Constraints to projected lines change when changing base sketch

[martin_mostboeck]

Hello,

I have a fully constrained base sketch and at a later point in the timeline a new sketch with projected lines of the base-extrusion.

Second sketch is also fully constrained, but to the projected lines.

So whenever I change sizes in the base sketch, some of the constraints attached to the projected lines show strange behavior and attach to kind of the invisible part of the rounded-edge-circle of the projected construction....

However despite the weird new positions, the constraints are not rendered invalid, they maintain active.
I tried around many hours, but could not solve that issue...
thanks for looking into it!

[davebYYPCU]

I have a fully constrained base sketch  ...

Nope.

You don't have to change parameter to break it, just moving the base sketch broke the circles.

I suspect the mirror/s in the base sketch, for your troubles, (not critical of you but,)

not the most robust way to draw two rectangles.

Would start there.

Might help....

[davebYYPCU]

Did some more digging, 

The tangent constraint here breaks - this is a serious bug, not just you but for everybody, the purple curve is an arc, and I thought it may convert to spline but doesn't do that either.

Side note your sketch is very busy, for each offset curve ring, you are placing multiple points on top of each other, this confuses Fusion at the best of times.

@jeff_strater @Phil.E 

@TrippyLighting - anyone else you know can get to this?

Breaks in this file, and my own independent checking.

Might help.....

[phil_eichmiller]

Logged as FUS-125743

This is the same as every dimension flipping case. If you increment the changes less than the value of the offsets it won't flip. Unfortunately, due to the nature of the constraint system, these cases are not fixed by any kind of global change. We have to take each one as a new case, but we have fixed many of these over time thanks to helpful people providing examples.

Thanks for providing a data file, this will help tremendously when fixing the issue.

[Phil.E]

Oops, I was logged into the forum on my teaching credentials. That answer above is from me.

What I mean is if the offset is 2mm, then increment the parameter changes by 1 mm, allowing the model to update, until it reaches the desired state.

[evanp4509U4JZ]

I frequently do the offsetting of concentric circles, mainly for bolt holes ie. head pocket, clearance, thread minor. What is the proper way to do it that fusion is happier with?

[davebYYPCU]

Try using a Centre point, and one or more Hole Commands from sketch.  

I am still digging in your file,

and thanks Phil.

[jeff_strater]

I would never bother with offsetting a circle.  Just create a new circle, and dimension between the two.  Offset can be tricky, because sometimes offset generates a whole new curve instead of updating the existing one.  I have not dug into your design at all, but I did notice this question.

[davebYYPCU · Accepted solution]

More digging, there is a workaround to your sketch flipping.

Avoid coincident / tangent constraints on the projected arc. 

My short construction line is 3.5 long, (radius value of the 7mm dia. fillet) and one end point is constrained to the mid point of the projected arc. (Replaces your tangent constraint)

The 90 deg construction arc is same radius as original box fillet.  Extend the lines to this arc.  After doing this I can't break the model.

Your tangent and other constraints were solving without error because they could flip to the 270 deg construction arc - a continuation of the projected arc.  (Is not required, and is for demo purposes delete it)

Workaround not needed at the origin end of the model as all jumping dimensions are working away from the origin.

Might help....

[evanp4509U4JZ]

Thank you Jeff and davebYYPCU. 

Didn't mean to threadjack. I roam around looking for problems that I've bulldozed through in the past and offsetting circles was one of them.

[martin_mostboeck]

Dear Guys,

Thanks so much for working this out. Thanks to your hints I solved it. The option from @davebYYPCU with the short 3.5mm construction line did break up again after some crazy dimensioning, but maybe I got the instruction wrong.
However what eventually worked was the hint with resketching a dimensioned (12.4mm in my skech) arc according to the radius of the fillet and then constrained the "hole-sketch" (tangential to the circle and coincident to the "legs") to that arc instead of towards the projected arc.

The behavior is not logical to me - I would love to understand the reason in order to prevent future issues in sketches, but I am lucky for now.
Thanks to this great community - I did not expect the kind of quick and indeep-feedback and solution!

[martin_mostboeck]

Dear @davebYYPCU ,

How do I show this constraint - info?

[Phil.E]

Martin,

Thanks for the response and I'm glad it's working for you.

Just to answer your question: In case you missed it, this behavior is not as-design behavior for Fusion. There should have been no problem doing the sketch the way you were doing it. As such, it is written up in a defect report and the sketch team will eventually look at it. As I tried to explain earlier, in order to fix this type of sketch issue we take them on a case by case basis and have consistently done so at every opportunity. Your file was another valuable case. Thanks for providing it! 

In order to see the list you're asking @davebYYPCU about, just use the left mouse button on any object in Fusion to see a list of all the objects behind your mouse pointer.  This is formally called "select other".

[davebYYPCU · Accepted solution]

I found that the constraints that are flipping don't generate an error state, because they are legal in this position.

(If the short construction line distorted, then you did not construct it correctly.  Not criticing)

This flipped condition is completely valid - note that the construction line did not flip. The midpoint is correctly working.

@Phil.E a couple more pics for demo.  Moral of the story, Tangen / coincident to projected arc, operates as a circle.

Therefore, the broken Tangency/ coincident is still correct to a circle.  Sketch team just needs to define a projected arc as an arc.

Workaround, constrain to a fully defined arc in the same place.

Might help.....