first watch this video

and the other ones in that series, if you havn't already watched them.

Also, you should read the SketchUcam Tools help so you understand each of the tools available. Knowing the tools makes it much easier to come up with a plan to achieve what you want.

How I would do that shape is in 3 parts.
first cut will remove all the waste around the islands and off the edge of the part a little, but leave a little material to be cleaned up.
second cut will cut the islands precisely.
third cut will cut around the outside.

I recently did exactly this sequence on a seat adjuster knob for my car and it worked perfectly.

So, attached find an example sketchup file, sample.skp. I just guessed dimensions, and assumed a material thickness of 20mm.
The 'platform' around the edge is 5mm. The bit I chose is 6mm. I enlarged the islands by 1mm to leave a little for cleanup, and the outline of the part by 3.5mm to ensure that it gets cut all the way to the edge. (just in the left most drawing, for the pockets!)
You can see that I added some lines to split up the area to be pocketed in such a way as to avoid sharp internal corners, the offset routines struggle with sharp internal corners (and the built in Sketchup one is worse than the one in SketchUcam).

Note that for complicated pockets, a smaller setover% is easier to work with than the 70% I used here.

So I set the pockets to be 100% deep, and set the material thickness to 15mm, then generate
Gcode for the first cut, which I saved to a file sample1.nc
The image below shows the material after the pocket cuts.


The second cuts are outside cuts around the islands, in the second drawing. Move the safe area to the second drawing registration point, set material thickness to 15mm, set overcut% to 100, and generate Gcode to sample2.nc
The image below shows the results of the island cleanup cuts.

Finally the 3rd drawing shows an outside cut with tabs. Here you have to set the material thickness to 20mm and your choice of overcut%, I used 101% to ensure it cuts through in the simulator but you can use 100% to avoid cutting your baseboard.
Notice I could have made the tabs thinner, say I wanted 2.5mm, that is 12.5% of material thickness, in the drawing they are 50%.
Move the safe area to the third drawing registration point, Generate Gcode to sample3.nc
Image below shows the end of this final cut.


Having generated 3 files, I used the joiner tool to join them together in order, and the result is the file sample.nc attached below.

Hope this helps....

 

much smaller! (-:
a few things to change.....

there are some vertices that are not 'flat' but because the item is so small the usual methods of flattening do not work (sketchup works internally to 0.001 inch no matter what units you select).
I selected the entire drawing and scaled it up by 10, flattened (select lines, right click, phlatboyz,phlatten) the leftmost drawing, then scaled back down by 0.1.
This enables the pocket tool to do a better job.

in that left hand drawing you did not expand the islands a little, nor the main outline by at least bitdiam/2.
expanding the islands is not critical, but expanding the main outline is needed to prevent pips on the final part. the bit has to overlap the cutline that the final outside cut will follow. look again at my images of the cut progress to see the pips that have to be cut off by the final pass.
I expanded the islands by 0.15mm so that the pocket outline (hold down CTRL for only the outline) could go between the islands without touching itself. weird stuff happens when cutlines cross!

in the second drawing, the top island did not generate Gcode because it too, was not flat enough to create a face between the island and the cutline. that face must exist.

corrected drawing attached

btw, does your CNC controller obey the feed rates in the Gcode? if so, 2450mm/min may be a little fast (-: