SMART-DIMENSION

Once you've added enough Dimensions/Relations to a sketch, it will become Fully Defined

It is critical and required that your sketches be Fully Defined before you're finished with the model

A fully defined sketch will have all BLACK entities along with the note at the bottom right, "Fully Defined" as well as the Sketch in the Drawing Tree will no longer have the (-) symbol next to it

Download DIMENSIONS.SLDPRT

File→Open→DIMENSIONS.SLDPRT

LMB Expand Arrow→RMB Sketch→LMB Edit Sketch

• Tools→Dimension→Smart

  • Any entities clicked will be added to the next Dimension

• Once the Entities have been properly selected, LMB an empty space outside of your geometry to anchor the dimension

• Press ESC to cancel the Dimension Tool

• If a Line is anchored to the Origin and has a Vertical Relation, Dimensioning the Length will Fully Define it

• To Dimension a Line, one option is to simply select the line

  • This will automatically select the distance between the start/end points

• LMB an empty space in the graphics area to anchor the Dimension→Type in the desired value

Another way to Dimension a line is to Dimension two entities that intersect the end points of the desired line

Dimensioning between a point and a line will give a dimension NormalTo the line

• When adding a Dimension between two points there are a few options

  • Vertical Distance

  • Horizontal Distance

  • Straight Line Distance

• Once the two points have been selected, move your cursor around the Graphics Area before you anchor the Dimension to change which type of Dimension will be added

You may Dimension to Theoretical Entities such as the Centerpoint of a Circle

• Arcs (Circles) are defined by Centerpoint location and Radius/Diameter

  • Remember the Diameter is equal to twice the Radius

• If an Arc doesn’t form a complete circle, the dimension will default to Radial, not Diametral

Notice how all the dimensions are all nicely placed outside the sketch region and easy to see and click

• To Dimension an Angle, select a reference line followed by the angled line

• Move the cursor around the Graphics Area before anchoring the Dimension to view different angular measurement options

• If you’d like a Smart Dimension to work as a readout and not force the Entities to conform:

• RMB the Dimension→Driven

• Driven = Readout

• Driving = Control

• Reverse process to restore control

By Default if you attempt to insert too many dimensions SolidWorks will prompt you to make the new Dimensions Driven

Exit Sketch

Edit Sketch2

Add SmartDimension between circle and edges of Extrusion

NOTE: In most cases, this geometry would be better defined using Concentric rather than trying to remember to Dimension the two values

• On the first click, the default Dimension is Diametral

• You may then LMB the original Arc to add the distance between Arcs

• Double LMB the Number Value to access input prompt to change value

• Type in desired Value

• Use MWU/MWD to increment the value

• Spin the Increment Wheel by LMB+Drag the graphic

Ordinate Dimensions are used when instead of measuring from Feature to Feature, you want to measure from a Datum

• Hole Tables - A single part with a variety of Hole sizes/placement

• Keep the Origin at a logical position that can easily be measured from

• To continue Dimensioning:

  • RMB any Ordinate Dimension→Add To Ordinate

• To move your Dimension, like to the opposite side:

  • RMB Dimension→Alignment→Break

1. HORIZONTAL ORDINATE DIMENSION

2. LMB DATUM (0 point)

3. ANCHOR DIMENSION

4. LMB EACH ENTITY IN DIRECTION (Left/Right)

5. ESC

6. REPEAT FOR VERTICAL ORDINATE DIMENSION

7. DOUBLE-LMB THE LARGEST DIMENSION FIRST

8. ENTER VALUE

9. DOUBLE-LMB THE NEXT LARGEST DIMENSION

10. REPEAT UNTIL THE SMALLEST DIMENSION HAS BEEN EDITED TO THE CORRECT VALUE