How to design free spline Stiffening Ribs on metal sheet

If your pattern is very complex, model the negative as a solid, and save it as a forming tool. Open a new sheet metal part, make a plate, then insert the forming tool to "stamp" the plate. The most time-consuming part in this process will be drawing your forming tool, based on its' complexity. If you can provide me an example of your design, I can show you the process in screenshots.

*UPDATE* Here is the process, including two files as examples attached:

1. Create the "negative" of your part.
2. Go to the sheet metal tab and select "Forming Tool".
3. Under the "Stopping Face" field, select the face that will come flush with the flat face of your sheet metal. If you add "Faces to Remove" this will cut holes in your sheet metal, so leave this blank if this is not your intention.
4. Go to the "Insertion Point" tab and move the point to where you want your forming tool to be located with.
5. Complete the feature. You should see the part color coded, cyan for stopping face, yellow for stamping faces, and red for removed faces.
6. Save this part in your SolidWorks directory where forming tools are stored (this part is important, otherwise SolidWorks will not recognize your part as a forming tool): C:\ProgramData\SolidWorks\SOLIDWORKS 2020\Design Library\forming tools

7. Start a new sheet metal part. Extrude a flat sheet with a thickness less than the minimum bend radius.
8. Open your design library tab on the right of your screen and navigate to your forming tools folder.
9. Click and drag your forming tool onto the surface you wish to stamp.
10. Go to the "Position" tab to accurately locate your tool onto the face of your sheet metal.
11. Finish the feature and your stamping should be complete.

NOTE: If you intend to make any changes to this part, you must edit the forming tool, then recreate the stamping on your sheet metal part.

Attached: Part1 is the stamped part, Part2 is the forming tool.