11 Replies Latest reply on Feb 5, 2016 5:28 PM by James Rhys-Davies

    Toolbox in Large Assembly Best Practices

    James Rhys-Davies

      Fresh from SOLIDWORKS World 2016 (best experience EVER) and it's time to start researching/implementing all of our new ideas and tactics!!


      We run large assemblies (>750 parts) with complicated geometry with multiple configurations, so you can imagine the performance nightmare this is creating for us! It's a necessary evil though.


      We currently use EPDM to manage our hardware with design tables, but are looking into the Toolbox. Does anybody have any recommendations on how to set this up so that it doesn't hurt our performance any more. We would of course slim out the toolbox to match our inventory.


      Can the hardware be loaded as a virtual part? Would that help or hurt us?


      I am looking for suggestions before I spend the time needed to optimize our toolbox.

        • Re: Toolbox in Large Assembly Best Practices
          Chris Clouser

          I frequently work with assemblies in the 30,000-70,000 part range.


          I have always hated toolbox.  Having used SolidWorks since the late '90's, toolbox has been one of my biggest nightmares.


          Many people will remember opening an assembly Monday morning and toolbox somehow didn't remember the hardware configurations you left off with on Friday afternoon.  Who knows why.  Maybe somebody installed the newest version of toolbox on the network overwriting the old one.  Or maybe the network is down and the configurations aren't on your desktop.  Who's to say.  But, you know something went wrong because all the hardware goes to some default configuration and usually this means all the bolts are super sized.  Then you need to try to remember what size you were using on dozens and dozens of parts to put it back.  An hour or two later you're back to where you left off and hoping it doesn't happen again.


          So I decided to come up with a solution that would never let me down.  I started by building my own library with toolbox parts that had only ONE configuration.  The part name would be that used in our in-house part numbering system.  the problem is that the toolbox parts have special properties that I needed to get rid of.  Long story.  Anyways, I abandoned toolbox parts all together.


          Now all I do is download the part from McMaster, Fastenal, or generate the part myself.  Save it under our in-house naming convention with our custom properties and that's it.  This is the simplest way to do it from a bookkeeping standpoint.  Even more stable if you save the part without the parametric features.  Apply some mate references and you have a nice, stable part that you should be able to rely on forever.


          Some people will probably come on here and say how great toolbox is and how you can configure this or that.  These guys probably are CAD administrators and are depending on a confusing file maintenance regimen in order to keep the paychecks coming in.  You can roll the dice if you want, but I'm way too busy designing things to deal with elaborate housekeeping of my files.


          Also, toolbox is lacking in a lot of areas, so I have to go find third party hardware on a regular basis anyways.  So since it's not 100% reliable when it comes to finding what you need, that's another reason to abandon it.

            • Re: Toolbox in Large Assembly Best Practices
              Umberto Zanola

              I agree with Chris.

              I make small assemblies so maintaining the whole thing would not be even an issue to begin with.

              Anyway I looked into the toolbox thing and stability problems aside it was slow as hell (on local drive) and I had the issue to unlink every component to make a clean copy of the assembly, so I ended up downloading dummy models for my needs.


              A previous coworker used it and now we have giant components here and there as he used to make undocumented customizations etc


              There are other threads about Toolbox and related horror stories on this forum, it seems that at DS tried to fix it a lot of times, but some bugs are just die hard...

                • Re: Toolbox in Large Assembly Best Practices
                  Chris Clouser

                  When toolbox first came out and I started using it I thought it was great.  But then all the problems started happening.  Not wanting to change my role from engineering to cad administration, I had to figure out a better way.


                  If I were to use toolbox, it would be to quickly design something and then replace toolbox components with something more stable once the design was being finalized.  But I'm not even sure this is much faster than just grabbing the hardware off of McMaster's website.  And usually when we prototype, we just buy all our hardware from them anyways, so that speeds up the prototype process.


                  I don't use PDM yet, but the new PDM Standard is something we might try.  In this case, if there were a way to save a toolbox part as a regular part in PDM with only one configuration, that might get me to consider using the toolbox again.

              • Re: Toolbox in Large Assembly Best Practices
                Chris Saller

                I also have had problems with Toolbox.

                If it's located on a shared server, and everyone uses only that folder, then OK.

                Once users start copying Toolbox parts onto their PCs and using those parts, it becomes a problem for other users.

                • Re: Toolbox in Large Assembly Best Practices
                  John Stoltzfus

                  Agreed 100% with Chris - I would never go back to Toolbox, maintaining a library of your own products isn't difficult.  I'll never forget opening file after file and having the bolts/screws come in 4 times the size.


