Part, surface, and assembly features can be arranged in a pattern to represent hole patterns or textures, slots, notches, or other symmetrical arrangements. In a multi-body part, a body can be patterned as multiple bodies. In an assembly, patterns are useful when creating weldment preparation and machining features.
NoteWhen patterning assembly features, participants (components affected by the feature) are automatically chosen based on the original bounding box of the feature pattern. In some cases, this technique results in the automatic selection of more participants than necessary to complete the pattern feature. To remove participants from a pattern feature, expand the feature in the browser to view its participants, right-click a participant, and then select Remove Participant. Removing unnecessary participants can improve feature performance.
Which features can be selected for patterns?
- Solid bodies or part features (for example extrusion, fillet)
- Work features (for example, work planes, work axis, work points)
- Surface features (for example, sweep surface, stitch, boundary patch)
- An entire solid (for example, the solid body that is the result of all solid features)
Note- In an assembly, only sketched assembly features can be patterned, including their dependent fillets and chamfers. Weld features cannot be patterned. Components and assembly features cannot be patterned together.
- In a sheet metal part, single flange or contour flange features that were created using multi-edge select cannot be patterned.
- Features that affect multiple bodies or the entire part can be patterned. The pattern result only affects a single body.
- Fillets created using all filets or all rounds and shell features cannot be patterned.
- Features based on the results of an intersect operation cannot be patterned.
How can I pattern work and surface features?
There are many reasons to pattern work features including to aid in construction of a part for skeletal modeling, or to define a pattern layout to be used for an assembly component pattern. Reasons for patterning surface features include creation of multiple construction surfaces to be used as termination surfaces, and creation of symmetric surface sets which can be used in a Stitch or Sculpt feature to form a solid.
Examples of using patterned work and surface features:
- A part with work features and solid features patterned in a similar way
You want to create multiple work axis which are each offset from the axis of a pattern of holes. Workflow: You model single occurrences of the hole and the offset axis, and then pattern the hole and the axis in a single step. Then you use the work axis to create specific assembly constraints.
- A part with multiple occurrences of a work feature along the sketched path
You want to create a pattern of work points along the path. Workflow: You model a part including a sketch path and a work point on the path. Then you use the rectangular pattern along the path to create multiple occurrences of the work point. In the assembly environment, you constrain the component relative to the original work point. Then you use the assembly Associative Pattern to pattern the component.
- A symmetric part with multiple surface features
You want to create a create a mirror of multiple construction surfaces to form a solid part. Workflow: You model half of the part using construction surfaces (Extrude, Loft, Fillet, and so on) on one side of the mirror plane. Then you use the Mirror feature to mirror the construction surfaces about the mirror plane. You can then select the surfaces for use with the Stitch or Sculpt feature to form a solid.
Notes on patterning work and surface features
- You can select work and surface features when creating Rectangular, Circular, and Mirror Patterns.
- All patterned work and surface features have a node in the browser with a unique name, and can be selected individually.
- Work features are primary pattern features, which means they can be patterned even if the dependent features are not included in the pattern.
- Surface features are primary pattern features, except for three secondary pattern features: fillet of a surface edge, chamfer of surface edges, and delete face (surface or solid face). Secondary features can only be patterned if the features on which they depend are also included in the pattern.
How can I pattern an entire solid body?
To pattern a solid body with features which cannot be patterned individually, use the Pattern a Solid selection with the Join option and pattern a part body and all associated features as a single solid. Use the Pattern a Solid selection with the Create new bodies option to create a pattern composed of multiple solid bodies.
Notes:
- The Pattern a solid option can be used when creating Rectangular, Circular, and Mirror Patterns.
- The patterned solid bodies using the Join option consist of the body generated by all solid features created before patterning. Reordering a feature with respect to the pattern changes the patterned body. For example, if a fillet was added after the pattern, reordering it before the pattern includes the fillet in the patterned body.
- A pattern of the entire solid can also include work features and surface features.
- For Mirror only: when the entire body is mirrored you can select a Remove Original option to get the part containing the mirrored occurrence, but not the original solid.
