Replicate selected parts, faces, or features along a sketch curve (or series of adjacent curves, edges on solid parts, and edges on wire parts) in the order of selection. Create new parts or modify existing parts by adding or removing material, or intersecting parts in its path. Curve pattern may also be used during an active sheet metal operation.

In the Feature toolbar:

Feature toolbar with Curve Pattern feature icon highlighted

Replicate selected parts, faces, or features along a sketch curve (or series of adjacent curves, edges on solid parts, and edges on wire parts) in the order of selection. Create new parts or modify existing parts by adding or removing material, or intersecting parts in its path. Curve pattern may also be used during an active sheet metal operation.

The Curve pattern feature tool allows you to replicate selected parts, faces, or features along a sketch curve (or series of adjacent curves, edges on solid parts, and edges on wire parts) in the order of selection. Create new parts or modify existing parts by adding or removing material, or intersecting parts in its path.

Click the Curve pattern feature tool and select the part to pattern. Then click the Path to pattern along field in the dialog and select the curve. Select Equal spacing to automatically space the instances along the curve, or select Distance to specify how far apart each instance should be. Select the Instance count to determine how many copies of the part are created. Check Keep orientation to preserve the orientation of the part being patterned.

You will see an error if the curve is not long enough to support the number of instances at the distance you set. You can adjust the Curve pattern settings, or you can individually delete or transform any entities after the pattern is complete.

Click the checkmark to accept the new curve pattern.

This video explores creating curve patterns using the Feature pattern and Face pattern options.

Click the Curve pattern feature tool and select Feature pattern for the pattern type. Then select the feature in the graphics area or in the Features list. Next, select the Path to pattern along field in the dialog and select the curve. Select Equal spacing to automatically space the instances along the curve, or select Distance to specify how far apart each instance should be. Enter the Instance count to determine how many copies of the feature are created along the curve. Check Keep orientation to preserve the orientation of the feature being patterned. Check Reapply features to regenerate the feature for each instance instead of recreating the initial pattern instance.

To apply a curve pattern to a face, select Face pattern for the pattern type. Then select the Faces to pattern in the graphics area. Select the Path to pattern along field in the dialog and select the curve. Select Equal spacing to automatically space the instances along the curve, or select Distance to specify how far apart each instance should be. Enter the Instance count to determine how many copies of the faces are created along the curve. Check Keep orientation to preserve the orientation of the faces being patterned.

Click the checkmark to accept the new curve pattern.

  1. Click Curve pattern icon.

    Curve pattern dialog

  2. Select the pattern type:
    • Part - To pattern an individual part
    • Feature - To pattern a specific feature (or features) listed in the Feature list (an extrude, fillet, sweep, sketch, etc.). Note that Feature does not work for sheet metal; see the Face pattern type for sheet metal modifications.
    • Face - To pattern a specific face on a specific part
  3. Select a Result operation type:
    • New - Create new material that results in a new part
    • Add - Create new material and add to the existing material
    • Remove - Take material away from existing material
    • Intersect - Leave material only where geometry overlaps
  4. With focus on the Entities to pattern field, select entities to replicate into a pattern.

    When selecting Faces to pattern, the Create SelectionCreate Selection Arrow Icon is useful to select related faces.

  5. Set focus in the Path to pattern along field, and then select a sketch curve (or series of adjacent curves, edges on solid parts, and edges on wire parts) along which to place the replicated pattern entities.
  6. Select a spacing option:
    • Equal spacing - Evenly distribute the requested number of instances along the curve.
    • Distance - Set how much space is offset from each instance
  7. (Distance spacing only) Enter the space to offset each instance in the Distance field.
  8. Enter the number of instances you want the pattern to have.
    • The minimum number of instances you can use is 1.
    • You will see an error if the curve is not long enough to support the number of instances in the Distance specified. You can decrease the offset between instances, decrease the number of instances, switch to the Equal spacing option, or choose a longer curve.
  9. Use Keep orientation to preserve the original orientation of the part/face/feature being patterned.
  10. (Feature pattern type only) Select Reapply features to regenerate the feature for each instance (specified in Instance count), in lieu of simply recreating the initial pattern instance.
  11. Click Accept checkmark icon.

Pattern an individual part.

A part was patterned along two adjacent sketch curves 10 times, creating new material:

example of a part patterned along two adjacent sketch curves 10 times, creating new material

Pattern a specific feature (or features) listed in the Feature list (an extrude, fillet, sweep, sketch, etc) without Reapply features selected (a faster, more lightweight feature pattern). This is not available for sheet metal.

