When you sketch the profile of a feature, ABAQUS/CAE projects onto the sketch sheet all the edges and vertices of the part or assembly that are in the same plane as the sketch plane. ABAQUS/CAE also projects all datum points and datum axes onto the sketch sheet, regardless of their location in the part or assembly. These projected points and lines are called reference geometry, and you can use them for reference while sketching.
You typically use reference geometry to position your sketch accurately by specifying a dimension between a sketched entity, such as a line or a vertex, and the reference geometry. You can also use reference geometry to realign the sketch grid. The sketch retains any reference geometry that is used to position or dimension the sketch—the reference geometry reappears when you use the Sketcher to edit the feature again. ABAQUS/CAE discards any reference geometry that is not used in the sketch.
If your part is complex, projecting only the edges, vertices, and datum points in the sketch plane onto the sketch sheet reduces the amount of clutter on the screen and makes the selection procedure more straightforward. However, your selection will be limited to only edges, vertices, and datum points that are in the sketch plane. If you want to use other edges, vertices, or datum points as references, you must project them onto the sketch plane as reference geometry by using the Project References tool 
. Alternatively, if you want to create new sketch edges from existing model edges, you can use the Project Edges tool 
(for more information, see “Projecting edges onto a sketch,” Section 19.15).
When you sketch a new feature, you can constrain the position of the sketch to the underlying reference geometry using one of the following methods:
Select entities from the reference geometry while sketching the new feature; for example, select a projected vertex to define the center of a circle or one end of a line.
Create a constraint, dimension, or parameter between the sketch and any projected reference geometry. For more information, see “Controlling sketch geometry,” Section 19.7.
When you exit the Sketcher, ABAQUS/CAE determines whether you have constrained the sketch to the reference geometry. If a constraint is found, ABAQUS/CAE creates a parent-child relationship between the new feature (the child) and the selected reference geometry (the parent). If no constraints are found, ABAQUS/CAE displays the following message in the message area: No sketch placement constraints specified on feature feature name. You do not have to constrain the sketch; but if you do not, its position relative to the underlying geometry of the part or assembly may change if you modify and regenerate the part or assembly.
If you save a stand-alone sketch, ABAQUS/CAE saves only the sketch and does not save any underlying reference geometry. As a result, if the sketch includes a dimension between a sketch line and a reference line, the dimension is not saved with the stand-alone version of the sketch.
The order in which you create features influences the available reference geometry. Feature-based modeling allows a child feature to be dependent on a parent feature but does not allow a parent to be dependent on a child. As a result, if a feature was created after the feature you are editing, the edges and vertices of the newer feature cannot be projected onto the sketch sheet. You can use the Query toolset to determine the order in which features were created; for more information, see “Using the Model Tree to obtain feature information,” Section 42.4.8.
