14 Replies Latest reply on Jan 16, 2008 11:07 PM by Joel Hoksbergen

    Meaningful Toolbox P/N & Descriptions??

    Joel Hoksbergen
      What is the easiest way to give a meaningful description to toolbox items, for display in a drawing BOM? For example, I would like the description for a screw to look like:
      SHCS 4-40 UNC x 5/16

      instead of SW's description of:
      HX-SHCS 0.112-40x0.3125x0.3125-C

      Does this mean that I need to create a new part for each screw I place, instead of a new configuration?

      Further, what if I want to assign a part number to the screw (say a McMaster P/N)? I am assuming I would then need to create a seperate SW part as I place the screw from Toolbox, but I am not sure. Is there a database file for the Toolbox that I can access and manipulate the description and P/N so I could then use the Toolbox without changing anything. I attached a graphic of what I don't want the BOM to look like (Items 9-11 for screws, Item 12 for O-Rings, the rest are not toolbox items).

      I am trying to avoid having to use a 3rd party software (Excel, Access) for creating my BOM, and then importing to SW. Then I lose the 'smart' BOM.

      Thanks,
      Joel
        • Meaningful Toolbox P/N & Descriptions??
          Kenneth Barrentine
          it can be done but it is a little involved. the biggest drawback is identical fasteners with different material/finish.

          we use toolbox to generate a model.
          we then do a "save as" into our design library with our p/n.
          strip out the unused configurations.
          fill out the custom properties.
          done.

          hth
          • Meaningful Toolbox P/N & Descriptions??
            Joel Hoksbergen
            So how would it be done if would want to have the toolbox be for say Black Oxide steel screws? Then if I had something different (stainless) I would create a new part.

            Joel
              • Meaningful Toolbox P/N & Descriptions??
                Michael C. Martin
                I share exactly the same struggle you have with Toolbox now and it sounds like we are after the same result. The help file for Toolbox indicates it is possible to have a configuration created for each type of 1/4-20 SOCHCS you wish to have. GREAT! I can have one for A574, GR5, SS, etc. The issue I am having after configuring Toolbox is the description custom property is not available if I use the same fastener in another model.

                SOMEbody must have conquered this.
                  • Meaningful Toolbox P/N & Descriptions??
                    Michael C. Martin
                    Here are my screen shots... (I hope they come through.)
                      • Meaningful Toolbox P/N & Descriptions??
                        Rodney Hall
                        The custom properties must be set up before any configs get created in your toolbox or else those configs that already existed will not have the custom properties that you setup. The best method is to create your custom toolbox setup prior to ever using your toolbox to generate anything. This is nice in theory, but who can know this in the begining? What I do is setup a clean toolbox from a fresh solidworks install and configure it to create new stand alone parts saved out to my specified directory. This allows me to edit each file independent of any other. Also I setup the toolbox so that I am able to name the file when the part is created and this saves me from having to open the file and do a "save as" then delete the original file. Hope this helps...
                        • Meaningful Toolbox P/N & Descriptions??
                          Rob Jensen
                          I've be struggling with toolbox for 2 years now.

                          If you create a new bolt, you can save the description and part number but you have to save it. If you just enter it in, it will show up with the long conf. name. You have to select the folder just under the favorites in the property manager.

                          currently, we create new parts and save then in our design library. until SW does something to make TB easier, i'm not touching it.
                            • Meaningful Toolbox P/N & Descriptions??
                              Joel Hoksbergen
                              One other question on this issue: Is there any implication to assembly file size/performance for using Toolbox configurations vs. saving as a new part number?

                              Joel
                                • Meaningful Toolbox P/N & Descriptions??
                                  Pete Yodis
                                  The way I conquered toolbox 6 years ago was to set it to create copies and not use the toolbox libarary to create configurations. If you set it to create copies, then all of angst with toolbox will go away. Most of the issues that were present 6 years ago have been solved with some of the items mentioned in this thread, but its still far easier I think to create a distinct and separate part file, name it whatever you want, give it a description, check it into and manage it in PDM, perform where used, copy it using pack and go, etc... We use toolbox as a parts generator and not a parts library. Toolbox parts are generally small in file size, so there doesn't seem to be much of a performance hit at all for us (500 part assemblies with as much as 2.4 GB of RAM in use).

