Working in Another Dimension

17 May, 2004 By: Kevin Schneider

Autodesk Inventor tricks make it easy to create advanced dimension types.

When creating working drawings in Autodesk Inventor, you often need dimensions that are a bit more complex than simple horizontal or vertical dimensions. Many dimensions are simply formatting options, but a first-time user may not realize how to create other, less common dimensions. The good news is that Inventor offers some special techniques that help you to easily create advanced dimension types. You can create:

  • dimensions to apparent intersections,
  • linear diametric and linear symmetric dimensions, and
  • three-point angular dimensions.

The dimensions of apparent intersections can be difficult to document. Most 2D CAD systems require you to make construction geometry to find the intersection point for lines that don't actually connect. Inventor lets you dimension to apparent intersections without requiring construction geometry.

To dimension to an apparent intersection, choose the Linear Dimension command. Select the first edge that defines the apparent intersection. Right-click to bring up the Context menu and select the Intersection option (figure 1).

Figure 1. Right-click and choose Intersection from the Context menu.

Next, choose the second edge that defines the intersection. You will see dotted lines that give a preview of the extension of the two edges. A yellow dot marks the apparent intersection (figure 2).

Figure 2. Apparent Intersection previews where lines will cross.

Repeat these steps if needed. You can use apparent intersections for both points on a linear dimension to get the results shown in figure 3.

Figure 3. Apparent Intersection repeated for two points on a linear dimension.

Linear diametric and linear symmetric dimensions (figure 4) are special-case dimensions that make it simpler to represent cylindrical features. Creating them in Autodesk Inventor is fast and easy.

Figure 4. Linear diametric dimension and linear symmetric dimension.

To create a linear diametric dimension, select the centerline about which you want to dimension.

Next, select a parallel line or point. While the dimension is previewing, right-click to bring up the linear dimension's Context menu (figure 5). Select Dimension Type, then Linear Diameter, and then click to place the dimension in the desired location (figure 6).

Figure 5. Linear Dimension Context menu.

Figure 6. Examples of linear diametric dimension in a DIN drawing are highlighted in red.

Many CAD tools don't offer easy ways to create these different diameter dimensions, even though they are defined and required by different drafting standards. Inventor makes it easy.

Creating an angular dimension most often requires using two nonparallel lines. However, this can be difficult to illustrate for something like a radial slot. The radial slot has no linear edges to use to dimension the angle of the slot (figure 7). Instead, it requires a three-point angle dimension.

Figure 7. A radial slot has no linear edges to define its dimensions.

To create the three-point angular dimension, select the first point that defines one side of the angle. Next, select the vertex of the angle as a second point. Finally, select the third point that defines the last side of the angle (figure 8).

Figure 8. Choose the endpoints and vertex for an angular dimension.

Figure 8. Choose the endpoints and vertex for an angular dimension.

An angle dimension cursor appears as you hover over this third point. Select it and place your dimension to finish (figure 9).

Figure 9. Use the angle dimension cursor to place the angular dimension.

3D modeling packages provide a lot of power, but without good working drawings and documentation, those 3D designs have little value. The preceding techniques make it easy to create special dimensions to produce accurate 3D designs more quickly and free up your time to focus on the design challenge at hand.

About the Author: Kevin Schneider

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