New Hole Command

[chris58]

I'm trying to get the hole in the center of this part.  I have selected the face (way off center to make a point).  When I select the edge though to give a reference for where I think the hole should be located (IE the center of the face), Inventor tries to put a hole on the edge.  I'm left with two holes with neither of them where I want them to be. 

Any help on what I'm doing wrong with the new hole command will be appreciated...

kelly.young has embedded your image for clarity.

[jhackney1972]

The forum will need your part to answer you question effectively.  I can create a similar part and place the hole without issue.

[mcgyvr]

This is how I've managed to get it working.. Not sure if its the "as designed" way..

I place the hole randomly on my round face..

Then hover back over the center point of that placed hole till the "move" icon comes up.. Then I select/drag it till its over the center point and it turns green..

Note: you must have tools..application options..sketch tab "Autoproject part origin on sketch create" checked for that to work..

ok.. found another way (thats probably the "as designed" way).. Place your hole anywhere on the face then simply move your mouse to be over the round edge and a "concentric" icon comes up and when you pick that it moves the hole to be concentric with the round face.. 

But I "think" thats what you were saying you were doing.. Works fine here if so.. Not sure what you are doing differently..  (maybe select other delay)

[chris58]

I put a sketch on the face and placed the hole on the sketch.  I know that's not how it's supposed to work, but couldn't let that stupid little hole hold me up any longer...

[johnsonshiue]

Hi Chris and Brian,

The concentric hole workflow is exactly like what John described. It should work. When picking a circular edge, the hole should be placed at the center. I cannot reproduce the behavior shown in images Chris attached.

Many thanks!

[Tom_Sturtevant]

Hi Chris,

As described above you should get a concentric cursor when you hover over a circular edge or cylindrical face.  Is your part cylindrical?  It is hard to tell for sure from the image.

Thanks,

T.0.M.

[chris58]

Yes the part is cylindrical.

[chris58]

You were able to put a hole in the center on this part that I attached???  It's still not working here.  I tried selecting the face, then selecting the edge, and selecting the edge, then the face.  either way, I end up with a hole on the face, and one on the edge.

[Tom_Sturtevant]

Hi Chris,

There are some problems currently with attaching Inventor data in the forum.  I see your attached image (jpg) but there is no ipt.  You should be able to zip it and attach the zip.

Thanks,

T.0.M.

[TheCADWhisperer]

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@chris58 wrote:

Yes the part is cylindrical.

---

One tip that I prefer is to never select the circular edge to place the circle, instead I always select the cylindrical face for concentricity.

First pick is the planar face and second pick is the cylindrical face.

This is a more robust technique if there is a chance that you might go back in history and make a edit (for example - a Chamfer) that would cause the original circular edge to be lost.  It is much less likely that you would go back in history and do a edit that would eliminate the cylindrical face.

Zip your *.ipt file here and let's see what is going on.

[chris58]

OK let's try this again...

[TheCADWhisperer · Accepted solution]

Wrong profile (projected spline rather than circle) in Sketch2 used for Extrusion1 - part is not cylindrical.

Sketches not fully defined.

I recommend that you convert your Projected geometry to Construction and then fully constrain your profile geometry (circle).

I (almost) never use Projected geometry to create features - I only use it for construction reference.

I (almost) always fully define each and every sketch entity as I create it.

You should have noticed that you could not snap the center of this circle to the spline.

You will need two additional sketch points for that. (3 points define a circle)

No dimension needed.

 3 Point Circle

[chris58]

Not sure how it went from an extruded circle, to a spline...

Could this have anything to do with the extrusion that split the part?

[TheCADWhisperer]

No. 

The issue is entirely and completely in Sketch2.

In Sketch2 you have a projected spline that sort of looks like a circle, and overtop of that spline you have an “eyeballed” circle. When you did the Extrude you accidentally selected the spline rather than the circle. This accident could not happen if you had changed the spline to construction. 

[johnsonshiue · Accepted solution]

Hi Chris,

This can happen in several ways. I don't think you use Spline command to create the geometry. It is possible you project geometry from an imported body. I have seen quite a few cases that our competitors convert cylinder to spline. The translators in Inventor have the ability to simplify geometry within certain tolerance. But, some cases exceeding the tolerance will remain spline.

Another possibility is you project a circular edge not in the direction perpendicular to the circle. As a result, the projection becomes a spline.

Anyway, at least we sort out the issue here. Inventor team worked particularly hard to ensure legacy workflows not affected by changes in Hole command.

Many thanks!