About Creating Entities in Sketcher
You can begin sketching entities by selecting a sketching tool and clicking inside the graphics window. When you select a sketching tool, a point that rubberbands to the pointer is created. After you select its location, the rem.aining geometry rubberbands to the pointer until you select points to place it. If you are working on a model, the point snaps to the part geometry, such as edges and curves, and the geometry is highlighted. System-generated weak dimensions necessary to solve the section are displayed when you finish sketching an entity. All sketching tools work in Continue mode.
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Dimensions are not displayed while a sketching tool is active.
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Any sketched entity can be designated as geometry or construction. Sketching tools create geometric entities by default. To create construction entities, click > 
Construction Mode. You can convert geometric entities into construction entities or vice versa:
Construction Mode. You can convert geometric entities into construction entities or vice versa:• To convert geometric entities to construction entities, select an entity then click Construction on the mini toolbar.
Construction entities are displayed with a dashed line style.
• To convert construction entities to geometric entities, select an entity then click Solid on the mini toolbar.
Geometric entities are displayed with a solid line style.
Points, centerlines, and coordinate systems have separate tools for creating datum or construction instances. You can use the Search tool to search for a datum created using the Point, Centerline, or Coordinate System Datum tools.
Dynamic Constraining
As you move the pointer, applicable constraints are offered and the geometry snaps to these constraints. The relevant existing geometry is highlighted. For example, a tangent constraint is offered when you sketch a line near the circumference of a circle. You can accept, lock, disable, or disregard the offered constraints.
Sometimes the sketch snaps to the model geometry automatically, and might change the resulting geometry. To prevent the sketch from snapping to the model geometry, perform one of these actions:
• To disable snapping for the current action, while the Sketch tab is open, hold down the SHIFT key while you sketch.
• To disable snapping by default, perform one of the following actions:
◦ Right-click in the sketch window to open the Sketcher shortcut menu. Click Snapping Settings and clear the Snap to Model Geometry check box.
◦ While the Sketch tab is open, click > and clear the Snap to Model Geometry check box.
◦ Click > > and under Sketcher references, clear the Allow snapping to model geometry check box.
References for snapping to model geometry can change depending on the location of your pointer. For example:
• When you hover over a midpoint or an endpoint of an edge, the edge is used as a reference. An edge reference creates a finite projection, which has a midpoint and endpoints.
• When you hover over the edge of a surface that is orthogonal to the sketching plane, the surface is used as a reference. A surface reference creates an infinite projection, which does not have a midpoint or endpoints.
Selecting Sketching Tools
The Sketching group contains tools to create the following entities:
• Lines
• Quadrilaterals
• Circles
• Arcs
• Ellipses
• Splines
• Fillets
• Chamfers
• Text
• Offset
• Thicken
• Project
• Centerline
• Point
• Coordinate system
| | Some of the sketching tools are also available using the mini toolbar. |
Using the Mouse or Keyboard in Sketcher
You can use the mouse or keyboard to perform the following operations:
• Click an entity to see the available options on the mini toolbar.
• Middle-click or press ESC to abort the current operation. Middle-click or press ESC again to exit the active tool.
• Right-click to lock an offered constraint while you are sketching. Right-click again to disable the constraint and right-click a third time to enable it again.
• Right-click the sketch window to access the shortcut menu. Commands change when an entity is selected.