59 Replies Latest reply on Jul 25, 2017 11:04 AM by Jim Steinmeyer

    Using Toolbox: Do or Don't?

    Samuel Leith

      Hello dear SW fellows,

      we are currently running SW 2012 (expired maintenance). We are re-enabling our maintenance and will update to SW 2014, latest SP.

       

      We experienced many problems in the past with the SW toolbox, such as the 'big screw' issue, and others.

      Also, I have read in the past dozens of posts of people having problems with the toolbox, especially when it came to the following:

       

      - Updating: problems when updating SW.

      - Sharing assemblies: problems either when sending assemblies with toolbox parts, or opening assemblies coming from a different company with a different toolbox installation.

      - Performance: large toolbox file size

       

       

      These are definitely all cons, but I am wondering if in 2014 the toolbox is better than it was in the past?

      At this time, we are downloading hardware 3D files from McMaster, and creating our own library. This works very well, but is extremely time consuming to build.

       

      I would love to use the SW toolbox, if I knew for sure it would be stable and problem-free; especially considering it has much more than screws and nuts, like retaining rings, bearings, etc etc.

       

      Also, at this time we are not using any PDM, but upon updating to SW 2014, we will also install Workgroup PDM.

      I assume we could place the toolbox in the WPDM, and only have to manage one toolbox for all users, correct?

       

      I look forward to hearing your opinions.

      Are people still manually building their own libraries, or is the toolbox more reliable now?

       

      Thank you.

        • Re: Using Toolbox: Do or Don't?
          Jamil Snead

          In my opinion the toolbox sucks and keeping your own library of hardware is better. At my company they used to use a common toolbox located on a network drive and I convinced them to start using our own standard parts library. Here's what I don't like about toolbox:

           

          1. In my experience inserting toolbox components is always slow, like it takes a few seconds for the component to load. Changing settings on a toolbox component (like changing the length of a screw) is laggy, and even just trying to select an edge or face of a toolbox component for mating causes a couple second delay (which doesn't sound like much but it's super annoying). This may result from the toolbox being on a network location.

          2. There are no material options for toolbox parts, so if you use steel screws in one place and stainless screws in another there is no way to differentiate them.

          3. It is a pain to set up custom part numbers and descriptions for toolbox components (and again you can't have different part numbers for material options).

           

          What I have set up is a standard library of parts that are located on a network drive and if you set it up in your design library then it is just as easy to pull parts from as toolbox (only faster). Plus you can have different files for whatever variations on the hardware you want (like different materials). For example, with a simple socket head cap screw I have a unique part file for a given Head style, material, finish, and thread size, and then in that part file I set up a design table to create configurations for each length option. I used a McMaster model as a starting point to create each model.

           

          So in my design library it looks like this (I don't know why one of the icons is messed up):

           

          hardware.PNG

           

          If you wanted fewer files you could consider using configurations to select thread size and length, which would create way more configs in each file but fewer files. Setting up the library is a lot of work up front, but I think it makes things much better down the road (especially for BOMs). You can have the files named whatever you want, you can have whatever custom properties you want in the files, and you can have your own internal part numbers show up on the BOM. Having the components in a network location hasn't caused any lagging for me like the toolbox components have.

           

          Even for other components like bearings and retaining rings we use our own library, but I only create them as needed, not all upfront. For example with retaining rings I have one file for each retaining ring type, material, and finish and use configs for the different size options.

           

          rings.PNG

           

          Using your own design library works great with PDM too (we use Workgroup PDM). You can identify the location for your standard library and disable revision control of them. So they will still be kept track of regarding where used and such but users won't check them in and out, they stay on a network location. I don't know if that makes any sense to you but in short using a custom library does work well in combination with WPDM.

           

          That may have been too much info but hopefully it helps you decide.

            • Re: Using Toolbox: Do or Don't?
              Kevin Godfrey

              I have different materials for my Toolbox components, as well as different BOM part numbers and descriptions. I think your speed issues might well be having a networked Toolbox.

               

              And for part numbers I export to Excel, use formulas to create part numbers and descriptions and re-import. It's quite fast and easy.

              • Re: Using Toolbox: Do or Don't?
                Jody Stiles

                My response to your concerns in red, below.

                Jamil Snead wrote:

                 

                In my opinion the toolbox sucks and keeping your own library of hardware is better. At my company they used to use a common toolbox located on a network drive and I convinced them to start using our own standard parts library. Here's what I don't like about toolbox:

                 

                1. In my experience inserting toolbox components is always slow, like it takes a few seconds for the component to load. Changing settings on a toolbox component (like changing the length of a screw) is laggy, and even just trying to select an edge or face of a toolbox component for mating causes a couple second delay (which doesn't sound like much but it's super annoying). This may result from the toolbox being on a network location.
                Toolbox was re-architectured in 2012 resulting in dramtically faster loading and editing times.  The data driving the Toolbox components was previously contained in an Access database file it is now contained in the part itself.  When was the last time you used Toolbox?  Was it still slow post-2012?

                2. There are no material options for toolbox parts, so if you use steel screws in one place and stainless screws in another there is no way to differentiate them.
                As noted elsewhere in the thread, you can add Custom Properties to Toolbox components and choose whether or not each Custom Property will generate a new configuration.  You can also tie a custom property to the Materials library so that it carries all of the mechanical properties with it.
                Custom Properties.png

                3. It is a pain to set up custom part numbers and descriptions for toolbox components (and again you can't have different part numbers for material options).
                As noted elsewhere, you can use the Import/Export menu to work with Excel to generate your Part Numbers, Descriptions, Comments, and Custom Properties.  If the Custom Property containing the material is set to create a new configuration for each option, you can set a Part Number, Description, and Comment up for each configuration.

                Import-Export.png

                What I have set up is a standard library of parts that are located on a network drive and if you set it up in your design library then it is just as easy to pull parts from as toolbox (only faster). Plus you can have different files for whatever variations on the hardware you want (like different materials). For example, with a simple socket head cap screw I have a unique part file for a given Head style, material, finish, and thread size, and then in that part file I set up a design table to create configurations for each length option. I used a McMaster model as a starting point to create each model.
                Toolbox has three modes of file creation: Configurations (this adds a configuration to the master part file when a variation is used), Create parts (this creates standalone files for each variation), and a hybrid mode of Configurations and Create parts (Using CTRL while dragging a component in will create a standalone part)

                 

                So in my design library it looks like this (I don't know why one of the icons is messed up):


                <image removed>

                 

                If you wanted fewer files you could consider using configurations to select thread size and length, which would create way more configs in each file but fewer files. Setting up the library is a lot of work up front, but I think it makes things much better down the road (especially for BOMs). You can have the files named whatever you want, you can have whatever custom properties you want in the files, and you can have your own internal part numbers show up on the BOM. Having the components in a network location hasn't caused any lagging for me like the toolbox components have.
                As noted above, you can add Custom Properties, assign your own Part Number, Description, and Comment as well as choose to create configurations or standalone parts.  You can customize the file names to your liking from within Toolbox Settings. 
                I'm curious what BOM functionality you are getting from the custom parts that you can't get from Toolbox.  Can you elaborate on this?
                Naming Customization.png

                 

                Even for other components like bearings and retaining rings we use our own library, but I only create them as needed, not all upfront. For example with retaining rings I have one file for each retaining ring type, material, and finish and use configs for the different size options.

