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When modeling a long shaft that will be turned on a lathe, a center drill hole is often specified. At the moment this can only be done with a revolve. if ti were added to hole command, it would be real easy.
It would be the wrong profile to represent an industry standard feature when a shaft has to be tuned using live or dead centers on a lathe. Closest would be 2 operations, first small hole for the pilot tip and than a countersink.
That would be a stopgap, but there are industry standard sizes of centerpoints, so unless you have that chart you are guessing what the diameter of the countersink is and the diameter of the pilot. THat is like suggesting to someone that needs to add a BSPP (G) [British Standard Pipe thread Parallel] thread to a part, just use ANSI straight Unified thread and change the note when you dimension it... At least you can modify the thread chart file and add in definitions of the other threads that AutoDesk didn't add to Inventor (thread.xls).
Adding centerpoint definitions to the countersink part of the Hole command would solve this problem. In a way I am surprised there isn't already a pulldown for countersinks based on standard Flat/Oval Head screw & Rivet sizes. Even when you select threaded hole it doesn't change the countersink or hole diameters.
Basically startup hole, select countersink, select centerpoint angle and size from a pulldown and hit OK.
What I have done is create a center drill hole using the hole feature. That can be saved as a feature and placed in/on any future part. I ended up doing this for my company's most commonly used center drill specs. i.e #2 x 1/8, and #3 x 7/32, etc. I used the center drill specs from the Machinerys Handbook and used that to determine the necessary paramets to generate the hole.
For example #2 x 1/8 would involve changing the hole style to countersink, the angle to 60°, the depth to 0.1187, the drill diameter to 0.078 and the drill point to 118°. Then you just change the placement to concentric, select the surface/plane you want to place the hole on and click on the concentric reference.
Go to Manage and select the publish feature in the Content Center box. once you select the Publish Feature, there is a Select Feature dropdown. Just use the browser to select the hole you jsut created (Hole1) and click next. This generates another box labeled "Author Hole" with a list of the available parameters (5 of them in my case). Click the double arrow to move all those parameters to the selected parameters and click next. Note: your Content Center must be configured as read/write. Name it what you will. unfortunately, it doesn't allow you to use # or other symbols that would be helpful to identify the center hole.
Hope this helps and ultimately I agree with you...Inventor should make thos available without having to go through all these steps.
