Intersect

The Intersect command lets you compute the intersection of the shape you define with the features you wish to modify. In other words, the resulting shape is the intersection between the shape of the Intersect and the shapes of the selected features.

This task shows you how to create an intersect feature from a prism.
Open the Intersect.CATPart document.

 

 

  1. Click the Intersect icon .
    The Intersect Feature dialog box is displayed.

  2. Select Remove Sweep.2 as the feature to modify.

    If you select several features, the field displays the number of selected elements. To act on this selection, just click the icon to display the Element list dialog box that allows you to:

    • view the selected elements
    • remove any element clicking the Remove button
    • replace any element using the Replace button and selecting a new one in the geometry or the specification tree.

    Wall

    You can control whether the wall is constructed inside or outside of the selected  profile. The default is an inside wall thickness. Please refer to Inside/Outside definition in Remove feature.

    Shape Definition

  3. Intersect features can have different shapes. The prism is the default shape. If you prefer a different shape, click any of the other three shapes available. To know how to create any of them, refer to the Prism, Sweep, Revolve, Thick Surface or External Shape tasks. For the purposes of our scenario, keep the default option.

  4. Select Sketch.4 as the profile defining the prism.
 

    Intersection Fillet

    The Intersection Fillet provides the capability to create fillets at the intersections with the targets. Also it provides the ability to keep the wall thickness constant when modifying wall creating feature that has set the constant wall option.

  1. Select Intersection radius and enter 1mm.

    Direction

  1. Check Normal to profile to extrude the profile normal to Sketch.4.

  2. Enter 60mm for First length and 30mm for Second length.

  3. Click OK to confirm the operation.

    The intersection between the defined prism you defined and Remove Sweep.2 looks like this:

    Intersect  Prism.X is added to the specification tree in the Solid Functional Set.X node.

 

    Control Wall Creation

    When the Intersect feature is applied to a "wall creating feature", in this case Pocket feature, and if the wall type is set to Use feature thickness and the target feature has a Constant wall thickness option, the Intersect feature has the capability to control the wall creation.
    Also Intersect feature has the ability to keep the wall thickness constant when modifying "wall creating features" that have been set the Constant wall thickness option.

  1. Click the Intersect icon .

  2. Select Shellable Prism.1 and Pocket.1 as Features to modify.

  3. Select Sketch.5 as Profile/Surface.

  4. Select Intersection radius and enter 3mm.

  5. Enter 60mm for First length and 30mm for Second length.

  6. Click OK.
 

More about the Wall Area

The Wall option lets you set if, or how, the Intersect Feature command creates walls along the intersecting surface.

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

  • Use body thickness: the 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 box becomes available. Wall thickness values can only by positive values.

  • Use feature thickness: the wall thickness will be the same thickness as the target feature.

However, if the target feature has no thickness parameter in its definition (for example if the target feature is an external feature), the Intersect Feature capability assigns the thickness value defined in Shell Properties to the wall. If this behavior does not meet your needs, you still can:

  • Set the thickness value to 0mm in Shell Properties before running Intersect Feature.

Or:

  • In the Intersect Feature dialog box, use Enter thickness and assign the value you need.