Solidworks Best Practices

Sketches

• Pre-modelling sketching! (That means pencil and paper, or ipad drawings!)

  • Don’t need full dimensions, just a pictoral representation of your concept

• Take advantage of Sketch + Part Symmetry

• Fully defined sketches - all lines must be black in your sketch when it’s done. The exceptions to this are splines, and the endpoints of construction lines. Generally good to at least constrain construction lines vertically and horizontally, even if their length isn’t defined

• Be careful about Auto-relations - can hold ctrl while drawing to prevent them from occuring

  • Auto-relations highlight the entity orange, and the relation will appear in yellow before you click

• Never use “Fully Define Sketch” - causes Solidworks to just guess what dimensions are important for your design, irrespective of your design intent

  • In a similar vein, never use the Fix relation - this just locks things in place

• Don’t use a dimension where a constraint/relation would work

• Selection boxes - if you start in top left, you get a blue box which only selects entities that are entirely within the box. If you start from the bottom right, you get a green box which selects every entity the box touches.

• Symmetry Vs. Midpoint - symmetry is always preferable to midpoint

  • To implement a symmetry relation, click two entities and an entity to mirror over, and add the symmetry constraint

• Sketch labels in feature tree

  • An Underdefined sketch has a next to the sketch name in the feature tree - this should never be there unless you’re using splines

  • Over-defined/unsolvable sketches - text in tree is yellow

  • Sketch with helping hand symbol - shared sketch, should probably avoid unless you have a good reason

  • Contour based (symbol is a polygonal shape with a hole in it) - should also have a really good reason to use this

• General rules for Sketches

  • 1 feature per sketch

    • Do not cross-reference sketches unless absolutely necessary

  • Always use closed loops (unless doing a thin feature)

  • Do not use fillets, chamfers, or patterns at the sketch level - only at feature level

• Convert entities

  • Project pre-existing sketches or entities into the active sketch

  • Generally stick to sketches and avoid converting entities on faces for stability

• Replace Sketch Entities

  • Maintains all relations in a feature while changing the sketch geometry from one entity to another (say, line to arc)

• Quirky Dimensioning tricks

  • Click on line, click endpoint of the line, you get a crosshairs, can then dimension the angle of the line without needing a reference geometry line

  • Dimension to tangent

• Should start sketches on a major coordinate plane instead of a face whenever possible

• Change Sketch Plane

  • If you started a sketch on the wrong plane, can right click on the sketch in the tree, hit edit sketch plane, and then select a new plane for the sketch to exist on.

  • This can sometimes cause your sketch to be flipped, but it’s easy enough to flip it back

• 3D sketches

  • Red arrows show which coordinate system you’re gonna sketch on (yellow plane also indicated)

  • Pressing the tab button will flip the coordinate system so you can sketch on different planes

• Quick 3D sketch - Weldments

  • Model what the solid inside your frame would look like instead of the 3D-sketched frame

  • Select all the edges, convert to lines, delete out the body to leave the weldment structure

  • Steps:

    • Make your 3D model

    • Press F5 to get selection filter - turn on edges filter

    • open 3D sketch

    • CTRL + A to select all edges

    • Convert entities to get a 3D sketch from the body edges

    • Convert 3D sketch into weldments

Parts/Features

• Starting a Part - The Correct Way! (example was a cube)

  • to get a center rectangle, start with a normal rectangle, draw 2 perpendicular construction lines, and use 2 symmetric constraints

  • Use bidirectional extrude to keep the origin centered on the part

• Feature Tree Features

  • Rollback bar - click + drag up to temporarily absorb features (appear as grayed out)

    • Helpful for reverse-engineering a part, or making edits to a feature several features back

  • Right click → Show flat tree view - shows all sketches and features in chronological order

  • Hit F8 to open flyout menu from tree - columns which appear are hide/show, hide/show bodies, appearances, and transparency

    • Lets you easily hide and show all of your sketches on the fly

  • Filter bar - allows you to search for specific items in the tree

  • Collapsing the tree - single left click on the empty space of the feature tree, and press Shift + C to collapse the tree. May not work if you accidentally select a specific item in the tree

  • Suppress components

• Feature naming + Folders

  • Features can be renamed and put in folders for better organization and clarity

• Show Parent/Child Dependencies

  • Dynamic Reference Visualization - right click on a part at top of feature tree and click dynamic reference visualization on the flyout menu - have to do this for both the parent and child option

  • Shows blue arrows for parents of a feature/sketch, purple arrows for children

  • Shows you dependencies, i.e. what features/sketches need to be intact for a given feature to rebuild properly

• Keeping a “Flat” feature tree

  • Minimize dependencies between features

  • Another argument for referencing sketches off of the major coordinate planes instead of faces of bodies - increases model robustness by reducing dependencies between features

• Design Intent

  • Trade-off with a flat tree. Can’t always keep a flat tree, which is ok!

