Designing PCB for fast data
When the difference is 290mm and the frequency is 30Mhz, do I need to worry about one signal reaching before the other?
  Is there a rule of thumb or a way to calculate what is the maximum difference in distances that is allowed for a specific signal frequency?
  


The propagation velocity is given roughly by the dielectric constant of the material of your pcb

$$ v \approx \frac{c}{\sqrt{\epsilon_r}}$$

(Actually it will be a bit higher because some of the signal travels in air rather than in the PCB)

For FR4, \$\epsilon_r\$ is roughly 4.5 (+/- 0.5). For flex material, you'll need to check the datasheet of your material.

The difference in time-of-arrival is just the difference in trace length divided by the velocity. 

And the rule-of-thumb in a digital design is that you need to satisfy the set-up and hold times for all the logic you are sending signals to. In some cases, you may also need to keep your clocks in sync between the different load components, but that is a design-specific requirement.


  Should the trace be thicker or thinner for fast data? will 8mil do?


For 30 MHz with a maximum trace length of 300 mm, the trace width is not critical. 

P.S.

For this design, if you don't have any special syncronization requirements, I'd rather minimize the total capacitance of the trace by running a single track that goes near all 7 loads, and make a short stub to each load, rather than have very long stubs leading to the loads from the point of origin.

P.P.S.

Your wavelength and trace length are in the realm of needing to worry about radiated emissions if you are planning to use or sell this in the US or Europe. Make sure you have a well-defined return path for each signal path, and remember the critical distances for EMI purposes are more realted to the signal's rise and fall times than on the repetition frequency.