I’d like to start a discussion on file management techniques and best practices.
Do you sort files by project?
Do you use detailed naming schemes or just part numbers?
Do you segregate parts, drawings, and assemblies?
Do you use virtual components?
IF you have to do it manually,
Sort by project, yes, but library files kept in central location. Files shared with other projects should stay in the other project folder, especially if they do not changed, and keep the same part number.
Whatever you do, unique file names. I would recommend part numbers for file names, descriptions as a property.
Segregate file types? no. Why would you? You can sort Windows Explorer by file type. Great way to screw up references.
Virtual components? I use them in the course of working, but I always save them out unless it’s just some kind of place holder that doesn’t need to go in the BOM and you don’t need a drawing, something like a customer’s reference part, or a representation of an instruction manual or a purchased tool being used. At the end, all virtual parts that require drawings or BOM entries are saved out as separate files.
Just because SolidWorks allows you to make sloppy crap doesn’t mean you have to do it.
https://dezignstuff.com/manual-file-management/
Use a PDM solution to manage your CAD data and a PLM to manage the rest of your data. 
Then you just need good meta-data!
The system you use should be dictated by your product and process. What works for one process and product won’t work for another.
Here we actually have a mixture. The saws and special machine divisions, which tend to be large projects with multiple assembles etc, tend to be managed by project. Much of our product lines which tend to be small assemblies or individual parts are generally organized by families. So for instance we have a product of lock nuts. We have different styles of these nuts. So all the different sizes tend to be under a single folder by family.
We also have a product that builds of a product where the base product is listed by part number and the created assembly that includes that product is listed by project.
So yeah, the directory structures, controls etc should make sense based on what your doing.
Before PDM:
Post PDM:
I’m pretty sure we’re still doing much of it wrong, just haven’t found a “right” way that we can actually implement. 
I sort project specific files by project. Common files that are used in multiple projects are in a single location.
I use descriptive names, but project specific files usually contain the project number as part of the file name.
No. All project specific files are in a single folder.
I used to use virtual components for things like concrete, that wouldn’t need to be detailed separately in a Drawing, but I stopped a few years ago when Solidworks developed a nasty habit of not including them in Pack and Go operations
Do you sort files by project?
During development only. After they are processed for release, they are sorted into PDM folders based on part type (Governor, brackets, tanks, panels). This is changing with Windchill to be by Product with sub folders for standard sections of our product. In addition there is a library of purchased components with sub folders for types (Screws, O-Rings, Contactors, PCBs, etc.)
With that said, we have a configurable product. Files for orders are placed in folders named by order number, each order can be unique.
Do you use detailed naming schemes or just part numbers?
Files are named by part family numbers. Inside the model, configurations are named as part numbers by adding a suffix number to the family number. Each family member is built using configurations. Family/Part numbers insure that each file is unique, descriptive name can get easily duplicated or require renaming later which is best avoided.
Files for orders prefix the order number to the family number for the file name. Again insuring uniqueness. If more than one is needed on an order, a sequential number is added as a suffix.
Do you segregate parts, drawings, and assemblies?
No, not sure why anyone would, can’t think of an advantage.
Do you use virtual components?
For purchased vendor parts that are assemblies, all internal components are virtual since we only assign a part number to the assembly we buy. Some flexible/deformable parts such as rubber bands, tape, wires, etc. Also reference models like walls and floors that are specific to that assembly.
Thanks for all your input. I fully realize I’ve inherited a less-than-stellar server full of data… 
That said, as a relatively inexperienced user (compared to most of you) I know I’ve made my fair share of data management oopsies as well.
The biggest issues we struggle with are filenames and library components. This is something that PDM will (hopefully) make easier to remedy than our current system of manually renaming and moving via SWX utilities. Also, I was taught to always segregate by file type, but now I’m honestly not sure why I ever accepted that as dogma…(???)
Pull all files into same folder.
Including templates, styles, favourites, macros etc.
Mike,
If it makes you feel any better, I took an engineering manager job where I was the 5th in the last 6 years, Didn’t learn that fun fact until one of the welders told me he didn’t need to follow my prints because I wouldn’t be there long enough to warm my chair. 
Anyway it seamed that each manager wanted to have things his own way and stored all of the previous work in an “old” file on the server. The “server” was the Plasma programmer’s machine with a CAD folder on it. Inside that folder was a folder named OLD MODELS. Along with the models and drawings, saved in project folders, was a folder named OLD OLD MODELS. Inside that folder along with the models was a folder named OLD OLD OLD MODELS…
Such fun.
