PartDesign LinearPattern

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PartDesign LinearPattern.svg PartDesign LinearPattern

Menu location
PartDesign → LinearPattern
Default shortcut
Introduced in version
See also


The PartDesign LinearPattern.svg LinearPattern tool creates evenly spaced copies of a feature in a linear direction. As of v0.17 and above the Linear pattern tool can pattern multiple features.

PartDesign LinearPattern example.svg

Above: An L-shaped pad (B) made on top of a base pad (A, also referred to as support) is used for a linear pattern. The result (C) is shown on the right.


To create a pattern:

  1. Select the feature (introduced in version 0.19 or several features) to be patterned.
  2. Press the PartDesign LinearPattern.svg LinearPattern button.
  3. Define the Direction. See Options.
  4. Define the Length (distance) between the last copied occurrence and the original feature.
  5. Set the number of Occurrences.
  6. If you have several features in the pattern, their order can be important, see for example the image in the PolarPattern feature. introduced in version 0.19 You can change the order by dragging the feature in the list and you will see the result immediately as preview.
  7. Press OK.

To add or remove features from an existing pattern:

  1. Press Add feature to add a feature to be patterned. The feature must be visible in the 3D view:
    1. Switch to the Model tree;
    2. Select in the tree the feature to be added and press Space to make it visible in the 3D view;
    3. Switch back to the Tasks panel;
    4. Select the feature in the 3D view; it will be added to the list.
    5. Repeat to add other features.
  2. Press Remove feature to remove a feature from the list, or right-click on the feature in the list and select Remove


LinearPattern parameters in v0.16 and below.
LinearPattern parameters in v0.17 and above.


When creating a linear pattern feature, the LinearPattern parameters dialogue offers different ways of specifying the pattern direction.

Horizontal sketch axis

Uses the horizontal axis of the sketch for direction.

Vertical sketch axis

Uses the vertical axis of the sketch for direction.

Normal sketch axis

v0.17 and above Uses the normal axis of the sketch for direction.

Select reference...

Allows you to select either a DatumLine or an edge of an object or a line of a sketch to use for direction.

Custom Sketch Axis

If the sketch which defines the feature to be patterned also contains a construction line (or lines), then the drop down list will contain one custom sketch axis for each construction line. The first construction line will be labelled Sketch axis 0.

Base (X/Y/Z) axis

v0.17 and above Select one of the Body Origin's standard axis (X, Y or Z) as direction.


  • Pattern shapes may not overlap one another except for the special case of only two occurrences (original plus one copy)
  • Any pattern shapes that do not overlap the original's support will be excluded. This ensures that a PartDesign feature always consists of a single, connected solid
  • For further limitations, see the mirrored feature