Inventor 2019 hole tool - picking sketch dimensions to drive hole dimensions

[jvalasek]

I often use a sketch of a hole in a cross section view to determine the location and depth of the hole as well as the diameter and depth of the counterbore or spotface.   Using that sketch to provide the parameters for hole and counterbore diameter and depths makes it extremely easy to adjust any aspect of the hole after it is created.  The screenshot should help show how I use this method.   

The problem is that the new hole tool does not allow for direct selection of the sketch dimensions to use as parameters. 

In 2018 and previous versions, using the sketch dimensions as hole parameters was as easy as clicking the box the parameter will go in, and then clicking on the chosen dimension. 

in 2019, the only options seem to be either clicking on the box and then typing the dimension's name, or clicking on the hole parameter you want to change, clicking on the flyout menu, clicking on "Reference Dimension", clicking on any feature in the model window, and then clicking on the chosen sketch dimension.  I feel like that shouldn't be necessary when the dimensions are already visible in a sketch. 

Is there some method for easily selecting visible dimensions while using the hole tool that I am not aware of, or was this broken in the latest version of the hole tool?  I would really like to have this ability back. 

Thanks

[jhackney1972]

You can still do the selection of sketch dimensions like you have in the past.  The workflow is a bit different.  Work from top of the dialog to the bottom.  Select you location first, then your settings for the hole, and then on the required input dimensions, select one at a time and touch the side arrow and pick "Reference Dimension" from the list.  Then hover over the feature containing your sketch dimensions to highlight and then the dimension you want to reference.  It picks up the variable automatically.  The Screencast will show it better.

[JoyceZhou]

Thanks for reporting the issue.

In R2019 for new Hole property panel, now we could use ctrl+click to select the sketch dimensions as driven dimension (quick way compared with Reference Dimension commands from Flyout menu). But this is only work for sketch point Hole now.

Your workflow seems using workpoint to create Hole, there is one issue (invgen-20697) for using ctrl+click to select the sketch dimension, which is under investigation. I will keep you updated if there is any progress.

Thanks,

[jvalasek]

Joyce,

Thank you for the reply, I did confirm that the ctrl+click to select dimensions works for a sketch point located hole and a concentric located hole, but not for work point located holes. 

Please keep me informed on this issue, I would much rather use work points and axis to define holes on a non-flat part than any other method, and the added difficulty to use the sketch parameters is extremely annoying.