- A pattern created with the Create new bodies option consists of solid bodies that can be edited as individual bodies.
Can one or more features in a pattern be hidden?
You can suppress individual occurrences of a feature in a pattern to allow a pattern to flow around another feature or an irregular shape or when creating a missing-tooth pattern. You cannot suppress the original base feature in the pattern. Individual features within a patterned occurrence also cannot be suppressed.
Which methods can be used to calculate patterns?
You can choose one of the following calculation methods:
- Optimized: Creates identical copies of selected features by patterning feature faces. Optimized is the fastest compute method, but presents some limitations, such as the inability to create overlapping occurrences or occurrences that intersect different faces than the faces of the original features. Use this option where possible to speed up pattern compute.
- Identical: Creates identical copies of selected features by replicating the results of original features. Use this option for identical features when the optimized method is not possible.
- Adjust: Creates potentially differing copies of selected features by patterning features and calculating extents or terminations of each pattern occurrence individually. Computation time can be lengthy for patterns with large numbers of occurrences. Use this option to preserve design intent by allowing pattern occurrences to adjust based upon feature extent or termination conditions such as a patterned feature which terminates on a model face.
Note- This option is not available for patterns of solid part bodies in an open or surface state.
- Because the Optimized calculation method copies and reproduces faces instead of features, it can produce different results than the Identical method. The following illustration shows the difference between Identical and Optimized calculation used for patterning of an extrusion with Through All termination type:
How can patterns be calculated faster?
Because patterns are multiples of one or more features, large patterns such as hole arrays or louvers can take a long time to calculate.
| | Adjust Patterns that terminate on the model face take longer to calculate because occurrences may be a different size. Occurrences are displayed in their true proportions. |
| | Identical You can speed up pattern calculations by specifying that all features in the pattern have identical termination. Intersection with a face determines the size of each feature, but they all are displayed as identical. |
What determines how individual features are oriented?
Rectangular patterns and patterns arranged along an irregular linear path have three options for positioning features. Because some features must be oriented in a particular way to be useful, you can experiment with the orientation options.
- Choose Identical to orient all features in the pattern the same as the first selected pattern, regardless of the shape of the path.
- Choose Direction 1 or Direction 2 to orient features along the specified path. Individual features are rotated with respect to the position of first selected feature to the start point of the path.
Autodesk Inventor computes the rotation angle based on the start point and the tangent vector, then spaces individual features along the path according to the spacing or distance you set. Individual features are rotated according to the first feature, so the rotation exaggerates with each occurrence.
For best results, position the first feature on the start point of the path. Features offset from the start point have exaggerated rotation.
For both rectangular and circular patterns, you can also choose Midplane to model the feature in a centered location, and then create a pattern where the occurrences are distributed on both sides of the original. When the occurrence count is even, the number of occurrences on either side of the original is not the same. In this case, use Direction Flip to indicate which side gets the extra occurrence. For 2D rectangular patterns use the Midplane option independently for either direction (Direction 1, Direction 2).
Can I create nested patterns of work and surface features?
You can pattern work and surface feature occurrences of another pattern individually, or create a nested pattern which includes all work or surface feature occurrences of the original pattern.
To create a nested pattern you can either select all work or surface feature occurrences, or the pattern itself. A nested pattern contains all occurrences of the original pattern, even if the occurrence count changes.
Assembly work features cannot be included in patterns.
Tips for creating patterns
Features selected for a pattern do not have to be geometrically identical or connected, but secondary features (such as corners, fillets, chamfers, delete face, chamfer of surface edges, or fillet of surface edge) are only patterned if their parent features are selected.
To define the axis for circular patterns you can select a linear edge, work axis, or cylindrical face.
To designate direction for rows and columns in rectangular patterns you can select:
- a linear edge
- a work axis
- a planar face or work plane, to use the normal of that plane as the linear direction.
To set the mirror plane, you can select:
- a work plane
- a planar face of a surface or construction surface.
To arrange features in an irregular shape, select a path constructed of lines, arcs, splines, trimmed ellipses, edges, or axes to set the direction of the pattern.