In the following example, the initial extrude was Up to next (bringing the extrude up to the face of the surface). Without Reapply features selected, the features patterned (extrude and fillet) are patterned from the initial features and not regenerated (so the Up to next does not update for each instance of the pattern):

example of Up to next Extrude without Reapply features selected

Pattern a specific feature (or features) listed in the Feature list (an extrude, fillet, sweep, sketch, etc) with Reapply features selected. This is available for sheet metal.

In the following example, the initial extrude was Up to next (bringing the extrude up to the face of the surface). With Reapply features selected, the features patterned (extrude and fillet) are regenerated for each instance of the pattern so Up to next is applied to each instance of the pattern:

example of Up to next Extrude with Reapply features selected

Pattern a specific face on a specific part.

A face was patterned along one sketch curve 5 times to remove material from the existing material:

example of a face patterned along a sketch 5 times to remove material from the existing material

New - Create new material that results in a new part:

Curve Pattern: new material

Add - Create material and add to the existing material (in this instance, Merge with all was selected):

Curve Pattern: add material

Take material away; select the part to pattern and then Remove:

Curve Pattern: remove

Leave material only where geometry overlaps.

Before:

example of geometry before Curve Pattern intersect

After:

example of geometry after Curve Pattern intersect

  • When patterning a feature, you can select anything in the feature list, in any order. Regardless of the order selected, the features are applied in the order listed in the Feature list.
  • If you select a pattern in the Feature list, you will pattern that pattern, but not the seed. In order to get the seed included, select it as well.
  • When patterning a boolean feature (Boolean, Split, etc), you must also select the features the boolean was applied to.
  • When creating Feature patterns, all aspects of a feature are applied; for example, the end conditions in an extrude feature. (By contrast, Face patterns do not recognize these types of modifiers.)
  • You can individually delete any entities after the pattern is complete.
  • If you use more than one sketch curve (or edge on solid parts, or edge on wire parts) to direct your pattern and it does not result as expected, try selecting the sketch curves in a different order.

  • If Reapply features is enabled for the feature pattern, external references will regenerate automatically on a per-instance basis.

    In a sketch, the seed sketch dimensions and constraints to the origin or default plane will not be reapplied. You can use this behavior to scope which dimensions or constraints are reapplied within a pattern:

    • You can pattern sketch features that are dimensioned or constrained to the origin or default planes and choose not reapply those dimensions and constraints.
    • You can also create explicit construction sketches along the default planes or origin when reapplying features along them.

  • If Mate connectors are Part patterned in a Part Studio, they will all be added to the Assembly when the Part Studio is inserted. If you don't see your Mate connectors when the Part Studio is inserted into the Assembly, make sure the Part is listed as the Mate connector owner entity.
  1. Tap Curve Pattern tool.

    Curve Pattern tool icon

    Curve Pattern dialog

  2. Select the pattern type:
    • Part - To pattern an individual part
    • Feature - To pattern a specific feature (or features) listed in the Feature list (an extrude, fillet, sweep, sketch, etc.)
    • Face - To pattern a specific face on a specific part
  3. Select a Result body operation type:
    • New - Create new material that results in a new part
    • Add - Create new material and add to the existing material
    • Remove - Take material away from existing material
    • Intersect - Leave material only where geometry overlaps
  4. With focus on the Entities to pattern field, select entities to replicate into a pattern.
  5. Set focus on the Path to pattern along field, and then select a sketch curve (or series of adjacent curves, edges on solid bodies, and edges on wire bodies) along which to place the replicated pattern entities.
  6. Select a spacing option:
    • Equal spacing - Evenly distribute the requested number of instances along the curve.
    • Distance - Set how much space is offset from each instance
  7. (Distance spacing only) Enter the space to offset each instance in the Distance field.
  8. Enter the number of instances you want the pattern to have.
    • The minimum number of instances you can use is 1.
    • You will see an error if the curve is not long enough to support the number of instances in the Distance specified. You can decrease the offset between instances, decrease the number of instances, switch to the Equal spacing option, or choose a longer curve.
  9. Toggle on Keep orientation to preserve the original orientation of the part/face/feature being patterned.
  10. Tap the checkmark.

Pattern an individual part.

A part was patterned along two adjacent sketch curves 10 times, creating new material.

Example of a curve part pattern

Pattern a specific feature (or features) listed in the Feature list (an extrude, fillet, sweep, sketch, etc.).

An extrude feature was patterned along two adjacent sketch curves 15 times, adding to the existing material.

Example of a curve feature pattern

Pattern a specific face on a specific part.

A face was patterned along one sketch curve 5 times to remove material from the existing material.

