The Reinforcement capability adds external strength by adding material to the outside of material volumes that the reinforcement intersects with in the same body.

This task shows you how to add reinforcements.

Open the Reinforcement.CATPart document.



  1. Click the Reinforcement icon .
    The Reinforcement dialog box is displayed.

  2. Select Sketch.2 as the planar profile to be used.

    The profile can be open or closed.

    If no profile is defined, clicking the Sketcher icon enables you to sketch the profile you need.

     If you are not satisfied with the profile you selected, note that you can:

    • click the Profile/Surface field again and select another sketch.

    • use any of these creation contextual commands available from the Profile/Surface field:


  3. Enter 8mm in the Length field to define the distance from the sketch plane up to the ceiling.

    To define the opening, enter the value of your choice in the Length field to define the distance from the sketch plane up to the opening.

    Instead of using the Length option, you can set To shell . This capability extends the reinforcement to a shellable volume in the active body, in the opposite direction of the height. The extension of the reinforcement profile must fit inside the boundaries of the shellable volume. Otherwise, no extension will occur.

  4. In the Width field, enter 4mm to define the width of the reinforcement. The width is distributed equally to both sides of the profile.

    Checking the Mirrored extent option extrudes the profile in the opposite direction using the same length value as the one defined for the first length.
    Clicking the Reverse Direction button reverses the extrusion direction. Another way of reversing the direction is by clicking the arrow in the geometry area.


    By default, the Normal to profile option  is checked, meaning that the profile is extruded normal to the sketch plane. If you wish to specify another direction, just uncheck the option, and then select a geometrical element to be used as the new reference.

    Clicking the Reverse Direction button reverses the extrusion direction.


  5. If you wish to define a draft angle, just click the Draft tab, then check the Angle field and enter the desired value in the Angle field.

    • Ceiling
    • Opening


    Checking the Lateral radius option enables you to fillet lateral edges. Then, you merely need to set the radius value of your choice.


    With Lateral radius option and Fillet profile ends option, you can apply fillets at the intersection or at the ends of the open profile of the reinforcement. Please see Prism for some examples.

    With lateral radius ON
    (Fillet profile end is OFF)
    With lateral radius and Fillet profile end ON

    In this scenario, we don't apply Lateral radius option.

  1. Check the Ceiling radius option to fillet the cylinder's top and enter 0.8mm to define the ceiling radius value.
    If the rest is to be shelled, you can check the Constant wall thickness option which propagates the fillets into the shell, thus maintaining a constant wall thickness.


    To define the wall, you can set one of the two options available from the Type drop down list:

    • Use body thickness: the reinforcement wall thickness is that of the active shelled body thickness.

    • Enter thickness: simply enter the value you want. After this option is selected, the value field becomes available. Wall thickness values can only by positive values.


    You can control whether the wall is constructed inside or outside of the selected  profile. The default is an inside wall thickness.

  1. For the purposes of our scenario, set the Enter thickness option and enter 2mm in the Thickness value field.

  2. Click OK to confirm and create the reinforcement. Reinforcement.X is added to the specification tree in the Solid Functional Set.X node.