Procedures
Arrange features in a circular pattern
On the 3D Model tab, Pattern panel, click Circular to multiply a part feature or body or an assembly feature and arrange the resulting features in an arc or a circle.
In an assembly, only sketched assembly features can be patterned, including their dependent fillets and chamfers. Weld features cannot be patterned.
If possible, constraints and iMates are retained, if they are included in the pattern. Some constraints may not survive and must be reapplied.
TipYou can suppress individual occurrences in a pattern (except the original feature) to allow the pattern to flow around another feature, an irregular shape, or create a missing-tooth pattern. In the browser, right-click the occurrence, and then click Suppress. You can also control visibility and translucency of surfaces and visibility of work features by expanding pattern occurrences in the browser and right-clicking on the feature to access visibility and translucency options
To begin, create one or more work or surface features to include in the pattern.
Pattern part or assemblyfeatures
| | - On the ribbon, click
 . In the Circular Pattern dialog box, click Pattern individual features (for parts). - Click Features. If there are multiple solid bodies in the file, the Solid selection arrow is available. Use this to specify the solid body to receive the feature. The solid body the feature is attached to is selected by default. You can choose to attach the pattern to a different solid if required.
- In the graphics window or in the model browser, select one or more features or bodies to arrange in a pattern.
- Select the axis (pivot point of angle) about which occurrences are repeated. The axis can be on a different plane from the feature being patterned.
- In the Count box, enter the number of occurrences in the pattern.
- In the Angle box, enter the angle, as follows:
- For Incremental positioning, the angle specifies the spacing between occurrences.
- For Fitted positioning, the angle specifies the total area the pattern feature occupies.
- Optionally, click the Midplane check box to distribute the feature occurrences on both sides of the original feature.
- Click Flip to reverse the pattern direction, if needed. If Midplane is selected and there is an even number of occurrences, click Flip to indicate which side gets the extra occurrence.
- Click More to specify the following settings:
- Under Creation Method, click Optimized to create an optimized pattern, click Identical to create identical features, or click Adjust to terminate features when it encounters a face.
- Under Positioning Method, click Incremental to space occurrences at the angle specified, or click Fitted to arrange occurrences within the specified angle.
- Click OK.
 Show Me how to create a circular pattern
Show Me how to create an incremental circular pattern Show Me how to adjust a feature pattern to the model Show Me how to distribute pattern occurrences evenly around the parent feature Show Me how to create a circular pattern without occurrence rotation
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NotePatterns created with the Optimized or Identical method calculate faster than the Adjust method. Using Adjust, the pattern terminates if it encounters a planar face, and can result in a feature whose size and shape differs from the original.
Pattern an entire part or body
Use the Pattern a solid selection with the Join option to pattern a solid body and create one unified solid body. Use the Pattern a solid selection with the Create new bodies option to create multiple individual bodies in the pattern. In a part, you can also select one or more work or surface features to be patterned along with the body. Assembly work features cannot be patterned.
| | - On the ribbon, click .
- In the Circular Pattern dialog box, select the Pattern a solid option.
- If needed, click Include Work/Surface Features. In the graphic window or in the model browser, select work and surface features to arrange in a pattern.
- If there are multiple solid bodies in the file, the Solid selection arrow is available. Select the body to participate in the pattern. Only one body can be selected.
- Select Join to pattern the body as a single unified body.
- Optionally, select Create new bodies and create a pattern consisting of individual solid bodies.
- Select the axis (pivot point of angle) about which occurrences are repeated. The axis can be on a different plane from the feature being patterned.
- In the Count box, enter the number of occurrences in the pattern.
- In the Angle box, enter the angle, as follows:
- For Incremental positioning, the angle specifies the spacing between occurrences.
- For Fitted positioning, the angle specifies the total area the pattern feature occupies.
- Optionally, click the Midplane check box to distribute the feature occurrences on both sides of the original feature.
- Click Flip to reverse the pattern direction if needed. If Midplane is selected and there is an even number of occurrences, click Flip to indicate which side gets the extra occurrence.
