Manual file management with SolidWorks

Anyone have any tips/suggestions/procedures on how you do manual file management with SolidWorks. We are currenlty using a PDM system, but we havent been very happy with it for the past 5 yrs. Its very complex, upgrades are a pain, and its very buggy. I am trying to get a flowchart created on how we would do a manual system. This would help figure out what we really need in a new PDM package or if we want to manage our documents manually.

Im very curious to find out if any users here are successful with a manual system.

Please post your views. Thanks.

We use a manual system where I work, and it has done everything we need. We've never used a PDM system for SW, but I have used some version control stuff for programming, so I'll try to give you some pros/cons of our manual system. Also, practically all of our design is on the assembly level with parts that are standard and don't change, like piping and fittings. So revisions really only happen with assemblies and drawings, not parts. Here is how we have stuff set up:

- We have all our SW part and assembly files on one network share, and all drawings on another. They don't really have to be separated, but it helps out some.

- In our mrp/erp database all our parts have a part number that looks like 123-45678 (3 numbers, dash, 5 numbers). The first three numbers generally tell what kind of part it is, and we refer to that as the "class code". (800- is engines, 130- is pipe, etc,)

- On the parts and assembly drive, everything is stored underneath a directory with the class code (first 3 digits of the part number). So pipe is under a directory called "130". Some of the directories also have a brief description after the number like "130 Pipe" or something like that.

- The different class code directories are structured in one of two ways depending on the type of part.

- The way we do stuff like pipe and beam that you have all sorts of lengths is that each assembly actually gets its own SW part file for each piece of pipe, so that way we only have the one configuration and if we change the length of pipe it doesn't affect any other assemblies. With parts like this, under the "130" directory, there are separate directories for each part number of pipe, so you have a directory like "130\12345" for pipes numbered "130-12345". In those directories we have all the part files for all the different pipe named something like "130-12345-00 (00003).sldprt". The 130-12345 is the part number, the

-00 is the revision, and the (00003) is just a counter because of all the different files we end up creating.

- For other parts like pipe fittings where you don't have all different lengths, all the parts are directly in the base class code directory, so a part for a flange might be in directory "271" with a filename of "271-12345-00". Once again, the part # is 271-12345 and the revision is 00.

- All the assemblies are stored in the same structure as the part files. The drawings are in a similar structure, just on a different network drive.

- Whenever we rev an assembly/drawing, we just increment the rev number on the file, so "330-12345-00.sldasm" becomes "330-12345-01.sldasm". We leave the old file in place for history. Also, all the pipe and other parts that we may change lengths on are also replaced with new copies so we don't mess up the old rev. We have a program (which I wrote) that does all this automatically.

That's the basic setup of our file system. We also have a little addin that makes part lookup easy, so the drafters just have to type in a part number and the program finds all associated parts/assemblies/drawings and gives a preview of them. All of our drafters work off of the network, which does slow some things down, but it keeps all the files in one place. They can copy stuff to their local hard drives, but they are expected to copy it back to the server every day so it gets backed up. Most guys just work off the network, as it's not too slow except for very large assemblies. We have a gigabit network, and the files are all served off of a samba share in linux, which we found to be faster than using a windows server on similar hardware. Also, the way our work is structured, only one person is on a certain project at a time, so there are rarely conflicts where two people are trying to edit the same file at the same time.

The system has worked well for us, and has changed slightly over the years of use, but not much (basically just some changes in how we used pipe and beam and such). We have been using this system since being on SW 98 or 98+, I'm not sure which (I wasn't here at the time we started using SW, I came on board when we were on SW 99).

We like the system as we don't have to buy a pdm product. While we don't have a history of small changes like you would with a pdm system, we do make backups every night that are saved for a short while, and some backups are saved permanently. So if someone messes up a file we can go back to what it was at the end of yesterday, which has been good enough for us. We have a fairly small drafting department, so I'm not sure how things would work with lots more people.

I hope that helps you, and feel free to ask any more questions you may have.

Jonathan Anderson snipped-for-privacy@jwoperating.com

The likelihood of success when working in manual file management with

3-4 people is very different from working with 10-20 people. My opinion is that 4 people is really about the upper limit of manual file management for the average group of users.

Everyone has a different way of doing things, and different reasons for doing whatever. For me, storing drawings in one place and models in another is just a disaster waiting to happen. Your drawings become disassociated from the parts, and you're screwed, or at least you would have a bit of a job re-assembling all the referenced parts/assemblies to make the drawing work again.

