This is intended both for novice users as well as users familiar with other design software but new to Solidworks. I'll be using language native to Solidworks without equivalencies to other terminology. It is a work in progress. First, I'd like to finish the framework. Later, I'd like to enhance it with User Interface (UI) images. UI tips will be the subject of a separate post.

All entities in Solidworks fall into a hierarchy. From beginning to end, this is it. I could draw a Venn diagram for it, but it would just be concentric circles resembling an onion. As such, in holistic terms, each holon transcends and includes the previous holon. I'll include general descriptions mixed in with contextual tips or suggestions I've learned. [Bracketed terms refer to default menu commands,] although they are also usable as icon buttons. Most can also be located with Search Commands window in the upper right, and by clicking on the Eyeglasses icon next to the Command in the search results, the UI will literally show you where the command is located in the menus, if available.

... (not sure if this is at beginning or somewhere along the way; semantics to consider)
This is the file you select when making any new Part, Assembly, or Drawing. It contains settings which you will always find useful, but can always be overridden manually.

Reference Geometry
All entities begin with an Origin representing (0,0,0) in Cartesian space. 2D entities such as a Sketch has the origin as the projection of the 3D Origin onto the 2D Plane of the sketch as (0,0).

Default Reference Geometry of Front Plane, Top Plane, and Right Plane are included, and can be augmented with custom Reference Geometry within your Part Template or Assembly Template, or augmented specifically for each item created. For example, I find it useful within Assemblies to have Primary Axes already defined within both part and assembly templates. The Y-Axis is created from intersection of Front Plane and Right Plane, and so on. I place them within a Folder in the Feature Tree and name the Folder "RefGeo" or such so that they take up less vertical area in my Feature Tree.

More Reference Geometry can be defined per use on the fly. A new Plane can be created from various constraints: Parallel to another Plane and Coincident to a Vertex, a distance (Offset, which includes Parallel) from another Plane or planar Face, Perpendicular to a Line and Coincident with its endpoint, and many more. Reference Geometry Planes are primarily what 2D Sketches are built upon, although any planar face of a Surface or Solid can also have a Sketch placed upon it (once those exist).

Comprised of Sketch Entities [Tools>Sketch Entities>], Sketches [Insert>Sketch or Insert>3D Sketch] are the basis of all Features and can be either 2D Sketch upon a Plane or 3D Sketch independant of planar limitations. The Sketch Tab shows most Sketch entities: point, line, arc, circle, ellipsoid, slot, polygon, rectangle, text. Any entity can be transformed into Construction lines, which are particularly useful as centerline entities but also useful as reference entities.

All Sketch Entities can be assigned Relations. Often, it is useful to allow Automatic Relations [Tools>Sketch Settings>Automatic Relations (toggled)] in a Sketch, which is represented by a yellow Relation Symbol shown on the entity being created. Simple Relations include: Vertical, Horizontal, Tangent, Coincident, Colinear, Concentric, Parallel, and Perpendicular. Even without Automatic relations, they can be implied in the creation of new entities and assigned manually later, which is represented by a white Relation Symbol is shown on the entity being created. A Dimension is a specific relation relative to selected entity(ies) in units and tolerances either selected on the fly or to defaults chosen in Document Properties [Tools>Options...>Document Properties tab>Units]. Your Unit System is also shown in the lower right corner of the UI, such as IPS for Inch, Pound, Second, or MMGS for Millimeter, Gram, Second, and can also be toggled from clicking that status bar area.

Within a sketch, Sketch Tools [Tools>Sketch Tools>] can be used to propagate entities further as follows. Fillets and Chamfers are automated combinations of lines and/or tangent arcs upon an intersection. Convert Entities projects existing Sketch Entities, Vertices, Edges, or Faces upon a 2D Sketch Plane only. Offset Entities creates parallel entities from source entites, and either source or new or both can be selected to convert to construction lines in the process. Mirror Entities, various Sketch Patterns, Move Entities, Copy Entities, and Rotate Entities do what their names say. Many of the Sketch Tools are unavailable to 3D Sketches as they are are not on a Plane as 2D Sketches are.

Default Sketch Tab icons can be expanded upon by right click on the ribbon and "Customize..." (also [Tools>Customize...]) which leads you to listings and representations of all available icons which can be dragged and dropped into the Sketch Tab ribbon. They stay there and are saved in your UI profile. Useful ones which I've added based on training and experience include Fit Spline, Split Entites, and Instant 2D (toggle). You can add what you find useful.

Surfaces [Insert>Surface>] are more flexible with more deforming commands available than Solids. One major revelation of training with Surfaces is that, while most users are introduced to Solids before Surfaces, all Solids are comprised of Surfaces.

Solids (or Solid Bodies) are enclosed Surface Bodies which are able to be assigned Material Properties that allow a Volume to be provided a Mass.

And I haven't even gotten to the useful stuff. To be continued..



Please be patient for more to come. Thanks.