22 Replies Latest reply on Jan 17, 2013 8:34 PM by Gary Lucas

    Getting started with SW the right way

    Gary Lucas

      I,m currently a Solid Edge user (V20) looking at moving to a new position using SW and setting everything up from scratch.  They just got SW and have no previous experience.

       

      A little background that explains where my questions are coming from.  I started using Solid Edge where a previous user had been using it for 5 years or more.  He had set it up from scratch and got no training other than a couple hours initially, and lots of calls to tech support.  When I started they gave me a seat of AutoCad and asked me to design a fairly complex Reverse Osmosis skid.  I owned a copy of Rhino, so I modeled the whole thing in Rhino then saved it as 2D AutoCad.  They were impressed enough that they bought me a seat of Solid Edge and expected the other user to train me.  Most of my questions were met with "It's difficult, you'll see" I immediately destroyed one of his models, because I had no idea of how much stuff was linked together!  So I joined the user group and started asking lots of questions of people who really were experts.

       

      A lot of what was done in using Solid Edge was done very poorly.  We design skids using lots of plastic pipe fittings and a lot of hardware, in zinc plated, 304 SS, 18-8, and316 SS.  All the hardware parts in our library didn't include the material in the description.  If it said "Hex Screw 1_2x3.par" you were supposed to know that that was an 18-8 Stainless, 1/2-13 threaded bolt!  So as the new guy constantly heard abut using our "standards" and having to memorize what the other guy considered to be standard!  What fun when the company decided that using Stainless for every fastener was killing us and we had to switch to zinc plated steel for most stuff.

       

      The other big issue is the organization of the library.  It seems kind of logical to have a path like Plumbing\Fittings\Elbows\PVC\Sch 80\2\elbow*.  So you are running a 2" Sch 80 PVC pipe, and you just placed the Elbow, and now you need a Tee.  You have to go all the way back up to fittings, then back down through the folders to Tee!  Imagine if the path was Plumbing\PVC Sch 80\2\Adapters,Bushings,Couplings,Elbows,Pipe,Tees, etc. how much faster that would be.

       

      Many of our parts were created using Family of Parts for things like hardware and pipe fittings.  It seemed like a great idea, except Solid Edge checked every member of the family every time you opened a file or hit update on a drawing, which took forever.  The other user moved the library from the daily backed up server to his own computer to speed things up, and in 5 years hadn't made a backup copy.  When I came on we had to move it back to the server.  When I realized where the problem was I volunteered to open, break the links, and resave several thousand part files.  The speed up was dramatic, and my skills doing this work got a lot faster!

       

      When you looked in the Edge Bar Tree in Solid Edge parts or assemblies unique to this particular job were named very similarly to the way parts in the library were.  So with a casual look at the tree you couldn't tell if it was safe to modify a part for this job, or you just destroyed another  model in a different job with your changes.  Even worse, some jobs had links going back and forth between multiple jobs!  You couldn't even easily copy a job safely because the only way to clearly be sure there weren't any links to the old jobs was to search through the entire list of parts and assemblies looking at the paths.  Now we identify all the parts and assemblies unique to a job with a job number prefix, which also makes copying easy and reliable too.

       

      One last thing.  I got someone to create me a macro that brought all of the file properties from the entire library into Excel.  I then created a whole new part numbering scheme and applied it to the Excel file, along with correcting lots of descriptions and such. Then we wrote the data back in to the library.  We now have another Excel macro that takes BOMs pasted in from Solid Edge and rolls up the materials with the same part numbers and varying lengths and such.  We then import that into AllOrders our BOM program linked to QuickBooks which then generates POs and Work Orders for the shop.  HUGE timesaver when a BOM has 300 items and 150 of them are short pieces of pipe!

       

      Now to my questions.

       

      I want to be able to model a complete wastewater plant, consisting of about 10 large equipment skids, half a dozen tanks with instrumentation, and all of the interconnecting piping.  I do this currently in Solid Edge on a five year old Dell with 4 Gb of memory.  I open the model with everything hidden, then display and work on what I need, or is in the way.  I only see the whole model on paper most of the time. I will now be using Windows 7 64bit, with 16 Gb of memory.  For models like this how do I want to make the library, parts, and assemblies?

