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Dimensions

Dimensions on a drawing measure the geometry of its views. They are attached to the views' edges and points, so they move with the view and update when the model changes.

Annotation tab > Dimension. The button holds the dimension tools: Dimension, Ordinate Dimension, Baseline Dimension, Chamfer Dimension and Arc Length. It shows the one used last; hover over it, or click its arrow, for the others. Model Items and Auto Arrange are beside it.

img/drawings/dimensions-sheet.png

A part's front view dimensioned: lengths in rows off the view, a diameter, a radius and an angle.

Each tool stays on after it adds a dimension, so you can go on to the next one. Press Esc to end it. While a tool is on, the edge, end or center under the pointer is highlighted. A click snaps to the end of an edge near the pointer and to the center of a circle or arc. All the selections for one dimension must be in the same view.

The dimension tools need a model on the drawing. Add a view first with Model View.

Dimension

Dimensions lengths, distances, diameters, radii and angles.

  1. Click Dimension.
  2. Select what to measure (below). After the first selection, the dimension it would make follows the pointer.
  3. Click where the dimension goes.

What you select sets the kind of dimension:

Select Dimension
A straight edge, then click away from the part Its length
A circle Its diameter
An arc Its radius
Two points (ends or centers), or a point and an edge The distance between them
Two straight edges at an angle The angle between them
Two parallel straight edges The distance between them
A circle and another point or edge The distance from the circle's center
Two centers, then a third center The angle at the first center, between the lines to the other two
A bolt circle (click on it, away from other geometry) Its diameter, through the centers of its holes

A circle or an arc goes straight to placing after one click. After one point or a straight edge, either select a second point or edge, or click away from the part to place the dimension of the first selection alone. After two centers, select a third center for an angle, or click where the distance goes. A curve that is neither a line nor a circle, such as a spline, has no size of its own: select a second point or edge.

Where you place a distance sets its direction: above or below the points it measures gives a horizontal dimension, beside them a vertical one, and anywhere else one aligned with the points. A horizontal or vertical edge is always dimensioned along itself. In an isometric or other pictorial view, a distance is measured in the model, along the model axis that runs across the direction you place it; set it with Measure along on its page.

Ordinate Dimension

Dimensions points as distances from an origin, in a row.

  1. Click Ordinate Dimension.
  2. Select the origin: an end of an edge, or a circle (its center).
  3. Click where the row goes: above or below the view for horizontal distances, or beside it for vertical ones. The origin's dimension, 0, is added there.
  4. Select each point to dimension: an end of an edge or a circle in the same view. Each one adds its distance from the origin to the row.
  5. Press Esc to end.

Selecting an ordinate dimension opens the Ordinate Dimension page: the Distance from the origin, its Text and Decimals (see Value), and Text Format.

Baseline Dimension

Dimensions points from a common base point, arranged in rows.

  1. Click Baseline Dimension.
  2. Select the base point: an end of an edge, or a circle (its center).
  3. Select each point to dimension: an end of an edge or a circle in the same view.
  4. Press Esc to end.

Each point adds a horizontal dimension from the base when it lies farther across than up from it, else a vertical one. It goes on the side of the view nearer the base. Then the dimensions made from this base are arranged in rows, as Auto Arrange does. The view's other dimensions stay where they are.

Chamfer Dimension

Dimensions a chamfer's size and angle, measured along an edge.

  1. Click Chamfer Dimension.
  2. Select the chamfer's line in the view.
  3. Select the edge it is measured along: an edge of the same view, at an angle to the chamfer.
  4. Click where the dimension goes.

A 45° chamfer gets a leader note, such as 2 X 45°, or C2 when Document Properties > Dimensions > 45° chamfers says so. See Drafting Standard. A chamfer at any other angle gets a length along the edge and an angle.

Arc Length

Dimensions the length of an arc.

  1. Click Arc Length.
  2. Select an arc.
  3. Click where the dimension goes.

The dimension is drawn on an arc concentric with the edge, with ⌒ before its value.

Model Items

Inserts the model's own dimensions into the sheet's views. Click Model Items. It adds:

  • Each driving dimension of the model's sketches, in a view that looks straight at the sketch's plane.
  • Each extrusion's depth, in a view that sees it from the side.
  • Each Hole feature's callout, in a view that looks down the hole.
  • The callouts of Thread features and library features, on an edge of the threaded face.

Only front, top, side and other orthographic views get model items; an isometric view gets none. Each item is added once per sheet: items already shown are skipped. The dimensions are laid out in rows off the sides of their views. Drag them to tidy the layout.

A model item's value follows the model. If nothing is added, the status bar says that the items are shown already, or that no view is normal to their sketches.

