21 Replies Latest reply on Nov 30, 2016 7:51 PM by Vladimir Urazhdin

    Solidworks BOM not saving Custom Information.

    Tyson Hueppelsheuser

      So I do mostly spool drawings at work here so I created a custom BOM which was basically the standard BOM template which i then just deleted the description row and added a new row called Material Info which i manually fill in with the heat numbers of fittings and material type etc. Now when i do a routing assembly i define the all the spools and create a plumbing drawing. I've also created a custom sheet format that suits my need. Now when I'm going through the steps to create the plumbing drawing, i select my custom BOM template to insert into each drawing page etc. But when i edit the table by filling in my materials info column or deleting a row that has a part I don't want to include in my BOM, then save and exit the drawing. Every table on every page gets reset (most of the way, some of the information i placed in the table stays in.) but to the point where the drawing looks like it was just imported. its very frustrating as every time I find the a mistake somewhere in the drawing and want to correct and re-print it i have to completely re-do the BOM and all the numbering.

      Ive attached a file where I've been running into this issue. It doesn't happen on small files only on files where I'm creating spool drawings. Ive also attached a previous print out of the file and what it supposed to look like.

          • Re: Solidworks BOM not saving Custom Information.
            Tyson Hueppelsheuser

            The problem still remains that you can have a different heat number every time i pull one of those parts off the shelf. also it doesn't fix the issue of the BOM re-populating columns I've deleted.

            • Re: Solidworks BOM not saving Custom Information.
              Elmar Klammer

              The material designation is independent from your heat number and stays constant i.e. ASTM 105 etc. I would separate the HN into a stand-alone configuration specific property. Insert your BOM table that includes your HN column.

              I assume you will have old HN values listed since they are saved into the part files i.e. opening an older version as a starting point

              Now save the BOM to excel. Open the exported bom file in excel. In Excel select all cells in the HN column except the header enter space and hit CTR-enter. That will replace all your HN's with a space (" "). I would send the excel bom with the empty HN values to my parts guy and ask him to enter the new individual HN into the excel file and send it back to you. Make sure he doesn't change the sort order of the BOM.  Now you select the new HN column including the header cell and hit CTR-C. Go to SW and select the HN column header and hit CTR-V. Solidworks will ask if you want to break the life-link. Make sure you select "NO". Save your drawing and all custom properties are now stored in your parts.

              No macro required. The copy paste will transfer the new values into the corresponding custom or configuration property i.a.w. if your BOM value pulls it from the custom prop, then it will go into the custom prop and vice versa.

               

              The advantage is that you will only enter HN's once in the whole process including your parts guy and eliminate redundant data transfer errors.

               

              That's it...pretty fast and simple

               

              Edit: You can just clear the cell value instead of entering a space. I suggest a space cause I can copy & paste the space into my SW bom to clear/replace existing property values. Your challenge starts when you use the same flange part model in different BOM's especially when they end up with none-identical heat numbers.

              That can easily happen. Then you will need to make copy and replace the cad part and assign a new part number. That can become cumber some quickly. If you need to track HN only for each sub assembly i.e. mark the HN only on the assembly drawing then I wouldn't use custom or config properties. This is more a document control requirement. In this case I would make the drawing just like you did. Export the BOM to excel. Enter all relevant HN data, then copy the complete list into a standard drawing table. Looks and feels identical to BOM tables it's simply static. That way you won't have to worry about parts being used in various sub assemblies.

              Add a header row to the static table so it can be identified as a table that won't auto update.

               

              That would be my preferred method

            • Re: Solidworks BOM not saving Custom Information.
              John Stoltzfus

              Anytime you have a part with multiple configurations the custom property is pulled from the Configurations Tab and a single item or the default item pulls the info from the Customs Tab. 

               

              Open up the part file and check the Configurations and Customs tab - you'll be able to tell right away which of the tabs it's pulling the info from..

                • Re: Solidworks BOM not saving Custom Information.
                  Tyson Hueppelsheuser

                  Maybe I wasn't clear but I don't want a custom property to be inputted from the part its self. I want the table to generate with a blank column that can be filled in by the user with information that changes on a job to job basis, and i'd like to be able to just fill it in right there on the drawing. Unfortunately anything I enter is being erased after saving, then closing and re-opening the drawing.

                    • Re: Solidworks BOM not saving Custom Information.
                      John Stoltzfus

                      Then you still need to do what I was saying check where the info is coming from - Delete it there or run a macro that deletes all your custom properties..

                       

                      Since SolidWorks has possibly the most awesome setup when it comes to Custom or Configuration properties, you have left me scratching my head, chewing my finger nails, and erratic blinking -  Which is ok I don't need to understand your workflow, but the biggest no no is that you're depending on user input for individual BOMs', scary, that info should be in the part file and follow the part file, input the information once and to avoid fat finger disease... 

