Before You Begin

Before you begin creating dimensions, you should be familiar with the concepts described in this section.

First of all, bear in mind that dimension creation in Drafting follows the general rules which apply to geometry creation in V5: the geometry to dimension must be contained within a "box" whose dimensions are 2.e+6mm (the coordinates can vary from -1,000,000 mm to +1,000,000 mm). Therefore, it is impossible to create dimensions for elements exceeding these dimensions.


Creating Dimensions

You can create (and therefore modify) the following types of dimensions:

Dimensions created on one element:

Dimensions created on two elements:

Note that you can create half-dimensions on distance, angle, diameter cylinder, diameter edge and diameter tangent dimensions but not on cumulate dimensions.

Modifying the Dimension Attributes

You can modify the following attributes at any time before you click to validate the dimension creation:

Modify while creating:

Modify while or just after creating:

Manipulating Dimensions

By default, when manipulating dimensions, you will use the following functionalities:

  • dimension following the cursor: go to Tools > Options > Mechanical Design > Drafting > Dimension tab, to use automatic positioning
  • global move: go to Tools > Options > Mechanical Design > Drafting  > Dimension tab, to move precisely dimension line, dimension value, secondary part of a dimension line.
  • blanking manipulators (available when modifying a dimension): go to Tools > Options > Mechanical Design > Drafting > Manipulators tab, not to visualize blanking manipulators or to visualize other manipulators either when creating or when modifying a dimension (Modify Overrun, Modify Blanking, Insert text before, Insert text after, Move value, Move dimension line, Move dimension line secondary part, Move dimension leader).
  • value snapped between the dimension lines symbols: go to Tools > Options > Mechanical Design > Drafting > Dimension tab, if you do not want to have the possibility to snap the dimension value between both symbols of the dimension line and/or you want to snap the dimension position on the grid.
  • during creation: to switch temporarily the Dimension following the cursor option, hold on the ctrl key.
  • during creation and edition: to switch temporarily the Snap by default option, hold on the shift key. Clicking on the dimension symbols will invert them.
  • during angle dimension creation: if the Dimension following the cursor option is activated, you can swap the angle sector according to the mouse position holding on the  ctrl and shift keys. If the  Dimension following the cursor option is not activated, you can swap to the complementary angle sector holding on the  ctrl key and clicking on the dimension line.

Dimension Tools

The Tools palette appears whenever you select a command for which specific options or value fields are available. This enables you to know immediately when specific tools are available for a command. The options or fields available in the Tools Palette depend on the command you selected. Only a few examples are provided here.

For example, if you select the Dimensions command, the Tools Palette may provide the following options:


Projected/Forced/True Length Dimension

  Projected Dimension (according to the cursor position) 


Force Dimension on Element


Force Horizontal Dimension in View


Force Vertical Dimension in View


 Force Dimension along a direction


True Length Dimensions (for isometric views only)


Remember that as you create the dimension in one mode, you can use the contextual menu and select another mode.

Dimension Properties    

You can apply given properties to all the dimensions you are going to create. For this, use the Dimension Properties and Numerical Properties toolbar.


Dimension Properties toolbar

  • Line type (regular, two parts, one part leader, or two parts leader)
  • Tolerance type 
  • Tolerance value
  • For the ISOCOMB combined tolerance, use the following type of syntax in the tolerance value field: H6 (+0.5 / -0.3) 

  • When editing an existing drawing, if you change your default unit choice in Tools > Options > General > Parameters and Measure > Units tab, then the numerical display format which best corresponds to the selected unit is automatically selected in the toolbar instead of the current default value.
  • The last five tolerance values typed in the Dimension properties toolbar are saved in a settings file and proposed in the list.

Numerical Properties toolbar

  • Numerical Display Format
  • Precision


When creating a new drawing, the Unit field (here: NUM.DIMM) drives the unit of the dimensions to be created.
The value which is used by default in this field for each type of dimension is usually defined by the
dimension styles (Tools > Standards  > [standard name] > Styles > [dimension style] > ValueDisplayFormat > MainValue > Name). However, if no value is defined by the styles, the one which will be used by default is that defined as your default unit choice in Tools > Options > General > Parameters and Measure > Units tab.

Using Styles 

You can use styles (i.e. a set of default values for each kind of element) when creating dimensions in drawings created with version V5 R11 and later (or pre-R11 drawings whose standard has been updated or changed in V5 R11 and later). Styles are defined in the standard used by the drawing and managed by the administrator.

When creating a dimension, the Style toolbar displays the styles available for this type of dimension. (By default, the Style toolbar is situated at the top left of screen.) If only one style is available, it will be used by default.

  If several styles are available for this type of dimension, you can choose the style that you want to use to create this dimension by selecting it from the Style toolbar.

Refer to Using Styles for more information.

In drawings created with versions up to V5 R10, you can create dimensions using default values. Refer to Setting Properties As Default in Pre-R11 Drawings and to Using Properties Set as Default in Pre-R11 Drawings for more information.