About Creating Dimensions

You can create a dimension and then change its properties.

• You can use this functionality through the Properties. Right-click the dimension and select Properties. In the Dimension Line tab, select the type of extension you want from the Extension list: From standard, Till center or Not till center.
• This functionality works with radius dimension and one-symbol diameter dimension.
• When you create a dimension between an axis and another element, the dimension created by the software is automatically a half dimension.

  To bypass this problem, clear the Half Dimension contextual command during the creation.

• The break value is taken into account whenever any distance dimension crosses over a break.

  
  
  

  
  
  

  The break value is considered to show the resulting dimension.

  
  
  

  Notes:

  • To change this option, follow the below steps:
    1. Right-click the dimension and select Properties.
    2. Click the Value tab.
    3. Under Dimension Type, clear the Take break into account check box.
  • The break value is taken into account only in the following cases:
    • For distance dimensions
    • For dimensions perpendicular to the break value
  • If you are an administrator, you can change the standards from the Standard Definition dialog box. For more information, see Length/Distance Dimension Styles.

• Right-click the dimension and select Null dimension allowed. By default, this option is not selected.

  If the two geometrical elements separated by a dimension value are moved and aligned, the dimension value is changed to 0 mm.

  You can also create a 0 mm dimension (null) value.

  
• You can generate errors when refreshing the dimensions in the following case:

  In this drawing, the dimension "80.14" is measured from the line B to the line C.

  
  
  If the corresponding part is modified and the chamfer is removed, and after the drawing is updated, the dimension is colored in fuchsia because the line B was removed with the chamfer.
  
  

Dimension Symbol Handles

You can change a dimension symbol handle directly from the symbol itself without using the Properties dialog box.

For this:

1. Go to Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Handles, and select the Modify symbol check box for the Creation and Modification options.
2. Create a dimension. Handles are displayed during dimension creation.
3. Right-click a handle and select the required symbol from Symbol Shape. For more information, see Handles.
4. Optionally, right-click the handle and select Reverse Symbol to reverse the direction of the handle symbol.

Important: The handle is displayed only for Symbol 1 and Symbol 2 of a dimension. It is not displayed for the Leader Symbol.

While creating angle dimensions, you can perform various operations on them. To do so, right-click the dimension and select Angle Sector.

You can choose the position of the angle dimension to be maintained:

Freely Oriented

While transforming a geometry, the angle dimension changes from acute angle to obtuse angle, or to reflex angle, and vice versa.

Maintained Angle

While transforming a geometry, the angle dimension maintains the angle even if you manipulate the geometry.

• Acute angle: Angle dimension between 0-90 degrees.
• Obtuse angle: Angle dimension between 90-180 degrees.
• Reflex angle: Angle dimension between 180-360 degrees.

If the Keep angle range check box is selected in Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Dimension, the angle dimensions created are maintained.

While editing the angle dimensions, you can perform this action on multiple angle dimensions. Based on the type of the dimensions selected, the following behaviors are available:

When all the selected dimensions are freely oriented with respect to geometry

If all the selected angle dimensions are freely oriented, the Keep angle range option is cleared.

When this option is selected, the angle dimensions maintain their angle type (acute, obtuse, or reflex) even if the geometry is modified.

When none of the selected dimensions are freely oriented with respect to geometry

If all the selected angle dimensions maintain their respective angle type (acute, obtuse, or reflex), the Keep angle range option is selected.

When this option is cleared, the angle dimensions become freely oriented with respect to geometry.

During heterogeneous selection

When one of the selected angle dimensions is freely oriented and other dimensions have maintained their respective angle type (acute, obtuse, or reflex), the Keep angle range option is selected.

When this option is cleared, the angle dimensions become freely oriented with respect to the geometry, that is, the type of angle dimension can change depending on geometry modification.

You can create dimensions that can, by default, drive the geometry.

To create driving s:

• Go to Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Dimension, and select the Create driving dimension check box.
• Create or modify the required dimension on the geometry. If required, you can use the Tools Palette and define the Value of the dimension.
  
  

For more information, see Creating Driving Dimensions.

True Length dimensions can be created using True Length Dimensions in the Tools Palette, or using the context menu.

Before creating true dimensions, make sure that you have not selected the Only create non-associative dimensions check box in Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Dimension section, Associativity on 3D, Dimensions associativity on 3D dialog box. To work, this functionality must be applied to an associative dimension.

You can create half dimensions.

For this, right-click the created dimension and select Half Dimension.

For more information, see Creating Half Dimensions.

As you create a dimension between two elements, one of these elements being a circle, you can select the extension line anchor.

To do this, you can:

• Right-click the dimension and select one of the available Extension Line anchor options (First Anchor, Second Anchor, Third Anchor).

  You can thus position the extension line:

  • At one extremity of the circle (First Anchor)
  • At the center of the circle (Second Anchor)
  • At one extremity of the circle (Third Anchor)

• Drag the yellow symbol to the one of the anchors (anchors appear when the pointer is over the yellow symbol):
  
  

Note: If you selected the Dimension following the cursor (CTRL toggles) check box in Me > Preferences > App Preferences > 3D Modeling > Mechanical Systems > Drafting > Dimension, to move the extension line anchor, you must press Ctrl before selecting the yellow symbol (to switch the option temporarily).