Home / Creo Parametric / Creating Datum Axes

Creating Datum Axes

Datum axes are particularly useful for making datum planes, placing items coaxially, and creating axis patterns.
• Definition:
– No mass, infinite linear reference
– Display length can be changed
• Uses:
– Construction geometry
– Reference
• Types:
– Auto axis
– Axis feature
– Geometry point
– Geometry centerline
Datum Axis Definition

Creating Datum Axes 1
Figure 1 — Various Datum Axis Types

Creating Datum Axes 2
Figure 2 — Geometry Axis (Centerline)
Created for Revolve Feature Datum axes are individual features that can be redefined, suppressed, hidden, or deleted. A datum axis is a linear reference that has no mass. It is infinite in length, but its display length can be edited by selecting a reference, specifying a value, or dragging the drag handle. Datum Axis Uses A datum axis can be used as construction geometry in a feature. It can also be used as a reference for:
• Other datum features, such as datum planes.
• Other features, such as a hole location.
• Assembling components.
Datum Axis Types

There are four different types of datum axes that can be created within Creo Parametric:
1. Auto Axis — Belongs to another feature and is created in the following two circumstances:
• A circle is extruded.
• A hole is created.
2. Axis Feature — Select almost any combination of geometry that defines a line in 3-D space. You can select single or multiple references which are set as a combination of Through, Normal, Tangent, and Center constraint types. The following types of axis features can be created:
• Through an edge.
• Normal to a plane.
• Through a cylindrical surface.
• Through the intersection of two planes or planar surfaces.
• Through two points or vertices.
• Through the center of an arc.
• Tangent to an edge.
• Through a point or vertex, normal to a plane.
• Through the X, Y, or Z axis of a coordinate system.
3. Geometry Point — When created in Sketcher and when the sketch is completed, the axis appears at the location of the geometry point, normal to the sketch plane. A geometry point within a sketch can only create axes when used for internal sketches of extrude features.
4.Geometry Centerline — Created only in Sketcher. A geometry centerline is created in the sketching plane, and when the sketch is completed,  it displays as a datum axis within the graphics window. A geometry centerline can be used as the axis of revolution for a revolve feature. When a geometry centerline is selected in Sketcher, you can right-click and select Construction to convert it to a sketch entity.Similarly, you can select a centerline and right-click and select Geometry to convert the centerline to a geometry centerline. Selecting Datum Axes You can select datum axes using the following methods:
• Select the axis line.
• Select the axis name tag.
• Select the axis in the model tree.
• Search for the axis by name in the search tool.

Leave a Reply

Your email address will not be published. Required fields are marked *