                        • Re: Solidworks BOM not saving Custom Information.
                          Tyson Hueppelsheuser

                          I'm sorry about my confusing work flow, I.m definitely open to new ideas on how to do this because Im the only person at my workplace that uses solidworks and everything i know is basically self taught, and I've only been using it for 3 years off and on. If you know of any video tutorials or such that shows this process I'd be very interested in seeing them.

                            • Re: Solidworks BOM not saving Custom Information.
                              John Stoltzfus

                              Good place to start is to read this post from start to finish if you can

                               

                              What are your most impressive tricks of solidworks, Please spread.

                               

                              We would be more than happy to share what you need, but it would be good if you get a little reading done, so you'll know what we're talking about etc... there are many different ways to approach part and assembly custom properties and part/assembly history..

                                • Re: Solidworks BOM not saving Custom Information.
                                  Tyson Hueppelsheuser

                                  I looked into that forum post, lots of useful information. I've officially noticed so many disastrous work flow habits haha... Just "getting it done" for the last 3 years basically, so now its time to really learn some new habits and go back and fix all my mistakes. I noticed you talking about a macro that you had developed for the mass custom properties table and i was unable to find the download for it. also any other material you have regarding the custom properties and BOMS would be greatly appreciated.

                                    • Re: Solidworks BOM not saving Custom Information.
                                      John Stoltzfus

                                      First off I don't write macros I can change them a little bit if required, but I need detailed instructions... 

                                       

                                      Custom Properties and Custom Property management takes a little getting acclimated to, but it's not that hard to learn.  To get the information you need it would be good for you to let us know what your workflow consists of, or rather what does your shop or employer require.  Most of the time minimal information ends up costing time later down the road, plus it doesn't take that much longer to input the proper information right away or after the design is approved.  It is all about being able to quickly find 2 - 3 or 10 year old components and models, if you do a lot of modeling or design most of those components will be long forgotten, but it's really sweet to open up a folder and everything is right there, except interchangeable hardware etc..

                                       

                                      Answering the following questions will get the other guys involved with their expertise, keep in mind that we work in different industries and work for different CAD Management practices so there will be a difference of opinions...   Questions are not listed in priority, just as them came...

                                       

                                      I did a lot of work in the Custom Bulk Material Handling Industry, and that included custom machinery, conveyors and storage etc, however now I work in the furniture industry, so each area has different approaches..

                                       

                                      1. Do you use single or multiple tab drawings?
                                      2. What release or version of SolidWorks (SW) are you using?
                                      3. How do you model top down or bottom up?
                                      4. Do you use multiple Assemblies and Sub-Assemblies for a project?
                                      5. How do you handle interchangeable components, do you use Toolbox?
                                      6. How many different Custom Properties do you require? Like Customer, Dates, Paint Specs......
                                      7. Do you have your own Drawing Template or just a SW Boiler Plate?
                                      8. Did you ever see Custom Property Tab Builder? If not do some searches and take a look, best guy that helped me back in the day was JOHN GEORGE

                                       

                                      I'm sure there will be more questions that will come up, but try these for starters

                                        • Re: Solidworks BOM not saving Custom Information.
                                          Tyson Hueppelsheuser

                                          1. My drawings are almost always multi tab drawings.

                                          2. Just upgraded to SW 2017 SP0 (glitch that i was having in 2016 was supposed to be repaired in 17)

                                          3. Bottom up

                                          4. Yes, I'd say 65 percent of what i do in solidworks is working with multiple assemblies and sub assemblies as I create pressure piping drawings for customers, thus the need to have heat numbers and material information stored in the BOM as the governing authorities in my area require the customer to have full material traceability in order to get their projects approved.

                                          5. I'm not totally clear on what you mean by interchangeable components, I guess the closest thing i use to interchangeable components would be things I've added to my routing library.

                                          6. I would really only require 2 one for heat numbers which change on a job to job basis so for a part i don't use often it may only have 1 heat number, but a common pipe nipple that i use all the time could 40 heat numbers. The other one for Material spec such as SA 105N, SA 106B etc...

                                          7. I've created a drawing template but i have to change all of the information in it manually as i just threw it together quickly one day and never linked any custom properties etc. which is something I'd like to work away from as much as possible.

                                          8.No I have not ever seen the Custom Property Tab Builder, but i will most definitely look into it.

                                           

                                          I've just really noticed as of late, now that things have slowed down a little, that im not nearly as efficient and having way to many user caused errors costing lots of lost time trouble shooting and im desperately attempting to learn some better practices in this downtime.

                                           

                                          Also my drawing template should be attached in the pack&go I uploaded at the beginning of this post.

                            • Re: Solidworks BOM not saving Custom Information.
                              Tyson Hueppelsheuser

                              Does anyone have an idea for adding heat number configurations to parts with multiple configurations already? for example I designed a library of reducer bushings with a design table instead of building 15 separate bushings, would i just make copies of the sizes and only change the heat numbers on the configurations? Any other ideas on how to do it would be appreciated.