Copy paste of the conversation i had with the manufacturer:
1) If you run a DRC check on your board, you will see it has 371 errors. These are fairly serious. Several are due to insufficient clearance between pads of the Wiznet chip. We recommend:
a) You shrink the pads of the Wiznet chip by 0.5mil (0.01mm) on each side (0.02mm total) so that from pad-to-pad there is at least 6mil (0.16mm) spacing between the pads. Then, you can set the DRC clearance parameters to 6mil. That will make your board slightly cheaper to fabricate.
You can leave the Wiznet chip as it is but you will need to specify 5mil clearances when making the PCB, which will make it cost a bit more.
b) In the Net Classes (under the Edit menu) you have 6mil clearances and hole sizes set for different net classes. If you do not need these, set these to 0 else they interfere with the regular DRC.
c) Set the minimum drill diameter in the DRC to 15mil (0.381mm) for lowest cost. Looking at the density of your board it doesn't seem to need the 8mil drills you currently have specified.
I just have one doubt, i have tried to lower the clearances to 3 mil for example, but still the errors don´t disappear, do you have any idea why this happens?
It is the net classes I mentioned in the last e-mail. Go to the Edit-->Net Classes menu. The settings there override the DRC.
And it worked