And to make matters even better, the models/files were basically named for the material and the dimensions, no real part numbers and, here’s the kicker, files from previous projects were saved into a new project folder without changing the name just the shape or dimension. <()>
Along with this fun I learned that the owner who was a former drafting instructor (hand only) had been told when he went from 2D to 3D that he could open his AutoCAD drawings in Inventor and they would be 3D models. After struggling with trying to make that happen for 6 months he scrapped Inventor and bought SolidWorks. 6 months later out goes SW and back to Inventor. I showed up about 3 years after that and it was still a mess.
So be encouraged. It could always be worse.
Classic. In another 10 years you’ll probably have REALLY OLD OLD OLD MODELS and REALLY REALLY REALLY OLD OLD OLD MODELS.
I always want to believe that people are generally intelligent…but often times the things people do make me start to believe otherwise.
The biggest issue we have here is that no one wants to put things in the same place or use the same naming conventions. For the most part “Products” are in the right place and named to the naming convention but everything else could be named anything and be anywhere. We even have one product group that refuses to do any designing on the PDM. So they do the design and once it’s approved and released they move it to the PDM…and don’t delete the original files.
The things I’ve found on peoples local machines is a bit disturbing as well. Someone set up someone’s machine as the license server for our G-Code simulating software, when ever he reboots or turns his machine off you lose your license and the software locks up.
During design, yes. Project folder with Mechanical/Electrical Design subfolders. Upon release, everything is renamed and moved (automatically) to folders containing blocks of 1000 numbers. So, folder 400xxx contains 400000 through 400999.
In the project folder, you can name things whatever you like. It’s a sandbox. Some parts never make it out of there, so there are no naming rules. The released parts have dumb, sequential numbers for file names. If users want to find something, they can search by whatever (part number, description, etc.) thanks to PDM.
Started out doing that back in 1998. Quickly determined it was a bad idea since SW likes to save things in the last place you saved something, so lots of files wound up in the wrong place.
Extensively during design. If I’m basing a design on an existing one, I save a copy of the top level assembly. As I touch parts to make modifications, I make them virtual, and give them a name that is descriptive but points back to the original in case I don’t actually end up changing the part (e.g. BRACKET - WAS 435123). Any upstream assemblies are also made virtual as needed. When the design is done, anything in the tree that is virtual (and doesn’t have a part number for its name) is saved to an external file before release.
I also use virtual parts for things such as tubing that need to be shown but don’t necessarily have to be on the BOM.
Another use case is models of purchased parts that are assemblies. Download an air cylinder as an assembly model, make all the parts in it virtual and change the names to something more descriptive (body, piston, rod, sensor, etc). Now this one thing we buy is in one file with one part number but can still be put in an assembly and be made flexible and such.
One key thing to remember about virtual parts is that SW makes a real file in your Windows TEMP folder, not the SW Backup folder. If you aren’t careful, you can run out of space, SW will not behave well and the reason won’t be obvious.
Sure, Solid Edge has Virtual components. Siemens actual does a descent job with this and explains VCs in a PDM or PLM tool.[
Wow..the owner should have know better. But I will say with Solid Edge you could take those 2D drawings and quickly generate your 3D models and then pass the dimensions onto the model as PMI (driving dimensions). You’d have to check the Siemens Solid Edge YouTube channel for the video but I’ve done this in the past too. Works pretty darn good.
Hey, you stole my PDM concept!
Yes, our projects are 1 and done. So an entire project resides in a project folder. No files are reused (well, rarely).
Our customer parts obviously get whatever the customer has deemed. However, our internal parts have a semi smart numbering scheme.
Example of one of our part numbers:
MF-012345-D01
The “MF” is a type designation. Choices are: MF = Machining Process; EC = Electro Chemical Machining Process; AS = Assembly; GA = Gauge, etc…
The 012345 is simple a serial number. Whatever the next serial number on the list.
If the file is the top level assembly, then the D01 is left out.
If it is a component or a sub assembly, then it gets either a D01 or an A01 (the 01 is a sub serial number for that project)
Not normally, no. It is easy to filter between the 3 types. Most of the time, we will segregate exported file types, but not always.
The only time I ever use virtual components is for purchased components that need to be a sub assembly.
Example: A De-sta-co clamp. The clamp normally comes in as a multi body part. If I need to show the clamp in opened and closed states (and I usually do), then I will split the multi body part into separate parts and add them to an assembly as virtual components. Then configure it as needed, then delete the original and the temporary parts that were created. That way we are only dealing with 1 file.