"Correct" way to best use the toolbox 4

[Andy330hp]

I've gotten to the point where I am dealing with the assorted fasteners currently used in our products. Some, it looks like the previous drafter drew from scratch. Some are from the toolbox. I am not too familiar with the different capabilities built into the toolbox. I am trying to clean up all our files and assign part numbers, and am trying to find the best way to deal with these items.

Should I have the models of the specific fasteners that we use in our parts directory, or should it reference the toolbox directory? I ask becuase I've read the following:
1. When you create a specific fastener using the toolbox, it defaults to creating a configuration in the "master" file in it's own directory
2. PDM/Works doesn't handle configurations well. (This fact depresses me for other reasons, since a number of our different parts are in configurations. I hope this gets fixed before we make the step up)

This makes me wonder, if we ever do get PDM/Works, are we going to run into problems using the toolbox how I thought it was supposed to be used. Let me stress again that I do not have very much experience with it, and may be using it incorrectly myself.

 

[Andy330hp]

Oh, and one other related question:

One of our fasteners is an M5x0.5, but all I can find in the toolbox is M5 x 0.8. Is there a way to add options to the toolbox, without actually drawing the part from scratch, ie add a column to it's "design table" so that it will automatically generate what I want?

 

[Andy330hp]

Another question(sorry everyone)

The inserted toolbox items don't have callouts on the threads. I can understand why this would've been very hard hard to automate, so I won't complain about that. But, I was thinking about editing the definition of the schematic thread so that a callout was present, but since it seems that a number of different thread configurations are possible, I don't want to attach a thread callout if it attaches to the master file and so is incorrect the next time somebody calls a slightly different config.

 

[MadMango]

Andy330hp, give this page a read over to see if it will help with any of your questions. Thanks to Matt Lombard for compiling this info.

http://www.frontiernet.net/~mlombard/Toolbox.html

MadMango
"Probable impossibilities are to be preferred to improbable possibilities."
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[Theophilus]

Andy330hp,

I don't know that I can help much--I'm checking these posts myself to optimize how I use Toolbox.

However, one thing may help in your nomenclature (maybe)? Could it be that the reason you cannot obtain a M5x0.5 fastener is that the 0.5 refers to inches instead of the expected mm? In that case, 0.5 mm would be too small to have adequate threads and therefore would not be included within the list of options in Toolbox.

MadMango, thanks for the link. I think I'll check it out too.




Jeff Mowry
DesignHaus Industrial Design

http://www.designhaus-i-d.com

 

[Andy330hp]

Theophilus,
I know that M5x0.5 threads exist, we have them on hand. It just so happens that it's not in the ansi metric toolbox. It may be that there are different sets of standards for metric fine and coarse threads, that I don't know.

I got a little ambitious, and opened the actual data sheets in access, and found that the column that contains the M3, M5, etc are prevented from having the same entry twice. So, there couldn't be an entry for M5 x 0.5 and M5 x 0.8. I don't know know why they did that, and didn't want to mess with it for now, unless somebody else posts that they have successfully altered these tables.

On a (possibly) unrelated note, for some reason my BOM in the assemblies is now looking at the configuration name instead of part number for toolbox items. Actually, it's a little more involved than that:
1. I have both the drw and asm files open at the same time
2. The part numbers are displaying correctly to begin with
3. I go into the asm
4. Select the toolbox item, RMB and select edit toolbox definition
5. select a different p/n, and exit
6.Refresh the drw it no longer looks at the part number.
7. Even if I go back again and select the original part, it still will no longer show the part number in the BOM

Any ideas?

 

[Andy330hp]

Oh, and I'm still wondering if, for data management purposes, it's better to create copies of the fasteners as individual parts vs always referencing the master file

 

[Andy330hp]

I feel like I'm talking to myself here, but....

I figured out the part number thing. In the configuration properties, the field "part number displayed when used in bill of materials" was set to user specified name. Which actually brings up ANOTHER question that's been bugging me:

It seems that there are a number of different instances where you can give a model a number. You can go file->properties and set up part numbers under custom AND under configuration specific, AND there's the previously mentioned tab under configuration properties. What pulls rank? It seems like the last one has first priority. And, if this is so, and it is set to document name, what happens if I set a part number in a file under it's properties but name it slightly different for whatever reason? What shows up in the BOM? Has this upset anyone else?

 

[macPT]

How we solved how to work with standard parts: we create them in a separate folder (called "standard parts&quot as parts (some are assemblies, when they are downloaded from manufacturers sites). Everything "out of the shelf", from fasteners to motors, used in our designs, is in this folder.

This way these parts can have the properties needed to process them in SW, when they are included in an assembly, as for any other part.

