Creating Welding Curve Beads

This task shows you how to create and trim a BiW Welding Curve Bead.
  There are several ways to create a curve bead:
  • a joint and a joint body are already created: click the desired icon and select the joint body in the selection tree.
  • a joint and a joint body are already created: select the joint body in the selection tree and click the desired icon (here is the example used for our scenario).
  • no joint body is created. Select the components or the publications, and click the desired icon: a joint and a joint body are created if needed.

Open the ABF_CurveBead.CATProduct document.
 
Make sure the curve bead Fastener Type is set up in the standard file.

  1. Select the joint body in the specification tree.

  2. Click BiW Welding CurveBead in the Welding toolbar.

    The BiW CurveBead Fastener Definition dialog box opens.

  3. Specify whether you wish to use the existing standard or not.

    If a standard has been imported, a curve bead is created using this standard. If not, you are able to define your own values for each attribute.
     
    If the last location method is different from Explicit, the ABF application creates a specification part associated to the assembly joint if this specification part does not already exist.
    You must not delete this specification part.

  4. Select the process type and the stacking.

  5. Define the functional parameters of the curve bead:

    • Robustness

    • Regulation

    • Finish

    • More>>: allows you to define Manufacturing parameters.

    • Discretization Method:

      • Unspecified: no discretization method is used. The default visualization is set in Tools > Options > General > Display > Performances > 3D Accuracy.

      • Sag: segments are defined on the curve according to the tolerance value set in the discretization parameter.
         

      • Step:  equidistant points are created on the curve according to the value set in the discretization parameter.
         

      • Discretization Parameter: distance value for each curve bead depending on the chosen discretization method.

        • distance = sag if the sag discretization method was chosen

        • distance = step if the step discretization method was chosen
    Both parameters will be used for the visualization of the curve bead and for the export/report.

  6. Specify the material.

  7. Specify the definition:

    • curve path

    • cylinder path

    • half cylinder path, etc.

  8. Define the diameter in the following cases:

    • Curve Path
    • Cylinder Pipe
    • Half Cylinder Pipe
    Curve Path
    Cylinder
    Half Cylinder

  9. Define the base and height in the following cases:

    • Diamond Pipe
    • Half Diamond Pipe
    • Rectangle Pipe
    • Half Rectangle Pipe
    Diamond Pipe
     
    Half Diamond Pipe
     
    Rectangle Pipe
     
    Half Rectangle Pipe

  10. Select the location (see below):

    According to the location you choose, different dialog boxes open, except when selecting the Explicit mode.

  11. Define the orientation of the curve bead by setting the K axis to either:

    • Same as Surface Material

    • Opposite to Surface Material
     
    To visualize the K axis, the K Axis Only option should be checked in Tools > Options.

  12. Click OK to create the curve bead.

    The curve bead (identified as Joint Element.xxx) is added to the specification tree, under the Assembly Joint Body node.
Annotations can be automatically created during the fastener creation. For more information, refer to Creating Fastener Annotations Automatically.

Locating the CurveBead

Along Curve

  1. Select the curve.

    Green arrows appear in the 3D geometry to let you know the end and start point of the curve bead:

  2. Click the More>> button to display further information.

  3. From the Along Curve Location dialog box, click the Swap Start and End Points button to change the curve direction.

     
    The Split Support Curve enables to trim the curve bead.
    The curvebead will be created along the original curve.

From Curve On Surface

  1. Select a curve, for instance a part edge.

    Most of the times, a surface is selected by default.
    Green arrows appear in the 3D geometry to let you know the end and start point of the curve bead.

  2. If needed, select a surface.

    If the surface could not be found, or if you want to select another surface, choose a surface in the drop-down list. To choose an unspecified zone, select Other (Zone Unspec) and then select the zone in the 3D geometry.

  3. Optionally modify the offset. In our example, we defined an offset of 10mm.

  4. Click the Swap Start and End Points button to change the curve direction.

  5. Click the Inverse  Offset button changes the offset curve bead position according to the original curve bead.

     
    The Split Support Curve enables to trim the curve bead.
    The curve bead will be created along the original curve offset.
    If several solutions are possible (for instance if there is a hole on the surfaces), you need to select the surface in the 3D geometry that is the closest to the curve bead to be created:

Intersect
Open the Intersect1.CATProduct document.
  1. Click the More>> button to display further information.
  2. Successively select two surfaces, either in the 3D geometry or in the specification tree.
    The curve bead is located at the intersection of the two surfaces.

    • You can as well select a plane as the surface.

    • Surfaces must belong to the joined components but may be different from the joint body zones.
  3. Click the Swap Start and End Points button to change the curve direction.

    The Split Support Curve enables to trim the curve bead.
    The curve bead will be created from the intersection of the two surfaces. Its normal is the normal to the first selected surface at the curve bead's start point.
    If several solutions are possible (for instance if there is a hole between the two surfaces), you need to select the surface in the 3D geometry that is the closest to the curve bead to be created:

Explicit
  • You need to select first one of the three other options (Along curve, from curve on surface, or Intersect) to be able to select the curve position.
  • When selecting the Explicit mode, the curve location is kept and it cannot be modified.
    The curve location is then a polyline, which is recalculated according to the selected curve, and does not reference the specification part anymore.
    When the location method switches to Explicit, the specification part is automatically deleted if it is empty.
  • The polyline is computed according to the discretization parameters. If it is set to Unspecified, the discretization value is calculated from the options defined in Tools > Options > General > Display > Performances > 3D Accuracy.
  • The Isolate command has the same behavior as the Explicit method: you can select the Isolate item from the contextual menu once the curve is created, by right-clicking the joint element.
 

Trimming a Curvebead

  1. Select the curvebead location. In our scenario, we selected the From Curve On Surface location.

  2. Check Split Support Curve.

    • This option is only available with all the location methods but the Explicit location method.
    • This option must be activated to be able to define the Start and End points values.
    The Repeat object after OK button appears in the BiW CurveBead Fastener Definition. Refer to the Repeating CurveBeads to create more curve beads using the currently created spot point as reference.
    The From Curve On Surface Location dialog box opens.

  3. Enter 0.2 for the Start point.

  4. Enter 0.7 for the End point.

  5. Click Preview in the BiW CurveBead Fastener Definition dialog box to preview the curve bead.

  6. Check Swap Start and End Points.

    The Start and End point coordinates are automatically recalculated and new values are displayed within the dialog box, but the curve bead position within the geometry does not change.
    The curvebead is modified with its start and end points recalculated.

  7. Click OK to create the trimmed curve bead.
 
Note that:
  • the selection of the curve must be done within the sub-components of the curve bead's reference product, except when for the Explicit location method.
  • When selecting the curve (except for the Explicit location method), it is recommended to select published elements in order to guaranty associativity between elements.
  • to authorize the selection of only published elements, check the following option using Tools > Options > Infrastructure > Part Infrastructure > General > Only use published elements for external selection keeping links.
  • when the On Support Surface and Explicit methods are activated, the application will ignore the active Part Infrastructure setting Only use published elements for external selection and will enable the usage of non published external geometry.