       

      Are libraries of parts and assemblies in Solid Works just Windows folders and sub folders, or is there a file management function?

       

      Are there any really complete standard hardware libraries out there worth downloading or buying?  A big concern is that lots of files I've gotten from various sources have WAY to much detail!  Do we really need to see an exact representation of threads on bolts?  How do you handle things like part numbers and such?  Does everybody use the same fields for the data?  For a standard library to be useful for export I will need a unique part number on every part, as well as the manufacturers part number.

       

      When you have an assembly with lots of short pieces of pipe of different lengths, how do you handle that?  Separate part file for each piece?  An adjustable length part?  A sketch with extrusion of the pipe cross section for each segment.  We've tried all three, and the most bulletproof is currently separate part files for each piece in Solid Edge.  We don't use a piping because we work with plastic pipe fittings, no standards, every manufacturer makes his parts a little different!

       

      Sorry for being so long winded, tough to get across what I am trying to do in just a few words.

       

      Gary H. Lucas

        • Re: Getting started with SW the right way
          Anna Wood

          Buy these books to start....

           

          http://www.amazon.com/SolidWorks-Administration-Bible-Matt-Lombard/dp/0470537264

           

          http://www.amazon.com/SolidWorks-2011-Parts-Bible-Lombard/dp/111800275X

           

          http://www.amazon.com/SolidWorks-2011-Assemblies-Bible-Lombard/dp/1118002768

           

          I would also get with your SolidWorks reseller to get some help and training.

           

          You may also want to look into Solid Professor as well.  http://www.solidprofessor.com/

           

          Read everything you can in this forum.  Even if you do not think it pertains to your situation.  You can learn a lot from everyone else's queries.

           

          Find the local SolidWorks User Group in your area.  http://www.swugn.org/swugn/directory.htm

           

          Cheers,

           

          Anna

          • Re: Getting started with SW the right way
            Peter Farnham

            Wow!

            I feel sorry for you already!

             

            As a working manager in our design department using Solidworks since 2003, I feel I have a lot of experience of trying one way and then another, to get Solidworks working in a sensible manner.

             

            I will try to direct you on a few things in no particular order.

            Files and documents are interchangable names.

             

            Pipe of different lengths-

            Most would say use configurations- don't do that as it will cause many headaches when used in assemblies. Add a new size and the document changes requiring every assembly and drawings with that document in it to have to resaved all the way up to the top assemblies and drawings.

            Been there, done that and regretted it ever since.

            What I would do is use a design table to set up configurations, get all the "standard" lengths you want and then save each as separate parts. Use only these single parts in you assemblies. Save the master document for future additions.

             

            Part numbering-

            I have tried many ways and finally found one that works the way windows file system works. Ie the files are listed in order!

            Use alpha-numerical not numerical- alpha as windows lists 1 then 11 before 1,2,3 ect..

            I use A- for parts, then B- for the first assembly, then C- for the assembly with a B-  assembly in it, working up the alphabet for each higher assembly.

            The advantage of this is that the listing in a windows folder starts with the parts first.

             

            Libraries-

            Thes are just as you have said, windows folders. You can set these libraries up first and then set the library "bit" using sldsetdocprop.exe in C:\Program Files\SolidWorks Corp\SolidWorks\Toolbox\data utilities. You can add these to Solidworks in file locations in the Solidworks options.

             

            Drawing documents-

             

            Make these dumb by importing all fields from the part or assembly documents, linking the fields in the drawing documents to the custom properties.

             

            Toolbox (hope you have got this).

            Setup up Hole wizard/toolbox to create copied parts. You then get a sensible Document name.

            You can assign materials to you toolbox parts as well. great time saver.

            Threads on bolts can be shown as simple (no thread), cosmetic (looks like a thread but flat) and schematic.

