Modify Tools: Fillet, Trim, Extend, Break, Offset, Move, Scale, Mirror, and Patterns

Overview#

Once rough geometry exists, you reshape it with the Modify tools and generate repetition with Mirror and the Pattern tools. These are the commands that turn a handful of lines into a finished profile: rounding corners, cutting away overshoot, parallel-copying an outline, and duplicating a feature around a circle.

Per Autodesk's help, the Sketch > Modify panel holds Fillet, the three Chamfer tools, Trim, Extend, Break, Sketch Scale, Offset, Blend Curve, Move/Copy and Change Parameters. Mirror, Rectangular Pattern and Circular Pattern are in the Create panel. Press S to search by name if a command is not where this page says.

Where to find it#

Note: not confirmed in Autodesk's documentation: single-key shortcuts such as T (Trim), O (Offset) and M (Move). They are common defaults but are not listed in the sketch help.

Fillet#

The Fillet tool places an arc of a specified radius at the intersection of two lines or arcs. Valid fillets are between: two intersecting lines, a point at two intersecting lines, two parallel lines, a line and an arc that intersect, or two circular arcs that intersect.

1. Choose Modify > Fillet.
2. Pause over the first object and click it, then pause over the second object (a preview appears) and click it.
3. Drag the radius manipulator handle or specify a radius value. The initial preview radius is proportional to the smaller of the selected objects.
4. Press Enter to end the tool. The fillet geometry and a radius dimension appear.

Note: not confirmed in Autodesk's documentation: filleting splines, and whether selecting several corners applies an Equal constraint. Check the badges after filleting.

Chamfer#

Three chamfer types are under Modify > Chamfer (switchable in the Sketch Palette Feature Options while the tool is active). Each works on a vertex or two lines:

• Equal Distance Chamfer: one distance for both sides; the second distance dimension is driven by the first.
• Distance And Angle Chamfer: a distance and an angle.
• Two Distance Chamfer: two independent distances (the first time you move a handle, both values adjust).

Trim#

Trim removes the portion of a curve between its intersections with other geometry.

1. Choose Modify > Trim.
2. Pause the cursor over sketch geometry to preview the trim, then click to trim to the next intersection. Keep clicking to trim more.
3. Press Enter to end the tool.
4. To trim many segments quickly, click and hold, then drag across each segment.
5. If no intersection exists, the geometry is deleted.

Trim is the standard way to clean up overlapping shapes. As general guidance, trim before you dimension, because dimensions and constraints attached to removed pieces can disappear.

Extend#

Extend lengthens a curve until it reaches another curve.

1. Choose Modify > Extend.
2. Pause the cursor over sketch geometry to preview the extension, then click to extend to the next intersection. Keep clicking to extend more.
3. Press Enter to end the tool. If no intersection exists, the geometry cannot be extended.

Extend is best used to close gaps or to lengthen a short segment to meet another curve.

Break#

Break splits a curve into two at intersection points with another curve.

1. Choose Modify > Break.
2. Pause the cursor over sketch geometry to preview where it will break, then click to break it. Keep clicking to break more, then press Enter.
3. The geometry becomes two or more segments where it intersects other sketch geometry, which you can then move, delete, or give different linetypes.

Use Break to change the linetype of just part of a line, to apply a dimension to one portion, or to split a long edge before trimming.

Offset#

Offset creates a new curve parallel to an existing one at a given distance.

1. Choose Modify > Offset; the Offset dialog opens.
2. Select a sketch curve, a chain of connected curves, or a profile (only one selection at a time).
3. Choose a Direction: One Side (Distance), Two Sides (Distance 1 and Distance 2) or Symmetric (one Distance applied to both sides). Click OK.
4. The offset geometry, offset distance dimensions and offset constraints appear. The new geometry stays associated with the original.

Other behavior from the help: Match Topology limits the offset distance so the child offset matches the topology of its parent curve. Deleting the offset glyph removes the association; deleting the offset dimension keeps the relationship but unlocks the distance (right-click the glyph > Add Offset Dimension to restore it). Offsetting an ellipse by clicking near an axis gives an ellipse; clicking away from the axes gives an oval.

Offset is useful for wall thickness on a 2D profile, gaskets and clearance outlines. As general guidance, tight inside corners can produce self-intersections that need trimming.

Move/Copy#

The Move/Copy tool moves selected sketch geometry: select it, then specify the new location. Autodesk's help also notes that you can move sketch geometry off the sketch plane to create a 3D sketch. With the tool active, selecting a spline point shows or hides the spline manipulator handles.

