Adaptive part fails in positional representation

[milesB]

Good day,

Please have a look at the attached 2011 assembly file. The cylinder part has been mated to a plane in the asembly, it is adaptive and this works fine until you modify the position of the plane in a positional representation.... Error

I only need to do this for layout purposes, think of a crane hook shown in different positions, It doesn't make much sense if you can't see the wire. Any work arounds / alternatives will do.

Cheers Guys

[IgorMir]

For "any" work around use iAssembly. That's the only thing which worked for me in similar circumstances.

Regards,

Igor.

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@milesB wrote:

 Any work arounds / alternatives will do.

Cheers Guys

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[milesB]

Did you create different length cylinders in iParts and call them in your iAssembly?

The iAssembly doesn't seem to allow parts to be adaptive in more than one instance.

I've also driving the part length parameter from an assembly parameter but it's not happy with this either.

More ideas ?

[IgorMir]

Yes, I did. The use of adaptivity is a big no-no in my workflow.

Igor.

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@milesB wrote:

Did you create different length cylinders in iParts and call them in your iAssembly?

[johnsonshiue]

Hi! If I understand this workflow correctly, you are hitting a limitation in Positional Representation. Basically, PosRep does not allow component geometry (part feature or assembly feature) to be changed from Master. The overrides are limited to component assembly constraints or position or degrees of freedom.

Thanks!

[IgorMir]

That is correct. The limitation of Positional Representation forced me (in one seldom instance when I tried to use Adaptivity) to use iPart instead. The part was a Concertina Cover for the portable lift. To show the lift in two stages (retracted and extended) I had to create two instances of the Concertina Cover using iPart.

Best Regards,

Igor.

[cadman777]

Gentlemen,

Has this software limitation been fixed in later releases?
If so, which release has full functionality?

Thanx ...

[johnsonshiue]

Hi! Unfortunately, the behavior has not been changed yet. Inventor part can only have one unique definition in one context. An adaptive part can change shape due to assembly constraints but its definition has to be unique within the assembly. PosReps have the potential to make the definition not unique, violating the restriction at the moment.

One can argue that why Cable&Harness components can be adaptive and can adjust according to PosRep. It is an exception and C&H components are limited to be referenced within the assembly they are originally created from.

Thanks!

[cadman777]

John,

Thanx for the update.

This is how it is, and never will change, right?

If "yes", then I'll use iAssemblies for this.

[johnsonshiue]

Hi! Nobody can say never. I can only comment on status quo. What I am trying to say is that to enable the ability, the efforts may not be trivial. It is probably why it works like this right now. The other thing to consider is the behavior model. C&H can do that because C&H is a specialized environment and users are not allowed to reuse C&H components in other content. Assuming we do allow this workflow for all adaptive parts, it means the adaptive parts can only reside in an assembly and it cannot be reused in other assemblies. It could be fairly confusing also. I am very sorry that I cannot provide any new information.

Thanks!

[cadman777]

John,

Thanx for your explanation.

I can live w/the present work-around, since I use it only occasionally.

I prefer Inventory's simple work-flow compared to SolidWorks.

There's no need to corrupt a simple work-flow w/complicated programming.

One thing you may want to consider adding to Inventor is another type of iPart or iAssembly that's "smart".

By "smart" I mean the same thing you are talking about:

A part or assembly that can have various positional representations, but it restricted in use to only one model.

Cheers ...

[dslemusp]

@cadman

I have been trying the workaround without any luck. I have a spring which I want to show in 3 diferent positions (Compressed, Free Lenght, Extended) within an assembly. The step of the workaround I have been following are.

- Create an iPart (instead of an adaptive part) with the 3 positions I want to display in the PosRep

- Create an iAssembly switching the 3 positions (Using the ipart)

My question is from here on how to create the PosRep. Could you be a little bit more specific how to use the PosRep with iParts.

I appreciate your help

Thank you

Daniel

[johnsonshiue]

Hi! I am not aware of a way deforming a part in two different representations in Inventor (except cables). Basically, component geometry cannot be changed between representations (Design View, PosRep, or LOD). The deformation can be simulated by driving a constraint leading to adaptive part to adapt. But, it is still within the same representation. The only workflow I am aware is to have a different part or different assembly,

Thanks!

[ravikmb5]

Here is an Example of an i Assembly

[kmeldfreyssinet]

Hi,

This will probably never change.

But maybe you could try this. I did not try so not sure if will work.

Make this wire (cylinder) longer and make extrusion in assembly to remove portion that is not needed.  Maybe this will be updating in positional representations. 

Will try later.

Cris.

[barnadaniel]

Hi,

(Sub)assemblies can be Flexible, which - if I understand correctly - means exactly what people (including myself) want to achieve in this thread (I want to show a vacuum bellows in different positions). Can this not be done for parts?

Thank you

Daniel

[johnsonshiue]

Hi! In a flexible subassembly, adaptive within the subassembly is allowed. But, if you want an adaptive part to be driven by constraints outside of the flexible subassembly, it will not work. It is because flexible and adaptive are mutually exclusive.

For a vacuum bellows, I assume the geometry for each part is fixed and the components have different relative positions, right? If yes, Positional Representation should work for you. But, if the geometry has to change in different positions (expanded vs collapsed), Positional Representation will not work. So, let me confirm with you. Is the part geometry the same in different positions?

Many thanks!

[barnadaniel]

Hello,

"But, if the geometry has to change in different positions (expanded vs collapsed), Positional Representation will not work. So, let me confirm with you. Is the part geometry the same in different positions?"

What I would like is the geometry of the part to change (a bellows is really 'flexible', in the true sense of the word). The analogy with the assemblies (adaptive vs. flexible) is the following:

- adaptive: a subassembly can be adaptive only in one single place. Adaptivity really drives the subassembly, its all other instances will reflect this adaptive change

- flexible: different instances of an assembly can be flexible in different ways in different environments. Flexibility is only driving that specific instance of the subassembly.

Transferring this concept to parts: adaptivity means the part is really changed (in one single location).  The (non-existent) flexibility would mean that different instances of a part are 'stretched' or distorted in a flexible way, by adjusting flexible features of it.  I am not sure though if it can be implemented easily, and if there is really a need for this. But for vacuum application I often face this problem: a given bellows (stock item, with given parameters) needs to be stretched in different ways at different locations.

Thank you

Daniel

[johnsonshiue]

Hi Daniel,

I understand your requirement. Unfortunately, the concept of flexible part is not yet available. We are aware of the requirement and we have done some research. It is something we are very interested in. Please sign up Inventor Beta program if you would like to learn more (https://bit.ly/InventorBeta).

Many thanks!

[peter.addicott]

Hi

Has anything been done about this? I am trying to make an Energy Chain drivable along a Telescopic Boom.  I just tried projecting the geometry and expected it to 'adapt' but obviously I was wrong.

Cheers

Peter