Parameters - Assembly to Part

[NachitoMax]

Hi

i usually create my parts and insert them into an assembly. I see this as the right thing to do however, there are instances where parts are created inside the assembly to fit into and depend on other parts. I have an instance where i have created about 60 parts inside the assembly. Most of these have the same thickness of 18mm. I now have the task of slightly increasing the thickness to 18.3mm.

So

I'd like to be able to create / edit a parameter inside the assembly file that all of the 60 parts can update from. i cannot figure this out though. I have tried to create an assembly parameter and link the part to it but i get a circular reference error. I also tried an excel sheet but it turns out that if i change any values, it alters them in ALL parts that are referenced to it. Unique linking doesnt seem worth while as i may as well stay as i am..........

Is there a decent worthy process of managing parameter value changes from an assembly to all of its parts? Code is options are good too.

I cannot see why this isnt a more user friendly option within Inventor as its very obvious that parts need to depend on other parts in most cases.

Its worth noting that in all of the 60 parts, they share the exact same parameter name of Main_Substrate

Look forward to any advice given

Thanks

Nigel

[pcrawley]

You should have a look at the skeletal modelling techniques that get discussed frequently here - or at least investigate derived parameters.

Meanwhile, you could do this easily with iLogic...

Get the iLogic "Code Injector" tool here: 

http://beinginventive.typepad.com/being-inventive/2012/08/major-upgrade-to-the-ilogic-code-injector-...

Run it, and select all the files you want to update.

In the "rule" area enter something like:

Main_Substrate = 18.3

iLogicVb.UpdateWhenDone = True

And run it.

This should inject the code into every part you selected and update it.

Notice there are options to delete the rule after it has run - that might be a good idea otherwise you might wonder what's going on in 6 months when you edit one part and it reverts to 18.3!

[Curtis_Waguespack]

Hi nmjshaw150,

In addtion to pcrawley's suggestions, there are a couple of iLogic rules at this link that should do the trick for you. You would run one of these from the assembly file:

http://forums.autodesk.com/t5/Inventor-Customization/ilogic-rule-for-each-part-in-the-assembly-to-ch...

 Creating a Basic iLogic Rule

http://inventortrenches.blogspot.com/2012/01/creating-basic-ilogic-rule-with-event.html

I hope this helps.

Best of luck to you in all of your Inventor pursuits,

Curtis

http://inventortrenches.blogspot.com

[PaulMunford]

Yep, iLogic is the only way to achieve this.

Check out this class from AU. There is a demonstration of exactly this toward the end.

There is an example of the code used in the handout:

http://au.autodesk.com/au-online/classes-on-demand/class-catalog/2013/product-design-suite/ma2604

[johnsonshiue]

Hi! Indeed, the Inventor inter-document parameter linking workflow is not as straight forward as it could be. Each ipt or iam file manages its own parameters table. A part exists an assembly does not mean the assembly has total control over the part, because the same part can exist in other assemblies.

Aside from the workflows you have already found (linking to iam or Excel or using iLogic or VBA), there is another commonly used technique called skeletal modeling. You can put all driving parameters in one skeletal part. Place the part in the assembly (make it invisible and referenced so it does not show up on BOM). For each part needing the parameters, just link or derive the parameters from the skeletal part.

Since you already have the parts created with commonly named parameter, I personally think the quickest way is to use iLogic rules to drive the parameter value.

Thanks!