Activity: Use relationships to align geometry


Use relationships to align geometry

In this activity, you will:

Launch the Activity: Use relationships to align geometry.

Using relationships to maintain symmetry

In addition to specifying that a line remains horizontal or vertical, also use a horizontal/vertical relationship to specify that one element remains horizontally or vertically aligned with respect to another element.

Use a vertical relationship to specify that the endpoints of vertical lines in the top view stay vertically aligned with the endpoints of the vertical lines in the front view.

This ensures that the vertical lines in the top view remain orthographically aligned to their corresponding elements in the top view, regardless of their size.

This technique is a powerful tool that can be used in many situations.

Apply a vertical relationship

  1. Choose Sketching tab→Relate group→Horizontal/Vertical .

  2. Position the cursor as shown in the following illustration, and when the endpoint relationship indicator displays, click.

  3. Position the cursor as shown in the following illustration, and when the endpoint relationship indicator displays, click. The line position updates.

Apply another vertical relationship

    The Horizontal/Vertical command should still be active.

  1. Position the cursor as shown in the following illustration, and when the endpoint relationship indicator displays, click.

  2. Position the cursor as shown in the following illustration, and when the endpoint relationship indicator displays, click. .

    The line position updates.

Apply a tangent relationship

  1. Choose Sketching tab→Relate group→Tangent .

  2. Position the cursor on the hidden line, as shown in the illustration, and when the line highlights, click.

  3. Position the cursor as shown in the bottom illustration, and when the circle highlights, click.

    4. The hidden line position in the front view updates to be tangent to the circle in the top view.

Apply another tangent relationship

    The Tangent command is still active.

  1. Position the cursor as shown in the illustration, and when the line highlights, click.

  2. Position the cursor as shown in the bottom illustration, and when the circle highlights, click.

    3. The hidden line position in the front view updates to be tangent to the circle in the top view.

Observe the results

Take a few moments to observe the tangent relationships you applied.

If the views do not match the illustration, use the Select command to delete the tangent relationships, and then apply them again.

Hide the geometric relationships

The steps to place dimensions and apply geometric relationships are finished.

In the next few steps, place centerline and center mark annotations.

Place a centerline

    In the next step, place a centerline on the hidden lines that represent the hole in the front view, as shown in the illustration.

  1. Choose Home tab→Annotation group→Centerline .

  2. On the Centerline command bar, ensure the By 2 Lines option is set.

Select the elements for the centerline

  1. Position the cursor over the hidden line shown in the illustration and click.

  2. Position the cursor over the hidden line shown in the bottom illustration and click.

Place a center mark

    In the next step, place a center mark on the circle in the top view.

  1. Choose Home tab→Annotation group→Center Mark .

  2. On the command bar, set the Projection Lines option .

Select the element for the center mark
Rename a variable

    In the next few steps, define new names for two of the dimensions placed and use these names to define a formula between the dimensions.

    This allows a change to the the length of the part, while keeping the circle centered on the part.

  1. Choose Home tab→Select group→Select.

  2. Position the cursor over the 100 millimeter dimension in the top view, and then right-click to display the shortcut menu.

  3. On the shortcut menu, click Edit Formula to display the Edit Formula command bar.

  4. On the Edit Formula command bar, in the Name box, type Length, and then press Enter.

  5. To finish renaming the variable, press Enter a second time, or click Accept (the green check mark) on the command bar.

Rename another variable and create a formula

  1. Right-click the 50 millimeter dimension to display the shortcut menu.

  2. On the shortcut menu, click Edit Formula to display the Edit Formula command bar.

  3. On the Edit Formula command bar, in the Name box, type HoleLoc, and then press Enter.

  4. The cursor moves to the Formula box.

  5. On the sheet, click the 100 millimeter dimension. Notice that the dimension name, Length, is pasted into the Formula box.

  6. In the Formula box, type /2.

  7. When the entire formula is as shown below, press Enter a second time, or click Accept (the green check mark).

    8. This specifies that the HoleLoc dimension should always be one half the value of the Length dimension (HoleLoc=Length/2).

Edit a dimension

    Edit the dimension that controls the part length in the top view. Because a formula was created a formula that associates the hole position to the part length, the hole will remain centered on the part.

  1. Verify the Select command is still active.

  2. Click the 100 millimeter dimension value, as shown in the illustration.

  3. In the value edit handle adjacent to the dimension, type 90, and then press Enter.

    Notice that the dimension that controls the circle position also updates, and the hole remains centered on the part.

Tip:

The dimension value, 45, is displayed in dark cyan. This indicates the dimension value is driven by its relationship to another element. In this case, it is related to the height dimension by a formula.

Save the file

  1. In the viewing commands group at bottom-right of the window, choose Fit to fit the view.

  2. On the Quick Access toolbar, choose Save to save the work.

Activity: Add driving dimensions Summary

© 2021 UDS