Pattern command (3D features)

Note:

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

Use the Pattern command (3D features) command to construct 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:

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.

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.

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).

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:

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:

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.

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

Pattern Command Bar

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