In Hole Tool: offset reference from intersection of two edges

[KrisR]

I need the hole at axis A4 a set distance away from axis A5 (yes, I moved A5 up in the tree). A5 is an axis I created myself, hoping I could dimension off of it. As far as I can tell, in the hole tool, there isn't a way to get a dimension from the intersection of two edges.

I know I can do this with a simple extrude; but I'd like to know how to do it with the hole tool.

Thank you

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[KevinBradberry]

When you create that hole by selecting a surface you should be presented with 2 green squares. Drage one square to Axis 5 and the other square to another desired reference point, you'll have to have 2 refs.

If you want Axis 5 to not show in your model tree, for cleanliness, you can create the axis on the fly while inside the Hole tool.

[KrisR]

Unfortunately, Kevin, it won't allow me to pick both the surface and A5.

[KevinBradberry]

Let me know if this helps.

http://communities.ptc.com/videos/2799#comment-5306

[Kevin]

There are a couple of ways to do this if I understand what you're looking for correctly. You could create a datum plane through A4 in the direction you want the hole to move then specify A4 and the datum plane as offset references. You can then constain the hole to move along the datum plane by selecting the drop down with offset and change it to align. You could also control the offset by creating a relation that sets the distance from the plane to 0. Another option is to use the radial type which has you specify a radial distance and angle reference.

[BrianMartin]

Hi Kris...

You can definitely do this. The two Kevin's have given some good information. You can simply pick the axis for the offset reference. You do NOT need TWO offset references. You can simply pick the axis and one orientation reference. This orientation reference is just used to help place the locating dimension.

In the image below, note that there's only ONE offset reference... the axis. You can choose multiple orientation references depending on where you want the dimension displayed.

Simply start the hole tool, place the hole on a surface as in Kevin's video. Select the axis as the first offset reference. Click in the Dimension Orientation Reference box and select any plane (except one parallel to the placement plane). You'll see how the different orientation references affect the display of the hole's locating dimensions.

If you need better instructions, just say so! Oh- and click the image above for a larger view!!

Thanks!

-Brian