You should be able to do it, generally the free Eagle license will let you open and view Eagle files that exceed the "free rules", eg. big dimensions or >2 Cu layers. But you just can't modify those files on the internal copper layers or outside the "free dimensions". But I think the CAM processor should still work.
Basically, in Eagle you've got a plethora of different layers, like a couple of hundred different types of layers.
When you physically make a board, you've got maybe 6-10 layers, or so. For example you've got top and bottom copper, top and bottom soldermask, top and bottom silkscreen, internal copper layers if it is a >2 layer board, top and bottom paste stencils, and the drill file.
What you do in the Eagle CAM Processor, to give you a really basic short explanation, is to go through each of the half-dozen or so "physical layers" of your board each of which will correspond to a Gerber file, and create a "map" which specifies which layer(s) of the hundreds of "Eagle internal" layers will "map" onto that physical layer.
For example you might have the "Top", "Pads". and "Vias" layers mapped onto the top copper layer, and the "Bottom", "Pads" and "Vias" layers mapped onto the bottom copper layer, and the "tPlace" layer mapped onto the top silkscreen, although you may add other layers such as tNames or tValues to the top silkscreen layer if you like.
I actually use a makefile to do it for me. But you can do it in the GUI in Eagle's CAM Processor setup.
.PHONY: gerbers
gerbers :
mkdir -p gerbers
mkdir -p temp
for f in `ls *.s#* *.b#* 2> /dev/null`; do mv $$f ./temp/; done
echo "Generating Gerber files..."
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTL $(PROJECT_NAME).brd Top Pads Vias Dimension > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GBL $(PROJECT_NAME).brd Bottom Pads Vias > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTO $(PROJECT_NAME).brd tPlace > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTP $(PROJECT_NAME).brd tCream > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GBO $(PROJECT_NAME).brd bPlace > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GTS $(PROJECT_NAME).brd tStop > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GBS $(PROJECT_NAME).brd bStop > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GML $(PROJECT_NAME).brd Milling > /dev/null
eagle -X -d GERBER_RS274X -o ./gerbers/$(PROJECT_NAME).GKO $(PROJECT_NAME).brd Dimension > /dev/null
eagle -X -d EXCELLON -o ./gerbers/$(PROJECT_NAME).TXT $(PROJECT_NAME).brd Drills Holes > /dev/null
zip $(PROJECT_NAME)-gerbers ./gerbers/*.*
image :
`gerbv --export=png --output=$(PROJECT_NAME)-pcb.png --dpi=$(GERBER_IMAGE_RESOLUTION) --background=#$(BACKGROUND_COLOUR) --f=#$(HOLES_COLOUR) \
gerbers/$(PROJECT_NAME).TXT --f=#$(SILKSCREEN_COLOUR) gerbers/$(PROJECT_NAME).GTO --f=#$(PADS_COLOUR) gerbers/$(PROJECT_NAME).GTS --f=#$(TOP_SOLDERMASK_COLOUR) \
gerbers/$(PROJECT_NAME).GTL --f=#$(BOTTOM_SOLDERMASK_COLOUR) gerbers/$(PROJECT_NAME).GBL &`
echo "Gerber photoplotter files and board preview rendering generated."