Handling Multiple States of a Part over it's LifeCycle

[Anonymous]

To preface: I'm a longtime SolidWorks user expanding my horizons. I'm part of a new engineering team and we have been using Inventor now for about 4 months (we've all come from different CAD packages... none of us have prior Inventor experience). I've learned quite a bit and I'm starting to drill into the finer points of Inventor's data management and modeling.  I'm trying to find a good workflow to handling fabricated parts in my assemblies. To clarify, here's my scenario:

Our team works modifications on existing systems. Often, we're fabricating parts that will be ultimately trimmed to fit the installation. These parts must first be fabricated (and we often fabricate to an oversized dimension), QC'd and documented "as fabricated". Then they will get trimmed as necessary on installation, and QC'd and documented again after install.

I'm trying to maintain data integrity by sourcing all of the documentation from the master assemblies created, so I'd like to avoid dealing with multiple parts if possible. In essence, I need to be able to show a part in 2 states: "As fabricated" and "as installed", but I need my BOM to maintain appropriate quantities as well.

Suggestions?

[mflayler]

Sounds like you need to do one of the following to accomplish this...

Assembly level cuts to trim your "as builts".  With Inventor a cut made in the assembly does not follow down to the part level and you simply document the Assembly as necessary.

Or

Convert your assembly to a Weldment.  If you do this, then you add your changes as Preparations before assembly/welding or as Machinings if the part is installed and then modified.

There are other methods but not as clean and it creates more files.  Those methods would involved Derived parts or family tables.  If you are using Vault I would definately avoid the latter if you can.

[mcgyvr]

To give an alternative to marks suggestion..

I personally would handle this with iparts.. (yes you stated you didn't want multiple parts but its a "bit" different as everything is handled in the "factory" ipart but yes the members are individual parts but you don't edit/open them at all)

One member of the factory would be the as fabricated and then another member to add the additional cuts (as installed)..

The "benefit" to iparts is that if you ever reuse the "as installed" you don't have to duplicate the assembly level cuts with each new assembly just place that as installed member again into a new assembly..

Depending on the specifics one method will work better for you..

I could care less about multiple "member" files as hard drive space is cheap and since they are all "managed" through the single ipart factory file you don't need to do anything with the member files..

[Curtis_Waguespack · Accepted solution]

Hi JMcCrory,

Ultimately what you want is this, but it does not exist yet:

http://forums.autodesk.com/t5/inventor-ideas/level-of-detail-for-parts/idi-p/3822718

The suggestions provided by others pretty much cover the options/workarounds, but I'll add that you can create a Derived part from your original source file and then add features to it. This creates a 2nd part file, but the two are linked, so that edits to the first update the second. This would be very similar to the iPart workflow, but there would be no "family table".

Derived parts:

http://help.autodesk.com/view/INVNTOR/2015/ENU/?guid=GUID-0A5D9D9B-8B6E-48A2-A1D9-54C0A57D171B

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

The iParts method is the closest I am used to in workflow (SolidWorks configurations would be how I would handle it there). I already use some iParts for fasteners and such, but it doesn't seem like the support is there for switching "on the fly" (or is it possible to use an iAssembly to do this?). I tried some assembly level cuts, but it felt as if performance suffered by the time I got halfway through the trims (about 20 cut-extrudes) - moving about the assembly became sluggish. It looks as if any method apart from assembly level features will require additional file overhead. The files themselves aren't really my concern... it's depicting the parts correctly in the model/drawing while maintaining the BOM integrity that is my focus...

Our workflow involves modeling the existing structure as it is, and then adding the necessary purchased and fabricated parts to build up to the final modification. The fabricated parts are collected into a single drawing with each part detailed for the fabricators. That drawing gets a BOM that is in essence a "build list". The parts ar QC'd against that drawing, and then moved to the install area amongst the purchased parts.

The overall assembly is then documented on a seperate drawing that has a different BOM (showing purchased parts, etc.). On install, engineering works closely with production to certify and document trims and adjustments required. Even though the parts are ultimately altered at the final product, the original fabricated state must still be documented.

To maintain our data integrity, the BOMs are driven from the single "master" assembly file. This way if things are added/subtracted during the engineering process, we can easily account for it in the BOM.

I'm going to explore the proposed solutions over the next couple of days... thank you guys fro your input. If there are any more suggestions - I'm all ears!

[Curtis_Waguespack]

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@Anonymous wrote:

...I already use some iParts for fasteners and such, but it doesn't seem like the support is there for switching "on the fly" ...

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Hi JMcCrory,

If you mean editing the part in context of the assembly, to add cut features, etc. based on other parts in the assembly, and so on, then you're correct, there is not a way to do this with an iPart. But if you mean simply switching bewteen the configurations from the assembly, then you can exapand the node in the browser and right click the table and choose "Change Component".

The derived part workflow would allow you to edit the part in context of the assembly.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[jalger]

Hi JMcCory,

Sounds like you need a Data Management Program... I know its a dirty word... Data management... 

You might want to look into Vault Pro, I think it will solve your issues.

Document control, Product lifecycles, True Revision Control (i.e. the ability to use different Versions of a file in different assemblies)

In any case, here is a link to Inventors, on again, off again friend the Vault:

http://www.autodesk.com/products/vault-family/features/product-data-management-for-manufacturing/gal...

I hope this helps,

James

[Anonymous]

The link to the "idea" thread about LoD for parts actually yielded the ideal solution for the moment - by duplicating the solid body part and using views, I can associate the views on the fly and not have to worry with BOM issues.

Thanks!