Putting revisions in the filename also can cause major problems especially if you use any kind of external references, incontext, split parts, derived parts or even just ocasionally make mistakes. The only way to make this really workable to have the latest revision have no rev in the filename, only old revisions are put into the filename. That insures that you don't break links for active documents, and old documents can be revived by renaming them.

Parts shared between several assemblies, parts or assemblies with more than one drawing each can cause both of the above schemes to completely wig out.

To me, there are a few things that are important:

- Avoid descriptive filenames. I prefer sequential filenames which are less likely to be duplicated. Descriptions can be handled in properties.

- Try to work locally. This will speed things up and limit crashes. This will probably mean copying things down from the network and putting them back up when you're done. Maybe your MRP has a way of flagging part numbers where changes are pending so other people don't start making duplicate or conflicting changes.

- To do work locally and still share files on a network, you ought to have a read-only shared area with one admin person with write access who is responsible for moving files into the read-only area

- The admin should understand SW file management thoroughly. If you separate an assembly from its parts or a drawing from what it references, you are causing yourself a nightmare.

- Revision history is difficult to keep track of manually, I don't think there is a truly fool-proof way of doing it. To me, the best way is to leave the sequential filename bare for the active revision, only appending the rev level when it is obsolete. Renaming a file like this (with a "save as copy" would work) will break the links, which is what you want for old revs. You don't want to break the links for current revs, which is what up revving the filename with a new rev level will do in many cases.

- It is a lot easier if you just keep a revision history of drawings, which can be done in tif, pdf or eDrawing. This elimiates most of your worries about referencing wrong revisions or breaking references to correct revisions.

Personally, I would just go for a simpler PDM system. All it takes is one person to have a file in the wrong place, and print a new drawing referencing an old part (or equally likely an old drawing with a new part). Or someone with full blown SolidWorks using a procedure meant only for Viewer or eDrawing user to print a drawing and send it out.

I managed a manual system for a while, and it is doable, but it is completely dependent on everyone knowing what they are doing and being perfectly consistant about it. If you overwrite files on a network, there is no "undo" or recycle bin.

Matt

Thanks Jonathan for your reply, Also thanks to Matt for his insight/suggestions. How many users do you have in your engineering dept? Our company has about 6-7 heavy SolidWorks users, and 3-4 casual users who mainly view files. On a new project, we sometimes have 2-3 people working on the same files.

Here is my draft idea after talking to other people who use a manual system.

1. The file system consists of 3 sections. Work area (which could be on a network drive for a team, or local drive for a single user), Vault (read-only to users, write access to the GateKeeper(s), this is where files are released to), and finally the Archive area (where revisions are saved). I also think it would be nice to separate the folders in the Vault by Machine.

QUESTION: What do you do for common parts? One company that I talked to said they actually copy a common part and rename it to a prefix of the machine they are working on. This stops everyone from referencing the same file in the "Standard Parts" directory. What does your company do?

If we have a folder called "Standard Parts" which has subfolders called for bearings, pipe fittings, nuts, etc, would users reference those parts in their assy when working in the Work area, or would they copy those files out of the Standard Parts folder?

1. When a user wants to work on a file, we have 2 options. A.) The user could copy the file out of the Vault or B.) The Gatekeeper could copy the file out of the Vault and keep track of who is working on what. If the user is allowed to bypass the Gatekeeper (A), im not sure how we would keep track of whos doing what. I did a test the other day on this. On one computer, I had a part open from a network drive. I added a hole to the part, and saved it (kept it open). I went on another computer and opened the file. SolidWorks stated that the file was open by user xxxx, do you want to open a copy. I chose "Yes". I then closed the part on the first computer, then deleted the hole on the second computer. I did a Save, and it wanted me to do a Save As. I then chose the same file, and it allowed me to do so.

QUESTION: I know this is how its suppose to work, but how do you stop people from doing this on a manual system?

1. After a user or Gatekeeper copies the file out, the user edits it.

QUESTION: This is another area im not sure what to do. If I want to have the assy open that this part is in, do I also copy the entire assy out of the Vault, or do I open the assy from the Vault, and redirect the part im working on to the Work area?

