Constraint Errorbug for valid constraint

[n_bonvin]

Hello, 

I keep having a problem in an assembly i'm working on and can't find a solution.

I have 3 variants  of my model  and 2 of  them keep  having a problem.

When I try to constraint "Echelle" in variant 1  and 3 it  keeps  telling  me that there in  as error in the  constraint  but when  I  accept  it anyway  there is no problem. Actually i'm  sure the  constraint  is valid, i  don't know  why  the error shows  up.Ifonly it wasthat there  would  be  no problem    but then when  I  change the parameter "AngleEchelle" in the  excel and update  the whole assembly the part "Echelle"  won't move untill I touch  it with  the  mouse  and move  it a little bit.

I uploaded the  whole file of my model. You have to open  the  file "AssemblageFosse" and the file "Paramètres" if you want to change the parameters. You can  find the parameter "AngleFosse" almost at the end of the  sheet Parametres on the excel file. I  uploaded the file with the variant 1. You have to try to constraint the  two points together  in order that "Echelle"  can move in  the  tube. I understand it is quite complex to jump in a project at this stage and hope I was clear.

Thanks for your help !

[CCarreiras · Accepted solution]

Hi!

I believe the problem isn't the constraints, but the errors in the sketches. 

The problem in the constrains is a consequence of that.

Also, your files are not all migrated for the same version, this cause also issues to the model.
Use Task Manager tool to migrate all the files for the actual version.

I can't find the parameter in excel to change... anyway... i think you dont need 3 stairs in the model, i would use only one and vary only the angle for the same stair, this way i will avoid the "suppress" step.

[WillL84]

I have this error on occasion as well. I'll add a constraint to a part that doesn't have any and it gives me the error. I click OK anyways and it lights up the red +. Then when I drag the part it snaps to where the constraint is supposed to have it and the red + goes away and everything is fine. It's strange.

[CCarreiras]

How do you control which "echelle" is active or suppressed?

Note:

 """I'll add a constraint to a part that doesn't have any and it gives me the error. """

If you have the red cross active due sick constrains, the new constrains you create will have that error message... even if they are well created... it's a odd behaviour, but it happens.

[WillL84]

But the thing is that if I drag the component it'll snap to where it was supposed to be and then the red cross goes away so there's no more error.

[CCarreiras]

Sorry, but i can not replicate what you're  saying.
Can you explain better?

 

 

[n_bonvin]

Actually these sketches have errors only because I didn't  find a way to supress sketches. So  for example when i'm  in 1  and  3 configuration  the sketch corresponding  to the  2  nd  configuration  will  show errors because  th egeometry  doen't exist.

I don't get what you want  me  to  do when  you tell  me  to  use Task  manager. is  there   an  auxiliary  app to  inventor  called task   manager ? Didn't find it.

I actually prefer to use 3 stairs than suppressing all  the  constraints. Because the  stair can  sometimes be  attached  to an other  tube when  i'm  in  the 3 Tube configuration for example.

This  is  the parameter  to  change to move the stair.

 

 This is the parameter to use to  change the  configuration  

 

[n_bonvin]

Guys...

I don't know why. Before in  configuration  1 and 3 when I constrained the  "Echelle" part I could not move it around the tube axes even if I didn't constrain the "Echelle" along the radius line you see in the tube.

Now the only probel that remains but that is not that impportant is why is it still poping up these error messages even if the constraint is valid ? 

[CCarreiras · Accepted solution]

There's several problems to fix.

First, sketches can't be suppressed, so, you must find ways to deal with that to avoid the errors.
Second, the red cross is on (as you can see in my images). i couldn't not get rid of it (i tried  rebuild, drag, etc, but it still on).

third, since the red cross is active (due sick constraints), you will have that odd behaviour when you create new constrains, even if they are well created, as you show in your video.

So...
I fixed both sick constrains (change them from flush to angle, i think is more stable for this case).
Fixing the sick constrains, the new ones will be ok.

 

[CCarreiras]

Also the rotation will work ok:

 

SO.....
You need now to fix the sketches. A sick model (red cross) will always work bad, sooner or later.

____________________

Sorry, is "Task Scheduller" not "Task Manager".
Anyway, it's only one file that needs migration, so you can do it manually: open and save it.

[n_bonvin]

Thanks a lot ! Yoou were right,   fixing all the other issues that I considered as not important helped me to solve the  problem.

Also the  tick  with the angle constraint  in place of the flush constraint worked well.

I didn't find a solution to oveercome the problem  that i cannot suppress a sketch. Do you have any idea ? 

For the moment I stiill have the red cross for these sketches but everything work fine despiite of that.

[CCarreiras]

---

@n_bonvin wrote:

I didn't find a solution to oveercome the problem  that i cannot suppress a sketch. Do you have any idea ? 

For the moment I stiill have the red cross for these sketches but everything work fine despiite of that.

---

You can let models with the red cross activated, sooner or later the problems will grow badly, and you will conclude that you spent tons of work hours for nothing...
Every time the red cross appears, it have to be fix immediately.

Regarding the "suppress sketch" theme... well, you have to follow the operations one by one and fix it.

I would check all the model and find alternatives.
Example, don't use projected geometry from features that could be suppressed, or you will loose those references ahead in the model.

[CCarreiras]

This feature.... is really needed?

OK, I GET IT...

[CCarreiras]

HI!

The part is fixed...

Check the part attached.

[n_bonvin]

I get what you told but in my case I NEVER  use lost projected geometry because if  it is  lost it  means I 'm not in this cinfiguration so I don't use it anyway. If  it doesn't work this way I 'll have to  replace each projected geometry in  the  sketches by a parametre driven  sketch. 

I  hope that such a feature  will be  added to inventor  because it  is  already working well when for example  you build a feature 2 on the  face of feature 1. When you suppress feature 1, it will automatically suppress feature 2.

[n_bonvin]

I get this  when I open your part ...

[CCarreiras · Accepted solution]

Well... i fix the model for one configuration, i was expected that you fixed for the others.

Anyway, it's all fixed now:

 

Tips:

Always project geometry from the main sketches, don't project the solids that can come and go, when they go, you will loose the references... obviously.

Stop creating new sketches with the same info, use existing sketches (even the main ones) to do the operations, they already exist.

The main sketches are signed in the image below.

[n_bonvin]

Oh yeah thanks for that advice, it definetely resolved all my problems. Thanks a lot !