- If appropriate, click More to specify the following options:
- Under Creation Method, choose Optimized to create optimized pattern, or choose Identical to create identical features.
- Under Positioning Method, click Incremental to space occurrences at the angle specified, or click Fitted to arrange occurrences within the specified angle.
- Click OK.
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Arrange features in a rectangular pattern
On the 3D Model tab, Pattern panel, click Rectangular to duplicate a feature and arrange the resulting features in a rectangular pattern, along a path, or bidirectionally from the original feature.
In an assembly, only sketched assembly features can be patterned, including their dependent fillets and chamfers. Weld features cannot be patterned.
You can arrange features in rows and columns by a specific count and spacing, suppressing individual features if appropriate. One or both directions can be a path (open or closed loop) constructed of lines, arcs, splines, or trimmed ellipses.
If possible, constraints and iMates are retained, if they are included in the pattern. Some constraints may not survive and must be reapplied.
TipYou can suppress individual occurrences in a pattern (except the original feature) to allow the pattern to flow around another feature, an irregular shape, or create a missing-tooth pattern. In the browser, right-click the occurrence, and then click Suppress. You can also suppress and restore visibility, and on patterned surface features you can change opacity.
Pattern part or assembly features
| | - On the ribbon, click . In the Rectangular Pattern dialog box, select the Pattern individual features option (for parts).
- Click Features and in the graphics window or in the model browser, select one or more features or bodies to include in the pattern. For parts, you can also select work features and surface features. Select the features to include in the pattern.
- If there are multiple solid bodies in the file, the Solid selection arrow is available. Select the body to participate in the pattern. Only one body can be selected.
- Click the path selector, and then select a surface or model body edge, work axis, line, arc, spline, planar face, work plane, or trimmed ellipse to indicate the direction of the column. Click Flip to change the column direction.
NoteWhen a work plane or planar face is selected, the normal of the plane is used as the linear direction.
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| | - Enter the count (number of features) for the column, and then click the drop-down arrow to specify pattern length. Select one:
- Spacing, and then enter distance between features.
- Total distance, and then enter distance of the column.
- Curve length to enter length of selected curve automatically.
- If the pattern has multiple rows, click Direction 2, and then set the row direction, count, and spacing, distance, or curve length.
- To distribute the pattern occurrences on both sides of the original, select the Midplane check box.
NoteWhen Midplane is selected and there is an even number of pattern occurrences, Flip specifies which side gets the extra column. - Click More to set a start point for one or both rows, set Termination Method, and Orientation Method:
- Click Start and then click a point on the path to indicate the start of one or both columns. If path is a closed loop, a start point is required.
- Under Compute, choose Optimized to create optimized pattern, Identical to create identical features, or Adjust to terminate features when it encounters a face.
- Under Orientation, select Identical to orient all features the same as the first selected, or select Direction 1 or Direction 2 to specify which path controls the rotation of pattern features.
Show Me how to create a rectangular pattern Show Me how to create a pattern along a path Show Me how to adjust a feature pattern to the model Show Me how to distribute pattern occurrences evenly around the parent feature Show Me how to create a circular pattern without occurrence rotation
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NotePatterns created with the Optimized or Identical method calculate faster than the Adjust method. Using Adjust, the pattern terminates if it encounters a planar face. This can result in a feature whose size and shape differs from the original.
Pattern an entire part
Use the Pattern a solid option to pattern an entire part or body. In a part, you can also select one or more work or surface features to be patterned along with the part. Assembly work features cannot be patterned.
| | - On the ribbon, click .
- In the Rectangular Pattern dialog box, select the Pattern a solid option.
- If needed, click Include Work/Surface Features. In the graphics window or in the model browser, select work or surface features to arrange in a pattern.
- If there are multiple solid bodies in the file, the Solid selection arrow is available. Select the body to include in the pattern. Only one body can be selected.
- Select Join to pattern the body as a single unified body.
- Optionally, select Create new bodies and select a body to create a pattern consisting of individual solid bodies.
- Click the path selector, and then select a surface or model body edge, work axis, line, arc, spline, planar face, work plane or trimmed ellipse to indicate the direction of the column. Click Flip to change the column direction.