                 

                <image removed>
                 

                Using your own design library works great with PDM too (we use Workgroup PDM). You can identify the location for your standard library and disable revision control of them. So they will still be kept track of regarding where used and such but users won't check them in and out, they stay on a network location. I don't know if that makes any sense to you but in short using a custom library does work well in combination with WPDM.
                True, WPDM is not ideal for handling Toolbox but it works well with EPDM and without any PDM (you can leave Toolbox external to WPDM without any issues) as it has its own permissions and settings.

                 

                That may have been too much info but hopefully it helps you decide.

                 

                - Jody

                  • Re: Using Toolbox: Do or Don't?
                    Jamil Snead

                    Thanks for that explanation Jody. It sounds like there have been a lot of improvements since I looked into it last. FYI we were on SolidWorks 2012 when it was all laggy like I described. We just upgraded from 2012 to 2014 recently but I haven't tried it since then. I suspected that it might have been because each part file has hundreds of configurations since it is one file for all sizes of a given type of hardware. You mentioned that you can have one file for each specific configuration so I wonder if that would make it perform better.

                     

                    I knew that you could set custom properties for the toolbox component but I didn't know about that option to create a new configuration for each option of a given parameter. That sounds like a good way to handle materials (but still that just multiplies the number of configs you have for a given file).

                     

                    Also I didn't know about that import/export for the custom properties, I thought you had to enter the properties in the toolbox manager. Importing from excel sounds way easier, so disregard my comment about the difficulty of adding custom properties.

                     

                    The BOM functionality I was referring to was just having internal part numbers and descriptions be able to show up, so that can be disregarded too.

                     

                    So after reading all that the only thing that would make me still shy away from toolbox would be if it is laggy. That alone is was annoying enough to make me want to use our own custom library. I'll give the toolbox a try next time I'm in the office and report on how it performs.

                     

                    The only other minor thing that I don't like about the toolbox is that the schematic threads are circular instead of helical, whereas our screw models in our custom library out of have helical threads. We make drawings for our hardware so I prefer the screw on the drawing to have threads that look right. Also the chamfer on the top of the SHCS looks large. But those are minor complaints and that alone wouldn't make me reject toolbox.

                      • Re: Using Toolbox: Do or Don't?
                        Jamil Snead

                        I tried out the toolbox again, and it is still slow for me. When I inserted a screw it took about 10 seconds before the Configure Component dialog came up on the left. After selecting the size it was another 3 seconds to OK out of it. When I want to move or mate the toolbox fastener clicking an edge works nice and fast, but if I select a face I get a 4-5 second delay before I can do anything else (I think it has something to do with the weird green arrow that pokes out the bottom of the screw when a face is selected). This is why I hate using the toolbox.

                         

                        It may have something to do with the fact that the toolbox is on a network drive, but this whole discussion is about adding custom properties and specially configuring toolbox, so I don't see how that would make any sense unless the toolbox was on a network location where everyone could access the same library.

                          • Re: Using Toolbox: Do or Don't?
                            Jody Stiles

                            Hi Jamil,

                             

                            Thanks for testing it out. 

                            1. Does the fastener you are inserting have a lot of configurations in it?  The more configs it has, the slower it'll be.  It's just the nature of the configuration beast. 
                            2. If you change to Toolbox Settings option from Create Configurations to Create Parts or Create Parts on CTRL-Drag does the performance improve after the first use? 
                            3. If you move the Toolbox to your local computer, does the performance improve?

                             

                            I appreciate your time in testing this out if you can.  If it's too much effort to do so, please don't worry about it.

                             

                            Jody

                              • Re: Using Toolbox: Do or Don't?
                                Jamil Snead

                                Hi Jody,

                                 

                                1. The screw I originally tried has 61 configurations in it. I tried with another screw that has only 2 configurations and the delay is 5 seconds for the Configure Component pane to come up, no noticeable delay when I ok out of it on a size that already exists, and a 2 second delay when I select a face.

                                2. If I change that setting will it immediately break every toolbox component into different parts for each configuration that is already present, for example will it create 61 parts for that screw alone right when I change the setting? Or does it only take effect for new sizes created after the change is made? There are a couple people here who still use the toolbox for non-production projects so I don't want to change anything that might mess them up.

                                3.  I don't have a toolbox installed on my local computer so that is not easy for me to try out right now. But I can try at home on my laptop with a local toolbox and let you know how that performs if you want.

                                  • Re: Using Toolbox: Do or Don't?
                                    Jody Stiles

                                    Hi Jamil,

                                    Jamil Snead wrote:

                                     

                                    Hi Jody,

                                     

                                    1. <snip>.

                                    2. If I change that setting will it immediately break every toolbox component into different parts for each configuration that is already present, for example will it create 61 parts for that screw alone right when I change the setting? Or does it only take effect for new sizes created after the change is made? There are a couple people here who still use the toolbox for non-production projects so I don't want to change anything that might mess them up.
                                    Changing the setting will create a new file the next time you drag a component into an assembly or if you edit the definition of an already assembled component.

                                    3.  I don't have a toolbox installed on my local computer so that is not easy for me to try out right now. But I can try at home on my laptop with a local toolbox and let you know how that performs if you want.


                                    Thank you for testing this.

                                      • Re: Using Toolbox: Do or Don't?
                                        Jamil Snead

                                        I changed that setting and I still encounter that delay for the Configure Components panel to appear (10 seconds for the screw that already has a lot of configs and 5 seconds for the screw with 2 configurations). Note that I also get this same delay if I right click and edit toolbox component if I want to change the size. Comparing this to my current method with a custom library, all I have to do to change a screw length is change the configuration (since every length option is created up front easily in a design table). If I want to change the screw thread then I need to do a replace component, so admittedly that probably takes longer than the toolbox with delays.

                                         

                                        When I created a new size and it took 14 seconds to create the new part and allow me continue (I set the location to save new parts to a network folder).

                                         

                                        With that new part if I click on a face I still get a 3 second delay before that green arrow pops up and I can do anything else. I discovered this delay only happens if I left click on a face (for example to move the component). I thought it happened when mating too, but it doesn't. I guess I thought that because I usually mate by selecting the entities first and then creating a mate, rather than starting a mate first and then selecting the entities. Also if I right click the delay is only about 1 second.

                                         

                                        Now I changed the location to save the components to a local folder (but the toolbox is still located on a network drive). I still get the delay for the configure component box to appear. Interestingly the delay is still 10 seconds even if I right click on one of the newly created parts that has its own file with 1 configuration, maybe because it stemmed from a file that originally had 61 configurations? The delay when clicking on a face is still there.

                              • Re: Using Toolbox: Do or Don't?
                                波 李

                                嗨,我可以向你请教一些关于 toolbox自定义属性的问题吗???

                                我怎么联系您?你有QQ 吗 ?? 多谢

                            • Re: Using Toolbox: Do or Don't?
                              Roland Schwarz

                              The most effective/least backfiring use of Toolbox I have seen is to use Toolbox to generate the 3D fastener model, then break it free from Toolbox (save as an independent part).  Otherwise, Toolbox just seems to be a perpetual source of broken or missing components.

                                • Re: Using Toolbox: Do or Don't?
                                  Glenn Schroeder

                                  Roland Schwarz wrote:

                                   

                                  The most effective/least backfiring use of Toolbox I have seen is to use Toolbox to generate the 3D fastener model, then break it free from Toolbox (save as an independent part).  Otherwise, Toolbox just seems to be a perpetual source of broken or missing components.

