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 splinesOver-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