Getting the red 2D-sketch origin back to the part's origin when they don't match up is a mystery that's been solved. I have no idea if this will ever be useful, but someone asked me this once, so I found an answer. The 'red' sketch origin represents the 0,0 point (i.e. the 2 dimensional X, Y) of the sketch itself, which is separate from the part's origin. Another way to look at this would be... *) Start a new sketch *) Draw something, with no releations to the part's origin *) Go to Tools-> Sketch Tools-> Modify *) Move the sketch somewhere else You will see the red sketch origin move. Now if you hover your cursor right over the red sketch origin, you will see in your status bar that it reads 0, 0 or very close to that. Anything you draw from now on will be offset from the red sketch origin. Try drawing a line and click on the endpoint. Look at your property manager. The X, Y parameters are there to edit. Guess what point in space those numbers relate to? The red sketch origin... not the part's. OK, the big question... how in the heck do you get the red sketch origin back to the part's origin??? The only way I know how, is to do this... *) Enable 'Origins' so you can see the part's origin *) Draw a sketch point anywhere, whith NO relations *) Click the sketch point and in the Property Manager, change the Parameter coordinates so that X and Y both read '0' *) Now your sketch point is exactly at the red sketch origin. Cool you're almost there! *) Enable "Snap to points" in your document options (this is the top secret hint) *) Go to Tools-> Sketch Tools-> Modify *) Place your cursor over the red sketch origin until you see the usual 'inferencing' symbol *) Click and Drag the red sketch origin to the part's origin *) Hover for a second or two until it 'snaps' into place That's it! Your origins now match up. At least it works in 2004 SP4.1 Mike Wilson
