Expressions

It is now possible to define properties using mathematical expressions. From the GUI, spin boxes or input fields that are bound to properties contain a blue icon. Clicking on the icon or typing the equal sign (=) brings up the expression editor for that particular property.

A FreeCAD expression is a mathematical expression following notation for the standard mathematical operators and functions as described below. In addition, the expression may reference other properties, and also use conditionals. Numbers in an expression may have an optional unit attached to them.

Numbers may use either a comma ',' or a decimal point '.' separating whole digits from decimals. When the decimal marker is used, it must be followed by at least one digit. Thus, the expressions 1.+2. and 1,+2, are invalid, but 1.0+2.0 and 1,0+2,0 are valid.

The constants pi and e are predefined, and must be written in lowercase.

Operators and functions are unit-aware, and require valid combinations of units, if supplied. For example, 2mm+4mm is a valid expression, while 2mm+4 is not (the reason for this is that an expression like 1in + 4 will most likely be interpreted as 1in + 4in by humans, but all units are converted to the SI system internally, and the system is not able to guess this).

You can refer to an object by its or by its. In the case of a, it must be enclosed in double and  symbols, such as.

Then you can reference any numerical property of this object. For example, to refer to a Cylinder's height, you may use or.

Supported Operators
The following operators are supported:

Supported Constants
The following constants are supported:

General Mathematical Functions
The mathematical functions listed below are available.

Multiple arguments to a function may be separated by either a semicolon ';' or a comma followed by a space ', '. In the latter case, the comma is converted to a semicolon after entry. When a semicolon is used, no trailing space is necessary.

Trigonometric functions use degree as their default unit. For radian measure, add rad following the first value in an expression. So e.g. cos(45) is the same as cos(pi rad / 4). These trigonometric functions are supported:

These functions for exponentiation and logarithmization are supported:

These functions for rounding, truncation and remainder are supported:

Statistical / Aggregate Functions
Aggregate functions take one or more arguments, separated by a semicolon ';' or a comma and a space ', '. Arguments may include references to cells in a spreadsheet. Cell references consist of the (CAPITAL) row letter followed by the column number. Arguments may include ranges of cells (two cell references separated by a colon), for example average(B1:B8).

These aggregate functions are supported:

Conditional Expressions
Conditional expressions are of the form '''condition ? resultTrue : resultFalse'''. The condition is defined as an expression that evaluates to either '0' (false) or non-zero (true).

The following relational operators are defined:

Units
Units can directly be used in expressions. The parser connects them to the previous value. So '2mm' or '2 mm' is valid while ' mm' is invalid because there is no preceding value.

All values must have a unit. Therefore you must in general use a unit for values in spreadsheets. In some cases it works even without a unit, for example if you have e.g. in spreadsheet cell B1 just the number 1.5 and refer to it for a pad height. This only works because the pad height predefines the unit mm that is used if no unit is given. It will nevertheless fail if you use for the pad height e.g. Sketch1.Constraints.Width - Spreadsheet.B1 because Sketch1.Constraints.Width has a unit and Spreadsheet.B1 has not.

Units with exponents can directly be entered. So e.g. mm^3 will be recognized as mm³ and m^3 will be recognized as m³.

If you have a variable with a name of a unit you must put the variable into << >> to prevent that it will be recognized as unit. For example if you have the dimension 'Sketch.Constraints.A' it would be recognized as unit ampere. Therefore you must write it in the expression as 'Sketch.Constraints.<>'.

The following units are recognized by the expression parser:

Amount of substance:

Angle:

Current:

Energy / Work:

Force:

Length:

Luminous intensity:

Mass:

Power:

Pressure:

Temperature:

Time:

Torque:

Volume:

The following commonly used units are not yet supported:

Reference To CAD-Data
It is possible to use data from the model itself in an expression. To reference a property use "object.property". If the property is a compound of fields, the individual fields can be accessed as "object.property.field".

The following table shows some examples:

Document-wide global variables
There is no concept of global variables in FreeCAD at the moment. Instead, arbitrary variables can be defined as cells in a spreadsheet using the Spreadsheet workbench, and then be given a name using the alias property for the cell (right-click on cell). Then they can be accessed from any expression just as any other object property.

Cross-document linking
It is possible (with limitations) to define a Property of an object in your current document (".FCstd" file) by using an Expression to reference a Property of an object contained in a different document (".FCstd" file). For example, a cell in a spreadsheet or the Length of a Part Cube, etc. in one document can be defined by an Expression that references the X Placement value or another Property of an object contained in a different document.

A document's name is used to reference it from other documents. When saving a document the first time, you choose a file name; this is usually different from the initial default "Unnamed1" (or its translated equivalent). To prevent links being lost when the master document is renamed upon saving, it is recommended that you first create the master document, create a spreadsheet inside it, and save it. Subsequently, you can still make changes to the file and its spreadsheet but you should not rename it.

Once the master document with the spreadsheet is created and saved (named), it is safe to create dependent documents. For example, assuming you name the master document "master", the spreadsheet "modelConstants", and give a cell an alias-name "Length", you can then access the value as:

master#modelConstants.Length

Note that the master document must be loaded for the values in the master to be available to the dependent document.

Unfortunately, the integrated checker sometimes claims that a valid name doesn't exist. Continue typing anyway. When you have completed the full reference, the button will become active.

Of course, it's up to you to load the corresponding documents later when you want to change anything.

Known issues / remaining tasks

 * The dependency graph is based on the relationship between document objects, not properties. This means that you cannot provide data to an object and query that same object for results. For example, even though there are no cyclic dependencies when the properties themselves are considered, you may not have an object which gets its dimensions from a spreadsheet and then display the volume of that object in the same spreadsheet. As a work-around, use multiple spreadsheets -- one to drive your model, and one for reporting.
 * The expression parser does not handle parentheses well, and is unable to properly parse some expressions. For example: "= (A1 > A2) ? 1 : 0" results in an error, while "= A1 > A2 ? 1 : 0" is accepted.  The expression "= 5 + ((A1>A2) ? 1 : 0)" cannot be entered in any form.
 * There is no expression manager implemented where all expressions in a document are listed, and can be created, deleted, queried, etc.
 * The names of Sketcher constraints must not contain any blanks when the value is calculated by an expression, see forum discussion.
 * Open bugs/tickets for Expressions can be found in the FreeCAD Bugtracker Expressions category