You're right, it was already there. Since this operation is not successful in NX11 itself, I tried in NX1847. Then I exported model using File -> Export -> Parasolid. And I imported the same in NX11 for your reference and have attached the part.
I exported Parasolid body from NX1847 and imported in NX11 because if part is saved in NX1847 (higher version), it can not be opened in lower version of NX (here NX11). But you can export geometry/model from higher version to any lower version of Parasolid and import it in lower NX version.
Check File -> Export -> Parasolid option in NX.
Your problem appears to be the version of NX you're using. Based on Part History, you're using NX 11.0.0, which is the base version. The last available maintenance release for this version was NX 11.0.2.
If I recreate the Delete Face feature with your part in NX 11.0.0 (your current version of NX 11) I can reproduce the issue, if I recreate the feature in NX 11.0.2 the topological error cannot be reproduced, but if I save your part and open it in NX 11.0.0 then the error occurs again. Therefore, one must assume the issue is inherent in NX 11.0.0 and fixed in a newer version of NX 11.
The error seems to be related to the Pattern Feature. If I suppress the two Pattern features (which suppresses the child Mirror features) the Delete Face is successful. Therefore, for your CFD study I'd suggest suppressing the Pattern features, create the Delete Face and then use Pattern Face to pattern faces left from the holes. Part file with suggested solution attached.
You should also consider installing the latest NX 11 maintenance release so that you don't continue to encounter this issue.