                                   

                                  +1 for me.  This is what I've done.  And just to clarify, when Roland said "break it free from Toolbox (save as an independent part)", I'm assuming he meant to also remove the Toolbox designation.  If he didn't, then I'll add that recommendation.

                                    • Re: Using Toolbox: Do or Don't?
                                      Samuel Leith

                                      Given the fact that issues we had seen in the past with Toolbox don't seem to all be fixed, I think this is what I might end up doing as well.

                                       

                                      A few questions regarding using the Toolbox to create the CAD and then breaking it from the toolbox:

                                       

                                      -Do you use one file per bolt and then set up configurations for each length?

                                      -Do you know if the Matching Cosmectic Thread folder for Interference Detection works?

                                       

                                      From your experience, any best practises that I should follow if taking this route?

                                      I guess I would install the toolbox locally on my computer only and create the hardware files and then upload them to the WorkGroup PDM for all to use.

                                        • Re: Using Toolbox: Do or Don't?
                                          Glenn Schroeder

                                          Samuel Leith wrote:

                                           

                                          Given the fact that issues we had seen in the past with Toolbox don't seem to all be fixed, I think this is what I might end up doing as well.

                                           

                                          A few questions regarding using the Toolbox to create the CAD and then breaking it from the toolbox:

                                           

                                          -Do you use one file per bolt and then set up configurations for each length?

                                          Yes.  One file for each size bolt (1/2, 5/8, etc.), with configurations for lengths.  And I don't try to include every possible length, just add as needed.  The same with washers (Flat, Hardened, and Lock) and nuts (Hex, Coupling, and Jam).

                                          -Do you know if the Matching Cosmectic Thread folder for Interference Detection works?


                                          No, I don't.

                                          From your experience, any best practises that I should follow if taking this route?

                                          I guess I would install the toolbox locally on my computer only and create the hardware files and then upload them to the WorkGroup PDM for all to use.


                                          We don't use PDM here, so I'm not qualified to answer that.  I've saved ours to our network library and generally copy them to the project folders as needed, so what you've described should work fine.
                                            • Re: Using Toolbox: Do or Don't?
                                              Samuel Leith

                                              And how do you handle different materials?

                                              Right now I do one file per size bolt per material, with configurations for lengths. So a 1/2 grade8 bolt is a different file from a 1/2 18-8 bolt.

                                               

                                              Just curious to see what people are doing...

                                              • Re: Using Toolbox: Do or Don't?
                                                Jamil Snead

                                                We use one file for each size bolt in a particular material, and use configs for lengths. So we'd have a file for 1/4-20 SHCS Steel Black Oxide, another file for 1/4-20 SHCS Stainless Steel, another file for 5/16-18 SHCS Steel Black Oxide, etc. There aren't that many length options that bolt come in, so I just create every length up to some limit I think is reasonable, for example for a 1/4-20 screw I might only make configs up to 2" long initially and add longer as needed. If you make the files for one material first then you can just copy them and all you need to change is the material property to make the other material files.

                                                 

                                                With regards to PDM, I don't think you need to bother checking them in. What works great for us is to put the files on a network location that everyone has access to and have all the users set that location as a Design Library. Then the parts will show up alongside the toolbox in the design library tab. Then in your Workgroup PDM options you can disable check-in of standard library files (because you probably don't need revision control of them).

                                        • Re: Using Toolbox: Do or Don't?
                                          Samuel Leith

                                          Getting 3D files from Mcmaster and create a length configurations is exactly what we're doing right now.

                                           

                                          It's just that on paper, the toolbox looks so great. Since we're about to update, I wanted to explore the possibility of finally using it in a production environment. From what I see, it looks like the majority of people are still building/using their own library, and are pretty much avoiding the toolbox. At best it looks like the toolbox is sometimes used to generate the 3D files, but not much else.

                                           

                                          It's a shame - I was hoping to hear that the toolbox was a reliable tool and that we should get started with it....

                                            • Re: Using Toolbox: Do or Don't?
                                              Glenn Schroeder

                                              Samuel Leith wrote:

                                               

                                               

                                              It's a shame - I was hoping to hear that the toolbox was a reliable tool and that we should get started with it....

                                               

                                              It's possible that you've only heard from the vocal minority that don't like it, and it may be better in recent releases, but there were several issues a year or two ago that made me abandon it.  You may like it if you give it a shot.

                                              • Re: Using Toolbox: Do or Don't?
                                                Jody Stiles

                                                Issues we had in the past drove companies to create their own libraries of parts.  We have made and continue to make strides every year to enhance Toolbox to better meet our users' needs.  You might want to investigate it for yourself and talk with your VAR about any concerns you might have.  Every situation is different and what doesn't work for one may not be an issue for another.

                                                  • Re: Using Toolbox: Do or Don't?
                                                    Joe Vinciguerra

                                                    Since we started using Toolbox in 2010 we've had some really frustrating issues with hardware resizing. I've added some of my favorite examples at the bottom. It seems completely random, and we've had CADimensions try to help multiple times over the years without any improvements.

                                                     

                                                    Things we've tried (including but not limited to):

                                                    • local toolbox location
                                                    • shared networked toolbox location
                                                    • starting with a fresh toolbox install
                                                    • verified reference points to correct toolbox location
                                                    • sent VAR cad files for evaluation
                                                    • changed read-only file and folder attributes through windows user permissions
                                                    • We keep up to date with service packs and version releases.

                                                     

                                                    This happens with older assemblies, all the way up to stuff created within the last couple months ago. It happens when opening a local assembly, it happens when opening from PDM, it happens when suppressing then unsuppressing hardware, it happens with small assemblies containing only a few bolts, it happens with large assemblies containing a thousand bolts, it happens to only some bolts in an assembly. It makes smaller hardware bigger, it makes bigger hardware smaller . . . to sizes we don't even use. But it does not do it every time!

                                                     

                                                    When it goes unnoticed in engineering (which can easily happen on some of the more complex machines we design), and moves into production, the Production Manager is up in Engineering screaming "Why would you specify an M3 screw for an M20 hole!?!)

                                                     

                                                    And it's been a known issue for several years according to my VAR and this post: https://forum.solidworks.com/message/183386#183386

                                                     

                                                    If there is a solution that I'm not aware of, please let me know. Else, I'd like to know if there are any plans to fix this.

                                                     

                                                    (Another problem that arose from networking the toolbox . . . upgrading is a pain the butt because of write access with multiple users. Again, no good suggestions from tech support at this point)

                                                     

                                                    BoltResizing_RB.jpg

                                                    screenshot.png

                                                    washers.jpg

                                                    • Re: Using Toolbox: Do or Don't?
                                                      Richard Wagenaar

                                                      We want to give a number to any standard part with configurations.

                                                      The number is in the Solidworks partfile name.

                                                      We make our standard parts with design tables.

                                                      But after SW2006 there is no "save last used configuration" anymore.

                                                      This has caused us hundreds of hours additional work and

                                                      design time for large projects have decreased dramatically.

                                                      We design a lot of machines consisting of standard parts.

                                                       

                                                      Suppose I insert a bearing (with all configs in it) with name 

                                                      for example 25#deep groove ballbearing and  config=6002

                                                      This part number 25 is used for example 20 times in 10 different subassemblies.

