Boston Device Blog

Solidworks Tips - Top Down Modeling

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Solidworks is an invaluable tool for the modern engineer and allows them to bring ideas to market quicker, prototype faster.  However, modeling a part, a sub-system, or a top-level assembly is often times easier said than done.  Often times, it takes not only an intricate understanding of what is to be designed and the engineering challenges, but also a good deal of planning ahead so that your model is "robust" and easily adaptable to downstream changes that inevitably occur as breadboarding, prototyping, and other outside variables drive design changes. 

One way of achieving a "robust" Solidworks design is through the practice of top down design.  What is top down design?  In the most simplistic sense, it is creating a hierarchy wherein the framework for an entire assembly is designed before that of the individual parts.  This framework, referred to as a "master model", behaves as the groundwork for which all the individual parts and components are created.   Because these parts are all parametrically linked together through the master model, it is possible to make numerous changes to parts within an assembly by merely revising the master model without fear of interferences or other design head-aches.  Here are some general tips to top down modeling;

Sketch your concept.  The easiest way to get out of the habit of bottom up modeling is to create a rough sketch of the system or the assembly that you are about to design.  This sketch is primarily used for identifying key engineering challenges and the necessary components that need to be designed or integrated into a system.

Build a "Master Model".  Now that a rough sketch has been created and all pertinent parts to a system have been identified it is time to create a master model in Solidworks.  Start by opening a new part file and from the rough sketch start laying down 2D sketches that will drive the base features to all the parts in an assembly.  Be sensitive to how your base features will be created (extrusion vs. revolve) and build the sketches accordingly.  Create new datum planes and features where necessary and fully define your sketches with dimensions and relations.  When complete save the part file and assign it some sort of nomenclature so that your recognize it as the master file.  An "_master" suffix works quite well.

Create the individual part files.  This is the time to break out the individual parts and finish up the design details.  Open up a new part file and go to Insert-> Part.  The Solidworks' File Open Window will now appear and from there you should select the the master model file which you previously designed.  In the Solidworks Feature Manager select the design features from the master model which you would like to carry over into the part file.  By clicking the green OK check mark, the master model is automatically located to the same reference planes which they were initially created.  After inserting the master model expand the design tree to view the various sketches and select the base sketch for the part which you would like to design.  Utilize the appropriate feature operation (i.e. Extrude, Revolve) to create the base feature for this new part.  After this is completed you can finish whatever detailing may need to be done to the part.  This same methodology can be applied to the remainder of the parts that need to be created.

Build the Assembly File.  The final step is integrating all your parts and up-front work into a final assembly file.  This is where you should recognize the benefits of the top down modeling scheme.  Start off by creating a new assembly file.  Before going ahead and inserting the part files in the assembly you are going to want to first want to insert an "Envelope" of your master model.  Go to Insert->Envelope->From File...  and select the master model file.  It may appear that nothing has happened, but take notice that in the modeling frame the cursor has a part icon beside it.  Click anywhere in the frame and an envelope of the master model will be dropped into model.  Similarly to a part file you will want to mate the Front, Right, and Top planes to that of the assembly file.  Now go ahead and start inserting the indivual parts into the assembly file and voila! there's your assembly.  Need to make changes to the assembly that impact the base features?  Simply expand the Envelope in the design tree and edit the base sketch as necessary and rebuild. 

Here is a short video of a simple calibration assembly being created using the top down modeling method.