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Create Spreadsheet

In one sentence: Add a new, empty spreadsheet object to the active FreeCAD document — the starting point for every parametric model driven by a spreadsheet.

Overview

Workbench: Spreadsheet · Menu: Spreadsheet → New Spreadsheet
Toolbar: Spreadsheet · Shortcut: none

Create Spreadsheet inserts a Spreadsheet::Sheet object into the model tree. The spreadsheet opens automatically as a tab in the FreeCAD view area, showing a familiar grid of rows and columns.

Intuition

A FreeCAD spreadsheet is not a separate file — it is a full model object, saved inside the .FCStd file alongside your geometry. This means:

  • The spreadsheet travels with the model; no external .xlsx or .csv to track.
  • It participates in the document's expression engine: cells can reference model properties and model features can reference cell values.
  • Multiple spreadsheets can coexist in one document (one per sub-assembly, for example).

The typical workflow is: create one spreadsheet per document → add alias-named rows for every key dimension → reference those aliases everywhere in the model → tune the design by editing the spreadsheet.

When to use it

  • Starting a new parametric model: create the spreadsheet before adding any geometry so dimensions can be defined upfront.
  • Adding parametric control to an existing model: create the spreadsheet, populate it with the current hard-coded values, set aliases, then replace the hard-coded numbers with spreadsheet references.

When NOT to use it

  • Simple models with one or two dimensions — direct formula entry in the constraint dialog is simpler. A spreadsheet adds value when multiple features share dimensions or when the design has many variants.

Step-by-step walkthrough

  1. Switch to the Spreadsheet workbench.
  2. Spreadsheet → New Spreadsheet (or click the toolbar button).
  3. A Spreadsheet object appears in the model tree. The spreadsheet editor opens in a new view tab.
  4. Click a cell (e.g. A1) and type a label: Length.
  5. Click B1 and type the value: 200 mm.
  6. Right-click B1 → Properties → set an alias: Length.
  7. In a sketch constraint, type =Spreadsheet.Length to link the constraint to this cell.

The spreadsheet editor

The spreadsheet editor is a grid view with:

Element Description
Cell address box Shows the address of the selected cell (e.g. B1). Editable — type an address and press Enter to jump there.
Content bar Shows and edits the raw content of the selected cell (formula or value).
Column headers A, B, C … Click to select a whole column.
Row headers 1, 2, 3 … Click to select a whole row.
Green cell border Indicates a cell has an alias set.

Keyboard shortcuts inside the editor

Key Action
Enter / Tab Confirm and move to the next cell (down / right)
Escape Cancel editing
Delete Clear selected cell(s)
Ctrl+C / Ctrl+V Copy / Paste cells
Ctrl+Z Undo

Renaming and multiple spreadsheets

A new spreadsheet is named Spreadsheet by default. To rename it:

  1. Right-click it in the model tree → Rename.
  2. Type a new internal name (e.g. Params).

References to cells use the internal name: Params.Length. If you rename the spreadsheet, all existing references update automatically.

To have multiple spreadsheets (e.g. one for dimensions, one for material properties), simply run New Spreadsheet again.

Python API

import FreeCAD as App

doc = App.newDocument()

# Create a spreadsheet
sheet = doc.addObject("Spreadsheet::Sheet", "Params")

# Set cell values
sheet.set("A1", "Length")
sheet.set("B1", "200 mm")

sheet.set("A2", "Width")
sheet.set("B2", "50 mm")

sheet.set("A3", "Height")
sheet.set("B3", "10 mm")

# Set aliases
sheet.setAlias("B1", "Length")
sheet.setAlias("B2", "Width")
sheet.setAlias("B3", "Height")

doc.recompute()

# Read cell values back
print(sheet.get("B1"))          # 200.0 (as float, unit stripped)
print(sheet.getAlias("B1"))     # "Length"

# Use alias in a formula
sheet.set("B4", "=B1 + B2")    # = 250 mm
doc.recompute()
print(sheet.get("B4"))          # 250.0

See also