                                                      But after the bearings have been inserted, we decide that the bearing should be bigger,

                                                      suppose it should be 6004 instead of 6002.

                                                      Till SW2006 we would have all the standard parts to set "save last used configuration"

                                                      and it was 1 mouseclick to update part 25 in every assembly.

                                                       

                                                      But after SW2006 a name of a part is not unique for it's configuration anymore,

                                                      which not only needs you to search for 20 parts in different assemblies and changing

                                                      the configuration each seperately but it also causes a lot of mistakes.

                                                      The number of mouseclicks to do these simply things (before SW2006) 

                                                      have easily increased 10-100 times more.

                                                       

                                                      This is one of the biggest inefficiencies we have in Solidworks after SW2006

                                                      when using standard parts with configurations.

                                                      I never understood why such a time, mouseclicks and error saver simply has been removed.

                                                       

                                                      Does Toolbox fix these problems?

                                                      We have many parts with configs that are not in toolbox like motors, 

                                                      pneumatic cilinders all kinds of non standard bearings etc etc.

                                                       

                                                      If Toolbox could fix the problems that were introduced after SW2006 with

                                                      discontinuing "last saved configuration" then it would make sense for us.

                                                        • Re: Using Toolbox: Do or Don't?
                                                          Jamil Snead

                                                          Jody has explained that you can configure toolbox to save a separate file for each configuration. Is that what you are talking about? So that if you want to change all instances of a fastener you can do a replace component instead of configuring each individual instance?

                                                            • Re: Using Toolbox: Do or Don't?
                                                              Richard Wagenaar

                                                              I think that is far too much work also.

                                                              We are thinking about making an external database

                                                              with the designtables that recognizes the part and allows

                                                              you to change to another standard size. A kind of VBA

                                                              application should change the dimensions of the existing part.

                                                              The problem is you can't change the current configurationname

                                                              which now is the part list info for us.

                                                              25 years ago we had a German Autodesk application called

                                                              Genius, they did it the same way in Autocad. When you edited

                                                              a standard part it recognized the part and showed the sizes

                                                              according to DIN/ANSI or your own standard.

                                                               

                                                               

                                                              Changing a named part to another size that has been used

                                                              several times should be easy as it happens so often.

                                                              It was so easy and logical before in SW2005.

                                                               

                                                              In SW2005 I opened the part with the configurations and

                                                              changed the configuration and all instances were automatically

                                                              changed of that standard part.

                                                              In the menu (see picture) there was a checkbox 

                                                              "Use component's "in use" or last saved configuration"

                                                              This is how it should be as a named (numbered) standard part is

                                                              unique, you should never have parts with the same file name and

                                                              different  sizes driven by configurations.

                                                               

                                                              I can't believe why they broke it and never fixed it.

                                                              Why does Solidworks remove such usefull options.

                                                              Maybe they broke it to sell us Toolbox??

                                                               

                                                              Anyway, there is no way Toolbox can fix what has

                                                              been broken after removing this usefull option.

                                                              "Use component's "in use" or last saved configuration"

                                                               

                                                               

                                                               

                                                               

                                                               

                                                              Use last saved configuration SW2005.JPG

                                                                • Re: Using Toolbox: Do or Don't?
                                                                  Jamil Snead

                                                                  They probably took away that option because it led to a lot of mistakes. Let's say you used that option for all of your bearings in an assembly. Then later you want to add a new size to the bearing, suddenly that new size is the last saved configuration and all of your bearings changed to that one without you knowing about it. I don't even know what the "in-use" configuration means. What if you are using several different configurations of that part in the same assembly. Which one is the "in-use" configuration?

                                                                    • Re: Using Toolbox: Do or Don't?
                                                                      Richard Wagenaar

                                                                      In use means the last saved configuration of this part.

                                                                      So how it looks while you open the part.

                                                                      You could have different sizes with the same partnumber in

                                                                      SW2005 too like it is now but we find that very tricky.

                                                                      When you want your part to behave "unique"  you choose

                                                                      this last saved option in the assembly where it is used.

                                                                      If you don't want that you don't set this option. It was

                                                                      much more flexible.

                                                                       

                                                                      If your bearing has the same filename it should be the same size everywhere

                                                                      in that machine for us.

                                                                      We always have a unique filename for one size of the bearing.

                                                                      A bearing starts with a number in the filename for us.

                                                                       

                                                                      What you explain with the mistakes is what is happening for us now

                                                                      without this option.

                                                                      We also have parts that we don't give a name,  for example a simple

                                                                      washer or bolt.  In that case we don't use a number for that part

                                                                      and we do not use "save last configuration".

                                                                       

                                                                      We use the numbers to have them unique. They are in stock under

                                                                      a certain number and the easiest way to manage it is by starting the

                                                                      part file name with a number. 

                                                                       

                                                                      Of course everybody has their own ways of managing part names,

                                                                      after learning from the mistakes we did it like I explained.

                                                          • Re: Using Toolbox: Do or Don't?
                                                            Theresa Ouderkirk

                                                            This is a long post. But in evaluating Toolbox I thought sharing our company’s process and discoveries story may help future users make the decision for themselves. Please note, we are using Solidworks 2013 and are about to update to 2014 now that most of the initial patches have released. And the problems we ran into may not pertain to your situation.

                                                             

                                                            We are trying to create standard operating procedures for our growing office and have been evaluating between the following methods as options for fastener addition to assembly models:

                                                            1) Toolbox

                                                            2) Design Tables in the Design Library

                                                            3) Separate Folder of individual Fastener Files

                                                             

                                                            Option 3 is what our company has had for years and has worked fine, but we want to try to increase efficiency and get everyone to use the same methods? So, we continue the evaluation.

                                                             

                                                            Option 1 is used by some of our engineers who have loved it, but it hasn’t historically been matched to our part numbers and they have to look up our inventory listing to ensure they are using options we have in stock if at all possible. So this process has been slow out of the box.

                                                             

                                                            Option 2 is new to us and seems to be working really well, but to replace fasteners, even with the built in “replace” option, you have to dig deep into the design library source files to choose the replaceable part, if it isn't already a configuration of the part that was originally chosen from the design library. It would be great if the design library had a replace function of its own to save time by avoiding this digging function, but we haven’t seen that yet.

                                                             

                                                            OUR COMPANY: When entering a fastener into our assembly models, we want our engineers to first try to find a fastener that would work from within our inventory, that we purchase on a regular bases, before creating the need to purchase a new fastener we don’t normally carry. We don't want to start purchasing a new fastener for their designs if we have something close that would work just fine. Our reasoning is that we want to purchase in bulk. However we sell and produce custom products. To increase efficiency, we are trying to avoid having to purchase one or two of any fastener for a product we will be producing once or twice a year. A whole bunch of this will get costly fast, so we limit the new designs so we can stick to some basic standard hardware. When creating designs, our engineers start with need and size then work with the BOMs later after the design is complete. So picking from our inventory, they choose size first, then list the part numbers later.

                                                             

                                                            OUR EXPERIENCES: In trying to get Toolbox to work for our purposes, we have played with Toolbox a bunch and have spent many hours on the phone with our support team learning how to customize toolbox and adjust it for our needs. Never at any point did we go behind the scenes and manual manipulate any models or any tables. We only worked through the existing functionality of the Toolbox Configurator.

                                                             

                                                            We have used the import export tool to enter all of our regularly purchased parts. We copied all the hardware models we could find into a single folder so we could eliminate searching for parts within the toolbox. We have created custom properties and have utilized the material choice options.

