Draft Dimension

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Revision as of 21:38, 7 November 2018 by Vocx (talk | contribs) (remove "a")

Draft Dimension

Menu location
Draft → Dimension
Workbenches
Draft, Arch
Default shortcut
D I
Introduced in version
-
See also
FlipDimension

Description

The dimension tool creates a dimension in the current document with two points defining the distance to measure, and a third point specifying where the dimension line passes.

How to use

  1. Press the Draft Dimension button, or press D then I keys.
  2. Click a point on the 3D view, or type a coordinate.
  3. Click a second point on the 3D view, or type a coordinate; the first two points define the measured distance.
  4. Click a third on the 3D view, or type a coordinate; the final point defines the position of the measurement line.

The measuring points can be changed after creation by changing the start and end properties.

The position of the measurement line can also be changed after creation by changing its direction property.

Available dimension types

Release the modifier (Alt or Shift) after picking a point or an edge.

  • Linear dimensions: hold the Alt key, or click on the select edge button, and pick a straight edge, then pick a second point to draw the dimension line parallel to that edge.
Note: you can also pre-select the edge before calling the tool.
  • Horizontal and vertical dimensions: pick one point, then pick a second point, then hold the Shift key and move the pointer horizontally or vertically, then pick a third point to draw the dimension line parallel to either the X axis or the Y axis.
Note 1: click and hold Shift and move the pointer in different directions many times until the dimension line aligns to the desired axis. Clicking Shift while the pointer is far from the first point will usually align the dimension to the X axis; if the pointer is close to the first point it will usually align the dimension to the Y axis.
Note 2: instead of picking two points, pick an edge while holding Alt.
  • Diameter dimensions: hold the Alt key and pick a curved edge, then pick a second point to draw the dimension line.
    • Radius dimensions: hold the Alt key and pick a curved edge, then hold the Shift key and pick a second point to draw the dimension line.
  • Angular dimensions: hold the Alt key and then pick two straight edges, then pick a point between the two edges to show the acute angle, or elsewhere to show the supplementary angle.

Note: by pre-selecting an edge, or by picking it with Alt or select edge, the dimension will become parametric, that is, it will remember which edge it is bound to. If the endpoints of that edge move later on, the dimension will follow them, and adjust the displayed measurement.

Options

  • Press X, Y or Z after a point to constrain the next point on the given axis.
  • To enter coordinates manually, simply enter the numbers, then press Enter between each X, Y and Z component.
  • Press R or click the checkbox to toggle relative mode. If relative mode is on, the coordinates of the next point are relative to the previous one; if not, they are absolute, taken from the origin (0,0,0).
  • Press T or click the checkbox to toggle continue mode. If continue mode is on, the Dimension tool will restart after you give the final point, allowing you to draw another dimension without pressing the tool button again; the following dimensions will start from the final point of the previous dimension, and will share the same baseline.
  • Press Ctrl while drawing to force snapping your point to the nearest snap location, independently of the distance.
  • Press Shift while drawing to constrain your next point horizontally or vertically in relation to the previous one, and to switch between diameter and radius modes.
  • Press Esc or the Close button to abort the current command, and finish continued dimensions; dimensions already placed will remain.

Properties

  • DataStart: The start point of the distance to measure
  • DataEnd: The end point of the distance to measure
  • DataDimline: A point through which the dimension line must pass
  • ViewDisplay Mode: Specifies if the text is aligned to the dimension lines or always faces the camera
  • ViewFont Size: The size of the letters
  • ViewExt Lines: The size of the extension lines (between the measurement points and the dimension line)
  • ViewText Position: Can be used to force the text to be displayed at a certain position
  • ViewText Spacing: Specifies the space between the text and the dimension line
  • ViewOverride: Specifies a text to display instead of the measurement. Insert "$dim", inside that text, to display the measurement value
  • ViewFont Name: The font to use to draw the text. It can be a font name, such as "Arial", a default style such as "sans", "serif" or "mono", or 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 generic one is used instead.
  • ViewArrow Type: The type of arrow to use
  • ViewArrow Size: The size of the arrows
  • ViewDecimals: The number of decimal places to display on the dimension
  • ViewFlip Arrows: Reverse the orientation of arrows
  • ViewUnit Override: Expresses the distance in the given unit (leave blank to use the system unit) introduced in version 0.17

Scripting

The Dimension tool can by used in macros and from the python console by using the following functions:

makeDimension (p1,p2,[p3])

or

makeDimension (object,i1,i2,p3)

or

makeDimension (objlist,indices,p3)
  • Creates a Dimension object with the dimension line passing through p3.
  • The Dimension object takes the Draft linewidth and color set in the command bar.
  • There are multiple ways to create a dimension, depending on the arguments you pass to it:
  1. (p1,p2,p3): creates a standard dimension from p1 to p2.
  2. (object,i1,i2,p3): creates a linked dimension to the given object, measuring the distance between its vertices indexed i1 and i2.
  3. (object,i1,mode,p3): creates a linked dimension to the given object, i1 is the index of the (curved) edge to measure, and mode is either "radius" or "diameter". Returns the newly created object.
makeAngularDimension (center,[angle1,angle2],p3)
  • creates an angular Dimension from the given center, with the given list of angles, passing through p3.
  • Returns the newly created object.

Example:

import FreeCAD,Draft
p1 = FreeCAD.Vector(0,0,0)
p2 = FreeCAD.Vector(1,1,0)
p3 = FreeCAD.Vector(2,0,0)
Draft.makeDimension(p1,p2,p3)

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