Sketcher External

Description
When a sketch is mapped to a face of a solid, the Sketcher External Geometry tool can be used to link to an edge or vertex of that solid. It works by inserting a linked construction geometry into the sketch. The default colour of externally linked edges, is magenta. As with standard non-linked construction geometry (blue), the externally linked geometry is only visible when the sketch is in edit mode and is not directly used in the subsequent result, from use of the sketch in another tool. Both types of construction geometry are used as a reference for constraints, within the sketch.

This tool is used constrain elements of a sketch with reference to an element of an external solid, to which the sketch has been mapped. For example, it could be used to pocket a hole in the centre of a solid or 30mm from one end etc..

The external geometry tool can only be applied to edges and/or vertices of the solid to which the sketch has been mapped. Consequently you can only link to elements of 3d solids. The edges may be straight, an arc or a circle.

You can not link to an external geometry of the solid which will be created from the sketch you are currently editing. This seems logical, however is a common issue when re-editing a sketch. When re-editing a sketch of a PartDesign feature which is mapped to the face of a solid (e.g. if you want to go back and change a sketch for a Pad002 where that sketch was mapped to a face of another Pad001) it is necessary to hide the solid the currently being edited sketch created (Pad002) and un-hide the previous solid (Pad001), so that you can see the previous solid (Pad001) if you wish to be able to apply the external geometry tool to one of its elements.



Use

 * Create a new sketch on face of a solid (Click on the solid face, then click the create sketch button) or map an existing sketch to a selected face of a solid (first select a single face of a solid then use the "Map Sketch to Face" tool).
 * Click the 'Sketcher External' button
 * Select the edge, or vertex, of the solid that you want to link to in the sketch (remember this must be an edge or vertex of the solid to which the sketch is mapped)

How to Tell If It Worked
If an edge is successfully linked it will have a magenta coloured line mapped over it (the vertices will be red), which will be visible in your sketch while your sketch is in edit mode.

Similarity to Construction Lines
External geometry (default colour magenta) lines are similar (default colour blue) Contruction lines except in that the external geometry magenta lines are parametrically linked back to an element of the solid to which the sketch is mapped. Construction geometry are lines that are internal to the sketch, are only visible when the sketch is in edit mode and will be used for constraint references only, and not directly for later solid operations, like Pad or Pocket.

Two Main Uses Of External Lines
In the PartDesign workbench work flow, the External Geometry tool is used to assist in the positioning of an aspect of the solid you are constructing, relative to the previous stage in its construction. In other work benches it can be used in other ways.

If you want a hole at a specific location in an object, this method should be used.

Option 2 must sometimes be used. If I need to subtract away multiple cutting bodies then I need those bodies to be separate from my original solid. In that case I will need to extrude my sketch to make a new separate solid, then use clone or rotate or array to make a bunch of parametric copies of it.
 * If I'm working with sketches, only individual sketches can be extruded or padded.
 * Extruding will create a new solid body.
 * Padding or using the pocket tool will NOT. They will use the sketch to alter your original solid.


 * Option 1: use pad or pocket to alter your solid, adding metal or making holes.
 * Option 2: use extrude to make your tool solid, then duplicate it with the above methods, and add or subtract it from your original solid.

Sneaky Usage, Dimension One Sketch Off Of Another
One can use this to dimension one sketch off of another using the following order of operations:
 * 1) Make sketch#1
 * 2) Pad or extrude it to make a solid, solid#1
 * 3) Make sketch#2 on the same plane as sketch#1
 * 4) Pull in solid#1 lines into sketch#2
 * 5) Pad or extrude sketch#2 to make solid#2
 * 6) Optional, hide solid#1

Example
The magenta lines are External Geometry selected on two objects of the same extrusion products with previous sketch. In this case they are used to create the constraints of tangency with the circumferences. The line on the smaller rectangle is not used. The active sketch with the basic forms hidden and external geometries visible.

When the sketch is closed, External Geometry lines are not visible.