Your written english is certainly fine, I suspect some of your problem may be that we tend to use North American slang and concepts that don't translate well (or at least so I was told by a translator who had to translate a technical presentation I gave in South America some years ago). So if you don't understand, just tell us so and get us to try to explain more clearly. That said your latest one is pretty good, only a couple of issues in the pcb svg:
1) There isn't a silkscreen group and copper1 is below what should be the silkscreen group. To fix that you need to select copper1 in the xml editor (I'm assuming Inkscape here!) and click unindent node on the xml editor tool bar twice to move copper1 in to group g7 (copper0 is correctly below copper1 so it will be fine when copper1 is moved). Now you need to add a silkscreen group by changing the id of group g9 to silkscreen (again with xml editor). Now we have a silkscreen group with two paths (board and contour) and in theory we should be fine, however when I look at the pcb view in fritzing only 3 sides of the board outline appear (the forth is missing) and exporting the gerber and checking it with gerbv shows the same on the gerber, thus the silkscreen isn't correct (or there is a fritzing bug). I tried replacing the path (because I haven't figured out how to modify a path in Inkscape 
) with a rectangle but the result is the same in Fritzing (only three sides to the board outline in pcb view) but it is correct in the gerber output (and thus would be fine on the board). I think this must be a Fritzing bug (or I'm just doing it wrong as I rarely make pcbs). However the solution that works (because it does in other pcbs) is to use 4 lines to replace the outline in silkscreen. That appears correctly in both Fritzing and the gerber and is what I have done here. Note the line ends are square and offset .005 (half the stroke width of 10 which is .01) as that seems to be what fritzing wants to do the right thing on the gerber. Note you may need to adjust the length of the lines in silkscreen to match the outline of the real board, as I used the lengths in the board path which may not be correct. Last but not least I adjusted the pad and hole size to be standard. At present they are .036 in and standard drill sizes are .035 (IC leads) and .038 (.1 header pins). Since it is most likely you will want (or at least want the option of) using .1 header pins I increased the pad size to make the holes .038. In theory in Inkscape the way to do this for circle pad is:
hole size = pad diameter - stroke-width*2
or
hole size = pad radius - stroke-width
(both these values are available in xml editor making them easy to find). However in this case I can't figure out what units Inkscape is using in xml editor (if anyone knows, please tell me!). None of mm, in, or px work out, so I cheated and did a copy/paste of one circular pad from a .1 connector from another pcb svg and pasted it in to our pcb svg. I then moved it in to copper0 (by indent node a couple of times) and copied its radius and stroke width values (r 2.0880001 stroke-width:1.44000006) from xml editor in whatever units Inkscape is using here before deleting it. Then in xml editor I changed the size of all the circles to those two values (and changed the id of circle14551 to connector57pad as connector57pad is currently the rectangle rather than the circle, Fritzing appears to correctly select the circle to set the hole size, but this change is more correct). Then I increased the size (by dragging the edges) of the rectangles till they again cover the circular pad and we are done. So create a sketch with the new part and add some connectors for testing and route all three views then save it. Now in pcb view select file->export->for production->extended gerber and produce the gerbers. First we use notepad (or any editor) to verify our hole size by editing Untitled Sketch_drill.txt which gets:
; NON-PLATED HOLES START AT T1
; THROUGH (PLATED) HOLES START AT T100
M48
INCH
T100C0.038000
%
T100
X019875Y018362
X009898Y007486
...
X016889Y018333
From which we see all of our holes are plated through (as desired) and set to .038 diameter. (the T100C0.038000 line which indicates the drill label is T100 and size is .038 inches as we wanted). Now using gerbv (or any other gerber viewer) to open the files
Untitled Sketch_copperBottom.gbl
Untitled Sketch_copperTop.gtl
Untitled Sketch_silkTop.gto
Untitled Sketch_drill.txt
which gets us the bottom/ top/ top silkscreen / drill layers and we see that there are pads with appropriate holes and traces matching what we saw in pcb view in fritzing ready to be shipped to a pcb house and cut to a pcb. I also see I'm a little to close on silkscreen between the board outline and the square pads on the top. Note the small indent in the board outline on the top two square pads. That probably means the top line on silkscreen needs to move up a bit. But over all you should now be away and ready to make more good parts . Nice job you have caught on much faster than I did. The modified part can be exported from the temp parts bin in the fzz file below.
RDM6300_1.fzz (29.6 KB)
Peter