Edit Inventor Sketch Coordinates

When you have an Inventor part sketch that has a dimension being referenced from a point that is not along the axis of the sketch, you will probably have to add a construction line to get the location dimension you desire.  In the example below the 120 mm dimension would be impossible if you did not add the construction line from the corner first.

There is a better way to handle this sketch.  You can move and rotate the sketch X,Y coordinate system, for this one sketch, to allow the placement of the required dimensions.  Below is the same sketch with the sketch coordinate system rotated to match the angled edge.  The same dimensions can be placed without the construction line.

One of the best features about using this method is that the sketch coordinate system is remembered for only the current sketch and will revert back to the part original sketch layout coordinates for any future sketches.  Since it is remembered, if you come back to this sketch, the sketch coordinate system is restored for any required editing.  I would like to step you through the process of establishing a new sketch coordinate system.  I will use the same model.  I will start by a new sketch on the face.  You will notice the original part orientation will place the sketch coordinates to match.

You will find the "Edit Coordinate System" tool under the Sketch tab on the Constrain panel in the drop down panel.

Inventor will prompt you to left click to select the existing origin.  Pick the small blue ball at the center of the existing sketch coordinate system.  The coordinate system will then be attached to your cursor so you can move it anywhere you desire.  Please note it will not actually physically float around but the "+" symbol beside your cursor arrow indicates that it is attached.

Next left click to select the point you want to be the new sketch origin.  I will be using the lower corner of the the angle cut for my example.  The sketch coordinate indicator will jump to the new location.

The next step is to align the desired sketch axis with the edge.  I will be using the X-axis.  Left click on top of the X-axis rod, not the arrowhead.  It will highlight as you pass over it to make sure you are ready to select it.

Next you want to left click to select the edge of the model you want to align the selected axis.  In my example I will select the angled model edge.  The sketch coordinate icon will align with the selected edge.  If it is flipped the wrong way simply right click and pick the "Flip Axis" command for the context menu.

The last step is to right click and select "OK" for the context menu or simple press the "Enter" key on the keyboard.  You will see the origin, X and Y axis shift to the new location.  The orientation of the sketch to the screen may be disturbing, but we will take care of that next.

The easiest way to re-orient the sketch so the sketch coordinate system is square to the screen is to select the "Look At" command located on the Navigation Panel and then pick the active sketch in the Inventor Browser.

Finish your sketch as you would normally do.  The next sketch you add to the part will follow the original sketch coordinate system.  If you edit this sketch, the modified sketch coordinate system will be restored.

You have to admit this is a very cool function to add your sketching ability and speed.