To Create a Fill Pattern
1. Select the feature that you want to pattern and click
Model >
Pattern. The
Pattern tab opens.
2. Select Fill from the list of pattern types. The Fill pattern options open.
3. Select an existing sketched curve, or click References > Define and sketch the area to be filled by the pattern.
|  In Sketcher, a read-only construction point is placed at the pattern leader origin, with horizontal and vertical construction lines passing through the point. |
Click
OK to complete the sketch. When you select a curve or quit Sketcher, a preview of the pattern grid is displayed, based on the default values. Each pattern member is identified by
.
4. Select a grid template.
| Click the arrow next to the  button to access the grid templates. |
5. To change the spacing between pattern member centers, type or select a value in the box adjacent to
. Alternatively, in the graphics window, drag the handle or double-click the value associated with the
Space label and type a new value.
6. To change the minimum distance between the pattern member centers and the sketch boundary, type or select a value in the box adjacent to
. A negative value makes the center lie outside the sketch. Alternatively, in the graphics window, drag the handle or double-click the value associated with the handle and type a new value.
7. To specify the rotation angle of the grid about the origin, type or select a value in the box adjacent to
. Alternatively, in the graphics window, drag the handle or double-click the value associated with the handle and type a value.
8. Set one or both of the following optional parameters for
circular and
spiral grids:
◦ To change the radial spacing, type or select a value in the box adjacent to
. Alternatively, in the graphics window, drag the handle or double-click the value associated with the handle and type a new value.
◦ To rotate pattern members about an origin, select the Follow template rotation check box on the Options tab.
9. Set one or more of the optional parameters on the Options tab:
◦ Regeneration option—Reduces regeneration time by selecting a more restrictive regeneration option, depending on the complexity of the pattern:
▪ Identical—All the pattern members are identical in size, are placed on the same surface, and do not intersect each other or part boundaries.
▪ Variable—The pattern members can vary in size, or be placed on different surfaces, but they cannot intersect each other or part boundaries.
▪ General—There are no pattern member restrictions.
◦ Use alternate origin—Uses an origin different than the default geometric center of the lead feature or geometry to place the pattern leader.
◦ Follow leader location—Offsets all pattern members from the sketch plane using the same distance as the pattern leader's offset.
◦ Follow surface shape—Positions pattern members to follow the shape of the selected surface. Click the collector and select a surface.
◦ Follow surface direction—Orients the pattern members to follow the surface direction.
10. To exclude a pattern member at a certain location, click the corresponding black dot that identifies the pattern member in the graphics window. The black dot changes to white (
) to show that the pattern member has been excluded. You can click the white dot again while redefining the pattern to re-include the pattern member.
11. Click
.