Dimensioning the Base

  1. Click Select (Standard toolbar).

    The colored tags show Sketch Relations. The tags SOLIDWORKS added when you created the rectangle indicate vertical, horizontal, and coincident relations.

    You can:
    • See a tooltip by hovering over a tag.
    • Modify or delete a sketch relation by double-clicking a tag.
    • Show or hide sketch relations by clicking View > Hide/Show > Sketch Relations.

    The sides of the rectangle that touch the origin are black. Because you started sketching at the origin, the vertex of these two sides is automatically coincident with the origin, as shown by the symbol . This relationship constrains the sketch.

    To constrain something is to add a restriction to the geometry of the model. In this case, by starting the sketch at the origin, you made the corner of the rectangle coincident with the origin.

    Relations and dimensions constrain geometry in parts; mates constrain components in assemblies. Relations can be added manually or automatically.

    For more information about the colors SOLIDWORKS uses to indicate the status of sketch entities (here, the sides of the rectangles), see Sketch Geometry Status in the SOLIDWORKS Connected help.

  2. Drag one of the blue sides or drag the vertex to resize the rectangle.
  3. Click Smart Dimension (Sketch tab).
  4. Select the top edge of the rectangle.
  5. Click above the line to place the dimension.
    If your system options are set appropriately, the Modify dialog box appears.
  6. Optional: If the Modify dialog box does not appear after the previous step, do the following:
    1. Click Options (Standard toolbar).
    2. In the left pane of the System Options tab, select General.
    3. In the right pane of the System Options tab, select Input dimension value.
    4. Click OK.
    5. Double-click the dimension to open the Modify dialog box.
  7. In the Modify dialog box, set the value to 120.
  8. Click .
    The sketch resizes to reflect the 120mm dimension.
  9. Click Zoom to Fit (Heads-up View toolbar) to display the entire rectangle and center it in the graphics area.
  10. Repeat steps 3-9, with a vertical line, setting the height of the rectangle to 120mm.

    The sketch is now fully defined, as shown in the status bar at the bottom of the SOLIDWORKS window.