'Two-Point-Center' Rectangle sketch changes in unpredictable manner on Flip Normal of Sketch WorkPlane

[Maxim-CADman77]

Recently I've discovered that flipping WorkPlane normal of the sketch containing Two-Point-Center-Rectangle changes it in unpredictable manner.

Steps to reproduce:
1. Create new IPT
2. Create three new user WorkPlanes (each at some offset from each of Origin WorkPlanes)
3. Make new user WorkAxis as Intersection of the two user WorkPlanes (turn off visibility for those two WorkPlanes)
4. Create new Sketch on the only visible user Workplane
5. Make sure Origin Point projection was created (if no create it manually)
6. Create new (2nd) sketch Point as projection of the user WorkAxis
7. Create Two-Point-Center-Sketch using the Origin-Projection-Sketch-Point as Center-Point and 2nd sketch Point as Angle-Point
8. Make sure the sketch is fully constrained and close it
9. Pick Sketch WorkPlane (that same which is the only visible one) and Flip its normal.
Witness disappearing all/some of the sketch Lines that form the rectangle.

To get more understanding of what happens with sketch I wrote some iLogic code, which I run before and after WorkPlane flipping: 

Dim oPD As PartDocument = ThisDoc.Document
Dim oCD As ComponentDefinition = oPD.ComponentDefinition
Dim oSk As PlanarSketch = oCD.Sketches(1)
logger.info("ConstraintStatus = " & [Enum].GetName(GetType(ConstraintStatusEnum), oSk.ConstraintStatus))
logger.info("SketchLines QTY = " & oSk.SketchLines.count)

Dim dLengthTot As Double
For Each oSL in oSk.SketchLines
	dLengthTot += oSL.Length
Next
logger.info("Total Lines Length = " & dLengthTot)

It shows that all lines are kept but their lengths changes (some cases lines even got zero length).

What I'm missing?

Can I bulletproof my sketch to have it unchanged after Flip Normal command execution?

PS: I can reproduce this issue in Inventor 2023.2 (and all earlier versions I've tested so far).

[Maxim-CADman77]

More then 150 views and no replies within almost ten months ...

I'm attaching the Inv21* sample where all sketch-lines got zero lengths on Sketch WorkPlane Normal Flip (the rule from the 1st post is embedded).
...and sketch gets fixed on second Flip Normal.

Hope @johnsonshiue is now have enough data to comment..

PS:
The issue can also be reproducible in most recent Inventor 2024.2.

PPS:
It is probably worth to move this thread to general Inventor discussion board.
UPDATE: Thanks!

[Maxim-CADman77]

Unlike 'Two-Point-Center' the 'Two-Point' Rectangle drawn by same two points seems unchanged (as expected) after Sketch WorkPlane Flip Normal.
Which means the issue is a defect of 'Two-Point-Center' Rectangle command.

[robbeRtek]

"Hello @Maxim-CADman77 , based on my experience: When a plane flips seemingly randomly, it is constructed based on one or more axes or lines. If the vector from the axis or line changes to the opposite direction, both the front and back sides of the plane flip. This effect propagates to any attached or associated planes, necessitating a model rebuild to ensure that these planes maintain consistency and do not act independently when vectors change direction. If you need to flip the normal of a plane using code, you should also adjust the PlanarSketch.NaturalAxisDirection:

' Change the plane
If ... Then
Dim plane As Workplane = ...
plane.FlipNormal()
Dim sk As PlanarSketch = ...
sk.NaturalAxisDirection = Not NaturalAxisDirection
End If
' I anticipate that errors may occur between these two actions, so consider suppressing warnings or deferring updates.

Thanks to accept solution

[Maxim-CADman77]

Thank you but Flipping WorkPlane Normal programmatically is not applicable in my case.

[robbeRtek]

place 2 planes from your ref(s), so you have 2 planes on same location but not attached on each other;
Make you sketch on one plane, attached other parts and stuf to the other plane, Hide the sketch plane for the user;
so if they selected the visibe plane and execute the flip command, the sketch is unchanged, because it attached to an other plane.
Thanks to accept work arround.

[Maxim-CADman77]

The workaround you proposed sounds a bit too complex.
Anyway thank you for your time but I'd rather prefer to get some official comments from Autodesk staff (hopefully accept the defect and get it fixed in one of the next updates).
IMHO, if Two-Point Rectangle survives the Flip Normal then there should be no reason for Two-Point-Center to break.

[robbeRtek]

I 've test with you're part,

I cann't rebuild the issue, not in an new part, not in yours
if I remove the projection from the axis, and add (+constain) this again, there is no issue any more,...

If you can rebuild the issues over and over, you can try it on an other inventor build.

mine build : 

I hope this is the solution.

Regards

[robbeRtek]

No issues

[Maxim-CADman77]

2023.2.1 seems half year obsolete, right? (I always update Inventors* ASAP and thus have 2023.4.1)

So after I've deleted the rectangle ang axis projection and recreate them the situation changed a bit but it is still far from expected (see the attached IPT):

*

I do have several releases installed because I need them to test Inventor-AddIns I'm developing.

[robbeRtek]

in 2024 there is no problem, tommorw i try your build.

We work not with the most recent versions, because they can have som issues, if you wait longer, they are mostly solved.
We draw still in 2019, for us, is this the best version. (the align detail vieuws, takes model center and not vieuw center (like all recent versions), the copy design tool, works for most tasks; in new version, the copy design tool breaks or not update  (all) projected sketch refs) through complex adaptive designs,...
In near feature we go to 2023, now we are testing our own copy design tool  that update all refs no matter what kind of ref.
regards

[Maxim-CADman77]

I've just reproduced the issue within Inventor 2024.2 by creating new IPT "from the scratch" (following the sequence I've posted in first post). See the IPT attached.

@robbeRtek 
Could you, please, post any of IPTs you've created trying to reproduce the issue?

PS:
Does Inventor development team know about the Copy Design issue you've suffer? What is a defect-code of the issue?
I see there were just some minor Copy-Design-related issue (INVGEN-61548) fixed in Update 2023.1.

[johnsonshiue]

Hi Folks,

I guess this has something to do with the project edge source with respect to the default sketch orientation. I don't have a good solution here. I am wondering if setting a UCS would be a better choice here. You may rotate the UCS (as oppose to flip the normal). The sketch coordinate on UCS plane should be always aligned to the UCS axes.

Many thanks!

[Maxim-CADman77]

@johnsonshiue any chances development team to look at this?

[johnsonshiue]

Hi Maxim,

I believe this issue was investigated in the past and there was no good solution found. Please feel free to escalate it with Autodesk Product Support. They can help report it as a defect and follow up with the project team.

Many thanks!