Sketcher External/en

Description
This tool pulls solid line geometry into your current sketch. Once these lines are pulled in, they will appear as magenta lines in the current sketch, and you can constrain and dimension sketch curves to them.

This is useful because it lets you constrain you sketch back to nearby solid edges.

You can ONLY pull in lines and edges that are on the same plane as the sketch plane. Only solid lines/edges can be pulled into the sketch, NOT 2D sketches or draft lines.

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

 * Start a sketch on face of a solid (Click on the solid face, then click the create sketch button)
 * Click the 'Sketcher External' button
 * Select, select the solid line that you want to pull into the sketch (remember this must be on the same plane that the sketch is on)

How to Tell If It Worked
If the line is successfully pulled in it will have a magenta color. If it was not pulled in, it will remain green.

Similarity to Construction Lines
External geometry magenta lines can be used like Contruction lines. Construction lines are lines that are internal to the sketch and will be used for constructing geometry only, and not for later solid operations, like extrusions.

Two Main Uses Of External Lines
There are two scenarios where you'll want to use this tool.

Option 1 is the simplest option. If you want a hole at a specific location in an object, this method should be used.

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

Some of the Part workbench tools can use a sketch for input. Where this is the case, the sketch can use the External geometry tool if the sketch is mapped to a face of a solid in a similar way to the PartDesign workbench.

Unlike a PartDesign tool, the result of a Part tool will be a separate solid and the placement parameters can be modified after construction. The sketch will define the location of the solid constructed from it, when its placement parameters are set to zero. Any changes made to these placement values will move the solid relative to the location defined by the sketch.

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.

In this case they are used as a reference for tangency constraints with the circumferences of one circle. They are also used as the reference for a horizontal and a vertical constraint to locate the centre of the second circle relative to the end and top of the Pad. This is the same sketch in edit mode, with the Pad upon which it is mapped hidden.

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