You can create a geometric face from orphan element faces in a part. Abaqus/CAE creates a new geometric face based on the nodal positions of the selected element faces. Vertices are created at edge nodes where there is a significant change in the element edge direction. The new face appears like other geometric faces in the model, and Abaqus/CAE stitches the new face to adjacent faces in the part. By default, the new face is associated with the mesh; you have the option to change this behavior. In the Model Tree, the new face appears as a Face from mesh feature. You cannot change the group of element faces that comprise the geometric face once it has been created; however, you can delete the face and create a new one, and you can stitch faces that were not stitched together in the original creation of the geometric face.
The new geometric face shares space with the existing orphan element faces in the model. This may result in some areas appearing with the gray unmeshed geometry coloring and others appearing with the dark green and visible element edges of the orphan mesh. This is similar to the appearance of a bottom-up meshed region, where the tan region coloring and the cyan mesh coloring appear together. You can suppress the orphan mesh in the Model Tree to view only the new geometry.
When creating geometry from orphan mesh faces, keep in mind your intended use for the resulting geometry. You want to create faces that will be a good basis for modification and meshing. For example, when you select orphan element faces, your selection should end at any sharp corners or other features so that the geometric face will also end there, creating a logical feature edge. If you do select element faces that span sharp corners, Abaqus/CAE will create a single geometric face that includes the corner—this geometry may be difficult or impossible to mesh using the available top-down meshing techniques.
Note: When you are working with solid orphan elements, selections that include element faces on both sides of a corner (multiple selections from the same orphan element) are not acceptable for creation of a single geometric face.
When Abaqus/CAE creates a geometric face, it stitches together small gaps between edges and small gaps between analytical surfaces by default. You can customize the tolerance values that determine whether small gaps will be stitched in either case, and you can turn off stitching completely for small gaps between edges. Deferring most or all of the stitching until late in the modeling process can be a more efficient modeling option because each stitching operation is processor intensive. Fitting of analytical surfaces cannot be deferred; you must perform this step before the new geometric face is created.
To create geometric faces from element faces:
From the main menu bar, select Tools
Geometry Edit.
Abaqus/CAE displays the Geometry Edit dialog box.
Tip:
You can also create geometric faces from element faces using the 
tool, located with the edit tools in the Part module toolbox. For a diagram of the edit tools in the toolbox, see “Using the Geometry Edit toolset,” Section 69.1.
From the dialog box, select the Face category and the From element faces method.
Select element faces for the new geometric face.
You can select element faces individually, by angle, by limiting angle, by layer, or by analytic shape. For more information on selecting objects in the viewport, see “Selecting objects within the current viewport,” Section 6.2. You can also select an existing surface. You cannot select element faces from two-dimensional or axisymmetric parts.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Surfaces on the right side of the prompt area.
If you want to control stitching, analytical surface fitting, and the mesh association options, click Options in the prompt area, and do any of the following from the dialog box that appears:
Toggle on Stitch with tolerance to apply stitching of nodes in the geometric face you create, and specify the stitching tolerance value.
In the Fit analytic surfaces with tolerance field, specify the stitching tolerance value you want to use for fitting together analytical surfaces in your selection.
By default, Abaqus/CAE associates the geometric face with the mesh. To change this behavior, toggle off Associate face with mesh.
Click OK to close the dialog box.
From the prompt area, click Done.
Abaqus/CAE creates the geometric face feature. The procedure restarts at Step 3 using the most recently used selection method.
To exit the procedure, either
click the cancel button 
in the prompt area, or
click mouse button 2 anywhere in the Abaqus/CAE window, or
select another operation from the Geometry Edit toolset or from the tools in the Part module.
