2019 Hole Tool - Feature direction is not intelligent (always wrong direction)

[CamperUnhappy]

When the 2019 hole tool was release I was pretty excited about it, but the more I use it, the more I want the old one back...

It seems like for my workflow (a lot of as-built parts) that the new hole tool could use some tweaking.  A lot of the time I use a shared sketch for parts meaning that I am given a sketch for a part and have to turn it into a model.  Since I have all the details already, it doesn't make sense to create multiple sketches for difference feature types.

When using the hole tool from a shared sketch, the implied direction for which direction the hole should go seems to have zero intelligence built into it to guess the correct direction.  I've had this on many occasions, but I guess the Tuesday after a long weekend and my first job of the day I'm not in much mood for this kind of thing so I'm finally bringing it up instead of just dealing with it.

This morning I created a very simple sheet metal bracket 5/8x9.5x30.  It has 6 holes in it of various sizes and I created the profile for the part as well as the hole locations all on one sketch.  When I go to put in the hole features for the plate, the hole direction seems to automatically assume that my holes are going in the -Z direction even through the default direction for my sheetmetal face was in the +Z direction, therefore my holes won't work unless I change the direction.  Not a huge deal, but why can't the hole feature analyze which direction it should probably go and adjust the hole tool window?

I guess the TLDR, the "Default" setting for the hole tool have zero intelligence built into it.

[gcook]

Agreed.  I've seen this a number of times.  And since the UI is new, you assume it is something about the interface you've screwed up.  Most annoying is that this is different behavior than the previous 15 years.

[3D4Play]

+1 this.

Aside from the non-intuitive interface, that issue has been present with the hole tool for quite some time. It's yet another item that should be on the "just do it"  list of things to fix in order to "help us make inventor better". Inventor seems to know when it can build a fillet, but it still can't figure out that a hole into empty space is...a hole in space.

Please go to the idea forum and vote up this idea:

https://forums.autodesk.com/t5/inventor-ideas/please-fix-existing-inventor-design-tool-funtionality-...

[johnsonshiue]

Hi Guys,

If I understood the logic correctly, the default hole drilling direction defaults to the opposite direction of the sketch normal. It assumes that the sketch is created on a face to be drilled. If it is based on a workplane and the face normal points away from the material direction, the default direction would be wrong. Could you share an example exhibiting the behavior not following the above explanation?

Many thanks!

[CamperUnhappy]

Here's an example of what I'm talking about.

I used the default location for the face, and the default settings for the hole tool.....but I used a shared sketch.  The hole tool doesn't consider for a single second that the only logical direction that a hole should be on such a simple part would be THROUGH the body that I just created from the very same sketch.  It's just one of those very simple operations that should just work without having to fiddle around with the settings in the hole tool wizard to figure out why my holes didn't work.

I work with keyboard shortcuts a lot and consider myself to be very fast and efficient (I've been a designer for 15 years now)......  but little nit-picky things like this kill productivity and frustrate me beyond belief from a piece of software that my company pays THOUSANDS of dollars a year for.  Here I am wasting 30 minutes of my day creating a screencast and trying to explain what is wrong with what should be a very simple tool to use.

[SBix26]

@johnsonshiue I, too, have experienced this with Inventor 2019, far more frequently than in previous versions.  I think there has been a change in the logic that sets the initial hole direction.

In the past, the Hole tool always defaulted toward the solid body and away from empty space.  If there was solid material in both directions, then it used the sketch plane anti-normal direction.  Now, it seems to simply use the plane anti-normal direction without regard to the presence of solid volume to be cut.  Additionally, the directional arrow (which one can drag to set the depth) is displayed pointing in the opposite direction, almost as if its direction is set by the old logic while the preview and geometry creation direction is set by the new logic.  I've finally gotten used to paying attention to the actual preview geometry (or lack thereof) to let me know that the hole is going the wrong direction.  It's annoying and unnecessary, in my opinion, and I'd really like to have the old hole direction logic back!

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Sam B
Inventor Pro 2019.1.1 | Windows 7 SP1
LinkedIn

[johnsonshiue]

Hi Guys,

I think my prior explanation still holds true. Yes, there is a change in behavior here. On 2018 or before, there are quite a few different hole placement types (sketch point, pick point, concentric, and on point). For non-sketch based holes, Inventor would figure out the logical drill direction based on where the body is. For sketch based holes, the direction is default to the opposite of sketch normal direction (like Extrusion).

On 2019, all the placement types are consolidated to sketch point. As a result, it carries over the sketch-based hole behavior. To certain degree, the behavior is consistent. However, the drilling logic is lost due to the placement consolidation.

There is room for improvement here for sure. In Extrude command, Cut does default to the material direction. So, it does not have to default to opposite of sketch normal. I will follow up with the project team to see what option we have.

Many thanks!

[3D4Play]

Johnson, my screenshot of the default hole tool action hasn't posted yet, but here's a video showing how the extrude/cut tool behavior differs based on the click order. I respectfully disagree with your statement "In Extrude command, Cut does default to the material direction." It does not, if you (intuitively?) tell it to cut before you make a geometry selection.

[Xun.Zhang]

Hello @3D4Play,

It is true in Extrude that switch to Cut once direction set to opposed.

However, it contains limitastion like -

1. The sketch is based on the face, not a workplane or offset surface from that face.

2. There is solid material there for cut extrusion

It seems rooms here for enhancement, send to user experience design team for more investigation.

Thanks for the feedback!

[3D4Play]

Thanks very much for the follow up. As with Johnson's statement, I also respectfully disagree with your characterization of the behavior.     If I select a cut extrude, the default direction should NEVER be where there is nothing to cut. If I want to make a hole, the direction should NEVER be where there is no material in which to place a hole. I will accept an exception in an assembly feature, because that is by design  based on user selection, and can effect a change across multiple parts. But, the sacrifice is that those features are not captured in the part drawing environment.

So, you state that the existing functionality has limitations. Yes, we know, and we are asking to "Please fix existing functionality", on the same fundamental level as this idea (please, add this hole, cut/extrude, and hole user interface to the list, and please upvote this idea):

  Please fix existing inventor design tool functionality: FG and BCD

[3D4Play]

My original reply did not post as expected. I want to share the screen shot I mentioned in light of this discussion. Thanks.