Applying Centerlines

How do you create centerlines in the front view using Inventor 10?

The simple answer is YES, you can add centerlines to Inventor drawings.

There are several ways to do add centerlines. in the Drawing Annotation Panel, notice that the Center Mark button has a pull-down menu. You can select Centerline to draw a centerline through a line of holes. If you select a each hole in a bolt circle, it will draw the bolt circle. If you select the center points of the circles where a hole cuts the surface of your part, Inventor will draw the centerline through those points. Sometimes I will create a sketch associated to a view and project those circles into the sketch; it makes it easier for me to select the correct geometry.

If you select Centerline Bisector, you can select two edges of a hole, slot or other shape and Inventor will create a centerline halfway between the two edges. This would work well for the holes in your right-hand flange; you could use the two hidden edges of the hole to create the centerline.

Sometimes, you need to use brute strength to create a centerline in a specific location. If you create a sketch that is associated with the view you are modifying, the sketch elements will move when you move the view. You can create this sketch by highlighting the view (so that the dashed line around the view is visible) and select Sketch from the toolbar. In this sketch, you can project any of the view's geometry and use sketch constraints and dimension to control the new lines and centerlines that you add. You need to pay attention to which line type you select; some of them are visible in your drawing and some of them are not.

Experiment with the functions, read the information in the Help files and decide which methods work best in each case.

If you right click on a view, you can click on "Automated Centrelines", which brings up the centreline menu as ahown below. This is a pretty quick way of adding centrelines to a view, and allows a fair choice as to what you wish to add. HTH,