                                                             

                                                            LESSON ONE: One large learning curve we went through is to find how to avoid broken toolbox links. OUR CHOICE: As a result we have chosen to create toolbox configurations instead of individual parts. WHY WE CHOSE: When saving individual parts, it actual separates the parts from Toolbox. Toolbox will recognize the separate files, but will no longer manipulate them from the Configurator. Thus if we want to add or remove a custom property in the future, it would no longer recognize the individual files, because it would not know with which of the new property options it is associated it. Or, if you removed a property, it may have previously created a separate model for each of the property options that are now null and void and it doesn’t know which model to use, so it doesn’t use any of them. This resulted in a lot of broken links and miss identified fasteners.

                                                             

                                                            We even tried the “duplicate part numbers for geometrically equal components” option to try to create multiple materials, but the same problem was created where the parts were technically no longer recognizable to Toolbox if we updated property options later. This also added a few other weird side effects that I am not remembering in detail enough right now to list.

                                                             

                                                            LESSON TWO: We did however find that updating properties was possible without losing all of your previously inserted data. You simply have to:

                                                            1. 1) Export the data you entered BEFORE changing the property options into excel. If you have a lot of properties chosen, the can take a really long time. Now you have the data safe in a Toolbox friendly format.
                                                            2. 2) Then, change the properties in the Configurator to what you want them to be and export the new excel table (which at this point is likely to be empty of your data depending on the changes you made, so EXPORTING your data BEFORE MAKING CHANGES is VERY important),
                                                            3. 3) Then either change the table with your data to match the new empty table format, and fill in any new data to match the new format. Or, move your data to the new table and add in any new information in the new columns.

                                                            It wasn’t a fast process, but it did allow us to NOT LOSE our previously entered data.

                                                             

                                                            LESSON THREE: We also went through a lot of searching to find out that Toolbox does NOT have models for several of the Imperial Standard hardware that we use regularly. I can find just about any fastener model we could want in metric, but can't find toolbox models for Nylock Nut, Nylock Nut Thin, or Toplock nuts with standard imperial measurements. We also cannot find a model for Clevis Pins that gives what we thought were standard combination options of diameter and length. All of these things we purchase regularly from the standard options listed online for sale to the public from large fastener vendors such as McMaster Carr.  These are fasteners that can be found in any hardware store here in the mid-west (Kansas). It doesn't make sense to us why these options would not be available, but have had to forfeit some toolbox usage to method options 2 and 3 above, right from the start, because of these omissions in Toolbox. There are several other “Standard” fasteners that are missing, but we purchase them on a rare enough basis that having a separate file for them wasn’t that big of a deal.

                                                             

                                                            Still we pushed forward to see if toolbox could possibly save us time with just the fastener models we need that ARE available in Toolbox. So we continued to set up toolbox for our use and trials.

                                                             

                                                            OUR CURRENT STATE and PROBLEM:

                                                            We now have everything set up with all of our standard hardware (those we could find a model for in toolbox) and were testing through it to see if it would actually run the way we want it to. Now we are running into another problem.

                                                             

                                                            BACKGROUND TO UNDERSTAND OUR CURRENT PROBLEM: Our part numbers were added to fasteners in number order of need. So as we needed a new fastener, it got the next consecutive number. So, if we ordered our fasteners by size, their part numbers would not be consecutive and vise versa; if we ordered the fasteners by part number, the fastener sizes would be all over the place and not in order. This causes toolbox efficiency problems as follows:

                                                             

                                                            When we add a toolbox part, it first auto inserts according to the hole size in the model, which is great. But, if we want to add a different nut size (Nylock nuts are larger), we may need a longer bolt. We can simply choose a different size in the properties box, which is also great.

                                                             

                                                            However, with all of the information and part numbers we have imported into Toolbox, it doesn't narrow the options by only that information. For example, all length options are available whether or not we have a part number associated with them or not, because it is filled into our matrix.

                                                            NOTE: Example: When narrowing down the options by unchecking them in Toolbox Configurator, if you want a single odd ball bolt length, then it must be available for ALL possible property combination of that bolt size. So if we want it to be available for only Stainless steel material, half inch diameter, then it will available for every other Half inch diameter bolt in every other active (with check mark) material listed in the materials property option. Causing an exponential number of options to choose from, every time you add a property. We have narrowed the properties options in Toolbox Configurator by un-checking as many as we could.

                                                             

                                                            Toolbox will list in a window sorted by Part Number all of the parts you imported. But, even after narrowing down their options by un-checking them in Toolbox Configurator so they are not available for the picking, our engineers still have thousands of combinations available to choose from. When they choose a combination of properties form the dialog box, the only way they can tell if they have chosen one of the couple hundred fasteners that we entered data for (our inventory) is by lucking out and choosing the exact properties combination of one of them. At that time, Toolbox will highlight the fastener of choice in the Part number window. But, it won’t scroll to it, so they may not even know it is highlighted. Toolbox will also not narrow down the options in the part number window, so they can pick one of the imported options listed that may be close to a size we have in inventory. They are essentially blind to the information we entered until it has been entered and accepted. OR, they can scroll through the several hundred options we did import, which would be great if they were looking for a specific part number, but they are looking for a size. And as mentioned before our part numbers are not consecutive with size, so the sizes are listed randomly because this list is only sorted by Part Number. 

                                                             

                                                            IN SUMMARY: Our engineers cannot tell via toolbox which of the toolbox property combination we actually did import into Toolbox, and thus cannot tell if we carry the part in inventory or not. At best it’s a crapshoot to pick one of a few hundred out of several thousand options.

                                                             

                                                            So this turned out to be quite the conundrum for us.

                                                             

                                                            It would be very helpful if toolbox would narrow down the visible options in the Part Number window as properties are chosen from the dialog box. Even if it narrowed it down by diameter or length, it would be a huge time savings.

                                                             

                                                            This detail of Toolbox is such a pain that we are thinking of forgoing toolbox all together. I spoke with our helpdesk and they said that Toolbox simply can't pull information in that direction to narrow down the list. It pulls information from the other direction to simply provide the list of the imported data in order of part number. We already have lists of this information, importing it into toolbox to list it, in a not so helpful sort order, did not improve things for us at all. And the list that Toolbox shows is much less user friendly than the excel sheet we started with. At least with the excel sheet they can sort the list.

                                                             

                                                            Toolbox for our engineers is suppose to help them work from the design and size to the part number. Making them look through the list of part numbers to find the size that is close to the one already chosen in toolbox is counterproductive.

                                                             

                                                            So we are back to the drawing board. We are probably going to start using design tables. The only problem I have found with this is in the replacement function, where we have to dig down into the design library to find the parts to replace them. And it would be nice if we could use the auto-sizing functionality that toolbox provides.

                                                             

                                                            So, I hope this helped at least one person out. And, I hope Toolbox improves in the future. But in the mean time, we are still struggling with its usability and hope something better and similar comes along soon.

                                                              • Re: Using Toolbox: Do or Don't?
                                                                Jamil Snead

                                                                That was a very good and thorough explanation of you situation. A couple of your problems might be helped by moving toward a design library of standard components instead of toolbox.