                                  Pete
                                  • Meaningful Toolbox P/N & Descriptions??
                                    Rob Jensen
                                    well, if you have 50 configurations of a .25-20 bolt in a assembly and you use 100 of them i think you'll have performance issues.

                                    i tried setting the toolbox browser to create new parts on creation, but when you do that you can't tell if a size already exsists like you can with the configurations.
                                      • Meaningful Toolbox P/N & Descriptions??
                                        Pete Yodis

                                         

                                        well, if you have 50 configurations of a .25-20 bolt in a assembly and you use 100 of them i think you'll have performance issues.

                                        First - with our assemblies this is not that likely. Maybe for others. Second are you saying that you use 1 of the configurations 100 times? Or are you saying that you are using 50 of the configurations in the assembly? If you use 1 of the configurations 100 times, and there are 50 configurations in the file - then I suspect it would be advantageuos to create a separate copy with just the config needed. If you are using 50 of the configurations in the same assembly file, then it may be advantageous to use confurations of just one part file. I suspect most models are somewhere in between.

                                        As far as being able to tell if a part has been used before... This is the same issue you would have with any other file in SolidWorks. We use PDMWorks and arrange our standard parts in logical standard projects. Standard parts follow a description convention. The file names are according to their part number. Its very easy to find if you have used a part before with PDMWorks in place - albeit not as fast as with toolbox configured as the part library. For us, we are not spending all day using toolbox - so this point it really moot. We fire toolbox up every once in a while if we need something - but not that often. As we create parts, they are checked into PDMWorks and everyone knows to check PDMWorks first. If its not there, then they create it and put it in for everyone to use. You could always create all the parts you would need up front and be done with it anyway...

                                        Pete
                                          • Meaningful Toolbox P/N & Descriptions??
                                            Rob Jensen
                                            Pete

                                            I don't even have toolbox set-up in a multi-use enviroment yet. I've been trying different things and nothing seems to work for us. I've been preaching PDM for 4 years now and upper management doesn't listen, so it's tough.

                                            I was just saying if the generic toolbox part (hex bolt_ai.sldprt) has 50 configurations of differnet thread sizes then it might not be a good option to use the the configurations.

                                            I have legacy hardware to deal with also, so i'm trying to draw a line in the sand and tell our users to start doing "whatever we decide" on whatever date.

                                            It's a mess...
                                              • Meaningful Toolbox P/N & Descriptions??
                                                Pete Yodis
                                                Feel for you Rob... It can be donwright nasty when there alot of users creating lots of data without strucutred organization. Unfortunately the longer you wait to implement something, the worse it is. I know plenty of stories where it got to the point that it was too much work to organize, so the status quote was kept...
                                                  • Meaningful Toolbox P/N & Descriptions??
                                                    Joel Hoksbergen
                                                    Back to the toolbox question: If I save every screw as a seperate part, and then place it in an assembly, what happens when I want to change the screw length. It is easy using "Edit Toolbox Definition". When I have seperate parts in a library do I then need to use "Replace Components"? Or does the Toolbox keep track of the new parts and grab the correct one?

                                                    Put another way, once a screw file is created is Toolbox ever used again to place that component in the future, or is it handled by "Insert Component". My preference would be to configure Toolbox to handle this.

                                                    Joel
                                                      • Meaningful Toolbox P/N & Descriptions??
                                                        Joel Hoksbergen
                                                        I think I have answered my question, some of you may have also answered it above but here is what I did.

                                                        I set up 'custom properties' in the 'configure toolbox' window (attached graphic). I then specified what toolboxes i want them applied to (see help for this window). I set it up to have PartNo, Description, Material, Finish, & Vendor custom properties. Some can be a list if you want. Then when you place this screw from the toolbox you can fill these in as you want. (I use McMaster P/N's). Then setting up the BOM to grab the corresponding custom properties, it displays correctly. I did have to change the P/N column properties to be a custom property, instead P/N default button (See graphics, note some screws are correct, the blank lines are screws that have not been updated.) If a screw has already been placed, you can edit toolbox definition (RMB from Feature Tree) and fill in these properties. It seems to work so far. It will be a hassle as new screws are added for first time, but then should go quickly.

                                                        Let me know if you have questions, or this doesn't make sense.

                                                        One final question, how do you apply a material to a screw so you have the correct weights? For example steel or aluminum screws. Right now they are just the default (no material specified)

                                                        Joel