you need additional surface shape control, the BlueSurf command provides a step to insert additional sketches.

BlueSurf command

Fri, 29 Mar 2013 19:18:15 +0000

Constructs a surface using existing sketches or part edges. You can use the BlueSurf command to construct complex surfaces that provide many editing options.

Input requirements
The sketches or edges can represent cross sections only (1) or cross sections (1) and guide curves (2). At a minimum, you must define two cross sections or one cross section and one guide curve.

The sketches or part edges can be open or closed.

Mixing open and closed elements
When constructing a bluesurf feature, you can use both open and closed elements in a single feature. For example, you can construct a bluesurf feature that uses a line and a closed element, such as a rectangle or a circle, as cross sections. In some situations, you may need to split elements or define vertex mapping parameters to construct the surface you want. For example, to construct a BlueSurf feature using a line and a circle, you must split the circle into two arcs. You can use the Split command to split the circle into two connected arcs.

Closing ends
When you create a BlueSurf feature using closed cross sections, you can use the End Capping options on the BlueSurf Options dialog box to specify whether the ends of the feature are left open (1) or closed (2). When you set the Close Ends option, a solid body is created.

Inserting sketches
You can use the Insert Sketch Step on the command bar to add new sketches to a BlueSurf feature. The geometry for the new sketch is created by intersecting a reference plane you define with the BlueSurf feature. You do not have to create the sketch geometry yourself. When you insert a sketch, the new geometry is a created as a b-spline curve. If you want the new geometry to consist of lines, arcs, or circles; you must create the new sketch manually outside of the BlueSurf command.

When you click the Insert Sketch button on the command bar, plane creation options are added to the command bar so you can define the position for the new reference plane. For example, you can use the Parallel Plane option to define an offset reference plane where you want additional control over the resultant surface.

You can then edit the sketch to change the surface shape.

When you add a cross section or guide curve to an existing BlueSurf feature using the Insert Sketch option, the new sketch is connected to the cross sections or guide curves. You can use the BlueSurf Options dialog box to specify whether Pierce Points or BlueDots are used to connect new section to the surface.

Note:

BlueDots are only available in the ordered modeling environment

Pierce points
When you set the Use Pierce Points option, connect relationships are used to tie the inserted sketch to the cross sections or guide curves it intersects. When you set the Use BlueDots option, BlueDot elements are used to tie the inserted sketch to the cross sections or guide curves it intersects. The option you specify also affects how you can edit the feature later.

When you connect the new sketch using the Use Pierce Points option, you can modify the cross sections or guide curves the new sketch intersects and the b-spline curve for the inserted sketch will update. The Use Pierce Points option is most suitable for models that must conform to engineering data or dimension-driven criteria; such as turbine blades, fan housings, and so forth. The Use Pierce Points options maintains the existing parent/child history of the model.

BlueDots
If you are working with a BlueSurf in the ordered environment, and you insert a sketch using the Use BlueDots option, you can also modify the BlueSurf feature by editing the position of the BlueDots using the Select Tool and the BlueDot Edit command bar. When you move a BlueDot, the portion of the sketches that are controlled by the BlueDot update, and that portion of the BlueSurf also updates.
The Use BlueDots option is most suitable for ordered models that are driven by esthetic requirements, such as consumer electronics products, bottle and container design, and so forth. When you use BlueDots to connect an inserted sketch, moving a BlueDot can also change the location of the reference planes of the sketches it connects.

This is because a BlueDot allows you to override the existing parent/child history of the model. For example, if you insert a sketch using a parallel reference plane with an offset value of 25 millimeters, editing the location of the BlueDot can also change the offset value of the reference plane.

This behavior can be preferable when exploring the esthetic possibilities of a surface, but can be counter-productive when working with engineered surfaces. In some cases, using BlueDots can also cause a model to take longer to update, because moving a BlueDot may require more of the model to recompute than a connect relationship would.

Note:

When you set the Use BlueDots option on the BlueSurf Options dialog box, but existing constraints prevent BlueDots from being created, then pierce points are created instead.

Creating new sketches manually (ordered modeling)
Alternately, you can also create new sketches for a BlueSurf feature using the Sketch command, or you can copy an existing sketch using the Tear-Off Sketch command. You can then edit the BlueSurf feature and add the new sketches as cross sections or guide curves.
For example, when you add new cross sections, the system adds them after the existing cross sections, regardless of their physical orientation with respect to the existing cross sections. You can use the Reorder option on the Advanced tab on the BlueSurf Options dialog box to define the cross section sequence.

