The model could not be sectioned correctly by the cut line.
Please verify that the cut line passes through the model or components.
The components that fail in the cut are:
55200 Name Part...
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The assembly is OK, no mistake in the constraints, the cut line goes through the model. In the clipped view, the part affected by the message is hidden. When the part is deleted, the cut is OK. But need the room for other detail views.
If @glaffont's solution doesn't work, there may be another reason.
When you do something about the solidworks MEP, you must have already noticed that it selects the view where to hang the annotation/sketch/detail/etc. This is noticeable by a dotted frame around the view.
With the sectional views, he sometimes selects another view (the right, top, etc.). And suddenly, the cutting line points into the void.
The simplest way would then be to select your starting view before anything else and then to do your section view afterwards
It's also possible that the cut line has a stress that has disappeared with a change or whatever.
Can you check by right-clicking on the cut line.
In the drop-down menu "edit cut line" or "edit sketch"
You left-click on your cut line
In the sketch tab, tap "View/Delete Relationships"
When the menu appears on the left, in the "relationships" box, you open the drop-down menu and go back to everything in this sketch.
From there, it will make you see all the relationships, if there are any in green, they are the ones that are wobbly and that generate a problem for you.
I will start from the principle of "erasing everything" and if necessary to recreate it do it later.
When you're done you come out of sketch mode with a "Ctrl+Q" and logically, it's no longer a problem.
On the other hand, the cut line must cross the entire volume body, otherwise check the box for section section or partial section in the options of your section view.
Coincidence: I have just been confronted with the same problem. The impacted component was surfaced, imported from a step and several of its faces had an error.
The repair of the errors with the import diagnosis made it possible to solve the problem.
I'll just add that if the part that causes the problem is from an import and even if no sign of error appears on the import functions, still make an import diagnosis: defects may still be present.
If the cut works well when the problematic part is removed, one solution is to make a configuration in the assembly without that part. Then in the drawing, take this configuration to make the cut and keep the default configuration for the other views that require this part.