My PCB vendor informed me today that a silk screen feature that is carried over into the copper layers, lands on traces and causes shorts (yellow box on the right).
Your problem might be in your output job Gerber configuration and your (and Samtec's) selection of mechanical layer.
If you drew the board outline on a particular mechanical layer and the Samtec library happened to use that same mechanical layer for the (non-overlay) outline of the connector you could have a problem iff you selected "Add to All Plots" for that layer in order to have the outline shown on each layer. Just because it's shown on the overlay layer does not mean it is not duplicated on another layer (and it may show up in Altium as overlay color or mechanical layer color depending on the which layer is on top at the moment).
In such a case you can move your outline to another layer and regenerate the Gerbers with the "Add to All Plots" tick removed from the previous layer and turned on for the new layer.
Alway inspect your Gerber files in Camtastic or some other Gerber viewing program, you can save a lot of time and irritation.
It is a problem, since the process does not know when creating that mask that it is silkscreen and not copper. He is telling you that yellow line ends up being a trace.
The connector model's silk-screen geometry must have been mistakenly placed on the copper layer instead of the silk-screen layer. Edit the model geometry.
Note, whatever U5 is, also has a problem, though you got lucky in this case in that it does not interferes with any of the surrounding traces.
The quickest (not necessarily the best) way to fix this problem is by modifying the actual layout. To do this, double click on the component causing the problem, then uncheck the "Lock Primitives" box. You can now 1) select the problem line or box, 2) right click and select properties, then 3) change the element to another layer. Or you could just delete it.