Cross section and guide curve connectivity
If you use a guide curve to construct a BlueSurf feature, the guide curve must intersect each cross section and be tangent continuous (the curve cannot have any sharp corners). To ensure that the guide curve stays intersected to the cross sections, you should add a connect relationship or a BlueDot at each intersection point.

End condition control
You can use the Tangency Control options on the BlueSurf Options dialog box to define the end condition options you want for the resultant surface. For example, you can specify that the surface is tangent to the adjacent surfaces.

Many of the end condition options allow you to dynamically adjust the surface using a graphic handle (1) or by modifying a variable in the variable table. For surfaces that have several graphic handles or variables for a single cross section, you can create a master variable for all the variables that control the cross section, then use a formula to drive all the variables for that cross section simultaneously.

BlueSurf features and lofted features
In many respects, a BlueSurf feature is constructed and behaves similarly to a lofted feature, such as a lofted surface or a lofted protrusion. For example, you can reorder cross sections, define vertex mapping rules, and define the end section conditions for a BlueSurf feature and a lofted feature.

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Curve command

Fri, 29 Mar 2013 19:01:58 +0000

Draws a smooth, B-spline curve by points. You can click and drag to define a freehand curve, or you can click to create edit points to define the curve. If you click edit points, you must define at least three points to create the curve.

When you create a curve, edit points (1) and curve control vertex points (2) are created to help you edit and control the shape of the curve.

Closing curves
You can use the Closed option on the Curve command bar to create a continuous line that forms a closed curve connected tangentially at the first and last point you click.

When editing a curve created from edit points, you also can use the Closed option to:

Close an open curve, without adding points.
Open a closed curve, without deleting points.

You cannot use this option to modify a freehand curve.

Displaying curves
You can use the options on the Curve command bar to control the display of a curve.
The Add/Remove Points button adds or removes edit points along the curve. When you add an edit point, the shape of the curve does not change. If the number of edit points on the curve is the same as the number of control vertex points, adding an edit point adds a corresponding control vertex point. The control vertex point moves to maintain the shape of the curve.
When you remove edit points, the control vertex points move, and the shape of the curve changes.

Note:

If there are only two edit points on the curve, you cannot remove an edit point from the curve.

See Insert or remove points on a curve.

The Show Polygon button turns on the control polygon of the curve. This polygon displays when the curve is not selected.

The edit points and control vertex points are handles that you can drag to change the shape of the curve.

Note:

You can also use these points as keypoints for relationships and dimensions.

The Show Curvature Comb button displays the curvature comb for the curve. This helps you determine how quickly or gradually curves change and where they change direction.

You can use the Curvature Comb Settings command to control the density and magnitude of the curve.

Editing curves
The Curve command bar controls how the shape of the curve changes when you make changes to the edit points and control vertex points.
The Shape Edit and Local Edit buttons control the shape of the curve when you move a point on the curve.
When you select the Shape Edit button, you affect the shape of the entire curve when you move a point on the curve.

When you select the Local Edit button, you affect the shape of the curve around the edit point.

With Local Edit, if you drag a vertex point on an unconstrained curve, no other vertex points will move. However, if you drag a vertex point on a curve that has some relationships, then other vertex points may move as well. This allows the curve to adapt to the new location of the vertex point you moved while still maintaining the relationships.

Note:

You cannot drag an edit point that is fully constrained.

Flexible
Rigid

Note:

Simplifying a curve can cause the relationships placed on a curve to be deleted.

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Working with .jt documents in Solid Edge

Mon, 25 Mar 2013 00:14:51 +0000

Opening jt documents in Solid Edge
You can open jt documents in Solid Edge assembly, part, or sheet metal with the Open command. On the Open File dialog box, after you select the jt (.jt) document you want to open, click the Options button to display the Import Options for jt Documents (.jt) dialog box. The jt document will always contain facet data, but you can use the dialog box to add wire and solid data to the document.

Note:
When importing assemblies containing more than 600 to 700 part files you need to set the value of the Import DoNotSave=On parameter in the translators ini file to Off. The Import DoNotSave parameter controls whether the Solid Edge part files are created during the translation, or on the initial save of the assembly file. Setting this value to off may take longer to translate but will consume less memory.

Solid Edge supports the following jt document structures:

Monolithic—Produces a single jt document, which can contain a single part, an assembly, and assembly structure information.
Per_Part—Produces a jt document containing an assembly structure and a folder containing the jt part documents.
Full_Shatter—Produces a jt document for each node in the assembly document.

Importing facet bodies
You can import facet bodies into Solid Edge Part and Assembly. A facet body is a surface representation defined by triangles.