             

            Make sure that everything is kept on the server, that includes Solidworks data, libraries, macros, templates ect

            This makes it easier if you employ more people and safer in case you pc crashes and burns.

             

            Once you have your pc setup as you like use copy settings wizard and store this file on the server too.

             

            Use a document control software, like pdmworks or enterprise, this is as important as the documents themselves. If your company refuses, then they will be fools and your job will be much much harder!

             

            As your are using a lot of piping, I would get the piping add-in for solidworks as it is a great time saver. This would also help a lot on your elbow location question.

             

            Once a year, set aside two weeks minimum to update templates, library folders etc.. if upgrading to a new release of Solidworks.

             

            Wait until at least sp1( some say sp3) before upgrading even if a fix is in sp0 that you require, as many things are "broken" that were fine in the previous year release.

             

            Step back and look at what you are trying to do. It may work on the products you have now, but add a new product line, will it work then?

             

            Some will not agree with me on these comments, but you want a easy job when working with many parts and assemblies, so please take note.

             

            Welcome to Solidworks!

              • Re: Getting started with SW the right way
                Gary Lucas

                Peter Farnham wrote:

                 

                Wow!

                I feel sorry for you already!

                 

                As a working manager in our design department using Solidworks since 2003, I feel I have a lot of experience of trying one way and then another, to get Solidworks working in a sensible manner.

                 

                I will try to direct you on a few things in no particular order.

                Files and documents are interchangable names.

                 

                Pipe of different lengths-

                Most would say use configurations- don't do that as it will cause many headaches when used in assemblies. Add a new size and the document changes requiring every assembly and drawings with that document in it to have to resaved all the way up to the top assemblies and drawings.

                Been there, done that and regretted it ever since.

                What I would do is use a design table to set up configurations, get all the "standard" lengths you want and then save each as separate parts. Use only these single parts in you assemblies. Save the master document for future additions.

                 

                This is the Family of Parts thing I mentioned before.

                 

                Part numbering-

                I have tried many ways and finally found one that works the way windows file system works. Ie the files are listed in order!

                Use alpha-numerical not numerical- alpha as windows lists 1 then 11 before 1,2,3 ect..

                I use A- for parts, then B- for the first assembly, then C- for the assembly with a B-  assembly in it, working up the alphabet for each higher assembly.

                The advantage of this is that the listing in a windows folder starts with the parts first.

                 

                Interesting idea you have here, I'll have to look into that farther.  In SE every part file in the library is named conventionally, while every part in a job file includes the 6 digit job number and an assembly designation as a prefix to the part name.

                 

                Libraries-

                Thes are just as you have said, windows folders. You can set these libraries up first and then set the library "bit" using sldsetdocprop.exe in C:\Program Files\SolidWorks Corp\SolidWorks\Toolbox\data utilities. You can add these to Solidworks in file locations in the Solidworks options.

                 

                What does this library bit do?

                 

                Drawing documents-

                 

                Make these dumb by importing all fields from the part or assembly documents, linking the fields in the drawing documents to the custom properties.

                 

                Toolbox (hope you have got this).

                 

                Is this toolbox a standard library that comes with SW?


                Setup up Hole wizard/toolbox to create copied parts. You then get a sensible Document name.

                You can assign materials to you toolbox parts as well. great time saver.

                Threads on bolts can be shown as simple (no thread), cosmetic (looks like a thread but flat) and schematic.

                 

                Make sure that everything is kept on the server, that includes Solidworks data, libraries, macros, templates ect

                This makes it easier if you employ more people and safer in case you pc crashes and burns.

                 

                Yep, and I don't trust anyone.  When we got a new server I copied every job I had ever worked on onto separate CDs before they made the move.  They planned on using the latest backup tape to copy everything to the new server.  Guess what, the back up tape drive was bad!  They had to copy everything manually.  If it had all gone south I would have been the only employee at the company who still had his data, and his job!

                 

                Once you have your pc setup as you like use copy settings wizard and store this file on the server too.

