7 Replies Latest reply on Jul 30, 2016 10:44 AM by Bill Toft

    Assembly BOM: a way to display Assembly Description in drawing??

    Sarah Dwight

      I have an assembly consisting of 2 parts.

      That assembly will be used as a sub assembly.

      I want to check the part Number and Description that will be used in the BOM for this sub-asy.

      When I check the same info for parts I use a BOM in the part drawing and it gives me the info I need.

      But when I use the same process in an assembly drawing I only get the part info, not the asy info I desire.

      Is there a way to do this in an assembly drawing?

        • Re: Assembly BOM: a way to display Assembly Description in drawing??
          Peter Kennedy

          I'm not sure about a BOM but why not just make a box with a note linked to your part number and assembly description on your drawing title block? If you always want it add it to your drawing template.

            • Re: Assembly BOM: a way to display Assembly Description in drawing??
              John Pagel

              I think Peter has the right answer here.  I am not sure there is a way to manipulate the BOM in the way you want Sarah (although I could be wrong).  This seems like it would be counter to the whole purpose of a BOM.  Although, up until now I did not realize you could drop a BOM into a part drawing and that it would populate.  However, most companies simply do as Peter said, and have templates with notes in the title block which are linked to their respective property.

            • Re: Assembly BOM: a way to display Assembly Description in drawing??
              Gianluca Mattaroccia

              Hi Sarah,

              let's see first if I understand your challenge here.

              You are purchasing two components from McMaster, each one with its name and part number.

              Next, you create an assembly with these two components.

              This Assembly will be part of a higher level assembly.

              So far so good?


              The BOM you are showing for the assembly in my opinion is correct, that's the way you list all the components needed to build the assembly in the drawing.

              Most likely you are trying to protect the info in your drawings, avoiding your customer going directly to the source.


              If you want to show only the assy info and hiding the components within, open the assy --> go on the configuration tab--> right-click on the configuration you desire and click properties.

              Where you see "Bill of Materials Options" choose the option "Hide". This option will hide all the children components when used as a sub-assy.


              Let me know if you need a screen shot. It would be ideal for you to upload your files for better understanding



              • Re: Assembly BOM: a way to display Assembly Description in drawing??
                Sarah Dwight

                Thanks for the replies. Let me explain more.


                So the reason for doing this is to check that the properties I desire are populated in the next level BOM. Gianluca - I am using the configuration property manager to alter the BOM already.

                I made this a SOP for when we download parts and we now use it for our assemblies too.

                I am checking a bunch of part/asy drawing my coworkers authored. So double-checking this at each level of an assembly would be great. Spelling errors are a bane to my existence, and since we enter this info manually they are numerous. I would rather catch them at part of sub-asy level than at top level.


                If I could get this to work I could drop a second BOM off the page on asy drawings or just include it.



                I got it to work like I want, but not feasibly. if you make an assembly of the sub-asy it gets the desired results using an indented BOM.

                Is there a formula to get the conf. prop. description?? and user defined part number?

                That way I could link it to a note as Peter   suggested.

                  • Re: Assembly BOM: a way to display Assembly Description in drawing??
                    John Pagel


                    Not sure how much this will help you, but I have a potential solution for you.  But, just to make sure I'm understanding...

                    The descriptions are being added by typing them into the configuration "Description".  The only way you know how to check this information without actually opening up the model is by dropping a BOM onto the drawing.  But, in assemblies (as opposed to parts) this is a bit clunky and requires a time consuming work around as described above.


                    Now, the solution (kind of)...

                    Obviously, it would be ideal if you could place a note in the title block for description, then link that to the description that is typed out in the configuration (Peter's suggestion).  But, as far as I know you cannot do this.  What you can do is link the note to "Configuration Name".  This is done in the Configuration Properties menu while in the model.

                    I do not know if this is helpful or not seeing as you would have to change your SOP to putting the description into the "Configuration Name" text box while in the model.  This requires convincing people to change their workflow and I know that is never easy.


                    But, if you are going to change your SOP, then I would suggest putting the description into the model under the part's properties menu  This is normally done with some sort of add-on software (such as SolidWorks PDM) but can also be done through SolidWorks directly.  In the model, select File, Properties.  Then, under the Custom tab, you can add the properties of the part (to include Description).  Then, you can add a note to the drawing that links to any of these properties.


                    I was a little surprised to see that your title block does not contain a spot for description as most I've seen do.  Of course, there may be a very good reason for this that I am unaware of.  If this is the case, then forget I mentioned it.


                    On the flip side, I am heading out for the weekend and will not be back until Monday (unless I get bored tonight), so don't think twice if I don't see your response until then.

                    • Re: Assembly BOM: a way to display Assembly Description in drawing??
                      Deepak Gupta

                      Let me try to understand the need once more; when you insert the sub assembly to next level assembly and in the BOM don't want to display the child components even with parts only or indented BOM but only the sub assembly details. If yes then set this value in the configuration property of that sub assembly.


                    • Re: Assembly BOM: a way to display Assembly Description in drawing??
                      Bill Toft


                      I use the Property Tab Builder to create a standard screen to enter custom properties for parts, assemblies & drawings.

                      I use "PartNo" for my part number property. I make the PartNo a configuration-specific property.

                      Then in the Configuration Properties (for both part & assembly), I use $PRP:"PartNo" as the User Specified Name for BOM.

                      In my drawing I map the custom properties to the fields in the title block.

                      In the drawing BOM, PartNo now shows up in the default column PART NUMBER. You can also insert columns in the BOM for other custom properties.


                      I find this gives me a quick & consistent way to edit ONE part number and make it usable in both BOMs and Drawing title blocks.


                      If you don't want to use Property Tab Builder, you can use File > Properties to add and edit custom properties.

                      I have attached a few screen shots

                      I found it worth the effort to get the part, assembly & drawing templates set up to use custom properties. That way you only need to go to one place (in the part or assembly) to make changes/update to the associated drawings.