Sketch Location

When you click on a sketch tool or double-click twice on a face or curve in the modeling window, you enter sketch mode, and a toolbar with additional sketching tools appears:

Sketch on a New Part – Allows you to create a new part before you start sketching. Any existing sketch curves will be imprinted onto the current part before the new one is created.

Move Current Sketch to a New Part – Allows you to retroactively move your current sketch to a new part.

Duplicate Reference Geometry – Allows you to create sketch curves from reference geometry.

Create Sketch Plane – Allows you to create a new sketch plane by selecting a new face.

Sketching Options – Allows you to modify your grid and snap settings.

Move Plane – Allows you to move the sketch plane by opening the Move tool.

While sketching, you can apply geometric relationships such as tangency and perpendicularity to lines, arcs, and circles using sketch constraints. As you sketch, Inspire automatically applies many sketch constraints for you. This behavior can be disabled using the Preferences window, which can also be used to modify the default angle measurements for certain constraints.

When you are finished sketching, right-click to exit the active sketch tool. At this point you are still in sketch mode; you may either select another sketch tool, click on a sketch curve to edit it, or right-click a second time to exit sketch mode entirely. When you exit sketch mode, the Push/Pull tool is automatically activated so that you can immediately pull your sketch into a solid.

Sketch Planes

When in sketch mode, a sketch plane is displayed. It is represented as a grid with major and minor lines, which can be adjusted using the Sketching Options tool in the sketch toolbar.


If you have parts displayed when you select a sketch tool, you define the sketch plane by clicking on a face of a part before you start sketching. If there are no parts displayed when you select a sketch tool, the global x-y plane is automatically designated as the sketch plane.

By default, Inspire maintains the current view of the sketch plane when sketching on a part. Clicking the View normal to grid icon will rotate the model so that the sketch plane is normal to the grid. Successive clicks will toggle back and forth between fitting the entire model in the view and zooming in on selected sketch curves.

Draw a sketch curve
  1. Click on a sketch tool, then click on a face to create a sketch plane. (If there is no existing geometry, the sketch plane will default to the x-y plane.) Alternatively, you can double-click twice on the face of a part, and a sketch plane will be automatically activated on the selected face.
  2. If you want your sketch to be a separate part, click the Create New Part icon.
  3. Your sketch tool is now activated and you can begin drawing curves with your next click on the sketch plane. Refer to the specific sketch tool under points/lines, rectangles, circles, or arcs for more details.
  4. When you are finished with a particular curve, right-click to finish. You are still in sketch mode and can select other sketch tools or edit existing sketch curves.
  5. When you are finished sketching, right-click again to exit sketch mode. At this point the sketch curves are imprinted and can no longer be edited.
  6. Upon exiting sketch mode, you are automatically placed into push/pull mode so that you can extrude your sketch into a solid if desired. Right-click again to exit push/pull mode.

Sketching tips:

  • To retroactively move a sketch to a new part, click the Move Current Sketch to a New Part tool on the sketching toolbar. A new part appears in the Model Browser, and all active sketch curves are moved to the new part.
  • To change the sketch plane, click the Create Sketch Plane tool in the sketching toolbar and select a new face, or use the Move Plane tool.
  • To create a sketch curve from existing reference geometry, click the Duplicate Reference Geometry tool in the sketching toolbar, or right-click on one of the red reference lines and select Create curves from all reference lines from the context menu. (Alternatively, if you only want to create a curve from a single reference line or curve, right-click and select Create curve from the context menu.) The selected reference lines are duplicated, turn black, and are highlighted in yellow to indicate that they are now sketch curves.
  • To make new parts from solids, exit sketch mode, right-click on a part to open the context menu, and select Make new parts from solids. Each solid body is placed in a separate part.
Edit a sketch curve
  1. While in sketch mode, left-click on a sketch curve to select it.
  2. Click and drag on the curve or an end point to reposition it; or when a curve is selected, enter a value in one of the text fields to change a parameter.
  3. Right-click on the curve to add or remove sketch constraints.
  4. Right-click on an empty space to exit editing mode, and right-click again to exit sketching mode.

Sketching tips:

  • When you sketch curves on a face of a part, the curves will automatically be imprinted onto the face when you exit sketch mode. Once curves are imprinted, they can no longer be edited.
  • If you create a sketch that does not touch an existing face, then when you exit sketch mode, faces will be created from any closed loops in the sketch. You can double-click any faces created this way to return to editing the original sketch.
  • To join two curves, click and drag an end point or center point of one curve until it touches an end point or center point of another curve. The two curves are permanently fused together.
  • To separate joined curves, use the Break tool, or make a copy of one curve by holding down the Command key and drag the copy to a new location. Then select the original curve again and press Delete.
Modify grid settings
  1. While in sketch mode, click the Sketching Options tool to open the Grid and Grid Snap window:
  2. Inspire has five progressive levels of grid spacing. To change the default spacing for a particular grid, enter a value in the Grid spacing text box.
  3. By default, Snap to grid is active. You can suspend snapping temporarily by pressing the Alt key. To disable grid snapping entirely, deselect the checkbox.
  4. Select View normal to plane on create if, when you create a sketch plane, you want Inspire to automatically rotate your view so that the sketch plane is normal to the view. If you want to maintain the current view of the sketch plane, deselect this option.
  5. Click OK.