Note: not confirmed in Autodesk's documentation: the Move Object / Create Copy / Point to Point / Set Pivot options described in older guides. Check the Move/Copy dialog in your build.

For constrained sketches, prefer editing dimensions instead of dragging geometry (general guidance).

Sketch Scale#

Scale resizes selected sketch geometry.

1. Choose Modify > Scale and click the sketch geometry to scale (you can keep selecting more).
2. Select the point from which to scale.
3. Specify the scale factor or drag the manipulator handle in the canvas.
4. Click OK or press Enter.

Scaling a sketch is helpful for traced images and imported DXF files that arrived at the wrong size. Calibrating an inserted canvas before tracing is covered on the text-and-imports page.

Mirror#

Mirror reflects geometry across a line.

1. Choose Create > Mirror; the Mirror dialog opens.
2. Select the sketch geometry to mirror.
3. Click Mirror Line and select the line or axis to mirror across.
4. Click OK. The geometry is mirrored across the Mirror Line.

The mirror line can be a construction line or a regular sketch line, and it cannot have curvature. To keep the mirror line from forming profiles, make it a construction line (general guidance).

Note: not confirmed in Autodesk's documentation: that mirrored geometry stays associative through Symmetry constraints. Check the constraint badges after mirroring.

Rectangular Pattern#

Duplicates geometry along one or two directions.

1. Choose Create > Rectangular Pattern; the dialog opens.
2. Select the sketch geometry to pattern.
3. Optionally select sketch geometry to define one or both Directions.
4. Choose the Distance Type: Extent distributes copies evenly along an overall Distance; Spacing spaces each copy at the Distance you specify.
5. For each direction set the Quantity and Distance (drag the handles or type values), and the Direction Type: One Direction or Symmetric (copies in two directions, symmetrically from the original).
6. Click OK. To edit later, double-click the pattern glyph next to the original instance.

To suppress an instance, uncheck the box next to it in the canvas; uncheck the Suppress setting to remove the check boxes.

Circular Pattern#

Duplicates geometry around a center point.

1. Choose Create > Circular Pattern; the dialog opens.
2. Select the sketch geometry to pattern.
3. Select the Center Point.
4. Choose an Angular Spacing: Full (copies evenly around a full circle), Angle (copies evenly along an angle you set, in one direction from the original) or Symmetric (along an angle, symmetrically from the original). Angle and Symmetric take a Total Angle.
5. Set the Quantity and click OK. To edit later, double-click the glyph at the center of the pattern.

Suppress instances by unchecking them in the canvas. Use it for bolt-hole patterns, gear teeth, and radial slots.

Options reference#

Tips and pitfalls#

Tip: Mirror and Pattern are far better than copying and pasting geometry. They remain associative, so a single dimension change updates every copy.

Tip: Use Offset in preference to drawing a parallel outline by hand. The offset constraint keeps the distance editable and updates when the original changes.

Tip: Trim first, dimension second (general guidance).

Warning: Dragging geometry that is part of a fully constrained sketch does not work: the solver restores the positions. Edit the dimensions instead.

Warning: A fillet applied before dimensioning can leave you without the original corner point to dimension to. Dimension to the original edges or to construction geometry that stays (general guidance).

Warning: Offsetting a closed profile inward by too large a distance can produce self-intersecting curves or nothing at all (general guidance).

Warning: Pattern instances are associated with the original and are edited through the pattern dialog.

Practice exercise#

1. Draw a 60 by 40 mm center rectangle on the origin.
2. Fillet the four corners with a 6 mm radius (one corner at a time with the Fillet tool). Add Equal constraints between the fillets if they do not have them.
3. Draw a 6 mm circle 20 mm from the left edge and 10 mm from the top edge. Mirror it across the horizontal construction line through the origin, then mirror both across the vertical axis, yielding four holes.
4. Offset the outer outline inward by 3 mm to get a groove outline.
5. Replace the four mirrored holes with a rectangular pattern for comparison: delete three of them and pattern the one remaining in 2 by 2 spacing.

Expected result: a rounded plate with four holes arranged symmetrically and an inner offset outline, all editable by changing one dimension.

Related#

• Lines, arcs, and points (02-sketching/lines-and-arcs)
• Shapes (02-sketching/shapes)
• Constraints (02-sketching/constraints)
• Dimensions (02-sketching/dimensions)