How do you create a datum plane symmetric to 2 edges?

[bmcdonald]

Problem: If i make a rectangular extrusion that is 100 wide then off set a datum plane 50 away from the edge it will be centered. If I edit the original piece to be 200 the off set datum plane remains 50 from the edge, no longer centered.

Question: How do I center a datum plane between two edges, so that it is symetrically constrained?

Brian Mc Donald

Technology Teacher

Kinnelon HS, Kinnelon NJ

I am aware that I could create the initial object symectrical to the origin, but my students don't always do this.

[TimBrotherhood]

You hit on the best solution, extruding symmetrical. It's really easy to 'Edit Definition' of the extrusion and change the option to equal both sides.

[dschenken]

Two methods come to mind.

In method one, create a relation that sets the offset of the datum plane equal to half the width of the rectangle. In feature information it will show the names of the dimensions: d0, d1, d2 are typical defaults. Pick the one that sets the rectangle width. Then edit the datum plane offset dimension and instead of entering a number enter, for example, d0/2. It will ask if you want to create a relation. Say yes.

In the second method, create a datum point on one edge of the rectangle and set it's location to ratio with a value of .5. Drag the datum plane lower in the model tree so it is after the datum point and redefine the datum plane to reference the point and be parallel to the original datum plane. You use the control key to pick a second constraint.