25 Replies Latest reply on Jun 19, 2018 11:21 AM by Paul Salvador

    Vote in Favor or Not | Part in Part? | What do you do?

    Derek Eldridge

      Lately I've been seeing a lot of people modeling with parts in parts.

      Part in Part = When a piece of hardware, such as a pin, or a pem nut, is inserted as a "part in part" to a block or sheet metal part.

      Inserting a Part into Another Part

       

      USE CASE

      It's like this, you have a part (solid model with pressed pins or sheet metal model with pem inserts) that will be contract manufactured with some kind of pressed insert. Documentation wise, the part will be ordered and delivered as 1 part, with a drawing that depicts dimensions and inserts. The inserts themselves will never be stocked, thus will never be ordered by themselves and do not need there own internal part number.

       

      The point, is to keep the model references clean, with a clear association of 1 p/n to 1 part to 1 drawing. (2 files total)

      Obviously, modeling wise, both parts can be placed in an assembly; and a drawing created for the assembly with a single p/n.

      This results in 4 electronic files to document 1 p/n:

      • 1 Drawing (Named as P/N)
      • 1 Assembly (Named as P/N)
      • 2 Parts (Named as P/N-01 & P/N-02)

       

      I WANT YOUR OPINION!

      1. Tell me why you are in favor, or not, for using the part in part method of modeling.
      2. If not in favor, tell me what you do to address the described use case above.
      3. Please list Pros/Cons to any method you are arguing for or against.
        • Re: Vote in Favor or Not | Part in Part? | What do you do?
          Steve Calvert

          Never have been in favor of a part to part relation except when doing machining on a casting part.  We have a PDM system and assemblies are just really easy with SW so I'd vote against it for most of the times.

           

          Steve C

          • Re: Vote in Favor or Not | Part in Part? | What do you do?
            Glenn Schroeder

            My general guideline (and it's my guideline, so I can deviate from it if I want to) is that anything that gets welded together is a single Part, so pretty much the only time I do it is if a hex nut, or something similar, is welded onto other bodies.  Since custom properties of the nut come over as cut list properties this works pretty well for my cut list.  Sounds similar to your situation.

            • Re: Vote in Favor or Not | Part in Part? | What do you do?
              Patrick Couture

              I'm doing the part in part process, especially for inserted pem. I order the finished part from a subcontractor that does the laser cutting and insertion of the pem so that way I send him one drawing (One part number) with two pages one with the inserted pem and the other only of the laser cut part.

              • Re: Vote in Favor or Not | Part in Part? | What do you do?
                Steve Calvert

                Sorry, my machine died mid sentence...

                 

                The main reason why it's good, IMHO, to have the set up Drawing, Assembly & Part is so that different people can be working at the same time on these files.  No, it doesn't happen much but I've been involved in doing drawings while others are working on assy/part.

                 

                And like I said above, in most cases, some kind of PDM system gives you better chance of keeping an idea of where that nut is used because sometimes that nut could be not available any more and how would you know?

                 

                Steve C

                • Re: Vote in Favor or Not | Part in Part? | What do you do?
                  Rubén Rodolfo Balderrama

                  It depends on the type of project that I am going to do, it will be the type of strategy that I apply.

                  1-Parties and related assemblies is my project ideal for most of the cases.

                  2-Part in part is only if I'm going to design a cutting tool where the complexity of it is complicated after relating.

                  3-Both methods equally in the same design.

                  By this I mean that one can not limit oneself to a particular type of strategy.

                   

                   

                  Only option 1 can give me all the data for a BOM, the following ones have their degree of complexity but it does not mean that it can not be done.

                  • Re: Vote in Favor or Not | Part in Part? | What do you do?
                    Matt Lombard

                    There are some situations where it's valid to model an "inseparable subassembly". like:

                    captive fasteners

                    weldments

                    an assembly you buy off the shelf as a single part number in your product where there is no internal relative motion

                    some manufacturing processes such as overmolding, or staking, soldering, welding, where differing materials are permanently joined

                    (items like batteries or tires are considered a single part even though they are not - as long as you're not the manufacturer)

                     

                    Does the individual part have its own part number at any time in your process? If you have to purchase a part to add it to something else, then you need to document the part as purchased (like a nut welded to a plate). But if the part is just part of the process (like a material molded over a bar to make a handle) then you wouldn't document the plastic pellets formed as a handle - only the plastic pellets in bulk for purchasing).

