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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 (minus) 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

  • 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

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