Inventor Folder Hierarchy and Project Structure???

[Superslinky]

Hey all, I am currently trying to setup and maintain some type of standards while using Inventor 2010 Routed Systems. Basically I'm trying to understand the folder hierarchy and how to use them with individual projects. For example, if I have job 0001 and the folder structure within that job are the typical inventor folder hierarchy do I have to setup a project template for each job? I think more specifically I need the laymans terms and instructions for understanding the folder stucture and how they are used and how I would use them for individual projects. I've been to the Autodesk site and although there are comprehensive documentation about it I don't see anything pertaining to multiple projects and directory stucture. I should also mention that we are like any typical engineering/design company and need to have our project seperated by clients, jobs, etc.

Any direction on how specific job setup would be appriciated. Please let me know if I can clarify further. I know that the description I gave is not the most detailed but once I have better understanding I'm sure I can explain further but as of right now I don't even know how to ask.

I'm hoping someone will get what I'm suggesting and be able to direct me.

Thanks everyone.

 

[Gymmeh]

Superslinky,


Well there are two different methods of setting up Inventor.
If you have vault or if you just have a "explorer" file structure.

How you set up your file structure also depends on how many files you have and how your machines are set up.

At my work we have legacy work in explorer file structure and all new work in vault. Our machines are larger with many many sub assy's -we just got a new $40,000 computer to open master assemblies which I have been using a lot - so we almost needed vault to manage the work.

our old files were set up to match our pre-inventor file structure with the inventor "project file" governing the file and all small sub assy's.

for example. All conveyors would be under one project file. with conveyor motors/gears/idlers as sub assemblies.
Our best practice is to have a naming method with will keep all files under the project with a unique name.

We had an outside consultant come to train half the engineers and then we all taught the rest of the guys.

A lot of how you set up things depends on a number of variables.

 

[Superslinky]

I think what I was thinking was that if I had job 1 on our network under my "working directory" and it was for "company a" and then there were a number of subfolders for other documentation I would want it to look something like:

working directory
company a
3d cad (for inventor)
workspace
workgroup
etc
2d
drawings
etc
corr (correspondence)
whatever (just and example
company b
workspace
and so on

These would all be individual inventor projects. We do not use vault and primarily only have one inventor user although we have a handful of people who will open inventor and "take a look".

What I've noticed is that when someone else opens the assembly, the content library doesn't reconnect (sort of speak). Also a lot of times I will take a project home to work on it and will copy the entire model directory to a usb drive and copy to my home pc. Once this is done I cant get standard fasteners and the such to be included. I've also got a situation where I have an assembly (lets call it 001a) that has an idw file assosiated with many drawings within and I'll have to rename the top assembly. The design assistant doesn't seem to want to let me rename the top assembly so I end up having to do it manually and then of course the idw doesn't know where the file went.

I just need some help and I don't need it in "the manual" terms. I need a good place to start in order to understand the technical terms and a better understanding of the inventory directy structure (and what each folder within means) and how to correctly use the design assistant to make file name changes, etc.

Please help@!

 

[EngAddict]

Structure looks ok, mine is like this (with some variations):

Project
CAD Data
Assemblies (Inventor)
Drawings (Inventor)
DWG
DWF
Drawing Forms
PDF
Pictures

etc

Some vary, and I don't always need them all. Sometimes I add ones when I have a project specific library and the like. I keep all correspondence away from the CAD data, based on our quality system. The cad folders above them get structured based on the model breakdown and the size of the project.

As for other people not being able to view your CC, sound like the parts have been stored on your local machine. Crate a common folder on the network and point the application options there. then everyone who opens a project will look to the same place.

If you copy files to take home use pack and go. This will collect all your parts that are in a library.

For renaming you have to understand the order in which Inventor references. idw -> ipn -> iam -> ipt, etc, so if you want to rename an assembly open the idw in DA and then it will maintain all links. The idw you may rename in explorer but if you get comfortable you can pretty much rename any part in explorer and resolve the link, if you have to, when you open it.

There are some good white papers from various AU classes around on this sort of material if you have a look.

Hope it helps

Stew

 

[Gymmeh]

We have a different structure because of the way we re-use projects.

