During the initial creation of a skin, you select one or more faces that you want to reinforce and, if desired, the number of skins that you want to create. After the skin is created, you can modify it in the following ways:
In the Property module, you can modify a skin by assigning it a section (a homogeneous shell section, a composite shell section, a membrane section, a surface section, or a gasket section), a material orientation, or a rebar reference orientation. You can also reverse the normal direction of a skin by assigning a normal direction to its underlying face. When you reverse the normal direction for a face, all skins assigned to that face inherit the new normal direction as well.
In the Mesh module, you can assign an element type to the skin. When you are prompted to select the regions to be assigned element types, you must select Skins from the list of object types in the Selection toolbar. If you assign a shell section to a skin, you must assign shell elements to the skin. Similarly, if you assign a membrane, surface, or gasket section, you must assign membrane, surface, or gasket elements.
You can obtain data from a skin by using the field and history output request editors in the Step module. In the Domain section of the editor, select Skin and choose the desired skin from the menu that appears. For more information, see “Creating an output request,” Section 14.12.1.
To create a skin reinforcement:
From the main menu bar in the Property module, select Special
SkinCreate.
Tip:
You can also click the 
tool in the Property module toolbox.
Use one of the following methods to select the faces to which you want to add skin reinforcements:
Selecting individual faces:
Click the arrow next to the Select entities on which to create a skin field in the prompt area, and select individually from the list that appears.
Select a face to which you want to add skin reinforcement.
[Shift] + Click on additional faces to add them to your selection.
If necessary, [Ctrl] + Click on selected faces to unselect them.
When you have finished selecting faces, click mouse button 2.
Specifying an existing set:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of sets that you have created.
Select the set of faces to which you want to add skin reinforcement, and click Continue.
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 Sets on the right side of the prompt area.
Selecting faces using the angle method:
Click the arrow next to the Select entities on which to create a skin field in the prompt area, and select by face angle from the list that appears.
Enter an angle (from 0° to 90°), and select a face. Abaqus/CAE selects every adjacent face from the selected face until the angle between the faces is equal to or exceeds the angle that you entered. (See “Using the angle and feature edge method to select multiple objects,” Section 6.2.3, for more information.)
After you use the by face angle method, you can [Shift] + Click on additional faces to add them to your selection or [Ctrl] + Click on selected faces to remove them from your selection. (See “Combining selection techniques,” Section 6.2.8, for more information.)
Tip: You can use the Selection toolbar to limit the types of objects that you can select in the viewport. For more information, see Chapter 6, “Selecting objects within the viewport.”
If desired, toggle on Multiple skins in the Prompt area to create more than one skin reinforcement for the selected face or faces.
Click Done to create the skin. If you are creating multiple skins, enter the number of skin layers you want to create, and click mouse button 2.
