7 Replies Latest reply on Feb 6, 2018 12:24 AM by Nikhil Phatak

    Parts, Sub assemblies, Assemblies, Drawings & their Revisions workflow or best practices

    Nikhil Phatak

      Dear Team / Experts / Professionals/Everyone,

      We will try to explain our Workflow and we will appreciate any suggestions and comments and discussions to find a better Solution regarding subject line

      Its regarding how to manage Solidworks Data or in fact any data while working in a design environment *(Of course with existing Software's and technologies that we already have with its maximum efficient use)

      01) We create a folder named Machine 01

      02) We create Part A, Part B, Part C

      03) Drawings of Part A, B & C are created and saved in same folder with Same names e.g. "Part A".slddrw...etc(Initially we used to save drawings with a different folder structure but due to pack and Go issues we place it in same folder now)

      04) Sub-assembly 01 is made with Parts A, B & C Saved in same folder with its corresponding "Sub-assembly 01" drawing.

      05) Sub-assembly 02 is made with Parts D, E & F following above steps with its corresponding "Sub-assembly 02" drawing.

      06) Main assembly is made with Two-sub assemblies 01 & 02 and its drawing is saved as "Main-assembly 01".

      So our Folder "Machine 01" looks like

      Part A.sldprt

      Part B.sldprt

      Part C.sldprt

      Part D.sldprt

      Part E.sldprt

      Part F.sldprt

      Part A.slddrw

      Part B.slddrw

      Part C.slddrw

      Part D.slddrw

      Part E.slddrw

      Part F.slddrw

      Sub-assembly 01.sldasm

      Sub-assembly 01.slddrw

      Sub-assembly 02.sldasm

      Sub-assembly 02.slddrw

      Main-assembly 01.sldasm

      Main-assembly 01.slddrw

      1. Now we want to revise Part A and Part D but both revisions should be maintained
      2. What is the optimum aproach with respect to handeling (Part revisions) , (Sub-assembly-Revisions) (Top-assembly revisions) and (Drawing revisions)
      3. If I change a small part in entire machine Should that Entire machine assembly, sub-assembly and their drawings be revised ??
      4. What if shape of that part is changed and not just parameters, so my sub-assmbly and main assembly will not be consistent with same revision number ??
      5. Kindly share your thoughts and ideas or suggestions as I think Solidworks Forum is the best place to look forward to.

        Sincere thanks in aadvance


      Our Current Method

      ****************************************Scenario 01********************************************************

      *01) We do Pack and Go to another Folder named "Machine 01_R1" (Keeping all components name same)

      *02) Make changes to Parts A & D, Update the drawings (Add note R1 in drawings) save everything in new folder "Machine 01_R1" and exit

      (So now we have 2 Folders of same machine with Two revisions R0 & R1.)

      (For every Machine for Every Revision huge amount of data will be stored by every person )

      ****************************************Scenario 02********************************************************

      *01) We do Pack and Go to another Folder named "Machine 01_R0"

         (We wont touch "Machine 01_R0" Rev R0 is archived)

      *02) Just Update the Parts A & D in current folders

      *02) "save as" Part A & Part D which will update all drawing references there itself, add custom property of Rev R1 to parts A &D.

      *03) Open Part A & D drawings which will auto update due to save as command, add a Revision note "save as" "Part A_R1", "Part D_R1" which holds Rev R1 information

      (But now I have no history of Rev R0 on my current parts)

      (If somebody ask me to show the changes made in "Part A from Rev 0 to Rev-1" then I have to dig in the archives which are stored day,date and person wise)

      (How can we keep a track of Revisions made) ?

      ****************************************Scenario 03*********************************************************************************************************************************************

      01) Do not bother about revisions at all :-) :-P

      (This makes life simple but in a long Run if Customer ask Spare parts of old design or record of older revisions and old design intent then we are in chaos)

      ****************************************Scenario 04*********************************************************************************************************************************************

      1. Use Workgroup PDM (Which we have no idea about).
      2. (We are not good with programming, neither we have time for typing codes and setting rules and admin regulations as frankly we do not want to be software administrators).
      3. Is it a good idea to handle product data by design team?

        Or should there be a seperate team just to handle and maintain design data with programming skill set ??

      4. We also are not sure about Workgroup PDM as we remeber to read somewhere that Workgroup PDM will stop after 2018 ? Is it so?


      P.S. We ae not looking for buying anything like (EPDM or PDM) We started this discussion just to use existing softwares and technologies to its maximum efficiency so please pardon.




        • Re: Parts, Sub assemblies, Assemblies, Drawings & their Revisions workflow or best practices
          Martin Solem



          Yes, Workgroup PDM is gone. Last release was 2017 SP5, and last year of support is 2018.

          It has been replaced with PDM Standard, which is a stripped version of Enterprise PDM. It's licensed like Workgroup PDM, so if you have SOLIDWORKS Professional or Premium licenses, you also have PDM Standard licenses. I really recommend looking into that, i think it will be well worth your time given your scenario descriptions.


