A
datum can be thought of as reference geometry or a construction aid that helps
you create a feature when the part does not contain the necessary geometry; you
create datum geometry using the
Datum toolset.
A datum is a feature of a part and is regenerated along with the rest of the
part. Furthermore, datum geometry is visible unless you toggle it off by
selecting ViewPart Display
OptionsDatum from the main
menu bar. A datum created in the
Part module
appears with each instance of the part in the
Assembly module
or any other assembly-based module.
Datum points are projected onto the Sketch plane in the Sketcher, and the
projected point can be selected. However, you cannot refer to datum axes or
planes in the Sketcher. Examples of how you might use datum planes and axes in
the
Part module
are given below.
Datum plane
You can sketch directly on datum planes, and any features you sketch on a
datum plane will be projected onto the part. Projecting a sketch from a datum
plane is useful if the part does not already contain a convenient sketch plane.
For example, suppose you want to cut a hole straight through the
three-dimensional triangular part shown in
Figure 1
parallel to the X-axis.
Figure 1. The desired cut feature.
The part does not already have a face that is suitable for sketching the
profile of the hole; sketching the profile directly on a face results in a hole
normal to the face, as shown in
Figure 2.
Figure 2. A cut normal to the face.
To cut the desired hole, first use the
Datum toolset
to create a datum plane on the Y–Z principal plane,
as shown in
Figure 3.
Figure 3. A datum plane.
Second, sketch the profile of the cut on the new datum plane, as shown in
Figure 4.
Figure 4. A sketch on the datum plane.
When you exit the Sketcher,
Abaqus/CAE
cuts the sketched hole through the part, perpendicular to the datum plane and
parallel to the X-axis. This cut is illustrated in
Figure 5.
Figure 5. The desired cut.
Datum
axis
You can use the
Datum toolset
to create a datum axis. You can then select the datum axis to control the
orientation of the part on the Sketcher grid when adding or modifying a feature
to a three-dimensional solid. Creating a datum axis is useful when the part
does not already contain the necessary axis.
For example, suppose you want to cut a slot through the part as shown in
Figure 6.
Figure 6. The desired slot.
Sketching the slot is difficult because selecting either of the two straight
edges of the part as the sketch's vertical axis causes the sketch gridlines to
align with the line you select, not with the X- or
Y-axis. To make it easier to create the slot with
the desired orientation, first use the
Datum toolset
to create a datum axis along the Y-axis, as shown in
Figure 7.
Figure 7. The datum axis.
When you select the datum axis to appear vertical and on the right, the
Sketcher starts, and its grid is aligned with the part's
X- and Y-axes, as shown
in
Figure 8.
