4 Replies Latest reply on Jun 22, 2015 1:35 PM by Matt Peneguy


    Alan Thomason

      I've tried to use the Toolbox fasteners, but I'm surprised how limited it seems.  I tried to insert two parts that I can purchase, AN4-53 and AN310-4 and neither are available in my example of Toolbox.  It is very possible that this is my ignorance of how Toolbox is supposed to work. 


      Does anyone have more experience with this?

        • Re: Toolbox
          John Stoltzfus

          There are a lot of people using Toolbox - but I'm not one of them, during a re-install around 5 years ago and it created so much havoc that I spent hours every time I would open an old file.  So I started to create my own, which can work the same, plus you can create your own custom properties and combine that with a design table, now you have something that's going to work.  Add the folder in your library folder, then it's just as simple as the toolbox option..  What I did is download one fastener from McMasterCarr and then added a design table and populated that - then I had all of the one diameter that is available etc..


          IMO - or just my 2 cents


          I have a couple of examples on 3dcontentcentral.com - type my name in the search bar and on the top left hand side of the screen there are different categories - select hardware and download whatever you want

          • Re: Toolbox
            Bob Van Dick



            Toolbox is far from complete.  I have used toolbox for many years and am beginning to think like John.  I don't know if it is worth the trouble using it any more.  Perhaps if you stayed with the same version of Solidworks it would be ok, but I have found that it is very glitchy when upgrading to new versions of Solidworks.  Parts created in different versions using toolbox parts have unpredictable results.  Every time I go back and have to revise a part done in a previous version that use toolbox parts, I have to double check to make sure the correct hardware is still being called out on the drawing.  I have had many cases in which Solidworks changed the hardware and if I hadn't checked the drawing, it would have hit the production floor.

            • Re: Toolbox
              John Stoltzfus

              Alan - Take a good look at this post


              Re: Using Toolbox: Do or Don't?


              There is a lot of good information in that post pro's and con's - however the last post echos what I have said.  One of the things to keep in mind is it is a little more difficult with design tables/configurations of the hardware.  I have my hardware setup within diameter, so when you design it is important to finalize the overall design and pic the proper diameter, for me it is easy to change length, however if I need to pick another diameter I need to insert another part, however once you insert/use hardware this way, you will remember to reduce the number of re-insertions, by picking the correct diameter the first time.


              The great thing would be to have a design table that handles all the Hex Head bolts, however the file would get too big and would slow down your computer.


              It's kind of pick your own poison deal........

                • Re: Toolbox
                  Matt Peneguy

                  John's link above is a good resource...It's always better to learn from other people's experiences than to spend the time sorting it out for yourself.


                  I agree adding parts to the toolbox is broken.  I have corrupted the database trying to get parts into it too many times to count.  Based on this and other problems with it we have abandoned the idea of using the toolbox as it was intended.  If you are storing designs to be used in the future and modify the toolbox, I highly recommend you consider your workflow very carefully and whether you want to be using toolbox, especially if you are working with projects that have hard deadlines.  If you have your toolbox break on you when your project is due the next day, you could be in a bad situation.


                  One seemingly good compromise we are using is to export a toolbox part by creating all of the configurations in the file via the Toolbox Settings app.  Then we copy it from the toolbox folder and use sldsetdocprop.exe (\Program Files\SolidWorks Corp\SolidWorks\Toolbox\data utilities) program to remove the toolbox flag from the file.  Then we just drag and drop the part into assemblies.  It is a little bit of work on the front end, but it seems to pay off because the part retains its "smartness" and can resize based on the hole you drop it into.  Plus, if you aren't too concerned with exact dimensions, you can copy and rename a standard nut as "Nylok" and have the part available instead of recreating a new part from scratch.


                  As listed above, using McMaster-Carr parts is also a great option because they provide great models, and you've got the part number inside of the part.  So, you can set up a workflow to map this info to your custom properties for your BOMs.  So, we also use this to supplement exporting toolbox parts.


                  Depending on your workflow and user base this may or may not work out well for you, but I hope it helps.