Draft Dimension/sv

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Label

Draft

Description

Linear dimensions based on edges and radial dimensions are parametric. This means that they will update if the measured edge is modified. Measured edges can belong to Draft objects but also to solid bodies. Angular dimensions are not parametric.

Draft Dimensions can be displayed on a TechDraw Workbench page using the TechDraw DraftView or TechDraw ArchView commands. Alternatively the TechDraw Workbench offer its own dimension commands. But these create dimensions that are only displayed on the drawing page and not in the 3D view.

Linear dimension defined by three points

Usage

See also: Draft Tray, Draft Snap and Draft Constrain.

Linear dimension

Radial dimension

1. Optionally select a circular edge in the 3D view.
2. Invoke the command as explained above.
3. The Dimension task panel opens. See Options for more information.
4. If you have not yet selected an edge do one of the following:
   • Press E or the Select edge button and select a circular edge in the 3D view.
   • Hold down the Alt key, select a circular edge in the 3D view and release the Alt key.
5. To position the dimension line do one of the following:
   • For a diameter dimension:
     • Pick a point in the 3D view, or type coordinates and press the Enter point button.
   • For a radial dimension:
     • Hold down the Shift key and pick a point in the 3D view.

Angular dimension

1. Invoke the command as explained above.
2. The Dimension task panel opens. See Options for more information.
3. Do one of the following:
   • Press E or the Select edge button and select a first straight edge in the 3D view. Repeat this to select a second straight edge.
   • Hold down the Alt key, select two straight edges in the 3D view and release the Alt key.
4. To position the dimension arc pick a point in the 3D view.
5. The displayed angle depends on the edges and the picked point.

Options

The single character keyboard shortcuts available in the task panel can be changed. See Draft Preferences. The shortcuts mentioned here are the default shortcuts (for version 1.0).

• To manually enter coordinates enter the X, Y and Z component, and press Enter after each. Or you can press the Enter point button when you have the desired values. It is advisable to move the pointer out of the 3D view before entering coordinates.
• Press R or click the Relative checkbox to toggle relative mode. If relative mode is on, coordinates are relative to the last point, if available, else they are relative to the coordinate system origin.
• Press G or click the Global checkbox to toggle global mode. If global mode is on, coordinates are relative to the global coordinate system, else they are relative to the working plane coordinate system.
• Press N or click the Continue checkbox to toggle continue mode. This mode only works for linear dimensions. If continue mode is on, the command will restart after finishing, allowing you to continue creating dimensions. All subsequent dimensions will start from the final point of the previous dimension, and will use the same baseline as the first dimension. Note that edge selection is not possible for subsequent dimensions.
• Press S to switch Draft snapping on or off.
• Press Esc or the Close button to finish the command.

Notes

• Linear and radial Draft Dimensions can be edited with the Draft Edit command.
• Draft Dimensions created or saved with FreeCAD version 0.21 are not backward compatible.

Properties

See also: Property editor.

A Draft Dimension object is derived from an App FeaturePython object and inherits all its properties. The following properties are additional unless otherwise stated:

Data linear and radial dimension

Dimension

• DataDimline (VectorDistance): specifies the point through which the dimension line passes.
• DataLinked Geometry (LinkSubList): specifies the object and its subelement(s) the dimension is linked to.
• DataNormal (Vector): specifies the normal of the plane of the text.
• Data (hidden)Support (Link): specifies the measured object.

Linear/radial dimension

• DataDirection (Vector): specifies the direction of the measurement.
• DataDistance (Length): (read-only) specifies the value of the measurement.
• DataEnd (VectorDistance): specifies the end point of the measurement.
• DataStart (VectorDistance): specifies the start point of the measurement.

Radial dimension

• DataDiameter (Bool): specifies if a radial dimension is displayed as a diameter dimension. Not used for linear dimensions.

Data angular dimension

Angular dimension

• DataAngle (Angle): (read-only) specifies the value of the measurement.
• DataCenter (VectorDistance): specifies the center of the measurement.
• DataFirst Angle (Angle): specifies the start angle of the measurement.
• DataLast Angle (Angle): specifies the end angle of the measurement.

Dimension

• DataDimline (VectorDistance): specifies the point through which the dimension arc passes.
• Data (hidden)Linked Geometry (LinkSubList): not used.
• Data (hidden)Normal (Vector): specifies the normal of the plane of the dimension.
• Data (hidden)Support (Link): not used.

View

Annotation

• VyAnnotation Style (Enumeration): specifies the annotation style applied to the dimension. See Draft AnnotationStyleEditor.
• VyScale Multiplier (Float): specifies the general scaling factor applied to the dimension.

Display Options

• VyDisplay Mode (Enumeration): specifies how the text is displayed. If it is World the text will be displayed on a plane defined by the DataNormal of the measurement. If it is Screen the text will always face the screen. This is an inherited property. The mentioned options are the renamed options (introduced in version 0.21).