                                                                 

                                                                It seems like a common method of setting up screw files is to have one file for each combination of thread size, material, finish, and that one file would have configurations for every length option. If you set up your library in this manner then changing lengths of a screw is as easy as changing the configuration, it would not require digging around in folders. However if you wanted to change from a button head to a socket head screw, then you would need to browse for the new file. But you can set up the folder structure of your design library in a way that makes it easy to navigate to the desired files.

                                                                 

                                                                As far as helping the engineers pick common sizes, that will be difficult. The best I can think of is to only create configurations on demand. So when an engineer pulls a certain screw into an assembly, it might only have a couple size options for what you have used before. If they need a new size then they would have to open the screw file, edit the design table, add a new length and assign the new part number. I don't know if you'd trust all of the engineers to do that without messing something up. You could also have one person in charge of updating the hardware and have all engineers go to them when new sizes are needed.

                                                                  • Re: Using Toolbox: Do or Don't?
                                                                    Theresa Ouderkirk

                                                                    Thank you Jamil!

                                                                     

                                                                    Yes, we are considering all of this. We do have a design library started and it is built exactly as you explained so far. The digging into files was specifically targeted at having to change thread sizes/diameters. And as far as trusting the engineers to not mess things up, well we don't really. We love our engineers and their brilliant minds, but also acknowledge their need for speed and efficiency and tendency to skip the insigificant details that results in messy paperwork. It's not their thing, so we have a document specialist and file manager to support them, so they can continue being exactly as they are, BRILLIANT, and nothing gets mixed up, messed up, or missed.

                                                                     

                                                                    So excellent suggestions! We've choose all of them!

                                                                     

                                                                    Thank you.

                                                                    TJ

                                                                      • Re: Using Toolbox: Do or Don't?
                                                                        Theresa Ouderkirk

                                                                        Just to close our story...

                                                                         

                                                                        In the end, after much evaluation, our company has "officially" decided to go with design tables and not use toolbox at all. We feel that toolbox has too many problems, and is lacking too many basic hardware elements for it to work for us. We think it would simply slow us down instead of adding benefit. Design tables are working marvelously for us, and because it is easier to access, we can update, add, change, etc any details we feel are necessary.

                                                                         

                                                                        Thanks everyone.

                                                                        TJ

                                                                    • Re: Using Toolbox: Do or Don't?
                                                                      John Layne

                                                                      Our company has just started thinking about testing Toolbox again and found your post. Wondering have you changed your opinion of Toolbox?.

                                                                       

                                                                      We abandoned Toolbox a number of years back and went with design libraries and configurations. We did this for pretty much the reasons you detailed in your post. 

                                                                       

                                                                      We too add part numbers as needed, and prefer to use sizes we have used in the past just to keep inventory under efficient control. We have some custom fasteners (head modifications, non standard lengths and buy these in minimum quantities of 10,000). So curious as to the current state of usefulness of Toolbox.

                                                                        • Re: Using Toolbox: Do or Don't?
                                                                          Doug Dina

                                                                          I have been using SW since 1996 and am aware that TB has its issues along the way. With a properly set up backend, I find the TB extremely fast and indispensable. It is bewildering to me when I read such negative reviews of it. Drag n drop, resize, and ... BOOM! there's the exact PN. I just haven't experienced many problems with it at all since line the late 90's. There hasn't been a design I've produced in years that wasn't done using TB. I've created custom TB parts, like rivets, SEMS screws and KEPS nuts, that act exactly like all of the other TB parts. Just need to set it up properly.

                                                                            • Re: Using Toolbox: Do or Don't?
                                                                              John Layne

                                                                              Our company has about 20 current products, we ship worldwide about 50,000 units per year.

                                                                              We design in Perth, and have 2 contract factories in China.

                                                                               

                                                                              We want to limit the number of ROHS compliant fasteners in stock, saves mistakes in the factories. At a wild guess we use less than a 75 different fasteners, probably a lot less. We don't want designers unnecessarily specifying one-off fasteners when there is something close in size, in stock at the factory. To make this easy the configs with part numbers are visible, and we debate the need to add new fasteners and part numbers.

                                                                               

                                                                              Sending assemblies with toolbox parts to outside users causes issues, part numbers get deleted if the outside user doesn't have the same toolbox database. I worked as a contractor for a number of years and have sent and received many assemblies from different companies, toolbox part numbers changing in BOM's was a pain the #$!@#$. The Chinese factories don't work exclusively for us, so we don't dictate how they use Toolbox sending pack and go files with all fasteners solves all our issues.

                                                                               

                                                                              We probably could change to toolbox, but the time to update legacy assemblies and no doubt with issues with conflicting part numbers, assuming we don't instruct factories to update the fastener to new part numbers. Out PDM system setup does not allow duplicate part numbers in the vault, nor should it, so the transition would be long and painful.

                                                                               

                                                                              Our library of fasteners is in PDM Professional, which is cached on the local users PC. We simply drag and drop into the assembly with smart mates use sketch patterns if required. All similar parts are off the same base model so switching out sizes and or styles is easy.

                                                                               

                                                                              I can see the advantages of Toolbox, if all design and manufacture is in-house.

                                                                        • Re: Using Toolbox: Do or Don't?
                                                                          Robert Bartz

                                                                          This reply is old, but I thought it would be a good information to those deciding weather to use Toolbox or not.

                                                                           

                                                                          I have worked as cad administrator in 3 different establishments in about 10 years. In the majority of people I've set up with toolbox I think they would have been better off without it. In the past I have been a BIG supporter of it because I believe it is going to improve to the point of if we don't use it we wish we did. In 10 years I haven't seen anybody working in departments agree with that.

                                                                           

                                                                          1. It doesn't have all fasteners. Most "pointed" screws are missing Those come in kind of handy for places that design office furniture. Pop rivets are missing, and a deluge of other fasteners we end up creating ourselves.  So that means there are (2) places for hardware. If you use design tables and library parts in pdm, that problem goes away and you can have 1 central method. Oh yeah I have suggested several times adding these, that was several years ago.

                                                                          2. Our dept. finds it way overcomplicated so its a struggle to enforce its use. I've been at it for 8 years and am still learning things. Many design engineers are lost, and it takes a few of us to figure out simple things like adding sizes or types. We are talking guys using Solidworks for 12 years, 3, and new people good luck with that.

                                                                          3. Slow: We use pdmworkgroup, (soon to use pdm pro), and boy do our Solidworks design table fasteners work slick compared to the slow toolbox. Instead of putting everything in a centralized vault it shoots these out to a local drive (pdmworks does not recommend checking in toolbox parts). Do you see a pattern here? two different types of fasteners now we have 2 different places.

                                                                          4. Bugs& bugs. We have at least 1-2 SPR's for bugs we have found in toolbox, for stuff like unable to exclude from BOM. No problems for the old configured parts.

                                                                          5. Creates exponential configurations: If you add properties to your fasteners with different suffixes it is creating thousands of configurations for example separate property for material and finish, you have to have a configuration for every finish  every material. We are conservative on properties. Your simple design table only creates the ones you need.

                                                                          6. Confusing fastener organization such as washers. They are in categories (ANSI inch) that most never refer to including McMaster Carr & Fastenal. Plain Type B, Preferred type, even degreed engineers who have to constantly ask which category there are in or create cheat sheets.

                                                                          7. Complicated to create drawings of groups of fasteners with revisions. Our plant requires drawings of all fasteners, if those drawings change a revision is necessary. Toolbox doesn't play well with revisions or grouping fasteners together on one drawing, in pdm they are not revision managed  (the normal Solidworks is a no brainer). We ended up creating an assembly with different toolbox fasteners in it and revise the assembly which revised the drawing. Your single design table driven part is much simpler than this.