NoteWhen a work plane or planar face is selected, the normal of the plane is used as the linear direction. - Enter the count (number of occurrences) for the column, and then click the drop-down arrow to specify pattern length. Select one:
- Spacing, and then enter distance between features.
- Total distance, and then enter distance of the column.
- Curve length to automatically enter length of selected curve.
- If the pattern has multiple rows, Click Direction 2 and set the row direction, count, and spacing, distance or curve length.
- To distribute the pattern occurrences on both sides of the original, select the Midplane check box.
NoteWhen Midplane is selected and there is an even number of pattern occurrences, Flip specifies which side gets the extra column. - Click More to set a start point for one or both rows, and Orientation Method:
- If appropriate, click Start, and then click a point on the path to indicate the start of one or both columns. If path is a closed loop, a start point is required.
- Under Compute, choose Optimized to create optimized pattern, or Identical to create identical features.
- Under Orientation, select Identical to orient all features the same as the first selected, or select Direction 1 or Direction 2 to specify which path controls the rotation of pattern features.
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Control visibility and opacity of pattern features
You can temporarily suppress the display of one or more solid features in a pattern. You can also hide all or some work or surface features. Features remain suppressed until you restore them.
You can also control the translucency of patterned features.
Control visibility of solid features
Suppress visibility of solid features:
- To suppress all occurrences, select the pattern icon in the browser, right-click, and then select Suppress.
- To suppress an individual occurrence, expand the pattern icon in the browser, select the occurrence, right-click, and then select Suppress.
Restore visibility of solid features:
- To restore all occurrences, select the pattern icon in the browser, right-click, and then select Unsuppress Features.
- To restore individual occurrences, expand the pattern icon in the browser, select the occurrence, right-click, and then select Unsuppress.
NoteOccurrences that have been suppressed individually must be restored individually.
Control visibility of work and surface features
To hide features:
- To hide all work features or surface features in all pattern occurrences, select the pattern icon in the browser, right-click, and then select Hide All Work Features or Hide All Surfaces.
- To hide an individual work or surface feature in a pattern occurrence, expand the pattern icon in the browser. Expand the occurrence icon in the browser, select the feature, right-click, and then switch off the Visibility option.
To restore visibility of work and surface features:
- Restore all work and surface features in all pattern occurrences, select the pattern icon in the browser, right-click, and then select Show All Work Features or Show All Surfaces.
- To restore individual features, expand the pattern icon in the browser. Expand the occurrence icon in the browser, select the feature, right-click, and then switch on the Visibility option.
Control opacity of surface features
When you create a surface, it is translucent and is the same color as a work plane. When you switch the Translucent option off, the surface becomes opaque.
To change opacity of surface features:
- To change opacity of all surface features in all pattern occurrences, select the pattern icon in the browser, right-click, and then select All Surfaces Opaque.
- To change opacity of an individual feature in a pattern occurrence, expand the pattern icon in the browser. Expand the occurrence icon in the browser, select the feature, right-click, and then switch off the Translucent option.
To restore opacity of surface features:
- To restore all surface features in all pattern occurrences to be transparent, select the pattern icon in the browser, right-click, and then select All Surfaces Translucent.
- To restore individual features, expand the pattern icon in the browser. Expand the occurrence icon in the browser, select the feature, right-click, and then switch off the Translucent option.
References
Circular pattern
Duplicates one or more features or bodies and arranges the resulting occurrences by a specific count and spacing in an arc or circle. All occurrences of a feature in a feature pattern are one feature, but individual occurrences are listed under the pattern feature icon in the browser. All occurrences of a new body in a pattern are individual bodies. The bodies are listed under the pattern feature icon in the browser. You can suppress or restore all occurrences or individual occurrences.
In an assembly, only sketched assembly features can be patterned, including their dependent fillets and chamfers. Weld features cannot be patterned.
| | Pattern individual features Use this option to pattern individual solid features, work features, and surface features. Assembly work features cannot be patterned.  Features selects solid features, work features, or surface features to include in the pattern. Selecting multiple features for duplication in a pattern increases calculation time.
