model libraries

We do it very similarly. We assign an in-house part number to everything we purchase, whether it be a relay, gearmotor, or a bolt. We have a program that lets you step through categories of parts and each pick filters the remaining boxes, until you ultimately get down to a unique part number. Then, if we have a SW model of it, a button is enabled, that when pushed, opens the model in SW in the correct config.

The reason I mentioned this first is because this functionality makes it the easiest way for users to find existing models. If you want people to do something your way, make your way the easiest.

Now, for the models. On our network we have a series of folders that contain the models in categories. If we create something like a bronze bushing, I try to model it such that it is conducive to a design table, and then go through all of our existing part numbers and create the model for all that we already have in the system. That way I have the ease & functionality of the DT, but am not spending time modeling many that we may never use. Now, there are exceptions, such as when there might only be 10 total, or something, in the family of parts. Then I might do them all straight out of the catalog.

When I build the model for the DT, I try to utilize dimensions that match the ones in the catalog. Example: build your model using the ID of a bearing listed in the catalog, rather than using a radius, which is half of the catalog value, and put them in the same order as the catalog. This has the benefit of, when entering new values, you just read straight across the catalog page and type in the numbers.

The other thing is to rename your dimensions Like ID, OD, LTB, etc. because you might add a config that is from some other catalog and the order isn't the same. By naming them, you can recognize where things go.

If we have models we download complete, like SEW gearmotors, SMC air parts, etc., we just store those as is, unless analysis says a DT would actually be a better option in the long run. We have done that once or twice.

A far as naming configs, we have standardized on the config name being our internal part number, and sometimes followed by a descriptor, such as

00125-617 .375".

Can't think of much else - kind of long, but you asked. :-)

WT

That my friend is going to be the hardest part.... I only have about 6 designers and I go through the process with someone EVERYDAY. It just amazes me :-).

Noel

Wayne- Thanks for your input. I shared your post with a colleague of mine, and we both are curious as to what program you use to "thumb through" the parts. Im glad to see that you do a DT in the same order as the dims in the cataloge. I wish more people did this. It makes it easier to figure out what is what. Also the naming of the dimensions is a very key point! I have planned on doing a descriptive file name, and then the configs would be the part number. Thanks again for your thoughts, I appreciate it a lot! Thanks for the post, even though it was long, but that is quite alright. I want good indepth information. Brent

The program to run through the parts is a home-grown VB program. Sorry. But, the concept is free.... :-)

WT

We figured the program was a home made program. I just wish I knew some VB now! More training!!! Brent

it sure will be! Brent

Let me say it again - you HAVE to make your way the easiest way to do it, then they will fall in step.

WT

Just had a two hour long meeting on how to deal with issues. I think we have come up with a pretty simple way of doing things. Getting the time to do the "house cleaning" is going to be the tough part. Mgmt doesnt want to lose valuable "engineering time". Sheesh! a little time now will save A LOT of time later! They just cant see it. Brent

You may want to think about using something like PDMWorks. I found that people were more diligent regarding issues like part naming conventions when we set up the vault. PDMWorks works with configurations as well as Toolbox hardware now. For what it's worth, we use our part number for the file name and enter the mfr. and mfrs. p/n as properties in PDMWorks.

A PDM "would" be very helpful here, in the fact that the way we handle our models it would make life soooooo much easier. The only reason we DONT have a PDM package is Cost. I think it possibly could have paid for itself by now in preventing errors. But I guess we will never know. We have a real problem with personal libraries, and without a PDM there will be no way of stopping it....actually thats a false statement, there is NO way to stop designers from having personal libraries. Im starting to realize its a never ending battle. Getting designers to give up newly modeled items is a big challenge, it takes a little more time to save it to a network folder than to model and keep on going. But they save it to their HD why not save it to the network, who knows. Brent

Here are our part library rules. We use drive P strictly for our "common parts library". We found that naming folders by discipline (electrical, pneumatic, etc.) would lead to confusion. Many parts overlap disciplines. We also found that naming folders by material (stainless steel, plastic, etc.) had similar problems. Therefore we settled on folders named by manufacturer.

Our hottest debate: whether or not we should use configurations for common parts. Without giving details, we eliminated configurations on common parts, save in-house parts and parts that have multiple positions (valve open or closed).

In addition, we use many different software and CAD packages, we decided to save all parts in the same directory. When opening a file using AutoCAD, my list of files in the dialog box will only show those files with a .dwg extension. Almost every program uses a similar feature.