                                                                          8 I think toolbox may have its place in more of a job shop- or mechanical only shop where "pointed screws" are never used. For administration of the thing, you will need to have 1 trained guru to keep it managed or else you will have a mess. A position not necessary for simple configured parts. All that administration and troubleshooting of another "system" costs money.

                                                                          9. Toolbox is a good reference for dimensions of the parts it has, for example the hex size of a bolt or thickness of a nut.

                                                                          10. If you change properties and delete others, toolbox quickly turns into a mess. It puts suffixes on the configurations that may not relate to the old ones.

                                                                          11. Pack and goes with other SW establishments get messy because the toolbox parts are named the same thing.

                                                                          12. If your network is slow or pokey don' use it collaboratively or else it will slow down your SW. 

                                                                           

                                                                          In conclusion I think toolbox can be used as a reference or in a small job shop(mechanical) establishment. Don't use it if you make things that use wood screws, or unusual fasteners because many are not in there & don't hold your breath if you ask them to be added. Send a person to your VAR's class on this before it is even set up and make sure that person knows it inside and out. If you have a larger engineering department over 5 people this person should set the parts up or else you'll have a mess, for example its easy to create a screw configuration and forget to select full thread vs. partial thread.  Some of the tips are called out in letter codes that are difficult to know what they mean. SW has made some valiant efforts to improve this but still has a ton of work and massive simplifications.

                                                                          • Re: Using Toolbox: Do or Don't?
                                                                            S. Casale

                                                                            My experience with the toolbox (TB) is a based on annoyance.

                                                                             

                                                                            Now that it's prefaced, I can be constructive.

                                                                             

                                                                            1. TB on a standalone machine is powerful and awesome!
                                                                            2. TB on a network or Vault requires attention.
                                                                            3. If using using with PDM (Vault), it is important to pay attention to the user configured settings. Understand that if a part is inserted and custom definition in an assembly, TB, SW and the Vault will need to check out various files (.xml and etc.). In my experience this is problematic as any network hiccup, or file based hiccup - 2013 and later (my only experience with TB), and the files do not get checked back in. Users rarely look at these files or even know about them. With that, if another user (differing from the last to customize or modify during said hiccup) adds a TB item to something and attempts to modify with custom definition, the assembly will keep the custom definition even through saving it. When anyone, including the last user who last saved the file reopens, the TB item will have reverted back to whatever was the last checked in config, and no custom specification will be there-lost because the file is not checked in by someone else who didn't know they had it checked out.
                                                                            4. Using Vault, users don't know they have checked out a file and they check it in without looking at the list of items referenced during check in.
                                                                            5. States affect TB files as well.
                                                                            6. Outside of the Vault environment, TB is fun when everyone knows how to use it.
                                                                              • Downside: In the configurator, it is easy for users to accidentally create a new folders with TB standards.The downside is there is no way to query the TB for customized configurations if one or more standard is duplicated or even created (i.e. if an 1/4-20 ANSI SHCS is accidentally made in a MIL Spec TB series, the only way to know it is by opening the series. If there are a series for NAS, NASM and many more a user could lose valuable time trying to find anything among the various folders).
                                                                            7. If you modify the actual database (Access), you better have your own copy of that version (i.e. ACCESS 2016) database (I believe legally you are required to as part of the end user agreement states the DB is only for use with SW). If you don't when you upgrade you may lose vital information, or configurations, or the ability to find them in the configurator.
                                                                            8. Upgrading SW and a toolbox on a network needs proper attention. This should be done with either the Administrative Image or the first computer on a network with Toolbox.
                                                                            9. A lot of users don't know that the hole wizard is controlled by the toolbox (toolbox configurator).

                                                                             

                                                                            The toolbox, in theory is great.

                                                                            • Re: Using Toolbox: Do or Don't?
                                                                              Grant Mattis

                                                                              Wow this thread is really making me think twice about working to implementing Toolbox. I had a conversation with a VAR to discuss the positive developments since the pre 2012 toolbox and was fairly convinced the previous issues I had were fully fixed. From this thread it sounds like there are still major issues even recently. Is there anyone that is a regular user of Toolbox and that has positive things to say?

                                                                                • Re: Using Toolbox: Do or Don't?
                                                                                  Doug Dina

                                                                                  Grant,

                                                                                  I'll paste my comment above, in case you missed it. I use it exclusively all the time and never have issues with it.

                                                                                   

                                                                                  "I have been using SW since 1996 and am aware that TB has its issues along the way. With a properly set up backend, I find the TB extremely fast and indispensable. It is bewildering to me when I read such negative reviews of it. Drag n drop, resize, and ... BOOM! there's the exact PN. I just haven't experienced many problems with it at all since line the late 90's. There hasn't been a design I've produced in years that wasn't done using TB. I've created custom TB parts, like rivets, SEMS screws and KEPS nuts, that act exactly like all of the other TB parts. Just need to set it up properly."

                                                                                    • Re: Using Toolbox: Do or Don't?
                                                                                      Dennis Dohogne

                                                                                      Grant Mattis, I heartily second what Doug Dina just wrote.  We've used Toolbox for about 10 years so that spans the 2012 issue that SWX had.  That particular issue just kept us from upgrading for a few months and nothing else.

                                                                                       

                                                                                      Here is what we did:

                                                                                      1. Exported the fasteners from our ERP system into a spreadsheet to include at least the information of the part number and description.

                                                                                      2. Exported from Toolbox a spreadsheet for each different fastener type.

                                                                                      3. Using simple Excel commands such as VLOOKUP we modified the spreadsheets from TB with the matching part number and description from our ERP system.

                                                                                      4. Import this modified spreadsheet back into TB.

                                                                                      5. Repeat the process for the other fastener types.

                                                                                      6. Enjoyed the use of Toolbox by selecting OUR fasteners containing OUR part number and description to properly show up in the BOM.  Consequently this also was a shorter list of fasteners to choose from since the list is populated with only our sizes, not all that exist in the world.

                                                                                       

                                                                                      The setup/customizing of TB is actually easy once you learn how to exploit the Export/Import function.  This work is FAR less than the work involved in doing this with separate part files and configurations.  In addition the TB parts carry some nice attributes such as smart mates and a flag to include/exclude them from BOMs or other selections.  In SWX2017 they introduced a nifty new feature where you can select a bunch of TB fasteners, even of different types, and RMB to Edit Toolbox Components and change all of them at once.  What's not to like?

                                                                                       

                                                                                      In my opinion a lot of folks never took the time to figure out how to fully capitalize on TB so they went another route.  That's perfectly fine, but I did that in SWX from 1995 to 2007.  In 2007 I went to a new company and was in charge of the design and manufacturing engineering groups.  Setting up Toolbox was one of many things I did there to dramatically improve our operations.  The only way I'll NOT use Toolbox is if I am at a company that doesn't have SWX.

                                                                                        • Re: Using Toolbox: Do or Don't?
                                                                                          Dennis Dohogne

                                                                                          By the way, our Toolbox is on the network and we have no issues with it that way.  It is actually better because when we add a fastener to our ERP and then to Toolbox we only have to add it once since everyone is pointed to the same TB.

