Creating Circles

You can create round using the Circle command. Once you have created one circle, you can create any other and in the meantime use the radius parameter from the circle first created.

This task shows you how to create a circle.

By default, circle centers appear on the sketch. If you do not need them, you can specify this.

Before you begin:

Ensure that Geometric Constraints and Dimensional Constraints are activated in the Sketch Tools toolbar.

Related Topics
Creating Three Point Circles
Creating Tri-Tangent Circles
Creating Circles Using Coordinates

Create a Circle

You can create a round using a Circle command.

  1. Click Circle in the Profile toolbar (Circle sub-toolbar).

  2. Click anywhere in the geometry area to locate the circle center, or if you know where this point must be located, use the Sketch Tools toolbar which now displays value fields for defining the point coordinates.

    These value fields are:

    • H: horizontal

    • V: vertical

    • R: radius

  3. For the purposes of our scenario, enter the circle center coordinates: H=30mm, V=30mm.

  4. Repeat the operation to define point on circle coordinates: just enter R=20mm.

    The circle is created.



    Tip: Constraints are assigned to this circle on the condition that:
    • You activated Dimensional Constraints in the Sketch tools toolbar before starting the scenario.
    • You entered coordinate values in the fields (you did not create the circle just by clicking).

Create a Circle Reusing a Circle Radius Value

To create a circle reusing a circle radius value, select the first circle and use the command Parameter > Copy Radius.

  1. Click Circle .

  2. Right-click the first circle and select Parameter > Copy Radius.

  3. Click to indicate the second circle location or use the Sketch tools toolbars to specify the circle center.



    The new circle is automatically created with the radius of the circle first created but not positioned.