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Getting Started

Your first SOLIDWORKS part, step by step

This tutorial builds a simple mounting plate — 100 × 60 × 20 mm with a Ø20 mm hole and rounded corners — using the four commands you will use in almost every part: Sketch, Smart Dimension, Extruded Boss/Base and Extruded Cut, plus Fillet. It takes about 15 minutes. At the end you check your model against a known mass, the same way certification exams do.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Rectangular aluminium mounting plate with a central hole and rounded corners modelled in CAD

Where to find it

File → New → Part → Sketch tab

What you will build

Feature Command Values
Plate Extruded Boss/Base Centre rectangle 100 × 60 mm, 20 mm deep
Hole Extruded Cut Ø20 mm, Through All, centred
Corners Fillet R5 on the four 20 mm edges
Material Edit Material 6061 aluminium, 2.70 g/cm³
Check Mass Properties 305.88 g, 113,287.61 mm³

The check values are calculated from the dimensions: 100 × 60 × 20 mm minus the Ø20 hole minus what the four R5 fillets remove. If you know the interface already, you can go straight to the steps.

Ready for more? Model the base plate next, then the other basic exercises.

Step by step

  1. 1

    Create a new part in millimetres

    File → New → Part → OK. Look at the bottom right of the window: it should say MMGS. If not, click it and choose MMGS (see units).

  2. 2

    Start a sketch on the Front Plane

    In the FeatureManager tree click Front Plane, then on the Sketch tab click Sketch. The view turns to face the plane.

  3. 3

    Draw a centre rectangle on the origin

    Choose Rectangle → Center Rectangle. Click on the origin (the red arrows) to place the centre, then click again anywhere to set the corner. Starting on the origin ties the sketch to it.

    Fully defined centre rectangle sketch 100 by 60 mm on the origin with black lines
    A centre rectangle on the origin, fully defined with two dimensions.
  4. 4

    Add dimensions with Smart Dimension

    Click Smart Dimension, click the top line and place the dimension; type 100 and press Enter. Click a vertical line and type 60. The lines turn from blue to black, and the status bar says Fully Defined — the sketch can no longer move.

  5. 5

    Extrude it into a solid

    On the Features tab click Extruded Boss/Base. Set Direction 1 to Blind and the depth to 20 mm, then click the green tick. You now have a plate.

    Extruded Boss preview of the plate with blind depth 20 mm
    Extruded Boss/Base turns the sketch into a 20 mm thick solid.
  6. 6

    Sketch the hole on the front face

    Click the large front face of the plate, then Sketch. Draw a Circle with its centre on the origin, and dimension its diameter 20. The circle turns black.

  7. 7

    Cut the hole through

    Features → Extruded Cut, end condition Through All, tick. The hole goes through the plate.

  8. 8

    Round the four corners

    Features → Fillet, radius 5 mm. Select the four short edges at the corners of the plate (the edges 20 mm long), then the tick. Fillets come last in most parts — they are easy to change and do not break the features before them.

  9. 9

    Add material and check the mass

    Right-click Material in the tree → Edit Material, choose the 6061 alloy in the aluminium group of the SOLIDWORKS materials and check that its density reads 2,700 kg/m³ (2.70 g/cm³) → Apply. Then Evaluate → Mass Properties. The mass should be about 305.88 g (volume 113,287.61 mm³). A different value means a dimension or the fillet selection is off.

    Mass Properties result showing mass about 305.88 grams for the aluminium mounting plate
    Your mass should be about 305.88 g with 6061 aluminium.
  10. 10

    Save the part

    File → Save As, name it mounting-plate.SLDPRT. Rename the features in the tree (slow double-click) — Plate, Hole, Corner fillets — so they are easy to find later.

Common mistakes

  • Starting the rectangle away from the origin. The sketch then needs extra dimensions to be fully defined.
  • Leaving sketches blue (under defined). They can change shape when you edit something else.
  • Filleting the 100 mm or 60 mm edges instead of the four 20 mm corner edges — the mass will not match.
  • Working in inches by mistake — 100 would become 100 inches. Check MMGS in the status bar first.

What to do next

  • Do the built-in Lesson 1 – Parts tutorial (Welcome dialog → Learn), which adds a boss, a cut, fillets and a shell.
  • Follow the learning plan for assemblies and drawings.
  • Learn each sketch tool properly in the sketching course.
  • Learn every feature used here — and many more — in the features course.
  • Save your projects in a clean folder structure from the start.
  • When you can model simple parts confidently, try the CSWA practice test — its modelling questions are checked by mass, just like this part.
  • Sketch turning red or the extrude failing? See sketch errors.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

What is the first thing to learn in SOLIDWORKS?

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Sketching on a plane, adding dimensions until the sketch is fully defined, and turning it into a solid with Extruded Boss/Base. Almost every part starts that way.

Why are my sketch lines blue?

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Blue means the sketch is under defined — it can still move. Add dimensions or relations until the lines turn black and the status bar says Fully Defined.

Which plane should I sketch on first?

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The one that matches how the part is viewed from the front. For a plate seen from the front, the Front Plane; for a part that sits on a table, often the Top Plane.

How long does it take to learn SOLIDWORKS basics?

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Most people can build simple parts after a few hours with the built-in tutorials. A structured course for parts, assemblies and drawings usually takes several days; see our learning plan.