Creating a Web

This section explains how to create a web, that is the main feature of an Aerospace SheetMetal Design part.

Open the Web1.CATPart document.

  1. Click Web .

    The Web definition dialog box is displayed.
  2. In the Support field, select the support geometry in the specification tree.

    The Material Direction is displayed, perpendicular to the geometrical support. You can reverse the direction by clicking the arrow or the Invert Material Dir button.

    The support can either be a plane, a closed sketch or a surface. It can also be non ruled surface.
  3. In the Boundary field, in the case of an open geometry, select the elements (curves, surfaces, planes or sketches) that limit the support geometry.

    The elements must be selected consecutively.
    They are displayed in the Boundary frame as well as in the 3D geometry, in the order you have just chosen them.
    When a closed profile can be built, a light preview of the web is available. Otherwise, click Preview.
    You can modify your boundaries by selecting an existing limit and using the following buttons to:
    • add a limit after the selected limit (Add After)

    • add a limit before the selected limit (Add Before)

    • replace a limit (Replace)

    • remove a limit (Remove)

    • select a limit more than one time (Insert)

    In the following example, we first select three elements to limit the web.
    Then we select Surface.1 and click on the pink sketch to add it to the web's definition.
    Then we select Surface.1 again and click on the yellow sketch to add it to the web's definition.
    Note that Surface.1 is displayed twice in the Web Definition dialog box.
    The Web is created according to several elements.


    • select several limits or several times the same limit to modify the existing limit (Multiple Sel). This option is available once you have selected Add After, Add Before, Replace: the Limits to Add dialog box appears to let you select the limits.
    The aim of the following example is to relimit the web so as to obtain the result as shown below.

    Web before relimitation


    Web after relimitation

    To do this, you have to select twice the same limit (vertical line).
    1. Select Sketch.2 in the Web definition dialog box, (also called Limit 2).
    2. Click on Replace to define a new limit.
    3. Click Multiple Sel. to select the sketches that are to be part of Limit 2.
    4. In the Replacing Limits dialog box, select each sketch clockwise to define Limit 2.
      You have to select sketch.5 (vertical line) twice: it is considered as Limit 1 then as Limit 5 once selection is over.


    • remove all limits (Remove All)
    Once you have modified the selection, a light preview is available. You can click the Preview button to display the result of the web.

    When the profile is defined by a list of geometrical elements, the following operations are performed:

    • the curves are projected on the web geometrical support

    • the surfaces are intersected with the web geometrical support

  1. Click OK.

    The web (identified as Web.1) is created and the specification tree is updated accordingly.
    In hybrid context, even though a web is created with several features, none are aggregated under the web in the specification tree.
    Yet, if you open a part created in a previous release, the specification tree will be displayed accordingly to the previous behavior. For more information about Hybrid Design, refer to the Hybrid Design section in the Part Design User's Guide.

Creating a surfacic web

Open the Web2.CATPart document.
  1. Click Web .

    The Web definition dialog box is displayed.
  2. Select Extrude.1 as the support of the web.

  3. Select a reference wire and an invariant point as references for the unfolding of the web.

    The reference wire must be located on one of the limits (if any) and the invariant point must be located on the reference wire.

    It is not necessary to construct a curve belonging to the boundary: if the selected element is a specification of the boundary, the reference wire will be automatically computed.

    In our example, we choose Extrude 4 and one of the corner located on this edge.
    While defining the reference wire, you can select an extrusion : it is the intersection between this extrusion and the web support that will be considered as the reference wire.


  4. In the Boundary field, select the elements that limit the support geometry.

    In our example, we chose Extrude 4, Project 1, Extrude 2 and Extrude 3 (but you can also select Sketch 6).
    A preview of the web (in red) and a preview of the unfolded web (in white) is displayed.
    If the white preview is not displayed, you have to reconsider the reference wire or the invariant point.
    The selection of limits is optional if you want the web to have the same dimensions and shape than the support.
    While defining the limits of the support geometry, you can select an extrusion : it is the intersection between this extrusion and the web support that will be  considered as the limit.
  5. Click OK.

    The web (identified as Web.1) is created and the specification tree is updated accordingly.
    • You cannot build a Joggle on a surfacic web while it is supported.
    • The supporting surface of a surfacic web must be ruled. A surfacic web can only be created if the supporting surface shows a tangency continuity.
    • The minimum curvature radius of the faces of the web must be significantly high compared to the height of the Surfacic Flange to build the Surfacic Flange.
    •  You can only build a surfacic flange on a non planar web if:
      • the OML is connex
      • there is only one possible surfacic flange

      In the following example, a surfacic flange cannot be computed with the red support.