What does setting a part as "adaptive" really mean?

[Anonymous]

I haven't been able to get a good grasp of what this does. Can anyone give me a summary of what setting a part as 'adaptive' does?

[MSD_takaseh]

Hello RobertWK,
Please see the help here.
Also some videos are available in YouTube.
Adaptive Autodesk Inventor 2015
Inventor Tips & Tricks - Adaptive Spring
8 Create adaptive parts
And more.

[johnsonshiue]

Hi! Indeed, Adaptivity is a workflow most Inventor users have hard time understanding. To understand Adaptivity, let's go back to the basics. At the moment, Inventor part can only have one geometric definition no matter where it is used. Any part, including Adaptive part has to obey the rule. You cannot have one part measuring 4" long in one assembly, while the same part measures 6" long in another assembly.

Adaptive part means the geometry can be influenced by another part or assembly constraint within the assembly. Let's say there are two parts in an assembly, Part1 and Part2. Part1 is adaptive and it is driven by Part2. Such adaptive relationship only exists in the particular assembly. Now, if I insert Part1 to another assembly and Part3 drives adaptive Part1, then Part1 has two geometric definitions in two different assemblies. This violates the rule I mentioned earlier. As a result, there has to be a switch stored in Part1 to show it is already adaptively used in an assembly. This is the reason why we have such option in Document Settings.

Many thanks!

[Anonymous]

I take it then that the adaptive changes or influences for that adaptive part are saved somewhere in the assembly document, and not the part document?

[johnsonshiue]

Hi Robert,

Not exactly like that. The adaptive change does alter the part document. But, the change comes from another component within the assembly the part resides in. Please note that a given part can reside in infinite number of assemblies. The adaptive part itself isn't aware where it is in and where the adaptive change comes from. But, the change is there and the part is aware that it is an adaptive part somewhere. Does it make sense?

Many thanks!

[Anonymous]

It makes a lot of sense, but let me provide this example and maybe it will become crystal clear.

If adaptive part1 is in assembly2 and assembly3, and in assembly2 it is influenced by dimension d0 and in assembly3 is it influenced by dimension d1, you're saying that the details for how the part is adaptive in assembly2 and assembly3 is stored somewhere inside part1?

[johnsonshiue · Accepted solution]

Hi Robert,

Unfortunately, adaptive Part1 can only be adaptive within one assembly. It cannot be adaptive in multiple assemblies. For example, Part1 is adaptive in Assembly1. It will not be adaptive in Assembly2 or 3. There is a document setting in Part1.ipt preventing it from happening. You can certainly make Part1 adaptive in Assembly1. Then turn adaptivity off after it adapts. Next, turn it on within Assembly2 and let it adapt. within Assembly2. But, the behavior will be very confusing. You cannot have one part representing two sets of geometry at the same time.

Many thanks!

[jtylerbc]

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@Anonymous wrote:

It makes a lot of sense, but let me provide this example and maybe it will become crystal clear.

If adaptive part1 is in assembly2 and assembly3, and in assembly2 it is influenced by dimension d0 and in assembly3 is it influenced by dimension d1, you're saying that the details for how the part is adaptive in assembly2 and assembly3 is stored somewhere inside part1? 

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To add to @johnsonshiue's explanation:  If you actually need the part to adapt to both assembly2 and assembly3, you would need two separate part files (part1a, part1b, etc.).  One would be adaptive in assembly2, and one in assembly 3.

If you then needed those parts to count as a total quantity of 2 in the parts list of an "assembly4" that contains assembly2 and assembly3, you can set their file names to be unique (part1a, part1b), but make their part numbers the same (part1).  This will cause the parts list to show them as being multiple instances of the same item, even though they are actually modeled as separate files to allow the adaptivity.

Aside from that limitation, you are correct in saying that the definition of the adaptivity is stored in the part.  Some common ways it appears are:

• Sketch geometry projected from another part in the assembly.  This is probably the most common type of adaptivity.  Unfortunately, that's mostly because it's very easy to create it accidentally.
• Solid or Surface body copied from one part to another using the "Copy Object" tool.
• Work features (most often planes) defined from geometry of another part in the assembly.

However, you also specifically mentioned parameter names (d0, etc.).  Adaptivity rarely, if ever, directly involves a parameter.  It is more about transferring geometry from one part to another, not numerical values.  Linking parameters from one part to another is a thing that exists in Inventor.  It is a very useful tool, but isn't technically considered adaptivity, even though it can have similar end results. 

If you have a problem that could potentially be solved using either method, you're generally better off choosing linked parameters, as they tend to be more reliable and stable than adaptivity.  They are also often much easier to understand (especially for newer users). 

Parameter linking does not, however, get you around the need for two part files if you need different geometry in two assemblies.  The same Inventor part file can't be two different shapes or sizes, regardless of whether or not it is adaptive. 

[Anonymous]

Thank you for the follow up, John.