- 7-1 Introduction
- 7-2 Terminology and Conventions-ANSI
- 7-3 Adding Dimensions to a Drawing
- 7-4 Drawing Scale
- 7-5 Units
- 7-6 Dimensioning Holes and Fillets
- 7-7 Dimensioning Counterbored and Countersunk Holes
- 7-8 Angular Dimensions
- 7-9 Ordinate Dimensions
- 7-10 Baseline Dimensions
- 7-11 Locating Dimensions
- 7-12 Fillets and Rounds
- 7-13 Rounded Shapes-Internal
- 7-14 Rounded Shapes-External
- 7-15 Irregular Surfaces
- 7-16 Polar Dimensions
- 7-17 Chamfers
- 7-18 Symbols and Abbreviations
- 7-19 Symmetrical and Centerline Symbols
- 7-20 Dimensioning to a Point
- 7-21 Dimensioning Section Views
- 7-22 Dimensioning Orthographic Views
- Chapter Projects
7-9 Ordinate Dimensions
Ordinate dimensions are dimensions based on an XY coordinate system. Ordinate dimensions do not include extension lines, dimension lines, or arrowheads but simply horizontal and vertical leader lines drawn directly from the features of the object. Ordinate dimensions are particularly useful when dimensioning an object that includes many small holes.
Figure 7-50 shows a part that is to be dimensioned using ordinate dimensions. Ordinate dimensions’ values are calculated from the XY origin, which, in this example, is the lower-left corner of the front view of the model.
Creating Ordinate Dimensions
See Figure 7-51.
1 Start a new Drawing document and create a top orthographic view of the part.
Use the dimensions shown in Figure 7-52 to create the drawing.
2 Click and extend the center marks and draw centerlines between the four corner holes.
3 Click the arrowhead located under the Smart Dimension tool and click the Horizontal Ordinate Dimension option.
4 Click the lower-left corner of the part to establish the origin for the dimensions.
5 Move the cursor away from the origin and define a location for the “0” dimension.
All other horizontal dimensions will align with this location.
6 Click the lower portion of each hole’s vertical centerline and the lower-right corner of the part.
7 Click the arrowhead located under the Smart Dimension tool and click the Vertical Ordinate Dimension option.
8 Click the lower-left corner of the part to establish the origin for the dimensions.
9 Click the left portion of each hole’s horizontal centerline and the upper-left corner of the part.
10 Add dimensions for the holes.
Figure 7-52 shows the dimensioned part.