Rules for facet bodies

When you import a jt facet body, it is stored in Solid Edge as a non-Parasolid body. The facet body is displayed in Feature PathFinder as a part copy. However, since the facet part copy is a non-Parasolid body, the rules are different than those for a normal part copy.

When a facet body is imported into Solid Edge Part, it is placed and treated as the base feature, but it is not considered a design body since no material can be added or removed from this type of feature.
Multiple facet bodies can exist in a part file as constructions. Only one of the facet part copies can be converted to a base feature in a document. Any other facet bodies are treated as constructions.
A document can contain both a facet part copy and design body (Brep). If a document contains both, only one can be converted to a base feature. Any other facet bodies are treated as constructions.
You cannot modify a facet part copy. If a multi-body facet jt files is imported into part, only one entry is added to the Feature PathFinder, and the multi-body facet is treated as a single entity.
A facet body from a jt files can be added to a Solid Edge document with either the Insert Part Copy command or the File Open command.
You cannot locate faces, edges, or vertices of a faceted body. You can only locate the entire body.
Commands that require faces, edges, or vertices as input will simply fail when trying to locate the faces, vertices or edges of a faceted body. For example, when drawing a sketch, the Sketch command will not locate faces, edge, and vertices of a faceted body. When the Solid Edge part file contains a facet body, any commands that only add or removes material from the base feature are disabled.
Commands that calculate physical properties are supported for facet bodies in a Solid Edge part document.
You can check for interference between facet bodies in a Solid Edge assembly document.

Displaying facet bodies
Faceted bodies are represented in Feature PathFinder with a unique icon and name. The color of the facet body is inherited from the sending system. You can control the display mode of the facet body in Solid Edge, as with any other design bodies. However, when the body is shaded, the edge display is never enabled. You can use the shortcut menu in either Feature PathFinder or the graphics window to show or hide the facet body.

JT documents in the Teamcenter managed environment
Teamcenter captures JT content in a dataset called DirectModel. The relation that connects a DirectModel Dataset to an Item Revision is IMAN_Rendering.

BOM synchronization is controlled by the Teamcenter preference SEEC_BOM_Synchronization. SEEC Administrator delivers this preference with BOM Synchronization off. To enable BOM synchronization, set the SEEC_BOM_Synchronization preference to true.

The Teamcenter preference SEEC_Foreign_Datasets determines what datasets to consider when a Solid Edge 3D dataset is not saved to the Item Revision. Preference syntax details are available in the Solid Edge Embedded Client Administrator's Guide.

For more information, see the Multi-CAD in the Teamcenter managed environment help topic.

Saving Solid Edge documents to the .jt file format
You can save Solid Edge assembly, part, and sheet metal documents in .jt format with the Save As command. On the Save As dialog box, after you select the Solid Edge document you want to save, click the Options button to display the Solid Edge to JT Translation Options dialog box. You can use the dialog box to control how the Solid Edge document is saved in .jt format.

The SePvTrn.ini file, found in the Solid Edge Program folder, is used to store the settings selected from the user interface. When you change a parameter in the options form, a new value is saved to the SePvTrn.ini file.

Note:
When you are working in a Teamcenter-managed environment through Solid Edge Embedded Client, the file SEECtoJT.ini is used to store settings selected for the user interface. The SEECtoJT.ini file is found in the Solid Edge Program folder.

Some parameters are not exposed through the user interface. You can use a text editor, such as Notepad, to set these parameters. However, if you edit this file, use extreme caution in setting these parameters. Errors in this file can adversely affect translation quality.

Note:
If you want to save documents to .jt format while working in Insight, you should set structureOption=MONOLITHIC.

Saving sheet metal files to the .jt file format
You can use the Export 3D Bodies parameter in the SePvTrn.ini file to specify how to save a sheet metal file to .jt format. By default, the parameter is set to 0, which includes only the design body in the .jt file. You can set the parameter to 1 to include only the flat body in the .jt file or to 3 to include all bodies in the .jt format.

Note:
If you set the parameter to 1 and there is no flat body for the sheet metal part, the .jt file includes the design body instead.

Saving PMI and coordinate systems to .jt format
You can use the Save PMI Data option on the Solid Edge to JT Translation Options dialog box to save all product manufacturing information (PMI) data and all model views to the JT file being created. When you select this option other JT save options are disabled and the appropriate options are set to support PMI data. Precise geometry is always sent when the Save PMI Data option is selected even if the Include Precise Geometry option is not set.

You can use the Save Coordinate System option on the Solid Edge to JT Translation Options dialog box to save the coordinate system to the JT file being created.

