My goal is to use Toolbox to generate fasteners with multiple material types and subsequently multiple part numbers associated with a single size of fastener. I have enabled the option in the browser to allow duplicate part numbers for dimensionally identical parts, thinking this should allow me to accomplish my goal. However, when I try to insert additional fasteners of the same type into an assembly and add another part number/descritpion entry into the fastener dialog, I get an error message stating "Part number xxxxx already exists with the current dialog specifications. Restoring dialog settings to that part number.". Am I missing something obvious here, or is this a bug?
Kevin, This is not a bug! The SWX language used concering multiple part numbers is misleading. You can create different configurations that share the same part number - such as a screw that has threads shown in one configuration and not shown in another configuration. You can not create geometrically equal parts/configurations with different part numbers. I noticed this terrible limitation in toolbox quite some time ago, complained about it to SolidWorks, my VAR, and to anyone else who would listen (search eng-tips.com or SolidWorks discussion forum), but to no avail, so I have toolbox set up here on all the users' machines to create copies of the master toolbox library/database. This is done through the browser configuration menu item and then the document properties tab. In this method, each part is its own seperate entity (file) and not configured like the toolbox master library/database parts. By copying the desired toolbox part, you end up with a file that has just the necessary configuration and no more. With this file you can name it, part number it, give it a density, description, approved source, etc .. all to your heart's desire. Now you can create geometrically equal parts that have different materials and therefore part numbers because they are separate files and not bound to the rules of the toolbox library parts. Please note when you create a copy - have an idea of where it gets placed and where you want it to end up - meaning directory location on your network or hard drive. We use PDM/Works here and one of our rules is not to use configurations to define more than one part number in a file (for simplicity reasons in data management). This method in toolbox falls right in line with our rules for use of SolidWorks. Also, we do check in the parts to our PDM/Works vault that are created by copying toolbox items. This makes it easy for others to drop and drag from the vault to utilize a part that has already been created. It also allows us to track where used information on our standard parts. I have set up folders/projects in PDM/Works that make it easy to browse and find parts based on their part number, description, material, approved source, etc.. Hope this helps. I'd be happy to discuss more if you like.
I have also run into this limitation. I do have my Toolbox set to create copies and I can create geometrically equal parts that have different materials and part numbers. TB creates files with -V1 appended to the file name. The problem I have is I can't reuse the file with the TB browser. It doesn't know the -V1 file exists. It will either use the default file (without the -V1) if I say 'Use existing', or it will create a new version -V2 if I say 'create copy'. I sounds like you get around this by not using the TB browser, but the drag and drop from your PDM/Works vault. I don't have a vault. So, my work around is to browse to the very large 'CopiedParts' directory and insert the part from there. Do I have any other options?
The problem you are having is not releated in any way to not having PDM/Works. I believe what is happening for you is that you are always using the default location for copied parts everytime you create a copy of a toolbox part. I'm assuming this is the "Copied Parts" folder near your toolbox directory. When you create copies of parts, toolbox (by default) names the file automatically for you and places it in the locaion that is specified under Toolbox(Menu) ... Browser Configuration ... Document Properties - Copy Directory. The defualt file name that toolbox assigns to the part is based on its description. If you try to create another copy of a geometrically equal part, toolbox tries to assign the same file name. At this point toolbox informs you that the copied part is the same as the one already created - really its just because you are trying to save the file to the copied folder and a file with that name already exists. Part of our standard here is that every SolidWorks file gets named by its part number. So for us, we just rename the file once it has been created to a valid company part number. That way we can create geometrically equal copies with different part numbers, etc.. because they are separate files with different file names. Also, I always am changing the location of the copy directory that I mentioned earlier. I change the location so the copied toolbox part is located in the same folder as the project that the assembly I am working on is in. It makes organizing files easier in my minds eye. Just click the browse button in the document properties box of the toolbox configurator and pick a new location - its easy. One side note, is that if you are creating copies of parts, then you can specify the file name by filling out the configuration name in the dialogue box for creating toolbox parts. I tried it and it works great. This saves you the hassle of renaming the part - an extra step. Try this - create a toolbox copy of one of its parts. Let toolbox name it for you. Then create the exact same part, but this time fill out a configuration name other than the one supplied by toolbox - try something that you know doesn't exist, like "stupid test part". You should be able to create the geometrically equal part. Hope this helps. Let me know.
Thanks for the confirmation and additional information. I guess I will be putting in an enhancement request to enable material properties to be associated to configurations.
I often wonder how many warm bodies they have at SolidWorks that have actually designed real parts in a real world environment? It seems like a fundamental requirement to be able to use varying types of materials for the same components? I hope some pro-active, insightful person at SolidWorks reads this thread and takes the initiative to fix this issue.