Creating a Positioned Sketch

In positioned sketch you specify the reference plane, the origin and the orientation of the absolute axis. Creating a positioned sketch ensures associativity with the 3D geometry (especially Power Copies and UDFs).

It enables you to define (and later change) explicitly the position of the sketch absolute axis. This offers the following advantages:


  • You can use the absolute axis directions like external references for the sketched profile geometry.

  • When the geometry of the 3D shape evolves and the associated position of the sketch changes, the shape of the sketched profile (2D geometry of the sketch) remains unchanged (even if the sketched profile is under-constrained).

This task shows you how to create a positioned sketch.

Before you begin:

Create a simple 3D shape similar to the one below. You are going to create a positioned sketch that will enable you to design the retaining bracket for this 3D shape.

  1. Click Positioned Sketch .

    The Sketch Positioning dialog box appears.



    You will position the sketch absolute axis as follows:

    • its origin will be on the axis of revolution,
    • its horizontal (H) direction will be parallel to the flat face,
    • its vertical (V) direction will be normal to the flat face.

  2. Move the mouse over the pad if you simply want to select the plane as you would do for a sliding sketch.

  3. Deactivate the Smart Mode if you want to select the support manually.



    Important: You can choose the type of support between two options: positioned or sliding. For detailed information, see Part Design User's Guide: Modifying 3D Shapes: Changing a Sketch Support: More about Changing Sketch Supports.

  4. Now choose the Origin and Orientation of the sketch.



  5. Activate the Smart Mode for any of them if you want to move the mouse over the pad and choose either the origin or the orientation. For detailed information, see Part Design User's Guide: Modifying 3D Shapes: Changing a Sketch Support: More about Changing Sketch Supports.



    The absolute axis of the sketch is now positioned on this axis. Its orientation has not changed.

  6. You will now specify the absolute axis orientation according to an edge of the flat face. Select Parallel to line in the Type field of the Orientation frame.

  7. Select an edge of the flat face.



    The absolute axis of the sketch is now oriented like the selected edge.

  8. Now invert the H direction and make the V direction normal to the flat face. To do this, start by selecting V Direction in the Orientation area to specify that you want the orientation to be defined according to the V direction. Select Reverse V to revert the V direction and select Swap to swap H and V directions.

    The sketch is now positioned as wanted.

  9. Click OK to validate and exit the Sketch Positioning dialog box.

    You are now in the Sketcher workbench and ready to sketch a profile for the retaining bracket.

    Note: In this scenario, you did not create any constraints on 2D geometry. The geometry is therefore under-constrained. Yet, if you move or resize the 3D shape (no matter how significantly), the profile you sketched will remain absolutely unchanged. Its shape will not be altered: thanks to the fact that the position of its absolute axis is explicitly defined, it is automatically pre-positioned in 3D before its 2D resolution.

  10. Click Exit Workbench .

    You are now back in Part Design workbench.