Sketch flips changes orientation.

[D0UGLAS]

Dear Forum

I have a recurring problem in sketches within a part file which have a knock on effect to features and assembly relations.

I cannot prevent the geometry changing direction.

Over the last 18 months I have tried all I can think of to solve this issue.

When the problem occurs in inventor, geometry and relations fail I am wise to it and can fix it it.

When it occurs in configurator 360 and the relations fail the model crashes and reports an error. 

See it action in inventor;

[Xun.Zhang]

Hi @D0UGLAS,

It seems a problem to me. It would be great if you can share a simple data with simple iLogic code to us to have a better investigation. Please send it to me via xun.zhang@autodesk.com if possible.

Thanks!

[Xun.Zhang]

Hi @D0UGLAS,

I replied you via email, you have to adjust the iLogic code to remove GOS parameter and edit the sketch to add symmetric constraint and delete the GOS parameter and re-pulish the model to C360.

Hope it helps! 

[D0UGLAS]

Thanks Xun,

It's quite easy to fix when modelling inventor, the difficulties occur when sketches flip, features are not formed correctly and or the relations fail in configurator 360.

[kelly.young]

@D0UGLAS does the square always remain centered?

If so instead of dimensioning to the edge on one side can you use a coincident constraint to the center line of the square to the hidden line?

Or make the dimensions functions of the width from both sides of the line so it doesn't jump?

Just trying to think of alternatives that might help.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Xun.Zhang]

Hi @kelly.young,

Thank you for the comments. I had an email conversation with @D0UGLAS and it's not a problem within Inventor since it's easier to be fixed. He is more care about how to deal with the problem within C360. Involved @xingyichuan who is the C360 expert here to help provide a solution.

[D0UGLAS]

.Hi Kelly

Thanks for the answer,

The solution you offer, under the right circumstances can still flip G_L/2 moves left and the f/x moves right, besides Some configurations demand the cut-out to be off set, and if I dimension the hidden line from the sketch origin it and the others can still swap direction and be thrown off of the model.

The real difficulty is; although fully defined the same geometry can be satisfied as a mirror image or a different orientation, this goes for all kinds of restraints,

I think I've tried them all! and I have learned a few tricks on the way.

Top ranked is to use ilogic to set the dimensions of inactive features to very small values.

Once the cut-out has flipped, the feature is wrong and pre-defined mates in the assembly document fail.

This is easy to fix in inventor but leads to model failure in configurator 360

A general note to any one who reads this thread

** PLEASE NOTE THIS OCCURS ONLY ON THE RUNNING OF ILOGIC RULES or PARAMETER CHANGES **

[Anonymous]

I'm building smart iParts. I think I met similar situations. The only safe way I found to get a stable direction is using workplanes. If for instance you want to work on a chosen side of the Z-axis then it is best to create a parallel workplane to XY.  Workplanes obey to parameters being positive or negative, by changing their side compared to the origin. If "+" would be left then"-" will be right. You can then attach the geometry to the steering workplane. It will move left or right also. This is different compared to dimensions. Dimensions will show negative when you drag them to the opposite side of a reference but afterwards they only obey to positive numbers and will stay on the side they are on.

[D0UGLAS]

Thanks Alex

This looks like it would work but my model would be a mass of planes!

[kelly.young]

@D0UGLAS researched a bit more and understand your issue a little better.

Setting up planes was going to be my next suggestion like @Anonymous mentions. 

Don't know if it happens rare enough that when you find the error you can go back and setup a plane?

Obviously not ideal, would hate to see a mass of planes like you state, but if it is just in a few instances it might be beneficial until a better solution is found. 

I'll continue to search on my end for something that may help.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[D0UGLAS]

Hello

I have found a solution some of the ilogic was before setting dimensions to the desired value,

resetting dimensions to zero!

Thus I have to set a minimum value

Code like this

Parameter("ENVELOPPE CONFIGURATOR", "E_H_L") = NEUF_L

Parameter("ENVELOPPE CONFIGURATOR", "E_H_Ht") = NEUF_Ht

Has to be like this

Parameter("ENVELOPPE CONFIGURATOR", "E_H_L") = max(100, NEUF_L)

Parameter("ENVELOPPE CONFIGURATOR", "E_H_Ht") = max(100, NEUF_Ht)

Regards

Douglas

[Xun.Zhang]

Hi Mr.Douglas,

This is awesome!!

[D0UGLAS · Accepted solution]

Hi Xun

This was not the entire solution,

I have found a solution some of the ilogic was before setting dimensions to the desired value
resetting dimensions to zero!

