工程图尺寸

您可以通过尺寸调色板来自定义选定尺寸（驱动尺寸与从动尺寸）的外观。选择某个尺寸即可显示尺寸调色板图标。

1. 在未选择工具的情况下，选择尺寸。
2. 此时将显示尺寸调色板图标 。
3. 将鼠标悬停在该图标上可打开调色板。（您也可以双击该尺寸来打开调色板）。
4. Set the following options in the palette. Some options may not appear in the palette, depending on the dimension type and other selected options.
   • Above text - Enter the text or symbol to appear above the dimension value.
   • Prefix text - Enter the text to appear as a prefix to the dimension value.
     
   • Count type - Use the dropdown to select a count type for the dimension.
     
   • Precision - Select the depth of unit precision (zero to 8 decimal places).

     Precision defined on a drawing dimension may be linked to the Properties panel through this Dimension palette by selecting the tolerance with “(Drawing)” beside it. Whenever the Properties panel tolerance precisions are updated, any dimension with the “(Drawing)” tolerance selected will also be updated. You can choose to link these properties (and unlink them) on a dimension-by-dimension basis.
     
     

   • Dimension units - Select the units of your choice. The currently selected unit is displayed in the dropdown label:

     • Choose from: Millimeters, Millimeters (Drawing), Centimeters, Meters, Inches, Inches fractional, Feet and inches, Feet, or Yards. This selection overrides the units for that dimension. If you later change the drawing units, the units for the dimension are not overridden. You can change the units back to (Drawing) if you want to inherit the drawing properties again.

     • When you choose units, you set two properties in the drawing or on a dimension - the Units property and the Fractional display property.

     • Drawing units are managed separately from Workspace units for Part Studios and assemblies
     • Feet and Inches is only available in drawings; it is not available for workspace units.
     • Toggle the Show/Hide units button as to display or hide the dimension units.
       .
   • Suffix text - Enter the text to appear as a suffix to the dimension value.
   • Below text - Enter the text or symbol to appear below the dimension value.
   • Symbol dropdown - Select a symbol to insert from the dropdown:
     
     

     Symbol	Name	Shortcut
     °	Degree	%%d
     ⌀	Diameter	%%c
     ℄	Centerline
     ⌵	Countersink
     ↧	Depth
     ⌴	Counterbore
     □	Square
     ⌒	Arc length
     ±	Plus/Minus	%%p
     Ⓤ	Unequally disposed profile
     Ⓘ	Independency
     	Continuous feature
     	Spot face
     ▷	Translation

   • Inspection dimension - Toggle to add or remove an oval frame around the dimension to indicate this is an inspection dimension.
   • Dual dimension - Toggle to specify whether to have a single unit dimension, single unit as specified for the drawing properties, or a dual unit dimension:

     

   • Tolerance - Select None, Symmetrical, Deviation, Limits, Basic, MIN, MAX, Fit, Fit with tolerance, or Fit (Tolerance only).
     • Set the upper and lower tolerance (available for Symmetrical, Deviation, or Limits)

       

     • Optionally, to set a Deviation or Limits tolerance to plus/plus (+/+) or minus/minus (-/-), click the plus (+) or minus (-) button, as required:

       

     • Set the Fit type, Shaft class, Hole class, and Fit standard (available for Fit, Fit with tolerance, or Fit (Tolerance only))
       
     • Set the precision depth of the Fit tolerance units, from 0 to 8 decimal places (available for Fit with tolerance or Fit (Tolerance only))
   • Reset text position - Toggle to reset the text to the previous location.
   • Parentheses - Toggle to add or remove parenthesis around the dimension field.
   • Toggle hole class visibility - (Available for Fit and Fit with tolerance options) Use this to show or hide the hole class in the dimension. When shown, select one of the following options:
     • Stacked without line
     • Stacked diagonally
     • Stacked with line
   • Toggle Radius/Diameter dimension - Use this to change a radial dimension to diameter or vice versa.

您也可以复制/粘贴到所有文本框，在尺寸和注释中也是如此。

Placing dimension text

• 选择两个图元后，会在预览模式下绘制尺寸，以便最终放置：

  

  

  

  

• 在预览过程中四处拖动文本可以将文本移至延长线以外，也可以在水平、竖直和对齐测量模式之间切换：

  

• 在工程图中从两个选定捕捉点向上或向下拖动文本可创建水平尺寸线：

  

• 将文本从两个选定捕捉点向工程图的一边拖动可创建竖直尺寸线：

  

• 在垂直于经过两个选定捕捉点的直线的方向上拖动文本可创建平行于这两个选定捕捉点的尺寸线：

  将光标悬停在标记上方可唤醒对齐关系。只有在预览模式下会这样。将光标划过其他工程图图元也可唤醒对齐关系，就像其他视图的图元一样。

  

选择尺寸工具后，您可以将光标移至表示环形边的边上方以“唤醒”中心标记。此标记一旦可见，将一直保持可见状态。

将光标移至边上方时，会出现橙色的环形捕捉点与竖直中心标记：

悬停光标后，橙色的捕捉点会消失，但是标记仍可见：

改变尺寸箭头的位置。用于显示箭头或记号的任何尺寸。

当您选择尺寸时，尺寸箭头或记号旁边会显示一个节点。单击节点可翻转尺寸的箭头。

要翻转尺寸箭头：

1. 在图形区域中，选择要更改的尺寸。
2. 将值拖动到新位置（箭头会相应地变化）。

使用鼠标右键单击可在任何尺寸上打开环境菜单，以访问该尺寸的命令选项列表。下面列出了这些命令选项。请注意，此处列出的所有命令并非都适用于每种类型的尺寸。

• 编辑 - 打开尺寸调色板以编辑尺寸。

• 粘贴 - 将尺寸与视图一起粘贴到当前位置。

• 清除选定内容 - 取消选择选定的尺寸。

• 缩放到合适大小 - 将整个工程图缩放到视图中。

• 删除 - 删除选定的尺寸。