- 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
It is important to understand that dimension values are not the same as mathematical units. Dimension values are manufacturing instructions and always include a tolerance, even if the tolerance value is not stated. Manufacturers use a predefined set of standard dimensions that are applied to any dimensional value that does not include a written tolerance. Standard tolerance values differ from organization to organization. Figure 7-18 shows a chart of standard tolerances.
In Figure 7-19 a distance is dimensioned twice: once as 5.50 and a second time as 5.5000. Mathematically these two values are equal, but they are not the same manufacturing instruction. The 5.50 value could, for example, have a standard tolerance of , whereas the 5.5000 value could have a standard tolerance of . A tolerance of is more difficult and therefore more expensive to manufacture than a tolerance of .
Figure 7-20 shows examples of units expressed in millimeters and in decimal inches. A zero is not required to the left of the decimal point for decimal inch values less than one. Millimeter values do not require zeros to the right of the decimal point. Millimeter and decimal inch values never include symbols; the units will be defined in the title block of the drawing.
Aligned dimensions are dimensions that are parallel to a slanted edge or surface. They are not horizontal or vertical. The units for aligned dimensions should be written horizontally. This is called unidirectional dimensioning.
Figure 7-21 shows the front, right-side, and isometric views of a part with a slanted surface. The dimensions were applied using the Smart Dimension tool. Note that the slanted dimension, aligned with the slanted surface, has unidirectional (horizontal) text. The hole dimension was created using the Note tool from the Annotation tab.
Figure 7-22 shows an object that has two holes, one blind and one completely through. The object has filleted corners. In this section we will add dimensions to the views.
The holes were drawn using the Hole Wizard tool. The Hole Wizard tool will automatically create a conical point to a blind hole.
1 Use the Smart Dimension tool and locate the two holes.
See Figure 7-23. In general, dimensions are applied from the inside out; that is, starting with the features in the middle of the part and working out to the overall dimensions. Leader lines are generally applied last, as they have more freedom of location.
2 Use the Linear Center Mark tool to draw a centerline between the two holes and use the Centerline tool to add the vertical centerline in the front and side views.
The centerline between the two holes indicates that the vertical 30 dimension applies to both holes.
3 Use the Smart Dimension tool and add a dimension to one of the filleted corners.
See Figure 7-24.
4 Click the fillet dimension again, go to the Dimension Text block on the Dimension PropertyManager, and type - 4 CORNERS as shown in Figure 7-25.
5 Click OK, Apply, and OK.
6 Use the Hole Callout tool on the Annotation panel and dimension the Ø16 hole.
The Ø16 hole goes completely through the part, so no depth specification is required. See Figure 7-26. The word THRU is optional and may be removed.
7 Use the Hole Callout tool and Dimension the Ø25 hole.
Complete the dimensions.
See Figure 7-29.