Editing Hole Feature Locations - can't seem to add or delete holes

[Anonymous]

Howdy:

Here's another one that vexes me, editing hole features.

I usually use the feature using a sketch to drive the hole locations, because that's what I'm used to AND I seem to find that existing holes it's either not possible or it's not easy to add or remove holes later.....

But I'm also finding, that I'm having trouble editing hole features with sketches.  I think that I've been able to add a new point and hole to a pattern before, but just now, I can't seem to make it work.

I have a concept part, created from another part that has "adaptive" or "incontext" hole locations.  I defined them by copying the holes into the sketch by projecting geometry, then placing a sketch point on top of the center point of the projected circle.....

So I saved this part as another part.  I unchecked "adaptive".  I made a few changes to the part that moved the holes slightly, since they weren't updating.

So I went into the sketch, and deleted the refs from the original sketch points so that I could recenter them and dimension them.

Exit sketch, and the holes did not follow the sketch points.  They are still on the projected points....  ARghh

So I edit the Hole Feature, and this is where I'm stumped.  In other CAD tools such as Solidworks, the sketch points selected for holes would be shown in the dialong box such that you can deselect them, and pick something else, but that is not the case here.  I want to "deselect all" the former locations, and repick the sketch points that are in the right location.

How do I do this?

Now, I know many of you probably do what I've been doing for months, just delete the feature and start over, but this hole is a drill spot face to mark a weld stud location, and I didn't want to mess around with figuring the depth again.  I should be able to edit these right?

Thanks

[Anonymous]

Can you post the part?

[Anonymous]

Hello John:

Well, I got it to work.

First off, for some reason, there were two sets of points on top of one another in the sketch.....  So I deleted those...

Second, though I was unable to "right-click" and "delete" or otherwise clear the references that the hole feature was using, I was able to fake it out by picking a different "placement option", and then picking againk "from sketch", thus allowing me to re-pick the points that I wanted.

So I guess I'll go back and re-distill my question:

Is there any way to UN-select a sketch point and then reselect the one that you want, without using the workaround to deselect them?

I'd really like to see a better way of knowing what is selected......

To take that one step further:  nevermind.....  I'll save that for another thread.  Well, OK - I often like to use "in-context" or "adaptive" to copy the bolt patterns in my assembly, and then easily remove them.

In Inventor, I find these "projected" sketch elements from the assembly to be really tenacious.  I just can't choose them and then hit the delete key.  They usually won't delete, or I find I have to edit that sketch back in context to remove them, so that I can then add traditional dimensions.

This goes back to knowing what is selected....  I really just want to blow away all the external references.  But I find that the only way to do this is to use the sketch tool that displays the "handles" so that you can delete the references ONE AT A TIME or edit the sketch in context and then delete the projected elements....

I so wish there was an easier way, and probably there is and I just don't know it.

Anyone?

[Anonymous]

If you make your sketch visible, then edit the hole feature, click the centers button, then hold down Ctrl to deselect. If you project holes from other parts in an assembly, the easiest way I know is to delete the reference from the browser. Or you can break the reference link, then you will be able to delete the reference. You do not need to add points on top of projected holes, just use the hole center.

[drawings]

I have found I have to delete the ground constraint on the point first.

I have an issue with the use of the ctrl key not working right if there is another point there. It ends up adding a second hole on top. This is also a problem with selecting regions in a sketch for extrusion. The ctrl key should only remove and not select a region.

[NigelHay]

I've had this trouble in the past. I found that, when deleting the old hole points, I have to window the area to select features & 'delete'. I then have to window it again to delete the double stacked points that you mention in your later post.