Unusable Flip Normal command (destroys simple Two-Point-Center-Rectangle sketch placed on the 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.

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).

PPS: I've also posted a bit extended version of this issue at API forum - https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/unusable-flip-normal-command-destroy...

[blandb]

Interesting....Curious, what is the reason you are needing to flip normal?

[kacper.suchomski]

Are you sure they're gone?
When inverting the normal, Inventor likes to move the sketches around.
Repeat the process and after inverting the normal, press F6 (or Fit on SpaceMouse). I think you will find your doom.

[blandb]

I believe I have replicated what was stated, and I get the same result....2022 test. Please see attached.

[Maxim-CADman77]

Recently I've created my first Inventor Add-In (Cross-Cutter) that automates creating Cross-Joints between interferencing flat bodies of MBP (Multi-Body Part).

I'd like user has possibility to flip slot cut direction (can be useful if bodies interfere at full depth ... if I'm not mistaken this case is called Cross-Halving-Joint). 
This approach worked ok until I make slot width value associative to thickness of mating body (which means add using of projected geometry to the sketch).

[kacper.suchomski]

It actually disappears, although zoom all shows you more space, as if it's supposed to find that sketch somewhere.

I have no more ideas.

Plane is like a sheet of paper. If you flip it, you get symmetry.
At the moment all I can think is, you have to decide the direction of the plane before you start working on it.

[Maxim-CADman77]

@kacper.suchomski 
"you have to decide the direction of the plane before you start working on it"

My Add-In determines correct direction for most joints, except those particular cases mentioned (with no clear criteria).
But I'd like provide the human with simple to use option to change the direction (who pays - that decides).

[blandb]

Since this is multi-body, can you just have a bi-directional cut, then just have the user choose which solids participate in the cut? Then direction doesn't matter?

[johnsonshiue]

Hi! I am wondering if UCS (parameter-driven) would help here. You can place the UCS anywhere in the model space. Then use 3 positional parameters and 3 rotational parameters to control the UCS. You may rotate the UCS around Z so that the sketch on the XY plane faces a different direction.

Many thanks!

[Maxim-CADman77]

@blandb 
Thank you for idea, but I don't see the way to create pair of Cross-Joint cuts with just one feature.

@johnsonshiue 
Thank you for idea, but I don't see how UCS introducing can help to overcome the issue described.

UPDATE:
I've already overcame influence of the issue to the functionality of my Add-In (now use more complex less-natural logic of rectangle creation) but I'll deliberately keep the thread unsolved in order Autodesk Inventor dev-team can see there is a defect to fix (although I don't believe they will).

[blandb]

I don't know how the add-in program works, but I was thinking using a shared sketch with bi-directional cuts, or using cut to surface and choose the bottom of the wood surfaces as cut distance and direction....just a thought

[pcrawley]

Can you construct your plane using other geometry? 

When you flip the normal, the plane is essentially rebuilt from scratch and the geometry attempts to reattach itself to the newly created Plane, but rarely succeeds 100%.  I'm worked on a project where thousands of workplanes were within a few degrees of 180° to each other, and every time you went past 180° the model would implode because the planes flipped.

The solution I came up with (eventually) was to create the plane from a sketch and parametrically drive the angle:

Rotating around an Axis is preferable, but fixed model edges are OK too.  It creates the correct result every time and I've stopped worrying about planes flipping with unpredictable results.

[cadman777]

I've used FlipNormal many times over the years, and can honestly say it's a crap shoot.

The types of sketches I've done this with are mostly railings and structural.

I found that sometimes FlipNormal mirrors correctly, other times it whacks out the wireframe.

But with a complex wireframe, it's still better than making it from scratch.

However, I never tried what Johnson said about using the UCS in the sketch to try to fix this.

I never tried doing it with iLogic or VBA.

Otherwise, FlipNormal has unpredictable results, from my experience.

The more complex the design, the more unpredictable the mirrored result.

[cadman777]

Nice video!

We call this a 'finger joint'.

[cadman777]

Can you drive the angle to 359.9999° without an error (like the angle dimension flipping)?

Wouldn't you get a reverse mirror if you used an angle, instead of getting a true mirror?

[pcrawley]

You can drive the angle as far as you like - and stop on 180, 360, 361 - it’s bullet proof. 

for the “Flip Normal” effect, you’d just toggle it between 0 and 180.  

[cadman777]

Thanx Peter, I'll have to remember to try that next time I want to do this.

[pcrawley]

Just in case anyone else finds it useful, here's a sample with a slider to control the rotation through 0 - 450° (just to demonstrate going past 360°).  Leave it on 180 or 360 close and reopen Inventor - it always comes back the way it should.  Bullet proof - because it isn't rebuilding the workplane, only moving it.

To emulate "flip normal", I'd just make the angle 0 or 180°.

[Maxim-CADman77]

@cadman777 

Just in case - here is Another Video demonstrating the complete project on a simplest sample 3 body model.

PS:
English is not my native lang ... but "Finger Joint" Wikipedia article shows something unrelated to what I've automated 😄.

[Maxim-CADman77]

@pcrawley 

As I wrote earlier I've already 'invented' the workaround for my needs (use parameter equations based on reference parameters).

As for other cases ... the workaround you've suggested has a bit limited application regarding sketch profile (circle, properly oriented rectangle, and some other).