Tutorial do esboço

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This page is a translated version of the page Sketcher tutorial and the translation is 7% complete.

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Base ExampleCommandModel.png Tutorial

Time to complete
10 minutes
FreeCAD version
0.16 or above
Example File(s)


This tutorial is meant to introduce the reader to the basic workflow of the Sketcher Workbench. We will be creating a sketch similar to the one shown below.

Sketcher tutorial result.png

The Sketcher workbench exists as a standalone module, but it is also accessible from within the PartDesign Workbench when it is required to create a profile.


  • FreeCAD version 0.16 or above


Creating a Sketch

  1. Create a new document
  2. Switch to the Sketcher Workbench by using the drop-down menu or by clicking on View menu > Workbench > Sketcher.
  3. Select Sketcher NewSketch.png New sketch
  4. You should see a dialog that prompts you to choose sketch orientation and provide an offset. We will not be using offset, and we will use the default plane
  5. Click OK and we can start to construct the sketch

We are now inside the Sketcher environment. Within it, we're able to make use of the majority of the tools that are available in this workbench.

In the Combo View, expand the option Edit controls and make sure Autoconstraints are enabled.

Creating geometry

Sketcher construction geometry

Construction geometry is used as guides for the creation of complex profiles. To access it, we need to enable Construction mode .

  1. Select Sketcher ToggleConstruction.png Construction Mode
  2. Select Sketcher Line.png Line by 2 point
  3. Approach the origin point in the sketch, the point should highlight and near your cursor this icon Sketcher ConstrainCoincident.png will appear.
  4. Select the point and extend the line diagonally up to an arbitrary length.
  5. Repeat this procedure until you've created five construction lines. Be sure to keep all of them diagonal.
  6. To exit construction mode, simply click again on Sketcher ToggleConstruction.png Construction Mode
Sketcher geometry

Sketcher geometry is used to create the closed profiles required to perform 3D operations in the PartDesign workbench.

  1. Select Sketcher Circle.png Circle
  2. Position its centerpoint on the origin of the sketch.
  3. Extend the circumference to an arbitrary length.

  1. Select Sketcher Arc.png Arc
  2. Approach the endpoint of one of the construction lines.
  3. Set the centerpoint' of the arc to be coincident with the endpoint.
  4. Select an arbitrary location of your cursor to be set as the beginning of the arc, by clicking once.
  5. Extend the arc an arbitrary amount, making sure the circumference opens outward (the empty space is facing towards the circle you created earlier).
  6. Repeat these steps for each construction line.

  1. Create an arc between each pair of the previous arcs, with their circumference pointing towards the circle.

We have now created the basic elements for our profile.


Constraints are used to constrain the Degrees of Freedom of points and curves within sketcher.

Geometric Constraints

They are used to establish relations between points and curves without the use of dimensions.

  1. Select all five construction lines.
  2. Select Sketcher ConstrainEqual.png Equal Length

  1. Select all five arcs centered on an endpoint of a line.
  2. Select Sketcher ConstrainEqual.png Equal Length
  3. Repeat for all five arcs that are not centered on an endpoint.

  1. Select the construction line that is closest to the vertical axis.
  2. Select Constraint Vertical.png Vertical

  1. Select the endpoint of an arc and the endpoint closest to it.
  2. Select Constraint Tangent.png Tangent
  3. Repeat for each endpoint, until a closed profile is created.

As of this step, we have now created a closed profile that can be adjusted with the desired dimensions.

Datum Constraints

These are used to specify the distance between points in a particular direction and the dimensions of curves.

  1. Select the vertically constrained construction line.
  2. Select Sketcher ConstrainDistanceY.png Vertical Distance
  3. Set the length to 30 mm.

  1. Select the vertical construction line and the line closest to it
  2. Select Constraint InternalAngle.png Internal Angle
  3. Set the angle to 72°
  4. Repeat the same procedure for each pair of adjacent lines.

  1. Select one of the arcs centered on the endpoint of a line.
  2. Select Sketcher ConstrainRadius.png Radius
  3. Set the radius to 8 mm.
  4. Do the same for an arc not centered on an endpoint. Set the radius to 11 mm.
  5. Set the center circle radius to 10 mm.

You should end up with a fully constrained sketch. It can be confirmed by noticing the change in color of all curves.

We are now finished with the basic workflow for the Sketcher Workbench.

Further Reading