Someone else probably has a better explanation than I, but here's what I would do: when you place the drawing in your sketch, use auto demension and everything will be constrained and demensioned so lines dont move relative to one another. Then you can constrain a point on the drawing to the origin of the sketch. (First you'll have to project the origin of the part in your sketch, THEN use the coincident constraint). See if that works.

[color blue]Thanks for the suggestion.  What I 'needed' to do was when I created the AutoCAD drawing (DWG) I needed to move the drawing so the part was somewhere near World UCS 0,0.  The World UCS seems to be where the origin is when you open the drawing in Inventor and then extrude it into a part.  That is the 'correct' way to do it.

I tried to create geometry relative to the origin and then dimension from that to the original part sketch but it always moved the new geometry rather then the drawing.  Can you constrain something to the origin in a sketch???

Thanks!  :O)

I think my way still works, although I too am anal about doing things the "right" way (but I'd rather stay in inventor :p). You can constrain to the origin of the sketch by first projecting the 3d origin of the part (ie, use the project tool in sketch on the origin of the part). Alternatively, you can fix constraint on a hole center placed at the origin (I prefer the first method). Once you have a point at the origin of your sketch to constrain to, you can coincident constraint to a point on your already auto demensioned, impoorted, autocad drawing.

And to add to that, if you project the origin immediately you can start drawing from the origin and it will place an automatic constraint and lock the sketch to the origin.

Sean Dotson, PE
Inventor Tutorials & More
www.sdotson.com
Your Webbased mCAD Discussion
www.mcadforums.com

The problem is opening an AutoCAD drawing as a sketch in a part, Inventor seems to tag the AutoCAD World UCS Origin as the new origin so if the AutoCAD drawing isn't near the 0,0 then neither will the Inventor sketch.

Any way to Copy/Paste items from an AutoCAD drawing into a sketch in Inventor without having to save it as a wblock or dwg and then open it with Inventor?  I could that easy with SolidWorks and the Window's clipboard.

Thanks,
Scott

Can you simply move the AutoCAD geometry to 0,0,0?

Sean Dotson, PE
Inventor Tutorials & More
www.sdotson.com
Your Webbased mCAD Discussion
www.mcadforums.com

Very good Sean!  That's what I ended up doing and other then that first "attempt" that is how to do it.  My worries is when I run across a part someone else made with the AutoCAD 0,0 out of position and then we have to "fix" it.  :O)

Thanks for the advice (this website rules!)

    ~ Phlyx ~

EASIEST METHOD THAT I HAVE FOUND------
Its true that not all, if any, 2D cad drawings have the origin in the right place to convert to and INV ipt drawing.
Its WAY to time consuming Wblocking and "prepping" for insertion.  
1. Insert the drawing file.
2. Edit sketch.
3. Draw a line from where you would want the origin to be  on the sketch to the current origin.
4. Now move the sketch from the first point to the end of the line at the current drawing origin.
5. Delete the (construction) line.
You dont have to start the line at the sketch point of where you want the origin to be.