How to Precisely Position an Un-Constrained Sketch
Sometimes a user does not wish to apply constaints and dimensions needed to fully shape and size a sketch. This could be because the data is imported from another CAD system, or it may be free-form, stylistic data (splines and such). However, it can be hard to align and locate the sketch precisely on the model, because each new constraint tugs the sketch out of shape instead of moving it. There are three good ways to accomplish this, depending on user taste, and also upon how much parametrization of the sketch you plan to eventually apply.
First, the easiest (read: lazy) way is to group-select all the lines, and choose TOOLS – BLOCKS – MAKE BLOCK. The lines are now all ‘frozen’ relative to each other, and can now only translate or rotate as a group. You may now apply sketch relations to the entire block to position it, and when finished, you may then EXPLODE the block to restore individual control to each line.
The second approach also requires that you first pre-select all the lines in the sketch. Then use the icon found under TOOLS – SKETCH TOOLS – MOVE, (you will also see the related tools ROTATE, SCALE, and COPY). These commands will allow you to position the selected lines very precisely, relative to a FROM and TO selection points, or by inputting jog distances or angles, and they result in no new parametric relations.
A third slick solution is to use Derived Sketch. A derived sketch is an associative copy of an existing sketch. It can only be positioned — it’s size and shape is always exactly the same as the original. This behavior is ideal for problems where you want to reference the original sketch several times, or where you prefer to leave the original data as a master sketch in its original location. One disadvantage of this approach is that it is all-or-nothing, you can only DERIVE a sketch that includes every line in the entire sketch, and the other two methods listed above will also work on a few selected lines.
How to establish a Symmetry relation between two construction lines
The SYMMETRY sketch relation can be applied when you have selected three things: a Construction Line (or ‘Centerline’), plus any two similar objects. The construction line becomes the axis of symmetry. However, if either of both of the objects you want to be symmetric, are themselves construction lines, this relation is NOT offered by the Constraints dialog. There is a simple work-around to this seeming limitation – temporarily change the two lines to be related, from construction lines, to solid. Then apply the Symmetry relation. Then change the properties of the lines back to “For Construction”. The Symmetry relation will continue to hold true no matter how the ‘construction’ property might be set.
While we are talking about the Symmetry relation, please note that the action of this relation is bi-directional. People tend to assume that the centerline will stay ‘fixed’, and the other two lines will be pulled to be symmetric across it. But if the centerline is not otherwise constrained, the symmetry relation can also ‘push’ on the centerline. This means you can use Symmetry to find a bisecting angle (between two fixed model edges, for example).