Solidworks best practices

I’ve been meaning to ask for a while now about everyone’s workflow when creating complex products and assemblies in Solidworks. Having learned NURBS (Alias/Rhino) before parametrics, I got used to creating large surfaces and solids and splitting them up to create all of the parts needed for the final product assembly. As a result, when I build in Solidworks I work within a single part file and create multi-body parts, rather than building as an assembly from the start. For me, it’s much easier to track my history and make changes throughout the process if everything is built together. Is this an acceptable practice? I’ve never had a factory come back complaining about it, but I’ve always felt like it’s not quite the way things should be done. Any input is appreciated.

I’ve been thinking about the same thing over the years and came to the conclusion that it’s just alright to build everything in a single file then export everything in separate files with the save body function. However it depends what kind of products you are doing. I think that we have this impression because the majority of Solidworks users are engineers and work with existing parts and hardware that are more suited for an assembly type build. If your products are not insanely complex and have a reasonnable amount of parts I think it’s alright to build everything together. In my case, I have to invent a lot of intricate snaps and mechanisms in the kitchen gadgets I do and it’s just easier in a single file. Also, most of my parts are new and I use few harware parts. You have to be careful in the way you build your 3d that all your radius are at the end of the build tree so the file doesnt get too slow. Other than that I have yet to find a huge drawback to working like that. Like a lot of softwares whatever’s most efficient for you works I guess !

For what its worth. I would have been crucified if I had done this at my old job. Then asked to rebuild the entire thing. At my current job I do exactly what you do. (but i dont hand off final production CAD there).

My old Standard practice: Example: small costumer electronic (rough overview)

-Design base form all external surfaces.
-Insert Split lines (part lines).
-Save out base form in 3 different copies. (this part had 3 main plastic pieces)
-Assemble these parts in an assembly.
-Cut away the main shape to form the shells of each part (each part has the exact same feature tree right now, just different cut patterns) (optional go back and have your sketches reference only one of the parts sketches - thus linking all the sketches)
-detail out production features in each part individually. (wall thickness, reveals, bosses, labels recess, etc)
-model and add in supplementary parts. referencing surfaces and sketches so its all parametric (labels, components, rubber feet, etc)

Also every feature is named and labeled, so if edits needed to happen by someone else, they wouldn’t spend forever trying to figure out where you made X feature.

Multi Body files have been successful for me for the past 12 years. My CAD workflow is the following, post front end design development (sketch, PS, rough proto modeling, etc.):

  1. Overall Modeling - Surfacing (major sections / plane construction)
  2. Design Radii, not manufacturing Radii
  3. Split Master File
  4. Save Bodies - Not Split Body feature
    4a. Convert to Assembly
  5. Individual part/component processing for manufacturing send out

This has been a bit cumbersome using the PDM Works. You have to structure your local folders in such a way so you don’t accidentally override files when checking parts out. Since I do both the ID and design engineering, I find ways that work best for me. However, in a shared studio environment, I believe folks just come together and do what works best for them.

The process of products gets much more involved past design and production. When you hit inventory management, fulfillment and purchasing, it helps to know if you can do things on the front end to help influence certain functions of the business. When it comes to the complexity of the business operations, CAD seems a lot less complex. Just a thought.

Haha. I’m actually just starting to get a taste of that and definitely have to agree.

Outside of this subject, I think we need to start another thread regarding financial analytics for product design. Part of my design function is to forecast cash outlays and ROI on my product concepts. The problem in my spreadsheets is that I’m spending most of my time laying out the graphics on excel. Every time the execs ask about my numbers, I tell them, “What you should really be concerned with is the page layout and the figure ground relationships between the numbers and headings!” You ask a designer to do accounting, that’s what you’re gonna get.

Seriously, very difficult stuff for me, hedge the risk, and run the numbers; It’s painstaking but it doesn’t just bridge the gap, it moves the land masses of design and business closer together.

On another note, has anyone used the cost accounting module in Solidworks…successfully?

You may want to look into the ‘master modeling’ approach / technique. The basic idea is that you “only create features in the master model that will be shared by 2 or more derived components.” You would then create a new part for every actual part, and use ‘insert part’ to insert the master model into them, then build from there.

I always feel like I’m doing SW wrong, but everyone I ask says there is no best practice.

I think that I follow Sain’s approach when doing a significantly complicated shape/assembly. Do a base part that I split. Shell the new parts and add in all of the technical stuff there.

I’ve worked with other people’s models that worked like VanDeBar and I wanted to kill myself. I couldn’t understand what was going on. It’s something to get used to I guess!

Same here, everything seems to be different everywhere. But the “top down” assembly approach. Is really nice when doing complex things, but a bit overkill on smaller items.

Maybe CADJunkie can chime in.

I’d like to take a step back and maybe be a bit more philosophical rather than down and dirty in the trenches for a moment.

So there’s an real and true inherent chicken or egg thing when it comes to Top Down vs Bottom up vs Single Multi-Body. (There’s a huge difference between Master Part files/Multi-Body modeling and Top Down) I feel like some take to one process or the other without really truly understanding the ever so subtle difference that may or may not be advantageous for your process. When working in groups, say smaller than 10 (and this is just pace holder) vs larger, non-interactive groups (i.e. not located directly in the same location or working in various silos) “Picking up the Ball” from another designer/engineer with the proper version. Below are just a few items that might help to shed some light.

Bottom Up


  • Dimensions for each part is located within that Part which for technical drawings can be helpful. Though many will say
    that the dimensions used to create a Part file are the same ones needed for 2D. (This almost by itself could be just a single
  • Much lighter (depending on geometry/features) with regards to rebuild time.
  • Reuse for other projects can be leveraged easier. (i.e. less baggage/weight to consider )


  • There’s no way to “see” the other Parts to design around it/in context to it.
  • Each individual models has to be put together in an Assembly. (Though a Part file can be inserted into a Part file… Read:
    Painful when considering this same process when done in an Assembly).
  • Surface continuity just isn’t as nice between two models created separately vs as a single body and split.

    Top Down


  • Can see the entire model/other Part files so that the design can be made with in-context tolerances.
  • By creating references across part files, update one model and any referenced models will update with it.
  • Changes can be pushed down and updated


  • Too many external/In context references can definitely slow rebuild time.
  • Unless in-context references are broken there’s really no way to do a true assembly without wrecking havoc. (in-context
    reference can be suspended so that updates don’t happen.)
  • Gets extra confusing if Part files are saved internally within an Assembly vs externally, especially from a file management

Multi-Body Part file


  • Many of the benefits of both Top Down and Bottom Up.
  • Less files to keep track of. Features available only at the Part level. (One could argue that editing a Part file at the assembly level
    nets the same result…)
  • Geometry Surface continuity if build as one body and then split apart.


  • Not possible to have movement to check for collision/interference/physical dynamics aka Assembly
  • Though geometry can be altered once bodies are split to their own respective Part files, the Master Part File controls true
    changes because that’s where the dimensions/relationships are held.
  • Making technical drawings of individual bodies, once save/inserted…etc into a new Part file is not possible when compared to
    bottom up.

This paradigm is pretty exclusive to Solidworks in terms of operations, functionality,…etc. I would not list these same items for say Creo, Inventor, or SolidEdge.

Great breakdown, Cadjunkie !

I guess it depends on the person who’s making the CAD. I’ve worked with people throughout the years that had great and nightmarish top down approach. Same for multi body. I think if you keep in mind to make your 3d comprehensive enough so that a coworker wouldn’t need explanations it’s fine. I tend to classify features with folders and rename features so that the next person gets the story. Also, like I said before it all depends on the complexity of the project.