Graphics

• VyArrow Size (Length): specifies the size of the symbols displayed at the ends of the dimension line or arc.
• VyArrow Type (Enumeration): specifies the type of symbol displayed at the ends of the dimension line or arc, which can be Dot, Circle, Arrow, Tick or Tick-2.
• VyDim Overshoot (Distance): specifies the additional length added to the dimension line. Not used for angular dimensions.
• VyExt Lines (Distance): specifies the length of the extension lines that go from the dimension line to the measured points. Use 0 for full extension lines. A negative value defines the gap between the ends of the extension lines and the measured points. A positive value defines the maximum length of the extension lines. Only used for linear dimensions.
• VyExt Overshoot (Distance): specifies the additional length of the extension lines beyond the dimension line. Not used for angular dimensions.
• VyFlip Arrows (Bool): specifies whether to flip the orientation of the symbols at the ends of the dimension line or arc. Only works if the symbols are arrows.
• VyLine Color (Color): specifies the color of the dimension line or arc, and the arrows.
• VyLine Width (Float): specifies the width of the lines or arc belonging to the dimension.
• VyShow Line (Bool): specifies whether to display the dimension line. Does not affect the display of extension lines and overshoots. Not used for angular dimensions.

Text

• VyFlip Text (Bool): specifies whether to flip the orientation of the text.
• VyFont Name (Font): specifies the font used to draw the text. It can be a font name, such as Arial, a default style such as sans, serif or mono, a family such as Arial,Helvetica,sans, or a name with a style such as Arial:Bold. If the given font is not found on the system, a default font is used instead.
• VyFont Size (Length): specifies the size of the letters. The text can be invisible in the 3D view if this value is very small.
• VyOverride (String): specifies a custom text to display instead of the actual measurement. Use the string $dim inside the text to include the measurement.
• VyText Color (Color): specifies the color of the text. introduced in version 0.21
• VyText Position (VectorDistance): specifies the position of the text in absolute coordinates. [0, 0, 0] will display the text in its default position near the dimension line or arc.
• VyText Spacing (Length): specifies the space between the text and the dimension line or arc.

Units

• VyDecimals (Integer): specifies the number of decimal places to display for the measurement.
• VyShow Unit (Bool): specifies whether to display the unit next to the numerical value of the measurement. Not used for angular dimensions.
• VyUnit Override (String): specifies the unit in which to express the measurement, for example, km, m, cm, mm, mi, ft, in or arch for arch units. Leave this blank to use the default unit. Not used for angular dimensions.

Scripting

See also: Autogenerated API documentation and FreeCAD Scripting Basics.

To create a Draft Dimension use the make_dimension method (introduced in version 0.19) of the Draft module. This method replaces the deprecated makeDimension method.

dimension = make_dimension(p1, p2, p3=None, p4=None)

There are various ways to invoke this method, depending on the arguments passed to it:

dimension = make_dimension(p1, p2, p3=None)
dimension = make_dimension(object, i1, i2, p4=None)
dimension = make_dimension(object, i1, mode, p4=None)

• Creates a linear dimension by measuring the distance between points p1 and p2.
• Creates a linear dimension linked to object, measuring the distance between its vertices indexed i1 and i2.
• Creates a circular dimension linked to object, with i1 being the index of the curved edge to measure, and mode being either "radius" or "diameter" to specify the type of dimension.
  • p3 in the first call, and p4 in the other two, specify an optional point through which the dimension line should go.
  • All points are defined by their FreeCAD.Vector.

To create an angular dimension use the following method:

dimension = make_angular_dimension(center, angles, p3, normal=None)
dimension = make_angular_dimension(center, [angle1, angle2], p3, normal=None)

• Creates an angular dimension from the given center point, the angles list with two elements, and the point p3 through which the arc should go.
  • If angle1 > angle2, the displayed angle is the difference angle1 - angle2; otherwise, the explementary angle is displayed, 360 - (angle2 - angle1).
  • The angles should be given in degrees.

The view properties of dimension can be changed by overwriting its attributes; for example, overwrite ViewObject.FontSize with the new size in millimeters.

Example:

import FreeCAD as App
import Draft

doc = App.newDocument()

p1 = App.Vector(0, 0, 0)
p2 = App.Vector(1000, 1000, 0)
p3 = App.Vector(-2500, 0, 0)
dimension1 = Draft.make_dimension(p1, p2, p3)
dimension1.ViewObject.FontSize = 200

polygon = Draft.make_polygon(3, radius=1000)
doc.recompute()

p4 = App.Vector(-2000, 1500, 0)
dimension2 = Draft.make_dimension(polygon, 1, 2, p4)
dimension2.ViewObject.FontSize = 200

center = App.Vector(2000, 0, 0)
p5 = App.Vector(3000, 1000, 0)
angle1 = 45
angle2 = 10
dimension3 = Draft.make_angular_dimension(center, [angle1, angle2], p5)
dimension3.ViewObject.FontSize = 200

dimension4 = Draft.make_angular_dimension(center, [angle2, angle1], p5*1.2)
dimension4.ViewObject.FontSize = 200

doc.recompute()

Text

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Draft

Draft

• Drafting: Line, Polyline, Fillet, Arc, Arc by 3 points, Circle, Ellipse, Rectangle, Polygon, B-spline, Cubic Bézier curve, Bézier curve, Point, Facebinder, ShapeString, Hatch
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• Context menu:
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  • Text: Open hyperlinks
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  • Working plane proxy: Write camera position, Write objects state

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