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Positioned Sketches

  • Overview

  • Benefits

  • Output Profile

  • Output Features



The default sketch type in V5 CATIA is not positioned.  The origin of this type of sketch is a projection of the origin of the part onto the sketch plane.  The orientation is aligned with the x,y,z direction of the part.  A Positioned Sketch is a sketch that has its origin location and/or orientation defined with construction geometry.  As the construction geometry changes the sketch position and/or orientation will change accordingly.


Benefits of Positioned Sketches


When defining part features that are not centered about the part origin or oriented about the part origin a positioned sketch can be much more robust than a non-positioned one.  Part of the reason for this is that it reduces the need to reference geometry outside of the sketch in order to define the features inside the sketch.  Since the origin and orientation of the sketch (which are presumably the origin and orientation of the solid feature to be created) are defined prior to entering the sketch most dimensions and constraints can be made with reference to the sketch origin.  In a regular sketch a change in position or orientation of the sketch could lead to having to redefine a lot of geometry internal to the sketch.

With a positioned sketch you only need to redefine the origin and orientation once when changes occur.  The geometry inside the sketch remains stable.

Horizontal and Vertical constraints are a convenient way to ensure a sketch is fully constrained.  Often when the orientation of a feature is modified these constraints can become invalid and have to be deleted and changed into parallel constraints (for example) in order to ensure the sketch is fully constrained.  With positioned sketches we redefine horizontal and vertical so that the constraints remain valid.  

Finally, parts and features made with positioned sketches are much easier to turn into PowerCopies.  It is very difficult to make a robust and adaptable PowerCopies without them.   


Output Profile


Note: Does not need to be a position sketch



When an output profile is created, its geometry is automatically removed from the sketch feature 3D result. In other words, output profiles are made available and updated independently from the sketch within the 3D area.

You can use profile features for creating Part Design or Generative Shape Design features.


Output profiles & features gives you more independent element available in 3D.


Output Features

Note: Does not need to be a position sketch

An output feature is created as a standard element, but it is viewed with a thicker graphic property in the Sketcher.It is made available in the 3D area and you can update it independently from the sketch, once in the 3D area. It is independent from the sketch 3D geometry. It is integrated as such both into the Parent/Children view and the specification tree.In order to keep the user's properties, the thickness is modified only if the geometry has thesame thickness as when the geometry was created.


Sketch2 has 4 output profiles & 1 output feature. Pad 1 is created from the output profile outer profile. The location of the hole is created from the output feature Knob center point.

Notice that the color of output elements can be unique.



  • Always use Position Sketches

  • Make use of Output Profile & Output Features

  • They will give every sketch more power

  • Output Features & Profile can be used in Power copy & publications


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