  • Balance design intent and robustness of model

• General rules of modelling

  • Start with main geometry

  • Most robust features (extrudes, cuts, revolves etc.) first

  • Less robust things later (fillets, etc.)

  • More stuff that I didn’t manage to copy :(

• Commenting

  • Can right click on a feature to add comment

• Display states

  • Used for visualization only

    • different color combinations, hide/show different parts/bodies

• Configurations

  • Used for physical differences

  • USE WITH CAUTION - often just ends up making CAD messy and not robust - very often breaks, and it’s typically better to just make a second part

• Absorbed vs. Unabsorbed features

  • Absorbed = used in feature

  • Unabsorbed = not used in features

• Thin features

  • Use lines instead of contours to create 3D feature geometry

    • Draw lines instead of contours in the sketch

    • Click “thin feature” box during extrude

    • Specify direction and thickness of the thin feature

      • Can do one direction, bidirectional etc.

• Hole Wizard

  • Always use, don’t be scared

    • Never do an extruded cut of the specified hole diameter!

  • You will regret not using it

• Fill Pattern

  • Very nice for lightening parts simply

  • May neglect half-shape cutouts that you’ll need to add manually

• Hole patterns using Multi-body parts

  • Multi-body part modelling is very powerful and robust

  • Always pattern bodies instead of features and faces when you can

  • Uncheck “Merge bodies” when doing an extrude

  • Do a linear pattern of a bodies to generate the 2D pattern

    • Body will be the “positive” of the negative shape you want to cut out

  • Use combine → subtract to subtract the array of bodies from the primary body

  • Lets you very easily go back and change the shape of the patterned cutout

• Speed tricks for Modelling

  • Instead of exiting out of a sketch to create a feature, just do the feature while inside the sketch

  • To make fillets faster, click one edge, wait for selection toolbar to come up, and click on the option that makes the most sense for your part. All edges that will be filleted will highlight pink

    • Make sure “Show selection toolbar” and “full preview” are on within the fillet menu when you select the fillet tool

  • Flip side to cut option in extrude cut - will extrude cut everything outside of a shape instead of inside

Assemblies

• Copy with Mates

  • right click part → copy with mates

    • Follow the steps to select the mates you want to copy, and where you want to copy them to

    • Very useful for duplicating hardware

    • If you pin the copy with mates menu, you can keep doing it repeatedly

• Assembly hotkeys/shortcuts

  • tab - hides part

  • Shift + Tab will unhide a part under your cursor

  • hold CTRL and click two faces - causes mate menu to pop up, and allows you to quickly add mates without ever opening the mate tool

  • CTRL + drag a component to duplicate

  • using right mouse key, click and rotate components to align them properly for mates

  • Flip mate alignment lets you switch direction of mates

  • Can CTRL + C the part name in the feature tree of an open part, and do CTRL + V in an assembly to copy it in. Can also drag and drop parts into an assembly

  • Right click-> change transparency on a part to make it transparent

  • When trying to select a face on a transparent part, can use “select other” to cycle through all things under your cursor that you may want to select, including transparent parts

Tips and Tricks

• Search - allows you to find any command, shows you where it is if you click the eye icon next to the command

• Selection Filter - useful

• Housekeeping - hide any tabs you never use - right click on the tab → tabs → uncheck stuff you don’t want

• Instant 3D → all the way to the right on the features tab. Lets you click on a face edit dimensions without going into the actual sketch for a feature

• Control + C = Toggle construction lone

• F5 = selection filter toolbar

• F8 = Display pane flyout

• Mouse Gestures!

  • Right click in a sketch and drag to get quick access to frequently used tools

  • At the part level, this lets you rapidly switch between views

• CTRL + 8 - does closest normal to wherever you’re looking, or click on a face to go normal to that face

  • Mapping this to the letter n can be handy

  • Doing CTRL + 8 twice will flip to the opposite side

• Press space bar to open a view select mode

• Customize → shortcut bars → can drag and drop commands onto toolbars

• Ask for feature tree reviews! (chief mechE, mechE heads are good people to ask)

  • Go feature by feature and get feedback

• CSWA and CSWP certifications - shows you what tools are available and where they are, but nothing beats experience

  • Greg hasn’t personally ever asked for this or been asked about this on a resume - demonstration of experience probably more important