                 

                Use a document control software, like pdmworks or enterprise, this is as important as the documents themselves. If your company refuses, then they will be fools and your job will be much much harder!

                 

                We don't have this now, and I can certainly see the value of it.  However right out the box I think it will be a tough sell.

                 

                As your are using a lot of piping, I would get the piping add-in for solidworks as it is a great time saver. This would also help a lot on your elbow location question.

                 

                I mentioned above that I mostly work with plastic pipe.  The metal pipe libraries that these add-ins use work very well. However the library would have to have the exact brand of fittings used to be useful for plastic pipe.  They don't have size standards in plastic!

                 

                Once a year, set aside two weeks minimum to update templates, library folders etc.. if upgrading to a new release of Solidworks.

                 

                Yes, SE also works in a translation mode when you upgrade unless you run updates on everthing.  I found that greatly improves performance.

                 

                Wait until at least sp1( some say sp3) before upgrading even if a fix is in sp0 that you require, as many things are "broken" that were fine in the previous year release.

                 

                Oh yeah, let the big boys with hundreds of seats and dedicated test personnel do the heavy lifting on that!

                 

                Step back and look at what you are trying to do. It may work on the products you have now, but add a new product line, will it work then?

                 

                Some will not agree with me on these comments, but you want a easy job when working with many parts and assemblies, so please take note.

                 

                Welcome to Solidworks!

                  • Re: Getting started with SW the right way
                    Peter Farnham

                    Toolbox comes with Solidworks professional and contains standard nuts, bolts bearings ect to international standards like Din, Iso and Ansi for example, and you can add you own items and assign materials.

                     

                    The Library "bit" tells the document control system that the document is a library item, so you can have or not have revision control.

                    Shows nice and blue in the listing for easier identification.

                     

                    Having document control systems has helped the company in many ways as we do a lot of prototyping and customer driven designs as well as standard equipment. It has also greatly helped in getting the ASME certification.

                    But for you a document control system will allow you to see at a glance what has been changed in all of the revisions.

                    You can copy a whole project and rename it and the documents within to a whole new project without affecting the existing project. no more re-doing the same thing twice.

                    The benefits are massive, you actually get time to design as opposed to spending hours looking after documents!

                    Is that not what your company wants? What used to take two months to do, I can now do in less than three weeks, not a bad return I say.

                     

                    "Yep, and I don't trust anyone" - lol!! I get called paranoid over this, haaha!! But your case proves the point. We have a daily, weekly and monthly tape backup with a daily off-site storage backup too, just for that reason. once bitten as they say.

                     

                    Go to this site for plastic piping that does meet standards- http://www.johnguest.com/Home/Home.aspx

                    We use their products on our equipment and they are very professional.

                     

                    Do I work for Solidworks? Not at all.

                    I just push them all the time to try to give us users a professional product that works. I have even spent a week of my time at their UK head quarters (Cambridge) to show them what needs to be fixed, and hats off to them, they did fix most of the problems I threw at them!

                     

                    Now we just need them to fix the "broken" things that used to work. lol

                    • Re: Getting started with SW the right way
                      Jeff Holliday

                      Regarding the document management - if you are using SWorks Pro or Premium, the Workgroup PDM is furnished no-cost. there is not a steep learning-curve and it would save time long-term if it was implemented at the beginning rather than playing catchup later.

                  • Re: Getting started with SW the right way
                    Jerry Steiger

                    Gary,

                     

                    Most everything that you did with Solid Edge will apply the same to SolidWorks.

                     

                    I would vote with Anna to get some training, but I have to admit that there are a lot of knowledgeable people who didn't.

                     

                    Jerry S.

                    • Re: Getting started with SW the right way
                      Nathan Coy

                      I'll second what Anna said, Matt's books are a must. 

                       

                      BUT

                       

                      I suggest hitting the help menu and checking out the SolidWorks Help, SolidWorks Tutorials, and there is also a link to a PDF called "Introducing SolidWorks" that gives a general overview of what's going on.