16 Replies Latest reply on Aug 27, 2014 1:06 PM by Jamil Snead

    Is it wise for a drawing to reference multiple parts/assemblies?

    Seth Renigar

      I know it is possible.  I'm just trying to get a general consensus whether this is a good idea or not.

       

      For example, if an assembly contains many parts, and you wanted to highlight one of the parts in it's own view for whatever reason (i.e. maybe there is not a good way to explode the assembly to show it), would it be better to reference the new view to the part model, or should you create a Display state in the assembly to show the part by itself, then reference the new view to that Display State of the assembly?

       

      My school of thought has always been that a drawing should only ever reference 1 part or assembly.

        • Re: Is it wise for a drawing to reference multiple parts/assemblies?
          Glenn Schroeder

          Almost every drawing I do references multiple models; main assembly, often one or more sub-assemblies, and multiple parts.  I've never noticed it causing any problems.  I'd hate to think how many Display States I'd need for some of my projects if I didn't do it that way.

           

          Your thought of only one model per drawing may be similar to what some people say about one drawing for each part.  If that works for you, that's great, but for what I'm doing it wouldn't make sense to have 25 or 30 separate drawing files to go into a single report.

            • Re: Is it wise for a drawing to reference multiple parts/assemblies?
              Seth Renigar

              Glenn, Deepak, & Jamil,

               

              I realize it can be done.  I just view it as not being good CAD practice, generally speaking.

               

              For example, do you use top level BOMs and balloons?  If so, how do you handle the balloons on your views that reference the Part model rather than a Display State of the assembly?  The balloon to the part model view can not be parametrically linked to the BOM.

               

              Here is where I'm at.  I am looking at an assembly drawing of one of our products, created by another designer here.  The first sheet shows the top level assembly exploded, a BOM, and balloons going to the parts in the exploded view.  I have no problems with this so far.  It makes sense.

               

              Then on sheet #2, there is a view of the carton the product goes in (yes, we show this sometimes, as packaging is part of the assembly BOM).  Then there are individual views of a few other part models that go into the final package carton, as loose parts.  All of these views on the 2nd sheet reference their individual part models, not the assembly.  And, these part models don't even exist in the top level assembly.  Yet there is a manual "text" balloon to each of these parts model views, and the BOM on Sheet 1 has been manually edited to add these part numbers to it.  To me, this completely takes away the point of parametric relationships between balloons and BOMs, and automatic updating if something were to change.  It also introduces more potential for human error when something in the assembly does change, as now the BOM and balloons have to all be checked manually.

               

              Is it just me being too anal about this sort of thing?  Or is this sort of thing common practice?

                • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                  Jamil Snead

                  In the situation you are describing I think you should at least have the packaging and loose parts as part of the main assembly, even if they are hidden. That way they will show up in the BOM automatically. Then also in a view of the individual part and as long as you have the view properties set to link balloon text to specified table and choose the assembly BOM from the drop down menu then the balloon will match the assembly BOM item number.

                  • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                    Glenn Schroeder

                    Seth Renigar wrote:

                     

                    Glenn, Deepak, & Jamil,

                     

                    I realize it can be done.  I just view it as not being good CAD practice, generally speaking.

                     

                    For example, do you use top level BOMs and balloons?  Yes.  If so, how do you handle the balloons on your views that reference the Part model rather than a Display State of the assembly?  The balloon to the part model view can not be parametrically linked to the BOM.  Yes, it can.  Right-click on the drawing view of the Part, choose "Properties" from the drop-down, check the box at bottom left of the Drawing View Properties dialog box for "Link balloon text to specified table" and choose the correct table from the drop-down.

                     

                    Here is where I'm at.  I am looking at an assembly drawing of one of our products, created by another designer here.  The first sheet shows the top level assembly exploded, a BOM, and balloons going to the parts in the exploded view.  I have no problems with this so far.  It makes sense.

