Recognize a dead solid in CATIA Sheet Metal

https://youtu.be/3C5kTUB88gc

This video is split in 2 parts:
1) Design of the part in CATIA Part Design. (0:14 to 7:22)
2) Recognition of the Dead Solid plate in Sheetmetal. (7:22 to 10:40)

You will see that you can transform a dead solid into a Sheet metal part. The algorithm recognize the manufacturing processed shape, such as bending, boss, hole, etc. You will be able to unfold/fold the part and make a drawing generating the unfolding lines.

  1. Step 1: Video


  2. Step 2: Create a fictional plate

    Create a new Part in Part Design

    Sketch a non closed profile

    Create a solid using the feature Pad with the option "Thick"

    -> use the option neutral fiber and put 2mm in value.

    Add 2mm fillet on the inner corner and 4mm fillter on the outer corner

    * This should look like a sheetmetal plate, but it is only a solid part *

    -

    (optional)

    Continue your design by adding other sketch profile perpendicular to first sketch

    Add holes, bosses, chamfer, etc.

    * Make it similar to a plate AND keep the same thickness all the time AND use fillets 2mm/4mm *

  3. Step 3: Transform the part in a dead solid

    * Now you part looks like a plate, you will transform it to a dead solid *

    Create another part in Part Design (with different name)

    In the first part, right click on the PartBody and select copy

    Switch to the new part, right click on the 3DShape and select "Paste Special"

    A panel appears, select "As Result"

    * You will have a dead solid now *

  4. Step 4: Recognize the sheetmetal

    Keep the part open, but switch to Sheet Metal Design Application

    Click on Sheet Metal Parameters

    • Thickness = 2mm
    • Bend Radius = 4mm (Or if you have a bigger fillet in your part, like in the video R10mm, put the biggest value)

    -

    Click on the Recognize feature

    Select the dead solid

    Select a face that will be the support when part is flatten

    (optional) you can do a manual recognition if the automatic recognition does not allows you to unfold the part

    Click on OK

    * Your part is now consider a a sheet metal part and can be unfolded *

  5. Step 5: Unfolded view in drawing (option)

    Insert a drawing in the 3DPart

    Go to drafting application

    Create normal views (front, side, top)

    Expand the action bar (click on small arrow ">")

    Select the unfold view

    Switch back to the sheet metal part and click on it

    * the view will be generated on the drawing and the bending lines should also appears in the view *


    • End of tutorial

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