How to re-position sketch data imported from a drawing
Method 1:
When 2D lines are imported from a drawing (via Insert - Sketch from Drawing, Insert - DXF/DWG, or a copy/paste technique) the sketch lines are almost always shifted to the right and above the origin of the desired sketch plane. This happens because the (0,0) origin point of a drawing is typically the lower-left corner of the drawing sheet. Trying to window-select and then drag and drop the imported sketch geometry to the desired location often causes just one or two entities to drag and resolve instead of moving the entire selection.
Instead, perform a window-select to group the entire set of sketch lines, and then use a Ctrl-Drag to re-locate the entities. As is usual, a Ctrl-drag method creates a copy of the entities. The reason for using a Ctrl-drag (instead of a Shift-drag, which would not leave a duplicate behind) is that the Shift-drag action does not allow you to snap the entities to another object like the origin.
To avoid creating a copy of the entities, once you've Ctrl-dragged them to get them moving, you can let go of the Ctrl key (but keep holding your mouse button). The software will now behave similar to a Shift-drag, moving instead of copying, and yet you will still have good snap inferencing.
Method 2:
In a complex sketch, the technique described above might still not be satisfactory. There is another way to accomplish the desired end result that takes a few more steps to perform but does not rely so much on precise mouse technique.
SolidWorks 2001Plus added some 2D to 3D tools to help in situations like this. If you want to relocate the entirety of the sketch, just select a sketch point that you would like to be aligned to the origin and choose Tools - Sketch Tools - Align - Sketch. This command is also located in your 2D to 3D toolbar. This moves the entire sketch contents so the selected point lines up with the model origin. Or, if you have lines from other adjacent sketches you wish to line up with, you must pre-select first a POINT in the current sketch, then a LINE in the target position, and the Align Sketch icon will slide the sketch point up to that datum.
Method 3, 4, and 5:
Are you kidding? Five methods for this? Yes indeed... this task is common enough for users who are migrating 2D data into Solidworks that a host of tools have evolved to satisfy every user style and level of sketching faculty. The last 3 methods are more general to sketching in a 3D part file, and are cited in an earlier tip titled “How to precisely position an un-constrained sketch”.