                     

                    Then on sheet #2, there is a view of the carton the product goes in (yes, we show this sometimes, as packaging is part of the assembly BOM).  Then there are individual views of a few other part models that go into the final package carton, as loose parts.  All of these views on the 2nd sheet reference their individual part models, not the assembly.  And, these part models don't even exist in the top level assembly.  Yet there is a manual "text" balloon to each of these parts model views, and the BOM on Sheet 1 has been manually edited to add these part numbers to it.  To me, this completely takes away the point of parametric relationships between balloons and BOMs, and automatic updating if something were to change.  It also introduces more potential for human error when something in the assembly does change, as now the BOM and balloons have to all be checked manually.  I agree that this was bad practice. Is it just me being too anal about this sort of thing?  Or is this sort of thing common practice?

                • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                  Deepak Gupta

                  Agree with Glenn that there should not be any issues. From what I've seen/observed this is more driven by how the system has been set up in a company. Some prefer one drawing for each whereas done says all related drawings in one drawing only. And in some there is combination of both (I'm more used to this one). Each system would have merits and demerits. So in my opinion you're the best judge on choosing that path. Good luck

                  • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                    Jamil Snead

                    It would probably be cleaner to only reference one file in the drawing, but it might be more work and complicate the assembly file. I don't think it's a big deal to include views of individual parts on the assembly drawing, I've done it myself. I've even had a view of the the top level assembly on a subassembly drawing, although I can't remember why. That is less ideal though, because if you want send out the files you'd have to include the main assembly too, and opening the drawing would take longer because it would need to load the main assembly.

                    • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                      Arvind Jain

                      Many companies follows the rule of one number for all, such as drawing, part etc, if that is the case than it make sense to have drawing referencing only one part of assembly.

                       

                      Also from the manufacturing point of view, machine shop doesn't need assembly drawing, especially when parts are machined by contractors, you would not allow to have them assembly drawings or other parts.

                      • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                        Merv Zell

                        Apart from abiding by your company's CAD standards, and then perhaps your country's CAD standards, I really don't see any issue with how you go about setting up your drawings...

                         

                        The main aim of a drawing is to communicate information, and depending on the purpose of a particular drawing (and its recipient), the style of drawing will change accordingly. There are no hard rules (outside of the above), and therefore I don't agree with the statement that its not good CAD practice.

                         

                        Yes, there are many instances where it is beneficial and indeed mandatory to have one part/assembly per drawing, but likewise there are many scenarios where your drawing might include a mix of parts, assemblies (weldments and sheet metal included) depending on purpose of the drawing. Where a drawing is produced to provide descriptive info (like for packaging), maybe you could create an assembly with all of the items required, then use a BOM for that assembly only.

                         

                        "For example, do you use top level BOMs and balloons?  If so, how do you handle the balloons on your views that reference the Part model rather than a Display State of the assembly?  The balloon to the part model view can not be parametrically linked to the BOM."

                         

                        We use top level BOMs and balloons, however for views for details of parts we add a view title annotation that includes the BOM Item number. It would be great if Solidworks had a way of linking that to the BOM automatically, but I haven't found a way to do that... If balloons are needed on that part/sub-assembly, the we will create a BOM/cut-list for that item.

                         

                        Some of our drawings produced for the workshop floor might have several sheets where there are a number of parts or subassemblies on them with their own BOM's or weldment cut lists (sometimes more than one BOM/cut list per sheet) - purely to produce a package for a particular job that enables easier management of the drawing information. This does potentially create more work with revision control, but it works for us... generally these drawings are job specific - one-offs. It then also becomes easier to archive the information.

                        • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                          Dwight Livingston

                          Seth

                           

                          Showing more than one model in a drawing may have unintended consequences for Pack and Go. We had a bunch of top-level drawings each with a view of a small label, an item that gets attached to most of our instruments. The draftsman included it as a view of the label model itself, rather than a detail of the assembly. To SolidWorks, it was a model with many drawings. When we used Pack and Go to get a top-level assembly with the drawings option turned on, it would of course include the label as a component, and then dutifully retrieve every drawing of that label. It also retrieved every component shown in those drawings, which was just about the whole library.

                           

                          Dwight

                          • Re: Is it wise for a drawing to reference multiple parts/assemblies?
                            Alex Chen

                            Hi, Seth:

                             

                            It is ok but not wise to reference multiple parts/assemblies in a drawing document.  It is not ok to duplicate definition of a part or assembly in multiple drawing documents though.

                             

                            My 2 cents,

                             

                            Alex