Lofted cut 3d sketch problem


I made the model is SW2016, so uploading the result will not help you since your model was made in SW2014.
I would use a sweep for this though.
I'll attach some photos:

  1. Step 1:

    On the right plane, create a simple two line sketch. Use the Pierce command to attach one end point to your Sketch 6, and another to connect to Sketch 7. The vertical portion of the sketch just extends beyond your model to avoid zero thickness errors.

  2. Step 2:

    Create a Surface sweep. The profile is the sketch you just made above. The path is Sketch 6, The guide curve is sketch 7.

  3. Step 3:

    Hide the solid body, or isolate the surface body.

  4. Step 4:

    Use the Fill Surface, Planar Surface, or Boundary Surface tool to fill in the bottom of the surface. I like Fill since it has an option to automatically merge the surfaces together.

  5. Step 5:

    Do a cut with the surface to remove the unwanted material.

  6. Step 6:

    All done

  7. Step 7:

    Now for the funny part: Pressing CTRL +Q (forced rebuild shortcut) results in the surface cut failing due to zero thickness geometry. So let's add a few more steps to fix it once and for all.

  8. Step 8:

    Delete the surface cut feature, and show the surface body if it is hidden.

  9. Step 9:

    Use the fill command to close the top of the surface body. Since it will not be a completely closed body let's use the Create Solid option as well.

  10. Step 10:

    There are a few ways to do this step but Combine is a good option. Just use the Subtract option. The main body is the Pen, and the Body to combine is the new solid we just made.
    Using combine will end up deleting the body used to make the cut. If you wanted to keep it for some reason, the Indent command would have been a better option.


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