These tools and default shortcuts are the same in SolidWorks 2024, 2025 and 2026 — the
core modelling workflow hasn't moved in years; each release adds options inside these
commands rather than relocating them. Steps assume the default interface. (Fusion 360 and
others have equivalents, but this section stays SolidWorks-focused.)
Identical · 2024 · 2025 · 2026
Essential shortcuts
- S
- Context shortcut toolbar at the cursor
- Space
- View orientation menu
- Ctrl+7
- Isometric view
- F
- Zoom to fit
- Ctrl+drag
- Copy the selection
- Ctrl+C / V
- Copy / paste a feature
- Ctrl+B
- Rebuild
- Tab
- Hide the body under the cursor
- arrows
- Rotate · Ctrl+arrows pan
Duplicate a body or feature
- Quickest: click the feature in the tree, Ctrl+C, click a face or plane, then Ctrl+V.
- With control: Insert ▸ Features ▸ Move/Copy Body, tick Copy, set the number of copies and an X/Y/Z offset.
- Sketch entities: select them and Ctrl+drag to drop a copy.
Array — linear pattern
- Features tab ▸ Linear Pattern.
- Under Features and Faces, pick the feature(s) to repeat.
- Direction 1: click an edge or axis, then set spacing and instance count.
- Add Direction 2 for a 2-D grid (optional).
- Green check to finish.
Array — circular pattern
- View ▸ Hide/Show ▸ Temporary Axes so you can see the centre axis.
- Features tab ▸ Circular Pattern.
- Pattern Axis: pick a circular edge or the temporary axis.
- Set 360°, tick Equal spacing, set the instance count.
- Pick the feature(s) or body, then green check.
Mirror
- Features tab ▸ Mirror.
- Mirror Face/Plane: pick a plane (e.g. Right).
- Features / Bodies to Mirror: select what to reflect.
- Green check.
Deform borders — Flex & Deform
Flex — bend, twist or taper a whole body
- Insert ▸ Features ▸ Flex, select the body.
- Choose Bending, Twisting, Tapering or Stretching.
- Drag the trim planes to limit the affected region, set the angle, check.
Deform — push an edge or region to a target
- Insert ▸ Features ▸ Deform.
- Curve to curve maps an edge onto a new curve; Point pushes a zone.
- Set the deform region / stiffness, then check.
Fold an edge — sheet metal
- Make it sheet metal: Insert ▸ Sheet Metal ▸ Base Flange (or Convert to Sheet Metal).
- Sheet Metal tab ▸ Edge Flange, click the edge to fold.
- Set the angle and flange length; use Edit Flange Profile to trim its shape.
- Green check — the bend, relief and flat pattern update automatically.
Hollow it out — Shell
- Insert ▸ Features ▸ Shell, set the wall thickness.
- Click the face(s) to leave open (those get removed); select none for a sealed hollow.
- Green check.
Tip
Shell before adding fillets, so the inner wall follows the rounded faces instead of fighting them.
Drive sizes with equations
- Tools ▸ Equations (or right-click a dimension ▸ Add Equation).
- Add a global variable, e.g. "wall" = 3mm.
- Set a dimension equal to it: click the dimension, type =, pick the variable.
Tip
Double-click a dimension and rename it, so equations read like length = 2 * width instead of D1@Sketch1.
One part, many sizes — Configurations
- Switch to the ConfigurationManager tab (top-left, beside the tree).
- Right-click the part name ▸ Add Configuration, name it (e.g. “M6”).
- Change dimensions or suppress features for that configuration.
Tip
For a whole size range at once, Insert ▸ Tables ▸ Design Table drives every configuration from one spreadsheet.
Combine bodies — add / cut / intersect
- Insert ▸ Features ▸ Combine.
- Add welds bodies into one; Subtract cuts tool bodies from a main body; Common keeps only the overlap.
- Pick the bodies, green check.
Tip
Model a stock block, then Subtract your part from a copy of it to preview exactly what the CNC removes.
Pattern along a path — curve-driven
- Features ▸ Pattern ▸ Curve Driven Pattern.
- Pick the feature to repeat.
- Pick an edge or sketch curve as the path; set count and spacing.
Tip
Turn on Equal spacing and Align to seed for evenly placed copies that keep the same orientation.
Edit mid-history — rollback bar
- Grab the blue rollback bar at the very bottom of the FeatureManager tree.
- Drag it up to roll the model back to an earlier point.
- Add a feature there — it inserts into history at that spot — then drag the bar back down.
Tip
Right-click any feature ▸ Rollback does the same jump in one click.
Mass & centre of gravity
- Assign material first: right-click Material in the tree ▸ Edit Material (e.g. AISI 1045 — see the alloy cards above).
- Tools ▸ Evaluate ▸ Mass Properties.
- Read mass, volume, surface area and centre of mass.
Tip
Tools ▸ Evaluate ▸ Measure gives instant distances, angles and radii straight off the model.
Select faster
- Right-click an edge ▸ Select Tangency to grab a whole rounded chain (perfect before filleting).
- Right-click ▸ Select Loop for a face's bounding edges.
- Buried face? Right-click ▸ Select Other, then hover the list to pick it.