Understanding jt attributes and Solid Edge properties
Documents saved in jt format contain attributes that describe the information contained in the document. These attributes are the equivalent of file properties used by Solid Edge to describe document information.
When you export a Solid Edge document to jt format , Solid Edge file properties are written where they can be read by viewers, and other CAD systems that read jt format.

When you import a jt to Solid Edge all jt user attributes are imported and saved as file properties. There is no file property associativity between the Solid Edge document and the jt document. In other words, if you change attribute values in the jt file, the changes are not updated in the Solid Edge file. There is no user interface to control the import of file properties. You can use the ImportjtProperties parameter in the SePvTrn.ini file. Setting the parameter to True enables the import of jt attributes to Solid Edge file properties. By default, the value is True. If the parameter does not exist in the SePvTrn.ini file, the default value of True is assumed and the attributes are imported.

The [Import Property map] section of the SePvTrn.ini file serves as a mapping table, allowing you to map jt attributes to Solid Edge file properties. The mapping table contains two columns. The left column is an exact match of the Solid Edge property page string and the right column is the string found in the jt file.

[Import Property map]
Document Number = I-DEAS Part Number
Author = Creator Project Name = I-DEAS Project
Density = CAD_Density

Note:
Parameters found in the [Import Property Map] section are case insensitive.

Physical properties are exported by IDEAS and NX with the same naming conventions. This provides a standard name used by the VIS viewers to display or calculate properties of a solid body. Solid Edge exports physical properties using the same naming convention.

Bulk translations
Use SePvAdp.exe, found in the Solid Edge Program folder to translate Solid Edge files through a standalone interface. The executable uses the SePvTrn.ini file to control the jt output translation settings. Any changes to the .ini file must be done prior to invoking the translator.

To run the executable, Solid Edge must be installed on the computer and SePvAdp.exe must exist in the Solid Edge Program folder. The executable does not launch a full version of Solid Edge, so it requires less memory, leaving more resources available for processing larger files. When you select the files for translation, any folder or file names containing spaces must be enclosed in quotation marks “ “.

Once started, the only indication that the translator is running is the presence of SePvAdp.exe on the Processes tab in Task Manager. Once the translation of all selected files is complete, the process ends and is no longer displayed in Task Manager. Subsequent exportation of the same input file to the same output folder will overwrite the existing jt file.

You can invoke the executable through Start→Run in Windows Explorer or through a command line prompt in a DOS window. Examples of the command line prompt include:

Single input file with jt file exported to same folder as input file

C:>”C:\Program Files\Solid Edge v#\Program\SePvAdp.exe”

Multiple input files with jt files exported to same folder as input files

C:>”C:\Program Files\Solid Edge v#\Program\SePvAdp.exe” and so forth.

Single input file with jt file exported to a different output folder

C:>”C:\Program Files\Solid Edge v#\Program\SePvAdp.exe” -g -o

Multiple input files with jt files exported to a different output folder

C:>”C:\Program Files\Solid Edge v#\Program\SePvAdp.exe” -g -o and so forth.

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Opening foreign files in Solid Edge

Selection Manager

Sun, 17 Mar 2013 17:15:59 +0000

The Selection Manager menu is available when you are in the Selection Manager mode. Enter the Selection Manager mode by pressing the Shift + Spacebar or you can choose Home tab→Select group→Select list→Selection Manager Mode .

To end the Selection Manager mode, press the Spacebar.

In selection manager mode, the cursor changes to in a part or sheet metal document and to in an assembly document.
While in the selection manager mode, click on a face in the select set to display the selection manager menu.

You can drag the menu to a new location to better visualize the model.

When you position the cursor over a menu option, elements in the graphics window that match the option criteria highlight. For example, if you select a cylindrical face and then position the cursor over the Concentric option in Selection Manager, any faces which are concentric to the selected face highlight so you can preview the Selection Manager criteria.