1. After the part(s) are modified, the user would give the file(s) to the Gatekeeper. The Gatekeeper would then either save the old part to the archive, or the user would. I like the idea of keeping the current revision as the same filename, but the archived revision would have the rev added to the filename. Ex. part 99900123.sldprt is modified, before replacing it in the Vault, the old file is saved to the Archive as 99900123_00.sldprt (revision 0). The drawing will also need to be archived, and linked up like Matt described. OR We could only save a PDF/eDrawing/Image file of the drawing of the drawing only. This would save us some time and confusion, but if we needed to go back to a revision later (which rarely happens), we would have to redo the old revision of the model (which may or may not be easy).

QUESTION: How do you handle revisions of assys? It seems like by keeping the filenames the same for parts, you wont be able to tell what revisions of the parts referenced by the assy where used on a certain revision of an assy. Ive heard some companies don't even rev their revisions, only the parts. Any insight would be helpful. Thanks.

I second Matt's suggestion. We started using a basic PDM system when we went from one ME to two and were glad that we did. The low-end systems are inexpensive and easy to use.

Jerry Steiger Tripod Data Systems "take the garbage out, dear"

As far as our department size goes, currently we have 4 full-time drafters that basically use SW all day (although occasionally they do some work in 2d on some old stuff). We also have 2 other engineers who do most of their own drafting, so they are pretty heavy users. After that we have some (varies from 3-6 or so) part-time students who work for us, most of which do some SW modeling at some time or another (their functions change periodically to give them different experiences, but there are usally at least a couple that are doing SW work mostly). Then we have about 5 or 6 others that mostly do viewing of files. So I guess that's about 6 heavy users, 2-4 part-time users, and 5-6 viewers.

I can definitely see Matt's point that a manual system would not work very well once you get more people, but we have not had problems yet. When it becomes too difficult to manage manually, I'm sure we will look at a PDM solution, however I think it will be quite a while before we add that many more people. I think that our system works well enough that there is no one here that would say that we could save enough time to be worth purchasing a PDM system right now.

As far as our common parts are concerned, all assemblies reference the same standard part files. This has not been a problem for us because we don't ever change those parts. If someone were to change the parts, I have a program that can automatically recreate most of them in a standard fashion.

You mentioned the issue of a user editing a part after it has been copied by the Gatekeeper. We don't have a gatekeeper system - all of our users have access to all parts/assemblies/drawings. I don't imagine that there is a way to force users to not edit something on their local machine after it has been copied over, but our 'incentive' is that if the user doesn't have the files on the main network drive, their work doesn't get backed up. Our guys know that if they mess something up that they didn't have in the proper place, then it's their problem to do the work over. But in reality, we have pretty competent people that rarely make mistakes like that.

Your next question was about just editing one part from an assembly. I'm not sure about that one. As I mentioned in my last post, most of our guys do work off of the network drive, and despite all the negative things said on this forum, we are fairly stable. Also, we rarely rev parts. We don't really manufacutre any parts ourselves, we just do assemlies and packaging. So all of our revisions and work is at the assembly level. We do have the occasion where one of our purchased parts is revved (say a new rev of an engine), so then we will have a part with a new rev, but then the new part rev would usually be included in a new rev of the assembly, so the old rev of the assembly would contain the old part.

All of our parts, drawings, and assemblies contain a revision number as part of the filename, and as part of the configuration name. This way it's easy to tell which rev of a part a certain assembly is using, or which assembly rev a certain drawing is using. As far as keeping our references straight when doing revisions, we have a custom program that does this for us. Basically, you just pick an assembly, give it a new rev number, and the program automatically copies everything needed into the correct places and replaces all the references accordingly for the new rev. This utility has definitely helped us deal with revisions.

I hope that helps you some. Also, just so you know, I'm not one of our heavy users - I just write and maintain software at my company, so I've written all of the custom addins that we use in SW. So I know about our file system, but I'm not a daily user in SW - I just know what I hear from the other guys. If you want to talk to one of our drafters, email me and I'll give you one of their email addresses. If you want to see a little of what we model, go to our website at

then click on J-W Power Company, then Package Fabrication Facility on the left. At the bottom of that page is a little animation with one of our models.

Jonathan Anderson

I have a sneaking suspicion that all it takes is one blunder with a mechanical PDM system & multiple users to blow more money than a PDM system plus the training to get everyone up to speed.

Bo

Upgrading to Solidworks Pro is not very expensive. This will allow you to get PDMWorks. It is very difficult to manage SolidWorks files manually. Keeping track of all the internal references between files and tracking revision levels is almost impossible without a PDM system.

If you know how PDMWorks, you can manage the system quite well.