tool reference

Sketch tools and constraints

Reference for every visible drawing, editing, constraint, pattern, and sketch input tool.

Start and finish a sketch#

Start a sketch from Model and choose Top (XY), Front (XZ), Right (YZ), a selected construction plane, or a selected planar model face. Draw and constrain geometry in Sketch, then finish the sketch to use its closed profiles in Model. Grid, Grid Size, Construction Mode, and Sketch Input control drawing aids and input behavior.

Sketch snapping#

The magnet control at the lower left turns automatic snapping on or off. With snapping enabled, Geometry First favors endpoints, centers, midpoints, and sketch edges before grid points. It can still fall back to the grid when no geometric target is close enough. Grid First favors the current grid first. The segmented priority control is dimmed while snapping is off.

Edit Points uses the same active grid spacing and snap priority as drawing. Dragged geometry is excluded from its own snap targets, so a point can move away from its previous position and snap to other sketch edges.

Snapping helps place geometry but does not create a persistent constraint. Turn the magnet off when you want completely unsnapped drawing, or add Coincident, Horizontal / Vertical, dimensions, and other constraints when a relationship must remain exact after later edits. Grid spacing comes from Settings > Grid Size; the untouched default follows the active project's unit, while a manually chosen spacing remains fixed. Locking the grid size keeps that spacing while zooming.

Sketch visibility#

The translucent-cube button in the lower-left Sketch footer shows or hides existing 3D bodies while you draw. Showing bodies helps when tracing projected geometry or relating a sketch to the part. Hiding them reduces visual obstruction. This is a viewport setting only and never deletes, suppresses, or exports a body differently.

Sketch measurement#

Use Dimension to measure and control sketch geometry. Choose Reference when you want a reported length, distance, radius, diameter, or angle that does not drive the solver; choose Driving when the value should resize or reposition geometry. For paired measurements, selection order determines which item moves and which remains the reference.

Sketch length inputs use the project's selected unit, including when you reopen a measured value for editing. New Offset, Slot, Text, Pattern, Fillet, and Chamfer drafts start with round values in that unit. Add a unit suffix such as `mm` or `in` when you want a different unit for one input.

The ruler button in the lower-left footer appears when the active sketch has dimensions. It shows or hides dimension annotations without removing the underlying dimensions or constraints. Hidden driving dimensions still control the sketch, and hidden reference dimensions still update their measured values.

Sketch footer actions#

Undo and Redo at the lower right operate on the active sketch while Sketch is open. Clear removes all geometry, dimensions, and constraints from the current sketch after confirmation. Use Clear only when the entire sketch should be emptied; use selection plus Delete or Undo for smaller corrections.

Sketch environment#

Settings > Sketch Input defines the Touch + Pencil interaction mode and default Grid Size for new work. Multi-Finger Undo & Redo enables two-finger tap for Undo and three-finger tap for Redo. Auto-Hide Used Sketches hides profiles, paths, axes, or guides after a model feature consumes them; it does not delete those sketches.

Construction Mode in the active drawing controls creates editable reference geometry. Construction entities can move, carry dimensions, and accept constraints, but do not contribute boundaries to closed profiles and therefore are not extruded as profile edges. Projected geometry is different: it is linked, read-only reference geometry until you use Break Link.

Draw geometry#

• Line creates connected straight segments. Rectangle and Polygon create closed straight-sided profiles; their available anchors control how placement expands from the first point.
• Polygon's Diameter measures its circumscribed circle. Enter a project variable in Diameter before Apply to keep the polygon and features built from it linked to that variable. A variable created separately does not resize an existing polygon that was drawn without that expression.
• Circle creates circular profiles. Arc creates curved segments. Slot creates a closed capsule-like profile.
• Spline creates smooth curves through editable points. Freehand creates streamlined curves from a drawn stroke.
• Text creates editable outline geometry from text, font, size, spacing, alignment, and straight or supported path placement.

Construction Mode creates reference geometry that helps constrain a sketch but does not form an extrudable profile.

Modify geometry#

• Transform moves, rotates, or scales selected sketch geometry. Edit Points exposes supported points and spline handles.
• Trim removes geometry at intersections. Boundary Trim keeps or removes geometry relative to a closed boundary. Circle Trim, Rectangle Trim, and Curve Trim create a temporary cutting boundary for the trim.
• Extend lengthens supported geometry to a boundary. Fillet rounds a sketch corner. Chamfer replaces a connected straight-line corner with an equal-distance bevel. Offset creates an edge or connected-loop offset.
• Repair fixes supported topology problems. Explode converts compound sources such as imported or text geometry into ordinary editable geometry.

Select the geometry requested by the active tool. Preview the result before applying it, and cancel when the highlighted result is not the intended region.

Constraints and dimensions#

• Coincident joins supported points. Horizontal / Vertical fixes line direction. Parallel and Perpendicular relate lines. Tangent relates compatible curves and lines.
• Equal gives compatible geometry the same size. Midpoint places a point at the middle of supported geometry. Concentric gives circles or arcs a shared center. Fix locks supported geometry.
• Dimension creates driving or reference dimensions for lengths, positions, radii, diameters, and angles according to what you select. Driving dimensions change geometry; reference dimensions report it. Numeric fields accept project variables and expressions.
• Project creates precise read-only sketch references from supported model edges. Projected geometry updates with its source. Break Link preserves the geometry without associativity; Relink assigns a replacement source after a reference is lost.

While a relationship constraint tool is active, choose **Manage Constraints** to see every constraint in the sketch, identify whether it is Driving or Reference, and delete individual constraints. Deletion participates in sketch Undo. If an older sketch opens with conflicting constraints, or a linked Project reference changes upstream, a persistent **Sketch constraints need attention** panel appears. Tap **Review Constraints** to find relationships marked **Unsatisfied**. Removing one of those relationships keeps the saved geometry in place; you can also revise the linked source and reopen the sketch. The warning clears when the relationships can all be satisfied.

For paired constraints, select the geometry that may move first and the reference geometry second. Fixed and linked projected references remain in place when a relationship solves. If a new placement dimension conflicts with an existing driving dimension on the same axis, MakerSolid keeps the existing driver and adds the new dimension as Reference, with an on-screen explanation; delete or change the existing driver before adding a replacement. Fully constraining a sketch makes later edits more predictable, but closed profiles can be used before every degree of freedom is constrained.

Patterns and input#

Mirror reflects selected geometry across a line. Linear Pattern repeats it along a direction. Circular Pattern repeats it around a center. Path Pattern repeats it along a manually selected ordered chain.

Import adds SVG or DXF vector geometry and provides placement and conversion controls. For SVG, root width and height values in `px`, or without a unit, use 96 pixels per inch; a `viewBox` scales those coordinates to the stated physical size. Reference Images adds an image underlay for tracing and alignment; the image is a reference rather than solid CAD geometry.

H/V and connected corners#

H/V aligns a line with the nearest sketch axis and preserves its existing shared endpoints with adjoining geometry. Reapplying the same orientation does not add another constraint. Incompatible H/V combinations are rejected without changing the sketch; use Manage Constraints to remove a conflicting relationship before retrying. Edit Points respects these axis relationships during a drag.