Deselect
Removes the focus element from the select set.
Clear Selection
Removes all elements from the select set.
3D Box Select
Specifies that you want to define a 3D box in the graphics window to add items to the select set. When using box selection, the elements which are inside or overlapping the 3D box are included in the selection.
Connected
Adds faces which are connected to the focus element. You can use the flyout options to specify what type of connected elements you want to add.
- Connected
  Adds all faces which are connected to the focus element.
- Interior Faces
  Adds all interior faces which are connected to the focus element.
- Exterior Faces
  Adds all exterior faces which are connected to the focus element.
Related Items
Adds elements that have a persistent relationship to the focus element.
Sets
Adds faces which are part of the same face set as the focus element. You can use the flyout options to specify whether system defined sets (features) or used-defined sets (face groups) are recognized.
- System Defined Set
  Adds faces which are part of the same system defined set as the focus element.
- User Defined
  Adds faces which are part of the same used defined set as the focus element.
Recognize
Adds all faces which are part of the same feature as the focus element. You can use the flyout options to specify what feature type is recognized.
- Feature
  Adds all faces which are part of the same feature as the focus element.
- Rib/Boss
  Adds all faces which are part of the same rib/boss as the focus element.
- Cutout
  Adds all faces which are part of the same cutout as the focus element.
Parallel
Adds planar faces or reference planes which are parallel to the focus element. You can use the flyout options to specify what type of parallel faces you want to add.
- Faces
  Adds all planes which are parallel to the focus element, regardless of whether they are aligned or opposing. This option supports the Use Box Selection option.
- Aligned
  Adds all planes which are parallel and face the same direction as the focus element. This option supports the Use Box Selection option.
- Opposing
  Adds all planes which are parallel and face the opposite direction as the focus element. This option supports the Use Box Selection option.
Perpendicular
Adds all planes which are perpendicular to the focus element. This option supports the Use Box Selection option.
Coplanar
Adds all planes which are coplanar to the focus element. This option supports the Use Box Selection option.
Concentric
Adds all faces that are concentric to the focus element. This option is available only on faces that are cylinders, cones, and tori, both partial and full. This option supports the Use Box Selection option.
Blend Chain
Adds faces which are part of the same blend chain as the focus element to the select set.
Equal Radius
Adds faces which have a radius equal to the focus element to the select set. This option is available only on faces that are partial cylinders, partial cones, and partial tori. This option supports the Use Box Selection option.
Equal Diameter
Adds faces which have a diameter equal to the focus face to the select set. This option is available only on faces that are full cylinders, full cones, and full tori. This option supports the Use Box Selection option.
Tangent Faces
Adds faces which are tangent to the focus element.
Tangent Chain
Adds faces which are part of the same blend chain or tangent to the same blend chain as the focus element.
Symmetric About
Adds faces which are symmetric to the focus element about the same reference plane type specified. You can use the flyout options to specify what type of reference plane you want to use as the symmetry plane.
- Base XY Plane
  Adds faces which are symmetric to the focus element about the base XY plane.
- Base YZ Plane
  Adds faces which are symmetric to the focus element about the base YZ plane.
- Base ZX Plane
  Adds faces which are symmetric to the focus element about the base ZX plane.
- Local Plane
  Adds faces which are symmetric to the focus element about a reference plane you select.
Axis
Adds faces which have an axis that is parallel or perpendicular to the focus element. This option is available only on faces that are cylinders, cones, and tori, both partial and full. You can use the flyout to specify whether the axis must be parallel or perpendicular.
- Parallel
  Adds faces which have an axis that is parallel to the focus element.
- Perpendicular
  Adds faces which have an axis that is perpendicular to the focus element.
Axis Aligned
Adds faces which have a cylindrical axis that is aligned (coplanar to) the axis of the selected element along the axis you specify. This option is available only on faces that are cylinders, cones, and tori, both partial and full. This option supports the Use Box Selection Option.
- Along X
  Adds faces which are coplanar to the axis of the selected element and the base X plane.
- Along Y
  Adds faces which are coplanar to the axis of the selected element and the base Y plane.
- Along Z
  Adds faces which are coplanar to the axis of the selected element and the base Z plane.
- User-Defined
  Adds faces which are coplanar to the axis of the selected element and a user-defined plane.
Similar Feature
Adds manufactured features, such as holes, that are similar to the selected feature. For example, if you have selected a hole feature, this option adds all hole features to the select set, regardless of hole size.
Identical Feature
Adds manufactured features, such as holes, that are identical to the selected feature. For example, if you have selected a hole feature, this option adds all hole features to the select set that are identical to the selected hole.
Identical Parts
Selects all the parts that are identical to the selected part. This option is available only when working in an assembly document.
Subassembly Parts
Selects all the parts that are in the same subassembly as the selected part. This option is available only when working in an assembly document.
Select Subassembly
Selects the subassembly to which the selected part belongs. This option is available only when working in an assembly document.
Use Box Selection
Specifies that you want to define a 3D box in the graphics window to add elements to or remove elements from the select set. When using box selection, the elements which are inside or overlapping the 3D box are included in the selection. This option is available only for specific menu options.
Deselect Items
Deselects elements that match the focus element criteria when set.

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Select command