Basic 3D-CAD: Creating a Sketch with Constraints and Dimensions

When you wish to create CAD geometry directly using 3D-CAD, you generally start by creating a sketch on a default sketch plane. A closed sketch becomes a solid body when you extrude it or revolve it in subsequent operations.

In this tutorial, you create a profile sketch of a graphics card fan hub.

To start sketching in 3D-CAD:

  1. Create a new Simcenter STAR-CCM+ simulation.
  2. Right-click the Geometry > 3D-CAD Models node and select New.

    The 3D-CAD environment launches and a 3D-CAD model is created. Within 3D-CAD, an object tree appears that is specific to the 3D-CAD model under construction. This tree contains Body Groups, Features, Design Filters, and Design Parameters nodes.

All geometry in CAD starts from a sketch. Sketches are drawn on sketch planes. 3D-CAD has three default sketch planes (XY, YZ, ZX) that pass through the origin (point [0, 0, 0]).

Create a sketch for the fan hub:

  1. In the 3D-CAD feature tree, right-click the XY sketch plane and select Create Sketch.
    Creating a sketch activates sketch mode, in which a grid is displayed on the sketch plane in the 3D-CAD View scene, and the Sketch panel opens.

  2. In the Sketch panel, under the Display Options, click (View Normal to Sketch Plane) to align the sketch plane with the plane of the screen.
    You can rotate the scene using the left mouse button, zoom in and out using the scroll wheel or middle mouse button, and pan the scene using the right mouse button. To realign the view with the sketch plane, click (View Normal to Sketch Plane).
  3. Specify a more suitable grid spacing for the primary and secondary grids:
    1. Click (Set Sketch Grid Spacing).
    2. In the Grid Spacing dialog, set Grid spacing to 0.005 m and Number of fine grid divisions to 5.0.
    3. Click OK.
  4. Using the wheel action of the middle mouse button, zoom in on the scene.
  5. Click (Create Line) and move the mouse over the grid in the 3D-CAD View scene.
    The mouse pointer has a purple sphere that is attached to it, which indicates the position of the point on the grid. The coordinates of this point are displayed in the Line Properties box of the Sketch panel, and change as you move the mouse. The (Snap to Grid) option is active by default, so the point jumps to an intersection between two grid lines as it approaches them.
  6. Move the mouse over the origin (position [0, 0]) and click to start drawing.


    The Line tool creates continuous lines, so the end point of the first line is the start point of the next. The coordinates that are shown in the Line Properties box are automatically updated as each line is defined.
  7. Move the mouse to the right and draw a horizontal line.


    As the line approaches the horizontal position, it snaps and changes to a yellow colour. An icon, depicting the horizontal constraint, appears above the mouse pointer. These visual cues indicate that when you click the mouse button, the horizontal constrain will be applied to the line.
  8. Click the left mouse button to place the second point.
    The horizontal line is constrained automatically.
  9. Press <Esc> to exit the line tool.
  10. Starting from the previous end point, use the line tool to complete the sketch as shown below. You need not press <Esc> after each line—continue clicking until you finally click on the start point of the initial line. When sketching horizontal lines, these are displayed in yellow. Vertical lines are displayed in red. After confirming the sketch position, all lines are displayed in the default blue color.


    The initial sketch does not have to be exact. Aim to draw the correct shape before you finalize the sketch.
Finalize the sketch by adding a fixation constraint and dimensions. Constraints maintain the shape of the overall sketch by constraining the movement or orientation of individual entities or groups of entities. Dimensions specify the size of individual entities. Typically, you apply constraints before you add dimensions.
  1. Right-click the point on the origin and select Apply Fixation Constraint.
  2. Add dimensions to the sketch:
    1. Right-click the bottom horizontal line and select Apply Length Dimension.
    2. In the Dimension dialog, set the length to 45 mm.
    3. Click OK.
  3. Continue to dimension the sketch using length dimensions. Use the following diagram as a guide:


    To relocate dimension arrows and their text, click and drag them away from the sketch lines.

Check the status of the sketch:
  1. Click (Show Status of Sketch Primitive).
    The status of sketch primitives indicates the validity of the sketch. Black edges and vertices indicate that the sketch is fully constrained. This feature is useful for finding issues such as small gaps in sketches or overlapping primitives. Leaving these issues undetected can lead to errors later in the design process.
  2. Click (Show Status of Sketch Primitive) again to hide the status of the sketch.
  3. In the Sketch panel, click OK to exit sketch mode.
    A sketch feature, Sketch 1, is added to the Features node.
  4. Rename the sketch feature to something more descriptive:
    1. Right-click Features > Sketch 1 and select Rename.
    2. In the inline editor, enter Fan Hub Profile.
  5. Save the simulation as foundationTutorial_1.sim.