Dragging in Inventor is Everywhere

In many Inventor command functions you have the opportunity to enter a function value or you can show Inventor the value by left clicking and "dragging" the displayed arrow.  In this article I hope to show you how to make this function as productive as possible.  Below is the extrusion command function that presents a "dragging" value entry.  You would simply left click the arrow and drag to the desired value.

Most all command functions which ask for a value also offer the drag arrow.  The commands cross both modeling and editing functions but depending on your configuration settings, you may not be getting the most from their use.  So I would like to talk about that first.  When I was a machine designer, my CAD manager told me to always design one, to use stock size materials when possible and two, when I had to machine cut material shoot for full inch dimensions, then halves and quarters of an inch.  He made it clear he did not want to see any eights or smaller of an inch unless it was necessary.  Of course we were a high tolerance machine builder and some dimensions had to be in the thousands of an inch and even ten thousands for special fits.  He believed using the largest inch division possible would speed shop production and I must say he was correct.  Just think how sending a piece of structural steel to the saw operator with a non-critical length as 36 47/64 inches instead of 36 3/4 inches would slow him down.  Sure he would probably cheat and round it but you never know.  

The configuration should be done in your companies part and assembly template files so it is available for all designs.  I will be using an inch part template but the same ideas applies to metric templates.  Open up the part template and on the Options panel under the Tools tab select Document Settings.

Select the Modeling tab in the Document Settings dialog box and enter your 3D Snap Spacing for both distance and angle dragging.  This will automatically keep the entry value to increments of the value you enter when you drag a function arrow.  In my case I have set 1/8 inch distance which will quickly give me enough accuracy for non-critical modeling but will also allow me to easily conform to my CAD manager rules just using the drag function, without keyboard entry.

I did not mention it but if you left click and drag on the ball at the base of the arrow, you can "drag" enter angle values in increments of the above setting, in my case 5 degrees.  This is not available in all functions.

Once you have saved your template, your next part or assembly model it will be easy to "drag" the value of your next extrusion, revolution or fillet radius just to mention a few functions.  Of course you can always over-ride the drag value by typing in an value you desire.

So that covers modeling functions but how about sketches.  You can accomplish the same thing in your Inventor sketches by configuring the Snap Spacing under the 2D Sketch section under the Sketch tab in the Document Settings dialog box.  Of course this should also be done in the part and assembly templates.  There is no setting for an increment angle.

There is one more configuration that needs to be set to allow 2D sketch snap spacing to work.  This is done in the Application Options dialog box located on the Options panel under the Tools tab.  On the Sketch tab, place a check mark beside the "Snap to grid" option.  You do not have to turn on the grid display, located in the same dialog box, unless you desire to have a visual grid during sketching.

You will get an odd readout when you are sketching lines at an angle if your Heads-Up-Display Dimension Input is set to "Polar Coordinates".  It is actually snapping to your snap settings but since it is on an angle, the values displayed are not intelligent.  If you change your Dimension Input to "Cartesian Coordinates", the values will display increments of your settings.  I do not believe this is an efficient setting but that is a personal opinion.

So give the Inventor dragging options a try.  If you would like to test before changing your default templates, make the configuration changes in one of your parts using your current template.  If you like them, transfer the settings to your default templates.