Pro Engineer/Sketcher

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Sketcher is used to create arbitrary geometries that will define the various features of a mechanical part. It is similar to the Sketch function in other 3D solid modeling software such as Unigraphics, Inventor, Solidworks, and CATIA.

Invoking and Finishing[edit | edit source]

Sketcher is invoked by clicking the Sketch Tool button on the Datum toolbar, or through the menu via "Insert > Model Datum > Sketch..."

Once invoked, a dialog box titled Sketch appears, asking the user for the Placement and other Properties of the sketch. The dialog appears with the Sketch Plane field highlighted, ready for the user to select some Datum Plane or part surface. In an new part file, at least three predefined Datum Planes should already be available: RIGHT, TOP, and FRONT. Simply choose one to begin; the sketch will later be placed on the chosen plane.

Once a plane is selected, the dialog suggests a reference plane. Choosing this plane is required to orient the sketch on the screen for the session. However, the choice is often irrelevant until existing geometry has already been modeled. The reference plane must be perpendicular to the sketch plane and must be designated as orientation Top, Bottom, Left, or Right. For example, if you had chosen the sketch plane to be TOP, Pro/Engineer may have suggested the RIGHT plane as the reference, with orientation Right. This means that the RIGHT plane will be placed on the Right side of the sketch. If Orientation is changed to Top, then the selected RIGHT plane will now be on the top of the sketch.

If desired, the sketch may be named at this time in the Properties tab of the dialog, but it can easily be renamed later.

Click the Sketch button to begin. Pro/Engineer changes the colorscheme as visual notification that the mode has changed. The available toolbars changes as well.

For convenience, the References tool is automatically invoked at the start of every sketch session. References allow a sketch to be placed and constrained relative to other geometries in the part outside of the sketch. For example, to draw a line across the diagonal of an existing solid brick, the sides of that brick would need to be referenced to the sketch. This is similar to the Project Geometry function in the sketchers of Unigraphics and Inventor. References show as dotted lines; by default the two other base datum planes have already been referenced in a new part sketch, which gives the user horizontal and vertical axes as a start. Most sketches need extra user-picked references. Once all desired ones are picked, ensuring that Reference Status reads Fully Placed, close the dialog.

At this time the sketch is free to be created using the various tools listed below.

Once the sketch is complete, choose Sketch > Done from the main menu or click the checkmark in the Sketcher Tools Toolbar. The sketch can be saved as a separate file at any time from the File menu or the File toolbar.

List of Sketching Tools[edit | edit source]

Sketcher Tools Toolbar

  • Select
  • Line
    • 2-point
    • Tangent Line
    • Center Line
  • Rectangle
  • Circle
    • Center/Point Circle
    • Concentric Circle
    • 3-Point Circle
    • 3-Tangent Circle
    • Ellipse
  • Arc
    • 3-Point Arc
    • Concentric Arc
    • Center/Endpoints Arc
    • 3-Tangent Arc
    • Conic Arc
  • Fillet
    • Circular
    • Elliptical
  • Spline
  • Point
    • Point
    • Reference Coordinate System
  • Create from Edge
    • on edge
    • offset from edge
  • Dimension
  • Modify
  • Constraints
    • Vertical
    • Horizontal
    • Perpendicular
    • Tangent
    • Midpoint
    • Coincident
    • Symmetric
    • Equal
    • Parallel
  • Text
  • Trim
    • Dynamic Trim
    • Cut/Extend
    • Divide
  • Copy
    • Mirror
    • Scale and Rotate
    • Copy
  • OK
  • Cancel

Datum Display Toolbar

  • Display Planes
  • Display Axes
  • Display Points
  • Display Coordinate Systems

Sketcher Toolbar

  • Orient Sketch to Screen
  • Toggle Display Dimensions
  • Toggle Display Constraints
  • Toggle Display Grid
  • Toggle Display Vertices

Differences From Other Parametric Sketching Systems[edit | edit source]

  • All sketches are always fully constrained. Pro/Engineer automatically suggests constraints to all sketch elements as soon as they are created; these are generally shown in gray and are called weak constraints. Constraints specified by the user are shown in a brighter color and are called strong constraints. Users may accept the automatically-chosen weak constraints by invoking the RMB context menu and selecting the Strong option. A Strong constraint may be weakened by invoking its context menu and selecting Delete.
  • Fully (strongly) constrained sketches can still be moved and reshaped. Other CAD packages consider all dimensions to be locks whereas Pro/Engineer allows the user to drag and modify even the strong dimensions already specified. To experiment with a geometry with particular constraints locked, the Lock option can be selected from a dimension's context menu.
  • There is no offset. It can be avoided by sketching entities and constraining them with dimensions and geometrical constraints.
  • Datum planes have positive and negative sides which are colored differently and have different behavior.
  • Pro/E Sketcher is simpler than similar sketchers in some other 3D CAD packages, as it has relatively few 2D entity toolbar buttons. Other CAD packages such as CATIA V5 have many more toolbars.