                     

                    You might have to involve your manufacturing and purchasing people in the discussion as well to make sure the solution serves everyone's needs.

                    • Re: Vote in Favor or Not | Part in Part? | What do you do?
                      Paul Salvador

                      Hello Derek,.. you bring up a good question... and I wonder.. will the user base request SW Corp to allow a *.sldprt to become a quasi-sldasm or allow for a PDM to extract consumed sub component/properties for this very purpose? 

                      • Re: Vote in Favor or Not | Part in Part? | What do you do?
                        Doug Liles

                        It would be helpful in our case.  We have sheet metal parts with pemserts and have in the past resorted to only showing them in a drawing view rather than trying to add them to a sheet metal part is 12 locations.

                         

                        Thanks

                        • Re: Vote in Favor or Not | Part in Part? | What do you do?
                          Jeremy Zuvich

                          A solution we use for this is making virtual parts and putting them into an assembly. You can make a library of parts that do not normally exist in your system (pins, PEM inserts, etc.), drop them into your assembly, then make them virtual. That way there is only one file (the assembly) with one drawing. This has the added benefit that if you want to make the part yourself at a later date, you can add these parts to your system.

                           

                          Edit: This solution is fine for smaller or less complex parts, but may not be great for more complicated files. If you have a sheet metal part with 5-6 PEM studs in it, that's fine. But if you have a complex weldment with 50 weld nuts, 22 PEM studs and 143 holes, this might not work well.

                            • Re: Vote in Favor or Not | Part in Part? | What do you do?
                              Derek Eldridge

                              Jeremy Zuvich, I wasn't sure if someone was going to say it. Virtual Parts is how I've been handling part in part as well. I feel there is more control over the "quasi-sldASM" in a real sldasm file and better control of the file structure. With no external links the files stay clean.

                               

                              A couple other notes on part in parts is that PDMworkgroup never showed the relationship in the assembly tree. Though granted PDMw has been abandon as of 2018, I don't know if the replacement has the same issue. We'll be moving to PDM professional (aka originally EPDM) soon and i'm not sure how the part in part will be represented there. On the same note, i'm not sure how the virtual parts will be searchable in PDMp as well.

                               

                              One issue i had recently with the virtual parts I use with PDMw is when I did a task scheduler "Convert Workgroup PDM Files" (2016 to 2017). All my virtual files did not convert and many were corrupted. We had to check back in versions someone luckily still had local. Then I had to manually convert the virtual files to the new version. (Open, Rebuild, Save, Checkin)

                               

                              Is anyone else using Virtual Parts to replace the part in part approach?

                            • Re: Vote in Favor or Not | Part in Part? | What do you do?
                              Derek Eldridge

                              Is there a way to convert a body in body to a solid body such that there is no longer an external reference?

                              Or convert it to an assembly with virtual parts?

                                • Re: Vote in Favor or Not | Part in Part? | What do you do?
                                  Matt Lombard

                                  There are 4 main body <=> part commands: (I'm not talking about deleting, splitting, or merging bodies, I'm taking about moving bodies between parts)

                                  Pull Functions:

                                       Insert part Insert one part into the active part.

                                       Insert into new part Places the current part into a new part

                                  Push Functions:

                                       Split Uses sketches planes or surfaces to split the current part into bodies which can then be saved out as separate parts

                                       Save Bodies Essentially just the last half of the Split feature.

                                   

                                  For a lot more indepth information, the SW2013 Bible has chapter 31 on multibodies and chapter 33 on master model techniques. These are just the chapters that focus on multibodies, other chapters also handle the topics. The conversation changes slightly if you are talking about solid vs surface bodies. Some of the 4 functions can deal with both, and some can't. I would be a big fan of SW compressing these 4 similar but not the same functions into one or two easy to understand functions that work for both solids and surfaces, and can be found from both the parent and child documents. I usually use Insert Part and Split.

                                  • Re: Vote in Favor or Not | Part in Part? | What do you do?
                                    Derek Eldridge

                                    Is there a way to convert a body in body to a solid body such that there is no longer an external reference?