          I recommend you contact your VAR for a demo, and there are also many good videos on youtube that can give you an idea of how you work with PDM. Key words: "pdm standard"

          • Re: Parts, Sub assemblies, Assemblies, Drawings & their Revisions workflow or best practices
            Sergio Monti

            Hi Nikhil,

            I'm in a small company but we manage big and sometimes complex bespoke machines with multilevel sub-assembly.

            We don't use PDM at the moment, as we are only two designer, but we still need to manage revisions, old drawings, spare parts, etc.

            The file structure is the same as yours: all parts, drawing and assemblies in the same folder.

            We use the following workflow:

            - Parts, Sub-Assembly and Drawings have the following file name: "PART NO."+Space+"Description" (I created a Macro to auto populate "Part No." and "Description" from filename)

            - Bespoke Bought-out parts file name: "SUPPLIER NAME" + " - " + "Description"

            - Once each drawing has been released we create an "official" PDF drawing, adding a revision letter in the file name. The drawing can be seen from everybody in the company

            - We issue a new revision on parts only if they are "exchangeable" with the previous revisions, otherwise we create a new part number

            - When issue a new revision, we do not change the file name on models, but just update the "Revision" property, hence all the models in the folder are up to date. Changes in the parts must be made with "Direct Editing", when possible, so that it's easy to go back to the previous revision, if needed.

            - We only keep the PDF drawings for old revisions, adding the "-OLD-" prefix, in an "ARCHIVE" sub-folder, just to make sure nobody uses them, but we can still access them.

            - When issue a new revision on a part, the parent sub-assembly doesn't change revision. We issue a new revision on a sub-assembly, and relevant BOM, when adding parts, removing parts or change quantities.


            It's working fine so far for me.

              • Re: Parts, Sub assemblies, Assemblies, Drawings & their Revisions workflow or best practices
                Nikhil Phatak

                Hi Sergio,

                * We liked the idea of Direct Editing and nowadays we are frequently using it without bothering about previous feature tree,

                For new parts however we prefer design from scratch,

                * I will try to save and maintain just PDF's of previous revisions for few machines and see how it works out for us and then we will implement it within our team.

                * For revisions of sub-assemblies and assemblies we are still trying to find a reasonable workflow.

                (I created a Macro to auto populate "Part No." and "Description" from filename)

                --We give Part No_Part Name & save it in a folder and from custom property tab builder we populate same Part no and      Part name as separate properties manually and then link it with drawing sheet formats and drawing templates.

                  So if anyone makes a mistake during form entry then it may create inconsistency with custom property and the actual    name of the part being saved.

                  Our programming skills are weak but if you can share that macro with us , we can try to use it (In fact we are curious      about how much time one should invest in learning VBA or C++ or .net as of now programming a complete bouncer for    us.


                Thanks and we appreciate your quick response 



                  • Re: Parts, Sub assemblies, Assemblies, Drawings & their Revisions workflow or best practices
                    Sergio Monti

                    Hi Nikhil,

                    we also always use standard features for design and usually direct editing just for revisions.

                    I know that some might not like to assign part numbers before have the BOM built and assign PNs afterwards can be better as you can use more "logical" rules.

                    Anyway, I introduced the PN in the file name because I often need to quickly open a model, or drawing, when only know a PN, or I need to open the drawing of a part looking at it from the assembly model. So now wherever we are looking at, we know exactly what we have and how to find the related documents straightaway.

                    I assign the PNs on creation because is not easy to rename files when they are linked to other document, even if I discovered, last Friday on this forum, a function I didn't know. It's possible to rename, move and replace by RMB on the file in Windows Explorer using the SOLIDWORKS menu without breaking the link to the other documents.


                    You can find attached the macro we use to populate custom properties "PN" and "Description" from filename.

                    You will find my name and company on the frame but you can easily modify it.

                • Re: Parts, Sub assemblies, Assemblies, Drawings & their Revisions workflow or best practices
                  Carrie Ives



                  If you can get PDM set up, that will help you be able to go back to different versions. If you don't, I would recommend something like Sergio Monti mentioned, naming your files with the part number, maybe part number_description. Have a revision property in each model. When a design is complete, make a zipped pack and go for each model/drawing including the revision. I would have a released folder somewhere that gets backed up to store these files. For example, PartA_RevA.zip would contain PartA.sldprt and PartA.slddrw. I also recommend a PDF of the released drawing. I would pack and go each assembly also to give you a way to go back. Using a zip file reduces the storage space quite a bit.


                  There are several macros available to save as PDF including the revision to a specific folder. I recommend using one and modifying it to your file location.

                    • Re: Parts, Sub assemblies, Assemblies, Drawings & their Revisions workflow or best practices
                      Nikhil Phatak

                      Carrie Ives,


                      One of our biggest setback in using even a PDM standard is that we are new to it and I have read on this forum about people using Work group PDM for a while and it getting discontinued by 2018. So their data got locked with work group PDM and VARS charge consultancy fees for migrating existing vaults to new vaults.

                      I don't know exactly what that "Locked" means.

                      Can anybody suggest , what happens if we decided not to use PDM standard midway. (Meaning Can we discontinue the use of PDM standard once we have stored our files in the vault and then later use it normally with windows explorer ??? may be by    uninstalling it or by closing the restrictions of the vault and make it available for everyone in a team )