Sketcher External

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.



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)

NOTE: If you are pulling in lines that are solid body edges AND lines in another sketch, make sure to hid the other sketch. You can only pull in the solid body lines/edges.

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.

External geometry magenta lines can be used as construction lines too, because they will not appear as sketch lines once you exit the sketch. But remember the external geometry magenta lines are parametrically linked back to a solid face.

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


 * Option 1: You want to add holes or extrudes(pads) to the current solid that you're sketching on
 * Option 2: You want to create tool bodies that are separate from your original solid
 * A tool body is a solid that you use as a tool in later addition/subtraction operations

Option 1 is the simplest option. 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.