CC2520 hardware design

You could get the measurements, but they would not be very useful to you since you would not only need to duplicate the measurements of the transmission lines, but also the relative placement of the RF components on the board to achieve the same RF characteristics on your board as the reference design uses.

The easiest way to ensure that your board will likely have the same RF performance as the CC2520 evaluation board is to copy every physical and electrical aspect of the RF and chip power supply/decoupling design from the CC2520 reference design.

They do provide the PCB layer1 and layer2 copper layouts in both gerber and PDF formats, and layer1 in DXF format also.  I have successfully opened all of the three types of the files, so it is possible to do that as a first step to copy the trace / component position data into your own PCB's design.

Here is a list of some free gerber viewer programs:

http://en.wikipedia.org/wiki/Gerber_File#External_links

Also under LINUX you can run either or both of the free 'gerbv' or 'gerbview' programs to view the gerber files if that is an easy option for you.

I can tell you from the gerber files that the transmission lines are formed with an 0.008 inch diameter trace and gerber aperture, but since they are not drawn as straight lines it is complicated to describe the route / length of them, and you should really just find a way to copy the gerber data into your own PCB's CAD program by some combination of manual and automated processes as a guide to positioning the traces and components.

I do not suggest making any assumptions about the line parameters, or that you can just change the position and shape of the electrical layout in the RF section.  Your guesses may be quite reasonable as to what will work, but unless you have the test equipment to analyze the RF performance of the resulting board, and the patience / funds to make several iterations of the board in case the performance of some of your design attempts isn't as desired, you would be well served to copy what TI says is a known working design.

From the DXF data I can tell:

TL1: 0.008 inch wide / less than 0.119 inch long

TL2: 0.008 inch wide / less than 0.166 inch long

TL3: 0.008 inch wide / less than 0.147 inch long

When I say "less than", I mean that there are several areas where the gerber data for the aperture line segments composing the trace overlap to provide smooth electrical and geometric continuity with the neighboring copper areas they connect to, and the overlapping areas is counted as part of the length of the line in the DXF segment series, but of course that is counting the length of the overlapping areas twice, so the real length is less than the stated value.

From looking quickly and not so carefully at the gerber data, for instance, I would estimate the exposed copper length of the 8 mil wide TL3 trace is more like 0.127 inch rather than the 0.147 inch value from the DXF data which apparently includes nearly 0.02 inches of overlapping copper from the difference in these observations.

So anyway there are the aproximate dimensions of the lines, but without also preserving their shapes and the physical placement of the other RF / power supply traces, I suspect you could end up with different RF performance than the actual reference design has.

Perhaps someone from TI can quote the design target impedance values and more accurate electrical lengths of the lines for better information on the proper layout?