 Solid is available if the part file contains more than one solid body. Selects the solid body to receive the pattern.
Finish features such as fillets and chamfers can be included in a pattern only if their parent feature is also selected. The same is true for a delete face feature. |
| | Pattern a solid Use this option to pattern a solid body, including features that you cannot pattern individually. The pattern can also include work and surface features. Not available in an assembly. Include Work/Surface Features selects one or more work or surface features from a part to pattern. Solid is available if the part file contains more than one solid body. Only one solid body can be included in the pattern. |
| | Join Attaches the pattern to the selected solid body. Use this option to pattern the solid as a single unified body. |
| | Create new bodies Creates a pattern consisting of multiple individual solid bodies. |
| | Rotation axis Specifies the axis (pivot point of angle) about which occurrences are repeated. The axis can be on a different plane from the feature being patterned. |
| | Flip Reverses direction of the pattern. When Midplane is selected and the occurrence count is even, flip indicates which side gets the extra occurrence. |
Placement
Defines the number of occurrences in the pattern, the angular spacing between occurrences, and the direction of the repetition. |
| | Count Specifies the number of occurrences in the pattern. |
| | Angle Angular spacing between occurrences depends on the positioning method. If you select Incremental positioning, the angle specifies the angular spacing between occurrences. If you choose Fitted positioning, the angle specifies the total area the pattern occupies. A negative value can be entered to create a pattern in the opposite direction. |
| | Midplane Specifies to distribute the feature occurrences on both sides of the original feature, which is typically created in a centered location. When the occurrence count is even, use Flip to determine which side gets the extra occurrence. |
(More)
Determines the method for calculating and positioning the patterned features. |
Creation Method | Optimized Creates identical copies of selected features by patterning feature faces. Optimized is the fastest compute method, but presents some limitations, such as the inability to create overlapping occurrences or occurrences that intersect different faces than the faces of the original features. Use this option where possible to speed up pattern compute. Identical Creates identical copies of selected features by replicating the results of original features. Use this option for identical features when the optimized method is not possible. Adjust Creates potentially differing copies of selected features by patterning features and calculating extents or terminations of each pattern occurrence individually. Computation time can be lengthy for patterns with large numbers of occurrences. Use this option to preserve design intent by allowing pattern occurrences to adjust based upon feature extent or termination conditions such as a patterned feature which terminates on a model face. NoteThis option is not available for patterns of solid part bodies in an open or surface state. |
Positioning Method | Incremental defines the spacing between features. You specify the number of occurrences in the pattern and the angle. The total area occupied by the pattern is calculated. Fitted patterns use an angle to define the total area the patterned features cover. You specify the number of occurrences and the total angle. Spacing between occurrences is calculated. Fitted positioning is usually a good choice if the design is likely to change, because the spacing of occurrences updates according to design intent. |
Rectangular pattern
Duplicates one or more features or bodies and arranges the resulting occurrences by a specific count and spacing in a rectangular pattern or along a linear path in one or both directions. Rows and columns can be lines, arc, splines, or trimmed ellipses.
All occurrences of a feature in a pattern are one feature, but individual occurrences are listed under the pattern feature icon in the browser. All occurrences of a new body in a pattern are individual bodies. The bodies are listed under the pattern feature icon in the browser. You can suppress or restore all occurrences or individual occurrences.
In an assembly, only sketched assembly features can be patterned, including their dependent fillets and chamfers. Weld features cannot be patterned.
