Fusion
You have a great big hole in your cutting surface so some of the solid is not completely contacting the solid body. The Split Body command required that all of the solid but be covered by the cutting surface. I know you want to conform to the shape of the cavity, but the cutting surface must be continuous across the entire body you want to split.
John Hackney, Retired
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Not sure what I am doing wrong.
Easier to tell you how to fix it. Diagnosing - hide the solid bodies.
Surface > Modify > Stitch the surface body. Zoom into the area that has red edges in this preview.
(There should not be any, for the Split Body to work.)
Surface > Modify > Unstitch your cutter.
I deleted the overlapping bodies, 72, 79, and 86., and found some more overlapping after that, so deleted those as well, 12, 13, 15 and 44 (in no particular order). Leaves a neater hole to repair.
I found the black line in Sketch 1, aligns to a point that may have caused all this. It's replaced with a new line to accord with the body I need. Old line is now construction.
Surface > Create > Patch, with chaining option turned OFF, select the new black line in sketch 1, then walk around the opening, near the 3d curves are there are lots of small curves to find in chaining order. After selecting the last edge required the new patch is provided, Press OK.
Surface > Modify > Stitch the cutter.
Modify > Split Body, worked for me, You know the rest...
(I have not chased the yellow sketch icon error, some projections from those deleted bodies will do that.)
Investigate Create > Ruled Surface > normal and / or Tangent edges, to eliminate so many Lofts.
Might help....
Split Body must have the result of creating 2 or more bodies to complete the operation successfully.
Your error message is accurate, it could not find 2 bodies using the cutter you had created.
(My rule of thumb - if Split body fails, the cutter is not large enough)
It is not closing the big hole that is the requirement. If the cutter can overlap, inside and outside, it will work.
You can cut the torus with a cutter that is not a disc, as long as the result gives 2 bodies for the result.
In the first example, the Split body fail, is likely due to Fusion's requirement for accuracy.
Stitching to a watertight shape, fixed the problem, most likely the small stitching / joining seam, closed the problem area.
In this latest (3rd) example you did have the required accuracy, so I presume the geometry did allow for a clean cut, without filling the hole.
Might help....
Interesting...
I narrowed down to 2 errors being seen by Fusion, by sliding the cut planes to eliminate the good areas, these 2 blocks are as small as I could get them without error.
Something makes the split body fail for these 2 blocks. Likely the original part body shape. Sliver faces or undercut is likely.
I suspect these 2 areas, as the original part is starting to cut slots into the bottom mold half.
I have not gone further with a draft analysis
Might help...
Undercuts are here, and or near it, I figure but not sure, your cutter body does not CUT in these regions to see two distinct bodies.
And this lower edge (in the larger error block) is not a cutting face, just a common edge between the cutter body, two mold pieces and the part, four bodies all meeting on this edge.
Might help.....