Tip
Toggle the Selection Filter toolbar with F5 to grab only edges, faces or vertices.
Mouse gestures — the speed trick
- Hold the right mouse button and flick in a direction — a radial menu fires that command.
- Set them at Tools ▸ Customize ▸ Mouse Gestures (up to 12 directions, separate per sketch / part / assembly / drawing).
Tip
Map your most-used commands (sketch, extrude, fillet, isometric) and you'll model almost without leaving the mouse.
Fillet pro tips
- Model fillets and chamfers last, as the final cosmetic features.
- Full Round fillet (three face sets) rounds the end of a rib or boss cleanly.
- Variable Size fillet tapers the radius along a single edge.
- If a fillet fails, shrink the radius or move it before the feature it's clashing with.
Habits that save hours
- Fully define sketches — they turn black; under-defined (blue) geometry drifts when you edit nearby.
- Name features and sketches in the tree; future-you will thank you.
- Force a full rebuild with Ctrl+Q when geometry misbehaves — plain Ctrl+B only rebuilds what changed.
- Build symmetric parts on the origin planes so Mirror and assembly mates stay trivial.
- One feature = one intent; many small features edit far easier than one giant sketch.
Sweep — a profile along a path
- Sketch the path on one plane; sketch the profile on a plane at the path's start.
- Insert ▸ Boss/Base ▸ Sweep (or Cut ▸ Sweep to remove material).
- Pick profile, then path; add guide curves or twist if needed.
Tip
Tubes, handles, gaskets and custom thread forms are all sweeps. Keep the profile small enough not to self-intersect on tight path corners.
Loft — blend between profiles
- Make two or more profile sketches on parallel planes.
- Insert ▸ Boss/Base ▸ Loft.
- Click each profile in order, near the same corner, so it doesn't twist; add guide curves or a centreline for control.
Tip
A round-to-square transition (e.g. a duct or a forged blank) is a classic loft. Selecting matching points keeps the surface clean.
Draft for cast & moulded parts
- Insert ▸ Features ▸ Draft.
- Set the Neutral Plane (stays fixed) and the pull direction.
- Set a draft angle (1–3° typical) and pick the faces to taper.
Tip
Cast, forged and injection-moulded parts need draft to release from the mould. Add it before fillets so the rounded edges inherit the taper.
Hole Wizard — proper holes
- Features ▸ Hole Wizard.
- Pick the type (counterbore, countersink, tap, pipe tap) and a standard (ISO / ANSI / DIN) and size.
- Switch to the Positions tab and click on the face to place each hole.
Tip
Tapped holes carry the real thread spec into the drawing and BOM — far better than a plain extruded circle.
Threads — real vs cosmetic
- Real geometry: Insert ▸ Features ▸ Thread — pick the edge, a thread profile and pitch.
- Lightweight: Insert ▸ Annotations ▸ Cosmetic Thread — no helix, but shows correctly in drawings.
Tip
Use cosmetic threads on most parts — real modelled helices are heavy and slow to rebuild. Save them for renders or thread-fit checks.
See inside — Section view
- Heads-up View toolbar ▸ Section View (or View ▸ Display ▸ Section View).
- Pick a plane, drag the offset handle to slice through.
- Add a second or third plane for a corner cut.
Tip
It's display-only — nothing is cut from the model. Great for checking wall thickness and internal clearances.
Reference planes & axes
- Features ▸ Reference Geometry ▸ Plane.
- Pick references: a face plus an offset, an edge plus an angle, or three points.
- Reference Geometry ▸ Axis for a spin axis (e.g. two planes, or a cylindrical face).
Tip
Build a plane in mid-air to start a sketch exactly where no face exists — essential for lofts and angled bosses.
Reuse edges — Convert & Offset
- Open a new sketch on a face.
- Select existing edges, then Sketch ▸ Convert Entities to project them flat into the sketch.
- Or Offset Entities to project them at a set distance in/out.
Tip
Converted edges stay linked to the original — change the parent and the new sketch follows. Perfect for matching mounting bosses to a housing's outline.
Engrave a part number — Split Line + Wrap
- Sketch your text with Tools ▸ Sketch Entities ▸ Text on a plane facing the surface.
- Insert ▸ Features ▸ Wrap, set Deboss (recessed) or Emboss, pick the curved face and a depth.
- For flat faces, an ordinary extruded cut works; Wrap is what makes it follow a cylinder.
Tip
Insert ▸ Curve ▸ Split Line projects a sketch onto a face to divide it — handy for a separate plated or knurled region.
Assemblies — find clashes
- Tools ▸ Evaluate ▸ Interference Detection.
- Run it on the whole assembly; each overlap is listed with its volume and highlighted.
- Use Clearance Verification to flag parts closer than a set gap.
Tip
Run this before any prototype order — catching a 0.2 mm overlap on screen is free; catching it in machined metal is not.
Top-down design (in-context)
- In an assembly, right-click a component ▸ Edit Part.
- Sketch using other parts' edges (Convert Entities) so the part fits them exactly.
- Exit edit — the link (an external reference, marked “→”) keeps it matched.
