Assembly from Part – No mates required

So far you must have been creating your assemblies from parts using Bottom Up method in which you first design and model parts, then insert them into an assembly and use mates to position the parts. To change the parts, you must edit them individually. These changes are then seen in the assembly OR using Top Down method in which one or more features of a part are defined by something in an assembly, such as a layout sketch or the geometry of another part. The design intent (sizes of features, placement of components in the assembly, proximity to other parts, etc.) comes from the top (the assembly) and moves down (into the parts).

Now take a case of multi body part which you might need as an assembly. The option might be to save the individual body as separate part using “Insert into New part” option, insert them into a new assembly and use mates to position the parts.

STOP using this method and let’s talk of a different and simple method/option called “Create Assembly” which will help us to create an assembly directly from a multi body part without getting into hassles of using Bottom Up method, hence saving a lot of time.

  1. Open or create the multi body part. I have created a steel table with legs and a table top. 
  2. Expand the Cut list or Solid body folder by clicking on the + sign next to Cut list or Solid body folder (As I have weldment part used for describing the method, you’ll see only cut list is being used in next steps)
  3. You will see the bodies contained in the different folder based on their shapes and sizes. Their name is automatically driven through SolidWorks.
  4. Rename (if you wish or need) their name to something meaningful or something you can recognize easily.
  5. Now right click on the cut list and select save bodies.
  6. Next you’ll see Save Bodies property manager. Click on Auto-assign Names.
  7. The names which you have given in step 4 will be applied to the bodies here. Don’t worry about the order of the bodies.
  8. Now comes the important step. Click on Browse under “Create Assembly” in the same Save Bodies property manager. This will prompt you to create/save a new assembly.
  9. Key in the required assembly name and click on save.
  10. Finally click OK under Save Bodies property manager to execute the command of creating the assembly.
  11. Hurray, you have just made an assembly from a multi body part. The new assembly will open up or in case it don’t, you can always open it up from the location where you saved it.
  12. Now you can use this new assembly for other assembly operations like exploded view, BOM, etc.
  13. Also any changes done in the part will be reflected in the assembly. 
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23 thoughts on “Assembly from Part – No mates required

  1. Peter

    Is there any way to get thread info onto the saved body?
    The weldments we make often have holes in tubes and plates that need to be machined before the weldment is assembled. I am looking to use the ‘save bodies’ command to make a set of parts and associated drawings of these components to have them machined.

    However, when I make drawings of the parts I cannot use the hole call-out tool and get thread data. Is there an option somewhere to get this data or am I missing something?

    Thanks,
    Peter

    Reply
      1. Peter

        I was using relative views before and only showing the required pieces to machine but the shop has requested individual drawings with associated part files. I guess I will either have to manually enter all hole info, or make each of the parts individually and assembly them together. It’s too bad because a top-down approach would be much more effective for most weldments but not having hole data is a major deal-breaker.

        Thanks Anyway,
        Peter

        Reply
          1. Peter

            Similarly to adding the hole in the part itself, that would provide the hole data as required. However, it means to change the weldment geometry and hole locations you would have to go to two separate files (update the geometry in the top level part then modify the holes in the assembly) eliminating some of the benefit of having a master part. We have multiple users accessing files without a PDM so file structure must be as intuitive as possible.

            It is a good idea though and may be helpful in some instances.

            Thanks,
            Peter

            Reply
            1. Deepak Gupta Post author

              I would rather suggest you to talk to manufacturing people and explain them the benefit of using Weldment or Multi-body rather than going for assembly and further more complications.

              Reply
  2. ELANGOVA

    hi i have created a frame assembly which contains about 20 parts but while saving it unfortunately i chanced the file type as part . my problem is nw i cant open tat in assembly if i open its showing the whole assembly as a part how can i convet it into assembly? pls help am in troble
    eelangovanmech@gmail.com

    Reply
    1. Deepak Gupta Post author

      The option with you have is to use the above method I have suggested and convert the part into assembly but they’ll be still dependent on the part file.

      The other option is to build them again..

      BTW what option you used for assembly/parts: Top down or Bottom up??

      Reply
      1. ELANGOVA

        its bottom up assembly. but i cant find cut list in my part and its nt a solid part surface part how to change surface body into solid body

        Reply
  3. Jilling

    Hi all, normally when creating a multi bodied part, you know which parts are the same and you don’t want listed as induvidual parts in your BOM. Before I save the bodies (after renaming!) and creating the assembly, I use the body delete feature to erase the duplicates. Of course, they will be missing in the assembly so have to be added manually :-( This may not be too hard to do, especially when using a pattern or better still, a feature driven pattern.

    Reply
    1. Deepak Gupta Post author

      Dwayne, you can’t combine them. And I didn’t understand the concept or idea of combining them. If they are same, they why the same part can’t be used via component pattern or inserting again.

      Reply
      1. Dwayne Gavel

        They (the legs) were combined in a cut list when the models was a weldment part, so it just seems counter-productive to have to alter the resulting assembly to get the desired BOM results. While it would be manageable on a simple example like this, such assembly restructuring on a more complex model might be considerably more difficult …

        Reply
          1. Dwayne Gavel

            Hi Deepak, I think there are actually 5 different line items in the BOM … 1x table top & 4x individual legs. Since the legs are all the same, I was hoping they would be recognized that way in the newly created assembly. I guess not.

            Reply
            1. Deepak Gupta Post author

              Yes there are 5 items with 4 leg as same. But they don’t behave same while you convert them to assembly.

              You raised a very valid point here and I’ll see if I can put up an Enhancement request.

              Reply
              1. Samuel

                Has this been fixed (at least as of SW2012)?
                I’m running SW 2011 and the issue described here is still a problem.

                That is, when converting a weldment to an assembly, the “cut-list grouping” is completely lost. In the resulting assembly file, parts that are identical are treated as different parts instead of being treated as different instances of the same part.

                Reply
                  1. Rob

                    Have you had a chance to post your work around? Losing the cut-list grouping (i.e. In your example having each leg become individual parts instead of one part use four times) makes this function of SW useless for us.

                    Reply
  4. Matt

    That’s a cool trick! I didn’t know you could do that. I do a lot of stuff like this at work and when I begin it seems like I either have to make a choice to draw it as a weldment or an assembly. This allows me to do both and make drawings of individual components if I start it as a weldment. I like how the assembly updates along with the original weldment when you modify your original weldment sketch.

    Reply
      1. Balaji

        Hi deepak, I want to save multibody into individual parts. I tried the the API CreateSaveBodyFeature, but it didn’t work. Can you please provide me the API / macro to save a multibody into individual parts.

        Reply

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