I'm not to familiar with Toolbox and maybe we are doing some extra work. But we have no complaints.

Regards

 

[pdybeck]

Andy,

I had many of the same questions you are asking - only about 4 or 5 months ago. What I decided on doing here with our use of Toolbox and with our use of PDM/Works is to not allow configurations within a file to describe more than one part number. Seems like a whopper at first, but it really simplifies data management (we do all configurations at the top level assemblies of our products be/c there are so many options for our cutomers to choose from on our products.) This notion has far reaching affects, as the Toolbox master database is a collection of files with configurations for each component that has ever been created during one of your SolidWorks sessions. It even affects how we treat castings and machinings of those castings - not as configurations, but as derived or base parts so that different part numbers are in different files. For us, I have set SolidWorks to always create a copy when inserting a toolbox part into an assembly. You can do this under the toolbox browser configurator, under document properties. You can also specify a default path where the copies will be placed. In this method, each standard component created by toolbox is its own separate file capable of being documented with any part number, material, finish, approved sources, etc... Also, when a copy is created, there is only the necessary config in the copied file, not all the configs that were ever created. If you are always working with the master toolbox parts, and don't create copies, you will see that you quickly run into limitations. For instance, with the master database you could not create a clevis pin (for example) of one material and its own part number, and then create another clevis pin that is geometrically equal but made from a different material with a different part number. Try it. Toolbox will not allow you to create geometrically equal configurations with different part numbers. Current lingo in SWX documentation is fuzzy on this - it basically says that you can have geometrically eqaul parts with the same part number (such as a screw with threads schematic, cosmetic, or none), but you can't have geometrically equal parts with different part numbers. I was very unhappy with this limitation and had been complaining about the problem to no avail. So, like I said earlier, stick with creating copies. Then you can manage the individual components in the vault. I decided to drop my begging and pleading when I saw the light. I have set up a project in the vault named hardware and there are subprojects under the hardware project for bolts, screws, nuts, retaining rings, etc... This is where the standard parts created by toolbox get checked into, or moved into once they are in the vault. A nice benefit is that you can see where used for each standard component in the vault, and obviously searching for standard components is now possible if you are dilligent enough to add information like material, finish, approved sources, etc... You can't do this if you don't check in Toolbox parts (this is actually an option in the vault admin tool for PDM/Works). For our users, they know the first place they should check when looking to use a standard part in an assembly of theirs - is the vault. If one they need is there, great, drop and drag it into you assembly. If its not there - it must be created using toolbox. It seems like an awful lot to think about all at once, beleive me these issues are definitely more complex than any you will face in a 2D world, but the functionalities the vault offers as far as storing, finding, and making information available to all individuals in a company, it is well worth the extra thought and work in the beginning/set up stage that you are in now.

 

[rokahn]

I'm using pdybeck's method of copying configured part files to a directory specified in the toolbox browser options. However, when I move the part/assembly files and these configured parts to a new PC, SW2004 doesn't find these configured parts, even if I move them to the same directory as the part/assembly files.

Where do I configure the new PC to tell it where to look for the configured parts? Do I set toolbox browser option to copy configured parts to this directory and it will also look there?

 

[pdybeck]

rokahn,

I am a bit confused about your post. If you have set toolbox to always create copies, the copied parts should not be configured parts as you mention. The only configuration that should be present in the file is the one that was created from the toolbox dialogue box. Also, we are not using a standard copied parts directory, although you could. We create the copied parts and then move them to the project area where we are developing our new product and place them there. Eventually they get checked into PDM/Works. But enough on that ... Did you check the references for the assembly before it was copied and after it was copied (on the copied assembly)? Did you copy the children of the assembly when you moved it to a new computer? Does your new computer have the ability to connect to the old one through the network? A good understanding of what is happening with files behind the scenes is needed to use toolbox in the way we are. You need to know what files are being created and where they are being located when you use toolbox if the setting for always create copies has been set. Sounds like you may have some parts in your assemblies that either didn't get copied along with the assembly, or some still may be parts from the toolbox database. If your copied assembly resides on the new PC, but the copied parts or toolbox database parts don't and your new PC can't connect to your old PC, then messages like these would be expected. We place our files on network directories so that when new PCs come, no files have to be moved, as well as for obvious back-up reasons, and for the ability to allow everyone to get to them. I may be able to help if you can give me more to go on. The first thing you should do is File, Find References within the assembly(ies) that is (are) giving you problems. Also, you could use SolidWorks Explorer to copy the assemblies and make sure to copy all the parts and subassemblies as well. SolidWorks Explorer is pretty easy to use if you haven't used it already.