Reference Dimensions
A reference dimension shows a size in the sketch without controlling it. A normal (driving) dimension holds the sketch to a number you typed. A reference dimension is the other way round: the sketch decides, and the dimension reads out the result. It is drawn in grey, in brackets, such as (2.000), and it changes by itself when the pieces it measures change.
When to Use It
- See the overall length of a drawing while only its parts are dimensioned
- Check a size, such as a diagonal, that other dimensions and relations already settle
- Keep a size on the sketch that must not fight the others
- Add the dimension a drawing needs without over defining the sketch
- Read a size that an Extrude depth formula can then use
Step by Step
- Open a sketch with some pieces that already have dimensions. See Smart Dimension.
- Click Dimension on the Sketch tab and pick a piece that is already sized, or two pieces whose size the sketch already settles. Type a number and press Enter.
- Because that dimension would over define the sketch, the box does not refuse it. It says so and asks Make it a reference dimension?
- Click Make it a reference dimension. A grey number in brackets appears. The number you typed is not used: the dimension shows the size the sketch really has.
- Change a driving dimension that moves those pieces. The bracketed number follows at once.
To make a reference dimension by choice, place the dimension as usual, click its number, and click Make reference in the box.
Switching Between Driving and Reference
- Click the number on the sketch. Right-clicking it opens the same box.
- Click Make reference on a driving dimension. It stops controlling the sketch, keeps its name, and shows the size the sketch has now. Nothing moves.
- Click Make driving on a reference dimension. It takes the size it shows and holds the sketch to it. If the sketch already sets that size, so that holding it would over define the sketch, the switch is refused and nothing changes. Make another dimension a reference first.
- Press Ctrl+Z once to take a switch back.
Options
- Make it a reference dimension: in the question that replaces a refused dimension, keeps the size as a reference dimension.
- Cancel: adds nothing, and the sketch is as it was.
- Make reference and Make driving: the switch in the box of any dimension except Fixed.
- Diameter and Radius, or Aligned, Horizontal and Vertical: still offered in the box of a reference dimension. They change what it measures; they never move anything.
Names, Equations and Saving
- A reference dimension has a name such as
D3@Sketch1, like any dimension, and can be renamed in its box. - Edit, Equations... lists it under Reference dimensions, read only. It cannot be given a formula, and a dimension's formula cannot read it, because its size comes from the pieces that formula would move. Switch it to driving first, or read a driving dimension instead.
- A formula for the Extrude depth can read a reference dimension. The depth is worked out once, when you press Extrude or Cut.
- Switching a dimension that has a formula to reference removes the formula, and is refused while another formula reads that dimension.
- Under Relations in Edit on the Sketch tab, a reference dimension is listed with the word (reference).
- A reference dimension is saved with the sketch. Extrude, then use Edit Sketch from the History, and it comes back as a reference dimension.
- Sketches saved before this release open as they were: every dimension in them drives. An older version of the viewer (before 6.344.0) does not show reference dimensions at all; it opens the sketch without them, and a sketch it saves keeps them.
Tips and What to Expect
- A reference dimension is never solved. It cannot make a sketch red or over defined, and it does not count toward fully defined.
- Delete one with Delete in its box or the cross in the Constraints list. Ctrl+Z puts it back.
- Trim and Extend let go of a reference dimension of the piece they change, as they do a driving one when it can no longer be kept. Reference dimensions on pieces that stay keep reading.
- Rotate and Scale for sketch pieces ignore reference dimensions; they still refuse pieces that carry a driving dimension or a relation.
- A reference angle shows the smaller angle of the pair, as a driving angle does.
Problems
- *The box will not take my number.* The dimension is a reference dimension. Click Make driving to type a size.
- *Make driving was refused.* The sketch already sets that size through other dimensions and relations. Make one of those a reference first, or delete it.
- *The question appears when I only wanted a driving dimension.* The sketch already sets that size, so a driving dimension would over define it. Cancel, then delete or switch the dimension that sets it.
- *A formula was refused with "is a reference dimension".* A dimension's formula cannot read a reference dimension. Use a driving dimension in the formula.