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.
- Open or create the multi body part. I have created a steel table with legs and a table top.
- 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)
- You will see the bodies contained in the different folder based on their shapes and sizes. Their name is automatically driven through SolidWorks.
- Rename (if you wish or need) their name to something meaningful or something you can recognize easily.
- Now right click on the cut list and select save bodies.
- Next you’ll see Save Bodies property manager. Click on Auto-assign Names.
- 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.
- 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.
- Key in the required assembly name and click on save.
- Finally click OK under Save Bodies property manager to execute the command of creating the assembly.
- 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.
- Now you can use this new assembly for other assembly operations like exploded view, BOM, etc.
- Also any changes done in the part will be reflected in the assembly.