Part Library Rules:

1) We have a drive called "Library" for our common parts. Map it to "P". 2) Under this drive are folders named after manufacturers (occasionally a vendor or two). There is a folder for 2D electrical and plumbing blocks as well. 3) Parts will be saved into the appropriate folder using the mfg. part number. Existing SolidWorks parts, that do not have configurations and which are modeled correctly, will be moved (via SolidWorks Explorer) to the new folder. 4) To make it clear, we will not use configurations on manufacturer parts, but we may on in-house parts. 5) If the part's appearance changes, yet still uses the same part number, a configuration would be acceptable. I.e. Configurations of a valve showing the handle in the open and in the closed position would be acceptable. The valve showing the handle on it and the handle removed would work too. 6) Avoid the use of subfolders. Inventor does make a folder called "Old Versions". You can ignore this when you see it. 7) If a common part "Start Part" exists, use it to create that type of part. I.e. PFA tees should be modeled from the same PFA tee starter so that replacing one tee with another is smooth. 8) Naming Convention: Use the mfg. part number for the file name. The mfg. should match the mfr./vendor name in Agile. Use uppercase letters only, except when following the replacement guidelines for characters (see below). Replacement Character Guideline: (space) = _ (underscore) / (slash) = l (lowercase "L") , (comma) or . (period) = - (dash) " (inch) or ' (feet) = IN, FT, etc. (uppercase) Example part number of a Spraying System nozzle: 27500D1l2-8-TEF 9) Common in-house parts may be stored in the InHouse folder. I will eventually make a drawing/drawings which show all the parts in this folder. 10) These folders can contain drawings, models, spreadsheets, etc.. Use your discretion, but try not to save every spec. sheet here. 11) When mfg parts require an assembly, name the components with the mfg number followed by an underscore (_) and then a one word description. For example, HG300-10-113_LEFT.SLDPRT and HG300-10-113_RIGHT.SLDPRT might make up the HG300-10-113.SLDASM.

___________________ Todd Bennett Celerity Group, Inc snipped-for-privacy@celerity.net

Brent,

I am using DBWorks (800.00 US per seat for Integrated SW user

--Enterprise version) and setting up a client to do this very thing.

One of the many nice features is a Category Wizard.

This wizard is called automatically upon saving a new part or assembly. There is a series of categories the user selects (three levels is standard) to categorize the parts. The nice thing is the program can automatically generate new part numbers (next non-inteligent number) as well as determine where to save the files. You can even set it up to not allow users to save library parts (or any other file for that matter) to their local hard drive. With a little more work the user can even specify how the description is filled in based on the categories choosen. Slightly more work involves filtering each type of part to include properties specific to each type of SW part or document.

Drawings are handles easily as well since the system knows how to fill in title blocks, add water marks, etc.....

Setting up the categories is pretty easy as Mechworks supplies you with a category maker. This is a pretty slick interface that determines the inter-relationships between database tables (default is Access- but can be upsized to MSDE or SQL as required).

It can be integrated to play well with Toolbox in a multi-user environment and can manage individual configuration of parts and assemblies.

What I like about the system is that once the rules are set up, individual engineers cannot change the business process. Administrators can lock the system up as tight as they want (including locking out users from accessing custom properties though the SW interface) and trying to by-pass the system (have SW save and saveas buttons map to DBWorks save and saveas buttons). ISO audits anyone?

The secret to having people conform to a system is to show the system makes their life easier and allows them to do their job better than their "own - save it on my local driver" version.

This requires an integrated approach that writing chunks of VB code, using macros, or writing procedures that no one can enforce cannot accomplish. I know, cause I spent years doing it for small companies I worked for.

Work group PDM's have come a long way in the last five years. They are simpler, easier to implement, and most importantly, deliver what they promise.

For a small company, this can be the best small investment they can make.

If they can't afford to take the time to do it right the first time.... how come they can find the time to make the same mistakes over, and over, and over..............

Cheers,

Len

I agree with Len Brent, Workgroup PDM solutions have come a long way in the last few years. They are relatively inexpensive (under $1,000/user) and don't require any full time CAD admin. You also don't need any consultants for the implementation. If your SW re-seller is worth a damn, they will be able to help you select the product that's best for your situation and should be able to give you some guidance regarding setting up the vault, permissions etc. They should also be able to assist with an ROI as well.

With any of the PDM solutions you can create a vault folder called Commercial Parts and that's the end of it. By assigning searchable attributes to the parts, you don't have to worry about which folder to stick a particular part in.

Also, most of these products now have the ability to vault all file types, not just SW files. You will be able to mix in Inventor, SW and Acad parts. The users will search on an attribute such as Mfr. p/n and a list of all applicable files will be returned.

I feel your pain. Anyone who is (or has) been involved with CAD admin goes through this.