                                                                                            • Re: Using Toolbox: Do or Don't?
                                                                                              Grant Mattis

                                                                                              Doug I did see your reply above but it was one of the very few positive ones. Dennis thanks for joining in too this was what I was looking for.

                                                                                               

                                                                                              How do you have your Toolbox setup? I will be integrating/matching with a fairly massive MRP/ERP database. Do you use configurations, parts or the hybrid method?

                                                                                               

                                                                                              Dennis what you explained is what I went through with the VAR and it makes perfect logical sense to me but there are also a lot of smart people above that have had major issues. I wonder if there is something I am missing that will grind everything to a halt as I am working on it.

                                                                                               

                                                                                              If we go this route it will be setup within EPDM on the network. Hopefully once it is implemented each user can do a get latest and basically be working as if they are local files. If we ever did a major update again the users just do another get latest.

                                                                                               

                                                                                              What about adding fastener types that are not already included in Toolbox? We use a lot of standard fasteners that are in TB but we also seem to use a lot of more unusual ones. The unusual ones that we used often I would want to get them into TB as well. Have you tried this and was it successful?

                                                                                               

                                                                                              Thanks for the insight.

                                                                                               

                                                                                              Grant

                                                                                                • Re: Using Toolbox: Do or Don't?
                                                                                                  Doug Dina

                                                                                                  All I can tell you, as Dennis did better than I did, that the TB admin must learn how to configure it and add parts and that clients learn how to use this before becoming so critical of it. I wish I had the bandwidth to train others on how to fully utilize it. I wouldn't want to be without it but realize there is a lot of resistance from SW user that have not spent the time in mastering it. The same goes for any addon that a person is not familiar with. For instance, I use Routing to cable all of my assemblies. Most SW users just cringe at the thought of learning an entirely new addon like Routing, Flow, or Simulation. But, all of these are feature-rich and offer considerable power and flexibility that ultimately reduce mistakes, greatly improve efficiency, and improve product reliability. The TB, when configured properly, falls very much in line with my last comment. I just drag in a TB type in and hover over a hole or feature, and it analyzes the hole or feature and offers a size to fit it. I then pick the material type, length or whatever options are available and the PN automatically updates. I can easily drag a screw to lengthen it whereby the PN updates in the assembly tree and in the BOM. The speed is lightening fast. I can easily change types globally using the TB window. I have also added parts to the TB that do not come with it and they have all of the features of an out-of-the-box TB part.

                                                                                                   

                                                                                                  Not sure what else to say, other than one needs to fully learn how to set it up and implement it. Based on my successful experience with it at my present company, management will be forcing all clients to use it in the coming months.

                                                                                                  • Re: Using Toolbox: Do or Don't?
                                                                                                    Dennis Dohogne

                                                                                                    We have a part number standard that all our fasteners begin with a "Z".  We did a complete part number dump from our ERP then sorted by part number and pulled out into a separate sheet the fasteners.  There we sorted these by type, size, length which matches the sort order of the TB exported file.  From there it was a pretty simple method to match these sorts in order to bring the part numbers and descriptions into the TB spreadsheet.

                                                                                                     

                                                                                                    We started this operation with our VAR walking us through it and he knew his stuff.  First we found the standards that govern our fasteners and made copies of them.  We use ANSI standard fasteners so we made two copies:  Sandar (Our company name, and this one for our metric fasteners, which are dominant) and Sandar Inch for the inch sizes.  It is these libraries we customized.

                                                                                                     

                                                                                                    If you have multiple users and they are using standalone seats you can still have them pointed to a networked location of TB and this is what I recommend.  You should have two responsible folks with the password to customize TB components.

                                                                                                     

                                                                                                    We have not had any problems with TB and would not be without it.

                                                                                                     

                                                                                                    As for adding custom items to TB, I must admit that we have not had that need.  If we make a customized item from a standard fastener, such as cross drilling a hole in a screw then that is stored under its new part number and not in TB.  If you search this forum you will find others that have easily and successfully added items to their TB, but we just have not had that need so I cannot speak to that.  Your VAR should be able to help with this as well.

                                                                                                     

                                                                                                    Sometimes when you cannot find the fastener in the standard you always use it is because the part is controlled by a different standard or none at all.  Nylocks, for example, apparently are governed by a DIN standard so I just drug that folder from the DIN standard into our company folder -pretty easy!.  However, inch size Nylocks apparently do not have a governing standard so they are not in TB.  We only use a few of these.  Since they are not in TB we downloaded the few inch Nylocks from McMaster-Carr and store them in a separate directory

                                                                                                     

                                                                                                    It doesn't matter if you setup the TB parts to be configured or separate files.  You won't see any difference in speed or anything else.  If you would look in your TB directory where the files are stored you would see a big difference, but who cares.  We happen to have ours setup for configured.

                                                                                                     

                                                                                                    Just in case I didn't say this before, we have not had any problems with TB and would not be without it.

                                                                                                      • Re: Using Toolbox: Do or Don't?
                                                                                                        Steven Dod

                                                                                                        I administer SWX with roughly 20 engineers/users.  We use PDM Pro and Toolbox in the Vault with pretty good success.  Yes, we see small delays when inserting and it is not all roses trying to set up custom parts but these quirks are easily offset by the ease of use.  When 2013 changed how TB is structured it corrupted our old TB and we basically had to start over.  Since then we have very little issue with Toolbox.  Today we use configurations for each size/type/property (RH/LH, GR5 GR8) but our VAR has suggested changing this to saving the part out separately.  They believe it will help our performance with large assemblies by keeping the file size down.  Our machines assemblies contain upwards of 5000-6000 parts with a good many of those from the Toolbox.  Even if we decide to change this setting, Toolbox will still control everything and I would recommend using Toolbox to anyone.

                                                                                                         

                                                                                                        Steve

                                                                                                          • Re: Using Toolbox: Do or Don't?
                                                                                                            Grant Mattis

                                                                                                            Steven thanks for joining in too. I think I said above that the VAR suggested using parts in TB rather then configs. We have rather large assemblies as well in the same range as you plus we can go one higher step, we really try to avoid it, for 15,000-20,000 parts.

                                                                                                             

                                                                                                            Does anyone have issues with using the same TB part with different materials and SW then overriding all previous instances etc..? Just looking for areas of pitfalls that we might fall into.

                                                                                                             

                                                                                                            Thanks for the advice. I am interested in hearing how to be successful if we choose to go in this direction.

                                                                                                             

                                                                                                            Grant

                                                                                                  • Re: Using Toolbox: Do or Don't?
                                                                                                    Dan Pihlaja

                                                                                                    Toolbox

                                                                                                     

                                                                                                    See this thread. 

                                                                                                • Re: Using Toolbox: Do or Don't?
                                                                                                  Jim Steinmeyer

                                                                                                  Since the Toolbox has become such an issue in the "Blood Boiling" thread I thought I would ask a question that I am sure would apply to the vast majority of the users here.

                                                                                                       My company has been using SW for a long time and with how flaky the Toolbox was in the past they completely went away from it and now have separate parts saved for all of the hardware. I really like smart fasteners and would like to be able to use them but detest having two models with the same part number, description and shape in the system. I am unaware of any way to implement Toolbox without either having duplicate parts or manually going through all the existing assemblies (20 years worth) and replacing the old fasteners. This could easily be a years long project without PDM.

                                                                                                       How do/have other companies dealt with implementing Toolbox after years of not using it?