Thus I have to set a minimum value

Code like this

Parameter("ENVELOPPE CONFIGURATOR", "E_H_L") = NEUF_L
Parameter("ENVELOPPE CONFIGURATOR", "E_H_Ht") = NEUF_Ht

and in some case like this

Parameter("ENVELOPPE CONFIGURATOR", "E_H_L") = Max(100, NEUF_L)
Parameter("ENVELOPPE CONFIGURATOR", "E_H_Ht") = Max(100, NEUF_Ht)

Has to be like this

Parameter("ENVELOPPE CONFIGURATOR", "E_H_L") = MaxOfMany(100, NEUF_L)
Parameter("ENVELOPPE CONFIGURATOR", "E_H_Ht") = MaxOfMany(100, NEUF_Ht)

Maybe someone can explain why I have to have a MaxOfMany for 2 values perhaps it is down to one of the values being a parameter?

The SCREENCAST is worth watching!

Regards

Douglas

[DonStauffer99]

I've had this problem, and as far as I can tell the parameter values are never being set to zero. They are not being set via iLogic either. They are a result of part derivation and manual parameter changes.

I disagree about it not being an Inventor problem. When a 2D sketch says "fully constrained" it should not be possible for any of the geometry to have more than one possible location. It should be possible to constrain in such a way to prevent that, without being told it would "overconstrain the sketch."

So far the best I've been able to come up with is to dimension the distance in one direction from some "fixed" point to a point on the flipping geometry, then from the other direction, limit that point's distance from some other "fixed" point. I accomplish this distance limitation by attaching two construction lines, joined with a coincident constraint, both dimensioned to half the maximum distance. The end of one construction line attaches to the "fixed" point, and the end of the other one attaches to the "flipping" geometry. This avoids the "overconstrained" message.

The problem is that sometimes, rather than simply forcing the geometry into the valid configuration, Inventor messes up the drawing, not conforming it to constraints and dimensions, and says it can't "solve" it. By removing constraints, moving things back into position manually, then putting the constraints back, I can get it back to where it needs to be. Same constraints Inventor says it couldn't solve! So there's another bug, and this workaround fails in some cases.

There has to be a solution. This is making Inventor unusable.

[DonStauffer99]

Is there a trick to making MaxOfMany work? I found that max must be all lowercase and the list must be semicolon-delimited. No capitalization and delimiter scheme I've tried will make MaxOfMany work in a dimension. I've been just doing max(a;max(b;max(c;...

[D0UGLAS]

Hi Don,

As it works fine for me, I don't think there is a trick? There could be an issue with units?

Using ilogic to calculate parameter L for user parameters A, B, C with a minimum of 20mm

ilogic code in an assembly or part.

L = MaxOfMany(A+B, A+C, 20 mm)

or for a sub assembly or part 

 Parameter("PART", "L") = MaxOfMany(A+B, A+C, 20 mm)

example A = 5, B = 26, C = 19

L = 31 

(MinOfMany would return L = 20)

example A = 5, B = 6, C = 9

L = 20

(MinOfMany would return L = 11)

I use these formats all the time with some very complex calculations.

Hope this helps.

[Anonymous]

The Sketcher in Inventor is not the best in the CAD-world. But if you are into Inventor it is what you have to work with. As far as mathematics are concerned you can create a rectangle with one fixed point, lengths for the long and the short side and horizontal and vertical constraints, to make it fully constrained. If you add 90° angles between basic work planes and the sides of the rectangle then the rectangle stays fully constrained and IV looks happy. This changes when you change the 90° to 91°. Now your constraints run into an error. The above case is pretty obvious but there are times where it is not that clear where the conflict is located.

One culprit is the Sketcher, when in a state that it can decide on the relations. I always sketch with CTRL-key "on", which - for some logic that escapes me - is creating un-controlled sketches. I add all constraints by hand because I want to be in control. Horizontal may be the best option in one location where perpendicular is the better choice somewhere else. I decide. When you leave it to Inventor then you can get a constraint between line 2 and line 11, that have nothing to do with eachother but happen to be at a 90° angle at the time you were sketching.

The main other cause for bad behaviour is sketches that are too complex. When is a sketch too complex ?  When just by looking at the constraints (F8) and the dimensions you can't predict how the sketch will look when you change values. If you can't see what's coming then Inventor also has problems. Remember : computers are faster, not smarter. (even at present : I'm a better driver and a better translator...)

Alex