Hole Feature does not update after adding points

[0x3FA5]

The Hole feature is derived from the hole sketch, that includes sketch points.

After adding some more holes to the sketch, you naturally expect that the derived feature will update accordingly, but this is not happening.

I guess it is hidden in some settings? Something like "Force update"?

[JDMather]

Sketch entities do not update Hole Features.

You will have to either Edit the Hole Feature and click on the additional sketch points

or

use Feature Pattern (when appropriate).

[0x3FA5]

This is strange to me..

Sounds like "Sketch dimensions do not update Extrude Features". 🙂

I want to believe there is a hidden setting, otherwise the control flow in Inventor features is lacking logic.

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@JDMather wrote:

Sketch entities do not update Hole Features.

You will have to either Edit the Hole Feature and click on the additional sketch points

or

use Feature Pattern (when appropriate).

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[JDMather]

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@0x3FA5 wrote:

Sounds like "Sketch dimensions do not update Extrude Features". 🙂

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This is an incorrect statement.

Sketch dimensions can most certainly be used to update Extrude Features.

[0x3FA5]

Exactly! 🙂

[mcgyvr]

Sketch points added after hole feature creation do not automatically get selected/consumed by the hole feature.

There is no setting to enable that functionality. 

After adding new sketch points you need to edit the feature to manually reselect the newly added points.

[swalton]

When I add closed loops to sketches, Inventor does not update the dependent extrude features with those extra loops.

Hole sketches behave the same way.

[johnsonshiue]

Hi! We have heard the similar request about the ability to add new holes by adding sketch points (mostly ex-SWX users). We did not pursue that route because existing Inventor users do not appreciate the behavior. They are worried the addition can lead unexpected result. Certainly, this can be argued either way.

There is still a workflow allowing "auto-population" to happen. Instead of creating multiple holes using sketch points, you can create just one hole. Then use Sketch-Driven Pattern to populate the hole to the remaining points. When you add more points, the pattern will update. This applies to all patternable features including Hole feature.

Many thanks!

[nathan_wostrel]

A good point to add relating to sketch-driven patterns is that you can also use a guide surface to control the orientation of the patterned features. This can greatly improve efficiency for later patterns that may require a rotation around an axis or going around a corner. Also, 3D sketches will work to pattern features around multiple faces that are not coplanar. It is a very powerful, underused feature. Thank you!

[CStilesCARE]

Aye, just to add my 2-cents on the matter, I NEVER have the hole feature create more than a single hole (I actually find it annoying that it auto-selects them all by default), because it doesn't seem to always recognize these as patterns when I want to reference for using something like bolted connections or associative patterns at assembly level.

I will always either:

• sketch the center for first hole, create the hole feature, then pattern using 2-axis and/or polar methods, or
• sketch the pattern of hole centers, create the hole feature from one point that makes most sense, then use sketch pattern to create the rest.

This always gives me patterns which I can use as reference when wanting to auto-pattern things like hardware or bolted connections and is so useful.

Only gripe is this associativity is lost on parts derived from the base one. Would be nice if that carried over...

[nathan_wostrel]

As a follow up to the associativity of features not carrying through, look at this topic https://forums.autodesk.com/t5/inventor-forum/sketch-copy-to-flat-pattern-in-a-derived-part/m-p/1057... and it might give you a little insight into how to maintain the sketch information through derived parts.