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I'm not sure if you can do such thing. Maybe at the drawing level there are more options.
I would suggest you to create an incomplete rib after you already sectioned the part. Not quite helpful I know, but it is a solution.
For representing gear teeth and splines, (similar issue), we include a thin cut where a tooth lies on the section plane. For internal splines this is typically all I model, to keep the view 'clean' - no actual tooth representation.
Of course, you should structure your model tree so that you can easily suppress such features if you want to do FEA; and if you choose not to model gear teeth then the mass calculation will be less accurate. But it's a good solution for drawings.
Not possible unless you mess with the model. In that case both Ruben's and Jonathan's suggestions would work.
For Ruben's, the section skips non-solidified surfaces.
For Jonathan's, that super-thin cut separating the rib from the model creates a separation in the cross-hatching. From there you can switch to X-Area (in the modify x-hatching menu), toggle to the rib x-hatching then erase the x-hatching.
there ia an old trick to worj this problem around
http://www.synthx.com/tom/sy_tip_9804.htm
http://www.mcadcentral.com/creo-drawing/15959-omitting-secti-n-lines-n-ribs.html
ANother way is to create the section in the part and add it to the desired drawing view, in the drawing view erase them hatch, create a boundary for the desired hatch area on the view ( you'll also want to set the associate to view setting for the sketch geometry, and hatch the area. Gives more control over spacing and angle than just using a sketch in part mode.