To create a profile you must choose a profile type and enter all of the data necessary to define the profile in the Edit Profile dialog box. See the following sections for detailed instructions:
The Create Profile dialog box allows you to specify which type of profile you want to define. You can define a shape-based profile by providing the geometric data from which Abaqus can calculate the engineering properties of the section. Alternatively, you can define a generalized profile by providing the engineering properties of the section directly. For more information, see “Beam section behavior,” Section 29.3.5 of the Abaqus Analysis User's Guide.
After you have assigned the beam section and beam orientation to the part, you can use the part display options to view an idealized representation of the shape-based or generalized beam profile. Displaying beam profiles is useful for checking that the correct profile has been assigned to a particular region and that the assigned beam orientation results in the expected orientation of the profile. For more information, see “Controlling beam profile display,” Section 76.7.
To choose a profile type:
From the main menu bar, select Profile
Create.
The Create Profile dialog box appears.
Tip:
You can also click Create in the Profile Manager or select the create profile tool 
in the Property module toolbox.
Enter a profile name. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select a profile shape, and click Continue.
The Edit Profile dialog box for the profile shape you have chosen appears.
In the Edit Profile dialog box, enter the required profile data. See the following sections for details:
Define a box profile by providing geometric data for a rectangular, hollow box.
To define a box profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the Width (a) field, enter the length of the segments parallel to the local 1-axis.
In the Height (b) field, enter the length of the segments parallel to the local 2-axis.
Click the arrow to the right of the Thickness field, and indicate how you want to define the thickness of each segment:
Select Uniform if each of the four segments of the box have the same thickness. If you select this option, enter the segment thickness in the Thickness field below.
Select Individual to enter a value for each segment individually. If you select this option, enter the following:
In the t1 field, enter the segment thickness labeled t1 in the diagram.
In the t2 field, enter the segment thickness labeled t2 in the diagram.
In the t3 field, enter the segment thickness labeled t3 in the diagram.
In the t4 field, enter the segment thickness labeled t4 in the diagram.
Click OK to save the profile and to close the Edit Profile dialog box.
Define a pipe profile by providing geometric data for a hollow circle and by selecting an integration scheme for a thin-walled pipe or a thick-walled pipe.
To define a pipe profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
From the Integration scheme options, specify a thin-walled pipe or a thick-walled pipe.
In the Radius field, enter the radius of the circle from the center of the pipe to the outside edge of the pipe wall.
In the Thickness field, enter the thickness of the pipe wall.
Click OK to save the profile and to close the Edit Profile dialog box.
Define a circular profile by providing geometric data for a solid circle.
To define a circular profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the r field, enter the radius of the circle.
Click OK to save the profile and to close the Edit Profile dialog box.
Define a rectangular profile by providing geometric data for a solid rectangle.
To define a rectangular profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the a field, enter the length of the rectangle edges parallel to the local 1-axis.
In the b field, enter the length of the rectangle edges parallel to the local 2-axis.
Click OK to save the profile and to close the Edit Profile dialog box.
Define a hexagonal profile by providing geometric data for a hollow hexagon.
To define a hexagonal profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the r field, enter the circumscribing radius.
In the t field, enter the wall thickness.
Click OK to save the profile and to close the Edit Profile dialog box.
Define a trapezoidal profile by providing geometric data for a solid trapezoid.
To define a trapezoidal profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the a field, enter the length of the lower edge of the trapezoid parallel to the local 1-axis.
In the b field, enter the height of the trapezoid parallel to the local 2-axis.
In the c field, enter the width of the top edge of the trapezoid parallel to the local 1-axis.
In the d field, enter the distance between the lower edge of the trapezoid and the local cross-section axis.
Click OK to save the profile and to close the Edit Profile dialog box.
Define an I-shaped profile by providing geometric data for an I-beam section.
To define an I-shaped profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the l field, enter the distance between the lower edge of the bottom flange and the local cross-section axis.
In the h field, enter the height of the I-shape, from the bottom edge to the top edge.
In the b1 field, enter the width of the lower flange parallel to the 1-axis.
In the b2 field, enter the width of the upper flange parallel to the 1-axis.
In the t1 field, enter the thickness of the lower flange.
In the t2 field, enter the thickness of the upper flange.
In the t3 field, enter the thickness of the segment joining the upper and lower flanges.
Click OK to save the profile and to close the Edit Profile dialog box.
Define an L-shaped profile by providing geometric data for an L-beam section.
To define an L-shaped profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the a field, enter the length of the flange parallel to the local 1-axis.
In the b field, enter the length of the flange parallel to the local 2-axis.
In the t1 field, enter the thickness of the flange parallel to the local 1-axis.
In the t2 field, enter the thickness of the flange parallel to the local 2-axis.
Click OK to save the profile and to close the Edit Profile dialog box.
Define a T-shaped profile by providing geometric data for a T-beam section.
To define a T-shaped profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the b field, enter the length of the segment parallel to the 1-axis.
In the h field, enter the height of the T-shape, from the bottom edge to the top edge.
In the l field, enter the distance between the lower edge and the local cross-section axis.
In the tf field, enter the thickness of the segment parallel to the local 1-axis.
In the tw field, enter the thickness of the segment parallel to the local 2-axis.
Click OK to save the profile and to close the Edit Profile dialog box.
You can create an arbitrary profile to model the shape of a simple, thin-walled, open or closed section. You define the profile by entering a series of points which are linked by straight line segments. For more information, see “Arbitrary, thin-walled, open and closed sections” in “Beam cross-section library,” Section 29.3.9 of the Abaqus Analysis User's Guide.
To define an arbitrary profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the data table, enter the local coordinates for Point 1.
For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
Enter the local coordinates for Point 2. The line joining Point 1 and Point 2 is labeled Segment 1-2 in the data table.
Enter a Thickness for Segment 1-2.
Enter the local coordinates for Point 3. The line between Point 2 and Point 3 is labeled Segment 2-3 in the data table.
Enter a Thickness for Segment 2-3.
Note: For each individual segment of an arbitrary section there is no bending stiffness about the line joining the end points of the segment. Thus, an arbitrary section must include at least two segments.
If necessary, enter local coordinates for additional points, and provide thicknesses for the resulting segments.
Click OK to save the profile and to close the Edit Profile dialog box.
When you create a generalized profile, you provide the engineering properties of the section directly in the Edit Profile dialog box. For more information, see “Beam section behavior,” Section 29.3.5 of the Abaqus Analysis User's Guide.
To define a generalized profile:
Display the Edit Profile dialog box, as described in “Choosing a profile type.”
In the Area field, enter the area of the profile shape.
In the I11 field, enter the moment of inertia for bending about the 1-axis of the section.
In the I12 field, enter the moment of inertia for cross-bending.
In the I22 field, enter the moment of inertia for bending about the 2-axis of the section.
In the J field, enter the torsional constant.
If the profile describes an open-section beam, enter the following:
In the Gamma O field, enter the sectoral moment, 
.
In the Gamma W field, enter the warping constant, 
.
Click OK to save the profile and to close the Edit Profile dialog box.