iLogic automation problem

[d.salas.lazzari]

Hello, I am having a problem with a model that I am analyzing. I have a bottom of a pressure vessel and some I profiles welded to it (FIG 1). I was trying to automatize some process, when the bottom diameter is equal or less thatn 1500mm the I profiles are suppressed (FIG 2 ignore the screws that are not yet automatized), but when it is over 1500 the I profiles vary in number and disposition. The problem is here, when i try to get back from a Diameter equal or less that 1500 to a higher diameter, the profiles are not updating, it seems that some error occurs when iLogic suppress and then unsuppress the profiles. (FIG 3).

Hope someone can help me with this, have a nice day to all!

FIG 1

FIG 2

FIG 3

iLogic rule

Anello inferiore.ipt.d0 = HE-DECI-2000-8-50-446.ipt.Di <----internal ring diameter change


If HE-DECI-2000-8-50-446.ipt.Do <= 1500 mm Then
Component.IsActive("BM-IPE120_1:1") = False  <---- suppression of I beams
Component.IsActive("BM-IPE120_2:1") = False
Component.IsActive("BM-IPE120_2:2") = False

' ***Divisione1***
Feature.IsActive("Anello inferiore.ipt", "Divisione1") = False <--- suppression of cuts in the internal ring

' ***Divisione2***
Feature.IsActive("Anello inferiore.ipt", "Divisione2") = False

' ***Divisione3***
Feature.IsActive("Anello inferiore.ipt", "Divisione3") = False
Else
Component.IsActive("BM-IPE120_1:1") = True
Component.IsActive("BM-IPE120_2:1") = True
Component.IsActive("BM-IPE120_2:2") = True

' ***Divisione1***
Feature.IsActive("Anello inferiore.ipt", "Divisione1") = True

' ***Divisione2***
Feature.IsActive("Anello inferiore.ipt", "Divisione2") = True

' ***Divisione3***
Feature.IsActive("Anello inferiore.ipt", "Divisione3") = True	


End If

[A.Acheson]

You may need to record how its manually done and replicate. The sequencing of steps may be off. Is it the constraints erroring out? My preference would be not to use suppression but rather change pattern qtys and part lengths etc. 

[d.salas.lazzari]

Hi @A.Acheson thanks for taking time to answer, the I beams are adaptive items, they are "modelled" using a curved surface that is associated with the bottom. The thing is, that somehow the adaptivity doesn't work anymore when the beams are reintegrated after the suppression

[A.Acheson]

Yes adaptive is a tricky workflow. Does the process work when you manually carry out the changes? Perhaps there is an update required or something missing in the code that isn't capturing the changes done manually. I have found that entering a part to edit or rebuild all is enough to update constraints etc. Unfortunately without a sample model it is very hard to assist with just code alone. Have you tried switching adaptivity off/on, suppress/unsuppress? Try in a sample assembly. 

[王承之pmhker]

If HE-DECI-2000-8-50-446.ipt.Do <= 1500 mm Then

The unit mm seems unnecessary, you can try to delete it

[d.salas.lazzari]

Hello @A.Acheson and happy new year!

So, the problem is still present even if I do it manually. It seems that the adaptivity is lost after the suppression of a part. The weird thing is that the "adaptive" icon is present, but it somehow doesn't calculate it.

I am attaching a clean copy of the model so you can see it:

1) I have created a module that should open automatically when you open the model, it is called Do_INPUT (in case it doesn't open for some reason). This way you can change the diameter in an easy way;

2) when you open it it should work with any change of diameter from 1501 mm and above;

3) when you hit the 1500mm the IPE profiles will disappear, then if you go back to a greater diameter dimension the IPE will reappear but no longer will update;

4) to reestablish the adaptivity, it is necessary to redefine the reference geometry of the surface that cuts the IPE profiles (in FIG 1 is the 3rd word "ridefinisci");

FIG 1

5) then you choose surface in the pop up window (FIG 2)

FIG 2

6) then you choose the bottom's internal surface (FIG 3)

FIG 3

and press ok, it has to be done for BM-IPE120_1:1 and BM-IPE120_2:1 parts.

At this point it is possible to change again the diameter, keeping it over 1500mm

This process made me think that the adaptivity is lost somehow when the part is suppressed. But why? The icon AND the connection to the bottom are still present after the un-suppressing of the parts.

Hope this can help you, thanks for your time!

[d.salas.lazzari]

Thank you for answering, the unit is no longer present in the code, but the problem still persist.

[A.Acheson]

I think you will need to change the approach on this. From this post and what you have already discovered suppressing the occurrence will remove adaptivity. So either turn visibility off or Drive the length from the main Part using a Derived solid or surface. See attached assembly showing derived method. 

[王承之pmhker]

can you share the files for test？

[Z0methink]

Anello inferiore.ipt.d0 = HE-DECI-2000-8-50-446.ipt.Di <----internal ring diameter change


If HE-DECI-2000-8-50-446.ipt.Do <= 1500 mm Then

[d.salas.lazzari]

Hello, files can be found in an upper post

[d.salas.lazzari]

Hello @Z0methink thanks for the post, I will correct that, but you can check the test file that is cleaned from non useful ipt and codes and the problem still persist

[d.salas.lazzari]

Hello @A.Acheson, thank you very much for the answer. It is unfortunate that Inventor doesn't compute after the unsuppression, even if the icons showing that adaptivity is active are there. I am studying to parametrize the profiles so they assum the shape inside the ipt file, for this kind of shape is ok, since it is regulare, if it wasn't, your solution is clearly the way to go as it is the most generic one.

I really hope Autodesk solve this in the future, it surely is a nice feature to have.

[Z0methink]

The problem is not in the code, but in the adaptive elements. You must get rid of them.

[Z0methink]

Copy Object and Solid Geometry

If the original geometry changes size or position, the copied geometry does not update.

You can copy a solid to the part environment by using the Derive command.