Example of a curve face pattern

New - Create new material that results in a new part.

Example of a curve pattern new material

Add - Create material and add to the existing material (in this instance, Merge with all was selected).

Example of a curve pattern add material

Take material away; select the part to pattern and then Remove.

Example of curve pattern remove

Leave material only where geometry overlaps.

Before:

Example before a curve pattern intersect

After:

Example after a curve pattern intersect

  • When patterning a feature, you are able to select anything in the feature list, in any order. Regardless of the order selected, the features are applied in the order listed in the Feature list.
  • If you select a pattern in the Feature list, you will pattern that pattern, but not the seed. In order to get the seed included, select it as well.
  • When patterning a boolean feature (Boolean, Split, etc.), you must also select the features the boolean was applied to.
  • When creating Feature patterns, all aspects of a feature are applied; for example, the end conditions in an extrude feature. (By contrast, Face patterns do not recognize these types of modifiers.)
  • You can individually delete any entities after the pattern is complete.
  • If you use more than one sketch curve (or edge on solid bodies, or edge on wire bodies) to direct your pattern and it does not result as expected, try selecting the sketch curves in a different order.
  • If Reapply features is enabled for the feature pattern, external references will regenerate automatically on a per-instance basis. In a sketch, dimensions and constraints from the seed sketch to the origin or a default plane will not be reapplied.
  1. Tap Curve Pattern tool.

    Curve pattern tool icon

    Example of Curve pattern dialog

  2. Select the pattern type:
    • Part - To pattern an individual part
    • Feature - To pattern a specific feature (or features) listed in the Feature list (an extrude, fillet, sweep, sketch, etc.)
    • Face - To pattern a specific face on a specific part
  3. Select a Result body operation type:
    • New - Create new material that results in a new part
    • Add - Create new material and add to the existing material
    • Remove - Take material away from existing material
    • Intersect - Leave material only where geometry overlaps
  4. With focus on the Entities to pattern field, select entities to replicate into a pattern.
  5. Set focus on the Path to pattern along field, and then select a sketch curve (or series of adjacent curves, edges on solid bodies, and edges on wire bodies) along which to place the replicated pattern entities.
  6. Select a spacing option:
    • Equal spacing - Evenly distribute the requested number of instances along the curve.
    • Distance - Set how much space is offset from each instance
  7. (Distance spacing only) Enter the space to offset each instance in the Distance field.
  8. Enter the number of instances you want the pattern to have.
    • The minimum number of instances you can use is 1.
    • You will see an error if the curve is not long enough to support the number of instances in the Distance specified. You can decrease the offset between instances, decrease the number of instances, switch to the Equal spacing option, or choose a longer curve.
  9. Toggle on Keep orientation to preserve the original orientation of the part/face/feature being patterned.
  10. Tap the checkmark.

Pattern an individual part.

A part was patterned along two adjacent sketch curves 10 times, creating new material.

Example of curve part pattern

Pattern a specific feature (or features) listed in the Feature list (an extrude, fillet, sweep, sketch, etc.).

An extrude feature was patterned along two adjacent sketch curves 15 times, adding to the existing material.

Example of curve feature pattern

Pattern a specific face on a specific part.

A face was patterned along one sketch curve 5 times to remove material from the existing material.

Example of curve face pattern

New - Create new material that results in a new part.

Example of curve pattern: new material

Add - Create material and add to the existing material (in this instance, Merge with all was selected).

Example of curve pattern: add material

Take material away; select the part to pattern and then Remove.

Example of curve pattern: remove

Leave material only where geometry overlaps.

Before:

Example of curve pattern: intersect

After:

Example of curve pattern: intersect

  • When patterning a feature, you are able to select anything in the feature list, in any order. Regardless of the order selected, the features are applied in the order listed in the Feature list.
  • If you select a pattern in the Feature list, you will pattern that pattern, but not the seed. In order to get the seed included, select it as well.
  • When patterning a boolean feature (Boolean, Split, etc.), you must also select the features the boolean was applied to.
  • When creating Feature patterns, all aspects of a feature are applied; for example, the end conditions in an extrude feature. (By contrast, Face patterns do not recognize these types of modifiers.)
  • You can individually delete any entities after the pattern is complete.
  • If you use more than one sketch curve (or edge on solid bodies, or edge on wire bodies) to direct your pattern and it does not result as expected, try selecting the sketch curves in a different order.
  • If Reapply features is enabled for the feature pattern, external references will regenerate automatically on a per-instance basis. In a sketch, dimensions and constraints from the seed sketch to the origin or a default plane will not be reapplied.