topic Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly in Inventor Forum

Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

Odalv_Arkonski — Wed, 11 Jun 2025 09:48:43 GMT

Hello,

I am trying to make a sketch-driven pattern of a hole in a part. The hole has a counterbore. A preview is shown when the sketch-driven feature is active. But when I click OK to execute this feature, the counterbore is missing.

Preview of the holes with counterborePattern of holes without the counterbore

Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

CCarreiras — Wed, 11 Jun 2025 10:33:50 GMT

Hi!

What version are you using?
Can you post your file here?

In version 2026 is working well:

Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

Odalv_Arkonski — Wed, 11 Jun 2025 10:53:21 GMT

Thanks for a quick reply. I am actually using version 2026. For some reason it's not working for me.

The sketch is derived from the master part (skeleton), but this wasn't causing any problems in previous versions.

I have attached this part.

Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

kacper.suchomski — Wed, 11 Jun 2025 11:05:39 GMT

You have not selected a base point.

(view in My Videos)

Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

Odalv_Arkonski — Wed, 11 Jun 2025 11:08:30 GMT

Thanks! Yes, not selecting the base point was causing this issue.

It's ok now.

Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

kacper.suchomski — Wed, 11 Jun 2025 11:16:08 GMT

Additional tip for the future:

You should not use a sketch construction point as a base point. You should use a sketch point, a model construction point, a geometric center (similar to Join), or even a geometric vertex or line center as a base point. In your case, this is not possible because of the sketch block (it can be edited, but it is not needed in this case). This is the practice as instructed in the orange infographic, although there is no direct mention of this on the help page.

https://help.autodesk.com/view/INVNTOR/2026/ENU/?guid=GUID-9B3D1B72-340A-4F3E-9AD1-80E6DDD91ED2

Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

Odalv_Arkonski — Wed, 11 Jun 2025 11:23:06 GMT

Thank you for the tip! Very useful info for my future work.

Re: Inventor 2026: Sketch-driven pattern of a hole in a part is not working properly

kacper.suchomski — Wed, 11 Jun 2025 11:43:07 GMT

You're welcome.

If you open your previous version, you'll see that you had 53 occurrences (52 is correct).

When you don't specify the base point directly; Inventor defines the base at the geometric center of the copied feature, and at the same time reads the sketch construction point as the next occurrence, even if the location is the same as the base.

In your case, the center of gravity was deep in the hole, so in the next occurrences Inventor moved them up so that the default base would be the same as the sketch points. If the hole was not through, but only had a depth equal to the material thickness - the remaining occurrences would not have the full depth. Experiment with the model and count the occurrences.

That's why it's important to both define all the inputs in the dialog and avoid sketching the sketch construction point at the base location. Otherwise, you can have a lot of problems, e.g. with automatic assembly and counting of bolted connections.

(view in My Videos)