                  A lot of people using SW in the late 90's early 2000 created their own libraries and I have literally 100's of fasteners and other products, so we created our files like the attached Socket Head Cap Screw, that way you can create your own custom properties and they change out easily as well.

                  • Re: Toolbox in Large Assembly Best Practices
                    Glenn Schroeder

                    I started with Toolbox parts, but have since removed the Toolbox designation from all of them.  They do have configurations, and I haven't had any problems related to them.  For example, I have one file for Ø3/4" bolts, with a configuration for each length.  And I didn't try to set up each length right away, I just add them as needed.  By doing this if I have a design change that requires a different length bolt it's much easier (and less prone to error messages) to change configurations than it is to change part files.  Similarly, I have one file for each size hex nut, with configurations for jam, coupling, etc.  Same for washers: configurations for flat, fender, hardened, and lock (the lock washer has a wedge-shaped cut that's suppressed in the other configurations).

                    • Re: Toolbox in Large Assembly Best Practices
                      James Rhys-Davies

                      Thanks for all the responses! We are using EPDM and currently have each type of bolt saved under one with file (i.e. "hex head bolt") with a design table  for the individual sizes. Very similarly to the one that John posted.



                      The problem that we're running into is that our assemblies are large and there is complex geometry so it's bringing our computers to their limits.


                      John, I noticed that you don't use the setting "is fastener", is there a reason why not? Just seeing the "mate reference" that you have in your files clears up some things! I will definitely be implementing that!



                      It is looking like nobody likes toolbox, so the best practice would be to create the sizes basically the way we have them now and then move them into the design library to speed up our assembly time.



                      Does anybody have any experience with loading hardware "virtually"?

                        • Re: Toolbox in Large Assembly Best Practices
                          John Stoltzfus

                          Rachel Mashburn wrote:


                          John, I noticed that you don't use the setting "is fastener", is there a reason why not? Just seeing the "mate reference" that you have in your files clears up some things! I will definitely be implementing that!



                          I don't use fasteners a lot anymore, so at the moment I do what Chris does, download individuals from McMaster.


                          As for the setting "is fastener" ? I guess I'm ignorant there, no idea, but something I gotta look up..


                          Using Mate References are a big plus.


                          No experience with virtual loading.

                          • Re: Toolbox in Large Assembly Best Practices
                            Chris Clouser

                            Rachel, I'm confused by your performance issues, a few thousand parts doesn't really constitute a big assembly.  You should be able to handle that easily with 3-4 year old computers.


                            Also, with EPDM you should have a performance advantage over how we're doing it without.


                            We run much larger assemblies than you're talking about off of a server located in a distant building, and we're managing OK.


                            We're looking forward to using PDM and getting a dedicated engineering server, which will greatly improve our performance, but something sounds off a bit if you guys are having issues with under 1000 components.


                            Right now I'm working on what we would consider a very simple assembly that has 1100 parts.  It's on the network.  There is nothing local, and it's very easy to work on.  The one thing that is a performance killer is a large patterned cut with several thousand holes.  I don't rebuild that one too often or it's time to go get some coffee.


                            We probably need some more clues to figure out what's going on.


                            Are you using helixed threads?  If you are, don't.  Helixes are computationally difficult.


                            Another bad practice is hardware patterns.  I have noticed a significant performance increase by putting each individual piece of hardware in by itself.  Mate references will make this process very fast.  One of my designers would always use patterns on his hardware and was having major performance issues.  I deleted all his patterns, put everything in separately, and it was much faster.


                            There were other things that he did that slowed down the performance.  I can't remember off the top of my head, but I had a different designer go through his work and do things a little differently and things got faster.


                            Another thing is that since you seem to suspect hardware, I would recommend trying a configuration that suppresses all the hardware and see how your performance is for comparison.  Just a thought.

                          • Re: Toolbox in Large Assembly Best Practices
                            Glenn Schroeder



                            Are you using sub-assemblies?

                            • Re: Toolbox in Large Assembly Best Practices
                              James Rhys-Davies

                              We are working through some performance issues now! There are some issues with our PDM that we are attempting to fix and hopefully that helps us out.


                              I work for a Marine Engine company, so we have an engine block/heads/intake in our model, so we have some complicated geometry. We do not use helixes or patterned components and we use sub-assemblies wherever possible. The upper level assembly actually has only sub-assemblies and no parts. None of the internal components of the block itself are in my model and it is outer geometry only.


                              We are welcome to any suggestions to help us out for sure! It's slow on the top-level assembly level and then when we do drawings of the entire engine with 5 pages of different configurations per drawing, it turns into a nightmare.