|Sketch → Sketcher geometries → Sketcher External|
|Introduced in version|
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 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 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.
- 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)
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 tool can, for example, be used as a reference for a constraint being used to position a hole in an object, at a specific location.
Use Of External Geometry in a Part Workbench Work Flow
Part Workbench tools make new separate solids, unlike PartDesign tools which make a new feature of a single solid.
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.
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.