Error during Extrude Join Distance from Face: "The feature as specified did not change the number of faces"

[JamesSlaven8282]

Is anyone else experiencing this problem with some Join Extrudes?

Extrude > Join Distance from Face produces an alert when the Start plane/face is on or within body being joined, the extrusion intersects and terminates within the body being joined.

No error when the extrusion does not intersect body being joined.

No error when the extrusion starts or terminates outside the body being joined.

No error when the sketch profiles being extruded are larger than the body being joined.

No errors with join between.

Example .ipt attached shows a number of test bodies. Green bodies are okay. Red bodies have error.

The error can be accepted and the extrude will be visible but use of the affected .ipt's will trigger further error dialogs downstream.

Thanks,

James

[Paul.Normand]

Hi James,

I don't think I've ever seen this error except in cases where you did a Join operation where you should have used a cut -  material is joined to the body and the object is unchanged - therefore the number of faces is identical when you finish. I can't tell what your original goal was on the 3 failures, but if you edit each feature and change the join to a cut, then the operation succeeds without errors and the body is modified.

If that wasn't what you were going for, can you elaborate a bit more on what the expected results should look like?

Thanks,

Paul

[chenj]

I also repeated this error. This error occurs when the starting plane of the extruded feature is not the sketch plane. If the sketch plane is the starting plane, there will be no problem. It may be a bug.

[SBix26]

This must be a bug.  The error message says the operation did not change the number of faces, but it obviously did: each of the three bodies changed from a hollow cylinder to a plugged hollow cylinder, exactly as defined.  There would be no problem except that they are now flagged as errors.

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Sam B
Inventor Pro 2022.2 | Windows 10 Home 21H1
LinkedIn

[JamesSlaven8282]

Thanks for your verification.

Re @Paul.Normand

The intent was to extrude a tube and cap the far end. A workflow I use often. It is quick, if I don't accidentally leave the Extrude command, without requiring additional work features (ex Patch>Thicken, New Sketch>Project, etc).

Re @SBix26 

Correct. The operation can be accepted leaving the features flagged which was not a notable issue until I modified a parameter which moved the location of the related sketch resulting in repeated alert dialogs. The feature appeared visually okay after moving the sketch location but when hovering over the feature in the model browser, the highlight would ghost the extrude in its' prior location (where it was created).

Thanks again. I'll check back for additional updates on this.

James

[johnsonshiue]

Hi Folks,

This is indeed a bug. I guess the check for modeling null ops makes a bad assumption. The warning is unnecessary. I will work with the project team to understand the error better.

Many thanks!

[johnsonshiue]

Hi! It has been reported as INVGEN-59588.

Many thanks!

[JamesSlaven8282]

Hello.

I am presently running the latest public release of Inventor 2023 and have again started experiencing the behavior relevant to this topic.
When extruding from a start plane that is not the sketch plane to a plane back toward the sketch and when the entire extrude is contained within the body to be joined, the feature in the browser gets flagged with an error yet is visible in the window.

I can add more detail once I’m back at my PC if anyone asks.

James 

I am posting this from my tablet so do not have the exact build but as of a few hours ago no updates were available.

[johnsonshiue]

Hi Folks,

I just checked the status of INVGEN-59588. The latest comment in the defect indicated that the defect is being fixed. However, the fix can only apply to the new release, not an existing release due to technical limitation.

Many thanks!