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 may be used as a reference for constraints within the sketch.

This tool is used to 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 it 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 it is necessary to hide the solid that was created from the currently being edited sketch and un-hide the previous solid. Now the previous solid is visible and you can apply the external geometry tool to one of its elements, if you wish.

As an example of this, imagine you have two pads, Pad001 and Pad002. Pad002 was created from a sketch that is attached to one face of Pad001. You want to edit this sketch. When you edit the sketch the solid Pad002 is visible in the scene. If you select an edge you might be selecting an edge of Pad002, which is not allowed. To overcome this you should hide Pad002 (using the space bar) and unhide Pad001. Now when you select an edge you will be selecting an edge of Pad001. You may want to enable the Selection View panel ; this panel will show you exactly which object you are selecting and is very helpful for understanding this common editing issue.



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), or double click a sketch in the model tree to open it for editing.
 * 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)

Selection rules
Selection rules for what objects can be imported differ drastically between FC v0.16 and FC v0.17.

v0.17

 * Only edges from objects from same coordinate system are allowed

That is, the sketch and the object must be in same Body, or in same Part, or both outside of any Parts and Bodies.

For example, If the open sketch is in Body, you can use another sketch from Body as external geometry, but you can't use a sketch from Body001, or an edge from a Part Cube in the root of the project. Use Shapebinder feature to bring in a copy of the object into the coordinate system of open sketch. Then you will be able to use edges of Shapebinder object.


 * No circular dependencies are allowed

That means, you can't link to Pocket made with this sketch.

Unlike in v0.16, sketch doesn't have to be on any face in order to use this tool. Links directly between sketches are possible, and encouraged.

v0.16 and older
You can only link to edges of the shape the sketch is mapped to.

For example. If Sketch was made on a face of Pad, you can only use edges of Pad. You can't use edges of Sketch that was used to make Pad. You can't use edges of Pad that are inherited onto a Pocket done with this sketch (you need to hide Pocket and unhide Pad to link new stuff in).

Sketch MUST be mapped to a face in order to use this tool.

Appearance When Successfully Linked
A (default magenta) coloured line will be overlaid when an edge is successfully linked (the vertices will be red), and will be visible in your sketch only 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.

Use Of External Geometry in a PartDesign Workbench Work Flow
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. PartDesign workbench is intended to produce one single solid, therefore these sketches with external geometry are used to create a new feature of that one single solid.

The external geometry can, for example, be used as a reference for a constraint being used to position a hole in an object at a specific location relative to an edge or vertex.

Use Of External Geometry in a Part Workbench Work Flow
You can use any Part geometry that is in coordinate system

Example
This, below, is a sketch mapped to the top face of a solid created from a Pad of a previous sketch. The magenta lines are External Geometry linked to two edges of this pre-existing Pad.

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 edit mode is closed, External Geometry lines are not visible.