Tip
Powerful but use sparingly: too many in-context links make a model fragile. Lock or break references once the design settles.
Automate — record a macro
- Tools ▸ Macro ▸ Record.
- Do the repetitive steps once, then Stop and save the .swp.
- Replay with Run, or bind it to a toolbar button / shortcut.
Tip
Great for chores like setting view orientation, exporting a STEP, or applying your standard material and appearance in one click.
Weldments — steel frames & a cut list
- Draw the frame skeleton as a 3D sketch (or a layout sketch) — just the centrelines.
- Weldments tab ▸ Structural Member; pick a standard profile (ISO / ANSI tube, angle, channel) and click the sketch segments to sleeve them.
- Trim/Extend to miter the corners; add Gusset, End Cap and Weld Bead features.
Tip
A Weldment Cut List auto-tallies every member's length and profile — drop it on a drawing and it's a ready stock-cutting list for the saw.
Flat pattern → DXF for laser / waterjet
- On a sheet-metal part, click Flatten (or activate the Flat-Pattern in the tree).
- File ▸ Save As ▸ DXF/DWG and choose to export the flat pattern.
- In the export options, send bend lines to their own layer.
Tip
Set the part's K-factor / bend allowance to match your shop's brake first, or the flat blank comes out the wrong length. The laser cuts the outline; the bend-line layer is just reference.
Rib — stiffen without bulk
- Open a sketch where the rib sits and draw an open contour (just the rib's line).
- Features ▸ Rib; set the thickness, the direction (parallel or normal to the sketch) and any draft.
- Green check — it grows down to the nearest faces automatically.
Tip
Ribs add stiffness for almost no mass. On moulded parts keep a rib ≈ 0.5–0.8× the wall thickness or the outside shows a sink mark.
Edit an imported STEP — direct editing
- A STEP/IGES opens as one dumb body with no feature history.
- Direct Editing tab ▸ Move Face to shift/rotate a face, Delete Face to remove one (with Patch to heal the gap), Replace Face to re-surface.
- Or FeatureWorks ▸ Recognize Features to rebuild an editable tree.
Tip
Delete Face on a boss, then let it patch, is the fastest way to clean a supplier model down to just the mounting interface you care about.
Lock a sketch — relations & Fully Define
- As you draw, add relations: coincident, collinear, equal, symmetric, tangent, concentric.
- Use a centreline + Dynamic Mirror to keep symmetry automatic.
- Tools ▸ Sketch Tools ▸ Fully Define Sketch auto-adds the missing dimensions/relations.
Tip
Black = fully defined (stable). Blue = under-defined (will drift). Red = over-defined — delete one conflicting relation to fix it. Aim for black before you extrude.
Surfaces — rescue a bad body
- Build surface bodies with Extrude / Loft / Boundary Surface for shapes a solid can't do.
- Surface ▸ Trim the overlaps, then Knit them into one watertight quilt.
- Thicken the quilt (or fill it) to turn it back into a solid.
Tip
When a messy import won't thicken or boolean, delete the bad faces, rebuild them as surfaces, knit and re-thicken — the standard repair workflow.
Mates that do real work
Advanced
- Width centres a tab in a slot; Symmetry and Profile Center auto-centre parts.
Mechanical
- Gear, Rack & Pinion, Cam, Hinge and Screw mates drive realistic motion.
Tip
A Gear mate with the right ratio spins two meshing gears together so you can sanity-check a mechanism before cutting metal.
Fill Pattern — grilles & knurls
- Features ▸ Pattern ▸ Fill Pattern.
- Pick a boundary (a face or a closed sketch) to fill.
- Choose a layout — hex, square, circular — set spacing, and the cut shape (hole, diamond, the built-in knurl, or your own feature).
Tip
This is the clean way to do speaker grilles, vent slots and knurled grip zones — one feature instead of hundreds of holes.
Make the drawing fast
- Hole Callout auto-reads a Hole Wizard hole's full spec, threads included.
- Model Items pulls every model dimension onto the views at once.
- Add GD&T & datum symbols from the Annotation tab; drop a BOM and auto-balloon the views.
Tip
If you dimensioned the model cleanly, Model Items populates most of the drawing for you — then you just tidy the placement.
Defeature — share without the IP
- Tools ▸ Defeature.
- Keep the outer envelope and the interfaces; let it strip internal detail and history.
- Save the result as a separate, simplified body.
Tip
Send a vendor the exact fit-and-clearance envelope of a part without handing over your full feature tree.
Sensors — guard a budget
- Right-click Sensors in the tree ▸ Add Sensor.
- Track Mass Properties, a Measurement, or Interference.
- Set a limit; the sensor turns red and warns the moment an edit crosses it.
Tip
Pin a mass sensor on a part that has to stay under a target weight, and you'll know instantly when a change blows the budget.
Keep big assemblies quick
- Open components Lightweight; switch on Large Assembly Mode.
- Give heavy sub-assemblies a SpeedPak config — it loads only the outer faces you actually mate to.
- Drop the Freeze bar below settled features so they stop rebuilding.
Tip
For navigation and measuring without loading everything, open the file in Large Design Review mode.