Our structure is:

Engineering
>Machine 1 (.ipt level)
>> .iam,.ipt, pdf's, etc.
>Machine 1a (.ipt)
>> Ditto
>Machine 2 (.ipt)
>> Ditto

There are a couple methods of renaming that work well.
A different method then EngAddict is to make a folder on your desk top. Inside this folder have a "temp.ipt" project file.

1. When you want rename a new project from machine 1 to machine 1a. you would copy all of machine 1 files except the .ipt into your desk top "Temp" folder.

2. Then you rename all the files to machine 1a file names.

3. Then open the main assembly for your new machine 1a and then it will ask you to re-link the parts. Then make sure you brows to your desktop Temp folder and find the correct file. when your finished the assembly should look correct. check it over carefully and then save.

4. Now you can copy the whole Temp folder and paste it in your engineering directory. Rename the folder and rename the .ipt to the project 1a.

The simplest way to learn this whole process it so make a 3 or 4 part assy, and move it around, rename it and see how it reacts. I use a couple different methods for renaming in explorer depending on the size of the assy and how i want to change things.

This is kind of a steep learning curve but its worth the trouble

good luck

 

[hrpi]

I'm an integrated/OEM type user so this might not apply due to your client-centric project approach, but I understand your dilemma. We also do projects for customers which creates similar issues.

Look backwards from ten years in the future, for your own answer.

I've used Inventor for years and I've amassed quite a large library of component parts that were not (or are still not) available either from Inventor's ContentCenter Library OR from the Internet (from mfr's, website or data exchange i.e. 3DContentCentral).


The $64k Q is how much of what you create MIGHT be recycled later on, for other customers/projects?


If some or all of it might be recycled, consider that your folder & file structure might become your own "Library".


I lose a LOT of time searching for and creating "editable" component parts made by other manufacturers. I save EVERYTHING I create. STL & IGES files are great for one time uses if they're standard parts like a bolt but otherwise, I lose countless hours on this topic.


Sorry to blather on but hopefully, my (partial horror) story might save you days or even weeks of work over the long haul.


After losing literally WEEKS or MONTHS of work by accidentally renaming, recycling, overwriting or modifying files that were (and should have remained) unique, not to mention that VERY painful hard drive failure, I set out to deploy Vault. I now use Vault MFG (fka ProductStream) also for future accounting-database integration.

Along the way, I created our entire file/folder structure that closely mimiced our internal part numbering system, which is based on Categories of parts. This helped me cross-link our Acounting System data to models, drawings, etc.

And, since NUMBERS sort more easily in Explorer than alpha names, it makes locating parts and assembly files VERY easy (Yes, I like the Dewey Decimal System).

Basic (simplified) Example:

0-Systems (Customer-Specific Projects - IAM's & IDW's)
1-Pumps
2-Valves
3-Seals
4-etc.

Next, as far as Inventor's "Project" files are concerned, Since EVERYTHING I use is Vaulted and I NEVER want to lose a moment searching for that custom part I made last year or even that custom metallurgical "Material Style" (or even a custom color), I keep EVERYTHING in ONE project file.

The benefit of this is obvious.

No matter what I'm working on, I can ALWAYS find what I'm looking for and that custom "Style" (i.e. C863 Manganese Bronze) I had to create last week is available at my fingertips.

Hope this helps you decide which way to go.




@ Gymmeh & EngAddict RE: renaming and recycling files:

Vault does almost all of this for me (you/us), creating copies & keeping track of them so manual re-linking is not necessary.

VERY Sleek tool, ESPECIALY because of it's native revision storage system and Parent/Child link handling.... Along with Automatic DWF creation capabilities.

Best of all, it saves EVERY version you ever checked back into the vault AS A BACKUP!!!!

Another benefit is Vault's ability to be backed up (it's an SQL database).

You can also download it's "Current" version of ALL files, complete with the foilder structure in one click by using (Get Entire Folder). Makes setting up a mobile workstation a snap, not to mention a simple way copy the entre thing.

VAULT IS A TRUE LIFE SAVER (WOOT WOOT)!!!

Best Wishes!

 

[Gymmeh]

I agree that vault is ace.

But i understand its not for every application