# Expressions

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This page is actively being modified by garya as of 2019-03-14.

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This message will be removed when these modifications are complete.

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 24px. 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 normal notation for the standard mathematical operators (+, -, * and /) 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).

## Supported Functions

### 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 degrees as their default unit;
for radian measure, add **rad** following the *first* value in an expression.
Example: cos(45) is the same as cos(pi rad / 4).

**Description**: Ceiling

**Returns**: The smallest integer value greater than or equal to x introduced in version 0.16

**Description**: Floor

**Returns**: The largest integer value less than or equal to x introduced in version 0.16

**Description**:

**Returns**: x rounded to the nearest integer introduced in version 0.16

**Description**: Truncate

**Returns**: x truncated to the nearest integer introduced in version 0.16

### Statistical / Aggregating Functions

The aggregating functions listed below are supported.
Aggregating 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).
Example: *average(B1:B8)*

**Description**: Number of cells from x through y

**Returns**: The number of cells from x through y, inclusive

**Description**: Standard deviation of values in cells x through y

**Returns**: Standard deviation

### 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 comparison operators are defined: ==, !=, >, <, >=, and <=.

The conditional statement has a bug regarding nested conditional statements. Only the true-result may contain another conditional statement. This is because parentheses are removed after an expression is entered. Trying to put a nested conditional statement in the false-result may result in incorrect parentheses causing a different result after saving and reopening the document.
Note: This may no longer be true; at least *some* false result conditionals work properly.

## 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:

CAD-Data | Call in expression | Result |
---|---|---|

Parametric Length of a Part-Workbench Cube | Cube.Length | Length with units mm |

Volume of the Cube | Cube.Shape.Volume | Volume in mm³ without units |

Type of the Cube-shape | Cube.Shape.ShapeType | String: Solid |

Label of the Cube | Cube.Label | String: Cube |

x-coordinate of center of mass of the Cube | Cube.Shape.CenterOfMass.x | x-coordinate in mm without units |

Value of constraint in a sketch | Constraints.Width | Numeric value of the named constraint 'Width' in the sketch |

Value of a spreadsheet alias | Spreadsheet.Depth | Value of the alias "Depth" in the spreadsheet "Spreadsheet" |

Value of a local property | Length | Value of the Length property in e.g a Pad object, if the expression is used in e.g Length2 in the same object. |

## 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's possible that you have a spreadsheet in one document and reference values from there in other documents.

Important note: You use a document's name to reference it from other documents. Now, when saving the document the first time you choose a certain file name and this is usually different to "Unnamed1" (or its translated version) and then the links are lost after reopening it. So, it's recommended to create first the master document, create a spreadsheet, save and close it. After reopening the name is set to the above file name. Afterwards you can still make changes and save the file but you shouldn't rename it.

Then create the further documents where you want to add expressions to. Assuming you named the master document "master" you can access an alias like this: master#Spreadsheet.Length

Unfortunately, the integrated checker is more confusing than helping because it always gives parser errors or claims that this or that doesn't exist. So, just continue on typing. When you are finished and the content is correct the OK suddenly becomes 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 graphs is based on the relationship between document objects, not properties. This means that you cannot provide data to and query the same object in e.g a spreadsheet, even though there are no cyclic dependency when just the properties are considered. As a work-around, use multiple spreadsheets, e.g one to drive your model, and one for reporting.
- There is no expression manager implemented where all expressions in a document are listed, and can be created, deleted, queries, etc.
- Open bugs/tickets for Expressions can be found in the FreeCAD Bugtracker Expressions category