| | Pattern individual features Use this option to pattern individual solid features, work features, and surface features. Assembly work features cannot be patterned. |
| | Features selects one or more solid features, work features, and surface features to include in the pattern. Selecting multiple features for duplication in a pattern increases calculation time. Finish features such as fillets and chamfers can be included in a pattern only if their parent feature is also selected. |
| | Solid is available if the part file contains more than one solid body. Selects the solid body to receive the pattern. |
| | Pattern a solid Use this option to pattern a solid body, including features that you cannot pattern individually. The pattern can also include work features and surface features. Not available in an assembly. |
| | Include Work/Surface Features selects one or more work or surface features to pattern. |
| | Solid If there are multiple solid bodies in the file, the Solid selection arrow is available. Select the body to include in the pattern. Only one body can be selected. |
| | Join Attaches the pattern to the selected solid body. Use this option to pattern the solid as a single unified body. |
| | Create new bodies Creates a pattern consisting of multiple individual solid bodies. |
Direction 1
Aligns selected features in the direction defined by selected edge, axis, or path. |
| | Direction Selects the direction in which occurrences are added. Direction arrow originates at the selection point. Path can be a 2D or 3D line, arc, spline, trimmed ellipse, or edge. Path can be an open or closed loop. Changes to the path update patterned feature spacing and distance. |
| | Flip Reverses direction of occurrences. When Midplane is selected and the occurrence count is even, indicates which side gets the extra occurrence. |
| | Midplane Creates a pattern where the occurrences are distributed on both sides of the original feature. For rectangular patterns, you can use midplane independently for either direction (Direction 1, Direction 2). |
| | Count Specifies the number of occurrences in the column or linear path. Must be greater than zero. |
| | Length Specifies spacing or distance between occurrences or distance the Direction 1 column spans. A negative value can be entered to create a pattern in the opposite direction. |
Distance, Spacing, or Curve Length | Specifies total distance of Direction 1 column, spacing between occurrences, or equally fitted to the length of the selected curve. Must be greater than zero. |
Direction 2
Specifies multiple occurrences in rows as well as columns. |
| | Path Selects the direction in which occurrences in rows are added. Direction arrow originates at the selection point. Path can be 2D or 3D line, arc, spline, trimmed ellipse, or edge. Path can be an open or closed loop. Changes to the path update patterned feature spacing and distance. |
| | Flip Reverses direction of occurrences. When midplane is selected and the occurrence count is even, flip indicates which side gets the extra occurrence. |
| | Midplane Creates a pattern where the occurrences are distributed on both sides of the original. For rectangular patterns, you can use midplane independently for either direction (Direction 1, Direction 2). |
| | Count Specifies the number of occurrences in the column or linear path. Must be greater than zero. |
| | Length Specifies spacing or distance between occurrences or distance the Direction 2 column spans. A negative value can be entered to create a pattern in the opposite direction. |
Distance, Spacing, or Curve Length | Specifies total distance of Direction 2 column, spacing between occurrences, or equally fitted to the length of the selected curve. Must be greater than zero. |
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Specifies the Start, Termination Method, and Orientation Method of the pattern. Patterned features can be of uniform or variable length. If length is uniform, the pattern calculates faster. If length is variable, each feature is calculated separately.
Direction 1 and 2 | Start Sets the start point for the first occurrence in both directions. If appropriate, pattern can start at any selectable point. |
Compute | Specifies how patterned features are calculated. Optimized Creates identical copies of selected features by patterning feature faces. Optimized is the fastest compute method, but presents some limitations, such as the inability to create overlapping occurrences or occurrences that intersect different faces than the faces of the original features. Use this option when it is possible to speed up the pattern compute. Identical Creates identical copies of selected features by replicating the results of original features. Use this option for identical features when the optimized method is not possible. Adjust Creates potentially differing copies of selected features by patterning features and calculating extents or terminations of each pattern occurrence individually. Computation time can be lengthy for patterns with large numbers of occurrences. Use this option to preserve design intent by allowing pattern occurrences to adjust based upon feature extent or termination conditions such as a patterned feature which terminates on a model face. NoteThis option is not available for patterns of solid part bodies in an open or surface state. |
Orientation Method | Specifies how patterned features are oriented. The orientation is determined by the first selected feature. Identical Each occurrence in the pattern is oriented the same as the first selected feature. Adjust to Direction 1 or Direction 2 Specifies which direction controls the position of patterned features. Rotates each occurrence so that it maintains its orientation to the 2D tangent vector of the path, based on the first selected feature. The angle exaggerates with each occurrence in the pattern. For best results, place the first occurrence on the start point of the path. |