                                    Or convert it to an assembly with virtual parts?

                                    I found an alternative solution to my question that was not mentioned.

                                    If a part has already been prepared as a Part in Part (aka Derived Parts) and you want to remove the external references the following will convert the features into solid bodies in the main part file. Thus eliminating any external references and/or permanently broken references.

                                    1. On the List External References for Parts and Features page. List External References for Parts and Features
                                    2. Check Box "Insert the features of original parts(s) if references are broken"
                                    3. Then Select Break All.

                                    This is not undo-able. But the result; folders are created for each external part, labeled with the external part names, and all features from each external part is imported into their respective folders. In other words, you are left with a multi bodied part, with no external references.

                                     

                                    Enhancement Request?

                                    However, this does not work when exporting a body ("Insert into new Part") as a method Matt was mentioning.

                                    If it did, it would be extremely useful for dividing up Master files such as device skins where all the parts are created in on master part file.

                                     

                                     

                                    EDIT:

                                    It should be noted, that when Break References is used without the Insert checkbox mentioned above, the external reference is forever more listed in the File -> Find References and I have not found a way to remove it completely after the fact. IOW, Break References may no longer have an active link back to the reference, but the external reference is still listed.

                                     

                                    EDIT2: (2018-06-18)

                                    In performing the above with some part in part files created by others in the past, I found that the "Insert the features of original..." fails if the external part contains "Mate References".

                                  • Re: Vote in Favor or Not | Part in Part? | What do you do?
                                    Carrie Ives

                                    My preference for inseparable assemblies is to use an assembly. This lets me create items that will be reused and keep them in a library (PEM) hardware. These models probably don't have a company part number (depends on the company) but rather are named with the vendor part number. I can easily create a BOM on my drawing listing the number of each type of hardware. (This is likely to be a BOM that lists the vendor part number. I also usually exclude the base sheetmetal part from the BOM.) It is also pretty easy to change from one size fastener to another. If I have a design table, it is very easy to switch out the hardware. If it isn't a table, but rather individual models, it isn't that hard to replace the components. I have not tried bringing these parts into my sheetmetal part using insert part.

                                     

                                    I have worked on parts where the SolidWorks PEM design library features were used. These were not separate bodies (I think, I'm going from memory here. I know the hole was created as part of the feature.) and we ended up having to manually count to determine how many of each size fastener there were. If we had to change size, we had to delete the feature and put a new one in. The hole was part of the library feature. DON'T GO DOWN THIS PATH. It was a big mess.

                                     

                                    If I am creating a plastic part with an overmold, I will use a multibody part for it.

                                     

                                    I have used a skeleton part inserted at the start of a part to bring in controlling design information. I found this worked pretty well for keeping things related through various renames and such (much cleaner than saving bodies if renames were involved).

                                     

                                    Release procedures vary from company to company and PDM (or lack of PDM) system. Think about the whole process for your company to determine what makes the most sense.

                                     

                                    I usually just send a PDF and STEP file out to my manufacturer and keep the SolidWorks native files in house.

                                     

                                    I have frozen external references, but do not recommend break references since you can't undo it.

                                    • Re: Vote in Favor or Not | Part in Part? | What do you do?
                                      Chris Saller

                                      I create assemblies all the time. Sometimes I will insert a part into a part for something like a helical insert into a plate; it's not an assembly.

                                      • Re: Vote in Favor or Not | Part in Part? | What do you do?
                                        Jim Moses

                                        Hi,

                                         

                                        I use assemblies, I use to do the part in part but one limitation I found was if you have to swap out parts I could never find a good way to get that to work without a bunch of missing links and dangling geometry in cuts and holes added.

                                         

                                        Either method will keep things linked, unless you do virtual parts then there is no links back to the base part which is fine for purchased items, not so much for internal product as its hard to manage.

                                         

                                        Regards,

                                        • Re: Vote in Favor or Not | Part in Part? | What do you do?
                                          David Matula

                                          lots of good info here.  I would say do what works best for your processes.  I do parts in parts for purchased items, casting machining, and a few other processes where I would have used configurations in the past.  screw up a configuration dim and the casting drawing changes. 

                                          Also why I like weldments, that used to be a huge assembly, now it comes in as one part and modifying is so much easier.