Tutorial: How to convert a .Step-File to an independent .CatPart-File in Catia V5

This Tutorial shows you how to convert a .stp-file (dead solid) to an independent .catpart-file (iso-constrained) in Catia V5.
Using project/intersect 3D-Elements.

  1. Step 1:

    -Open a new .CatPart-file in Catia
    -Open the .stp-file you want to convert
    -Copy the dead solid of the the .stp-file

  2. Step 2:

    -Paste the dead solid in your new .CatPart-file
    (right click --> paste special --> as result)
    -Close the .stp-file

  3. Step 3:

    -Change the color of the dead solid
    (right click --> properties --> graphic --> color)

  4. Step 4:

    -Add a sketch on your CatPart and intersect the dead solid.
    (insert --> operation --> 3D geometry --> Intersect 3D elements)
    *Sketch support need to be a midplane of the dead solid*

  5. Step 5:

    -Open the sketch analysis tool
    -Switch to "Use-edges" tab
    -Select the intersected geometry and isolate it

    *You can also isolate the geometry by selecting it --> right click --> selected objects --> isolate*

  6. Step 6:

    -Get your sketch iso-constrained

    (You can use the "Sketch solving status tool" to check if your sketch is iso-constrained or under constrained)

  7. Step 7:

    -Create a shaft of your sketch

  8. Step 8:

    -Add a second sketch on top of the screw and select the lines of the screw head
    -Project the Lines from the dead solid into your sketch
    (insert --> operation --> 3D geometry --> project 3D elements)

    *Make sure to isolate the projected geometry prior you leave the sketch*

  9. Step 9:

    -Create a pocket of your sketch

  10. Step 10:

    The blue and grey shimmering surfaces are a sign that you have done all right.
    If you are not sure - switch the render style to "wireframe"
    (view --> render style --> wireframe)

    Now you can delete the dead solid and the work is done.