Auto Arrange

Arranges dimensions in evenly spaced rows off their view. Select a view, or a dimension in it, and click Auto Arrange. With nothing selected, it arranges the dimensions of every view on the sheet.

Auto Arrange moves the horizontal, vertical and aligned dimensions. Each one stays on the side of the view it is on. The shortest go nearest the view, and dimensions whose spans don't overlap share a row. Each one's text is centered on what it measures. The rows are Between dimensions apart, and the first row that far off the view: set it in Document Properties > Dimensions. See Drafting Standard.

Radius, diameter and angle dimensions are left where they are.

Editing a Dimension

Click a dimension to select it. Its Dimension page opens in the property panel. Every change shows on the sheet as you make it. Click OK to keep the changes as one undo step, or Cancel to put the dimension back as it was. While the page is open, Ctrl+Z takes back its changes one at a time.

img/drawings/dimensions-page.png

The Dimension page of a selected diameter dimension, with a bilateral tolerance.

Value

The page shows the value measured, or the angle.

Text
The dimension's text. <> stands for the value, as in 2X <> or <> TYP. Leave it empty to show the value alone.
Decimals
How many decimals the value shows, from 0 to 4, trailing zeros kept. Drawing default shows as many as it needs, up to the units' usual.
Show as
For a circle or an arc: Radius (R), Diameter (⌀), or, for a dimension of a single circle, Linear diameter: the diameter straight across the circle, between extension lines. It is horizontal with the text above or below the circle, vertical with the text beside it.
Controlled radius (CR)
For a radius: shows CR in place of R, for an arc with no flats or reversals (ASME Y14.5).
Count alike fillets
For a radius, when the fillet feature rounds several arcs of the same radius in the view: shows their count before the radius, such as 4X R5. The field shows the count. On by default.
Measure along
For a distance in a pictorial view: the model direction it measures, Model X, Model Y or Model Z. Auto measures along the axis the points lie along, else the true length between them.
Diameter (⌀)
For a distance: shows ⌀ before the value. It is set by itself when the dimension spans the two sides of a cylinder seen from the side.

Tolerance

Type
Option Shows
None The value alone
Symmetric (±) The value ± one tolerance
Bilateral (+/-) The value with its two deviations
Limits The largest and smallest sizes, stacked
Basic (boxed) The value in a box, for a basic dimension toleranced by a feature control frame
Upper deviation, Lower deviation
The deviations from the nominal size, in the drawing's units, or degrees for an angle. Enter the lower one with its sign, such as -0.1. For Symmetric, only the upper one is shown: the ± value. With an ASME drafting standard they are called Plus tolerance and Minus tolerance. Both accept an expression, such as 0.1/2, or a parameter of the model.

Text Format

Height
The text height on paper. Leave it empty for the height in Document Properties > Annotations.
Layer
The layer the dimension is on. Shown when the drawing has layers. See Layers.

Editing the Text

Double-click a dimension, or right-click it > Edit Text…, to edit its text in the Dimension Text dialog:

  • The text box. <> Value inserts <>, which shows the measured value.
  • Symbols: drafting symbols such as ⌀, °, ± and the GD&T symbols, inserted at the caret.
  • Text: nX (a count prefix, such as 2X), TYP, (REF) (puts the selected text, or all of it, in parentheses), THRU, EQ SP, New Line, and ABC, which converts the text to capitals.
  • Properties: Insert Property… inserts a field of the drawing or its model, such as {PartNumber}, which fills itself in.
  • Value: Decimals and Tolerance, as on the page.
  • Preview: the text as it will read.

Click OK to keep it as one undo step.

Moving a Dimension

Drag a dimension to move it. With Tools > Options > Files > Snap annotations as they are dragged on (the default), a linear dimension snaps into line with a parallel dimension in the same view, to the dimension spacing from one, or to the spacing off the view. A radius or diameter snaps its text in line with, or the spacing above or below, another one of the view. The status bar says what it snapped to.

A selected linear dimension has a grip at the start of each extension line:

  • Drag a grip along its extension line to shorten it. It snaps to where the line crosses the view's edges, and back to the point it measures.
  • Drop a grip on another point of the part, an end or a center, to measure from there. A model item changed this way becomes the drawing's own dimension.

Deleting a Dimension

Select it and press Del, or right-click it > Delete. Deleting a view deletes its dimensions too.

Dangling Dimensions

A dimension whose edge is gone from the model, after a feature was deleted or changed, is dangling. It shows in red on the sheet, with the value it showed last, where it was. The design tree lists it under its sheet as the value followed by (Dangling). Delete it, or add it again on the geometry the model now has.