Creating Sweeps in Creo

Along with extrude, blend, revolve, and so forth, sweep is a core capability of a robust 3D CAD software, like Creo. Sweeps are used to create shapes that can’t be achieved with simple extrusions or revolutions, making them ideal for modeling pipes, springs, threads, and routed components.

Creo supports several sweep types to address different design needs:

• Sweep: for general path-based geometry
• Helical sweep: for parameter-driven helical shapes
• Volume helical sweep: for removing solid material along a helical path

Creo Tooltips

Since Creo 12, updated tooltips include images and text to be more descriptive of options, tools, etc. Hover over a button and a tooltip will pop up, providing more information to help you understand how to use the feature to best meet your needs.

Creating a Sweep

A Sweep creates a 3D shape by pulling a 2D sketch along one or more trajectories. A trajectory is a curve that defines how geometry moves through space. The user-defined trajectory for a sweep can be a sketch, curve, or model edge.

Standard sweeps are commonly used for designing tubing, structural members, and profiles that must follow complex paths.

To create a sweep in Creo:

1. From the Model ribbon bar menu, open the Sweep tool.
2. Select the trajectory.
3. Sketch a section for sweeping or select a pre-defined section from the Sketcher Palette. Reminder: The section is the profile shape that will be swept along the trajectory. In the video below, the T-shaped profile was selected from the Sketcher Palette menu.
4. If you selected a pre-defined section, edit the dimensions and reference point.
5. Drag the reference point to the center of the trajectory.
6. Preview the geometry and complete the feature.

From there, you can add rounds (fillets), arcs, sweep circles, rectangles, etc. to achieve the desired design.

Creating a Helical Sweep

A Helical Sweep differs from a standard Sweep in one important way: the trajectory is generated automatically in Creo by using helical parameters instead of the user defining an explicit curve. With a Helical Sweep, you’ll define values like:

• Axis of rotation (Helix axis)
• Pitch (distance between helix turns)
• Sketch profile (the shape and diameter of the helix)
• Sketch section (the shape to be swept along the helix)

Helical sweeps are used for springs, threads, coils, or any other helical geometry. To create a helical sweep in Creo:

1. From the Model ribbon bar, select Helical Sweep from the Sweep types list.
2. Define your Axis of Rotation followed by the Sketch Profile to define the length and diameter of the helical sweep.
3. Sketch a section for sweeping or select a pre-defined section from the Sketcher Palette.
4. If you selected a pre-defined section, edit the dimensions and reference point.
5. Drag the reference point to the center of the trajectory.
6. Define the Pitch of the helical sweep.
7. Preview the geometry and complete the feature.

Creating a Volume Helical Sweep

A Volume Helical Sweep differs from a Helical Sweep in that the Volume Helical Sweep is used to accurately model geometry that results from cutting tools used in manufacturing operations. A Helical Sweep builds a shape along a helical path. A Volume Helical Sweep models the machining process to achieve precise geometry.

Volume Helical Sweeps are useful for designing features that are created by a cutting tool moving in a helical path (e.g. threads, grooves, channels, augers, etc.). To create a Volume Helical Sweep in Creo:

1. In an opened part file, select Volume Helical Sweep from the Sweep types list in the Model ribbon bar.
2. Define the Axis of Rotation followed by the Sketch Profile.
3. Select the Section tab to create the section which will be swept along the part.
4. Define the Pitch of the Volume Helical Sweep.
5. Preview the geometry and complete the feature.

From here, you can view the helical path of the section, adjust tilt angle, and more to get precise designs for your 3D model.

Constant vs. Variable Section Sweeps

When creating sweeps, one of the first design decisions is whether the sweeps should be a constant or variable section.

A Constant Section maintains the same section shape and size along the entire trajectory. This is ideal when uniform geometry is required, like pipes, rails, or structural members. A Variable Section, however, allows the section to change size or shape along the trajectory. Variable Sweeps are useful when a feature needs to be tapered, reinforce zones, or attain specific performance. 

Follow the Creo LinkedIn page

Follow Creo on LinkedIn to stay updated on the latest tips & tricks, feature highlights, and more!

Follow us on LinkedIn

Sweeps with Tangent Trajectories

Sometimes, you may be creating a sweep feature with geometry already existing in your 3D model. This is when Tangent Trajectories can be extremely useful. When you mark trajectories as tangent in Creo, the section will flow smoothly from one path to the next so the resulting surfaces blend nicely with the existing geometry.

In Creo, you can set a trajectory as tangent by checking the T box in References Tab of the sweeps menu, or by using the Tangency Tab.

Surface Sweeps

In addition to solid features, sweeps can be used to create surface geometry. A Surface Sweep moves a section along a trajectory without creating a solid model. Surface sweeps are commonly used for creating complex surfaces or supporting advanced shape development. In Creo, you can easily choose if a feature is a solid or surface sweep by choosing the Type, on the left side of the model ribbon, when designing your sweep.

Looking Ahead

Sweeps offer a versatile toolbox for creating geometry that can follow both simple and complex paths. By understanding when to use standard sweeps, helical and volume helical sweeps, constant versus variable sections, etc. designers can build 3D models that are creative and robust.

Learn more on the PTC Learning Connector

Free tutorials, certifications, and self-guided or instructor led classes ensure you get the most out of Creo.

Sign up Now!