When I drop a Library Feature, like a Sheet Metal stamping tool, into a part, I cannot get it to rotate 90 degrees from where it originally landed.
Sketches usually contain a lot of Horizontal and Vertical (H, V) relations. But when you drop a feature into a new part, the base sketch will re-orient itself to the target plane’s H and V directions, thus preventing you from being able to rotate the sketch. The real problem here is that, face by face, the choice of the H and V directions is a fairly arbitrary one, dependent upon hidden rules in the software.
Solution 1: Set your own baseline
When constructing a Library Feature, for example a Sheet Metal Stamp, do NOT use Horizontal and Vertical relations. Instead, pick one line (or construction line) in your sketch as a baseline for determining orientation. Make the first line at some exaggerated angle away from horizontal, to avoid getting H or V snaps. Have all your other lines relate to it with Perpendicular or Parallel relations. When you deploy the stamping tool into a part, you will be able to orient it to any angle, by putting a relation (H, or V, or Parallel, or an Angle dimension) to that base line.
Solution 2: Override default H and V relations
If you’ve already built a complicated sketch and it is already riddled with H and V relations, then Solution 1 above is not so fun. Imagine that each sketch is a set of lines lying on it’s own sheet of clear mylar – your usual Sketch relations and editing commands restrain how the lines relate to each other, relative to the mylar sheet’s (0,0) corner.
You can over-ride the H and V relations in the sketch using the command under TOOLS –> SKETCH TOOLS –> MODIFY. This will pull up a dialog that allows you to drag, rotate, and even scale a sketch, provided that you have NOT YET ADDED ANY RELATIONS or dimensions that would locate the sketch in space. But the MODIFY command ignores all the relations within the sketch, and instead allows you to grab the corners of the entire mylar sheet, and slide or rotate the sketch in space – and the H and V relations slide along with it. In the case of a sheet metal tool, you usually only have to rotate the sketch +/- 90 degrees in this dialog, then you close it and add dimensions to finish the location.
What happens if you HAVE already added relations to locate in space? The MODIFY command throws a warning message that the sketch is not free to move.
