I have an IC and it has a big rectangular GND pad in the middle of the IC, I have to drop several via to the GND pad. How I or the board shop can do to prevent the GND via leak to the other PWR planes?
Not sure I'm understanding your term of "Leaking". When the stitching vias are placed with DRP and copper shapes are re-poured there should be no shorting.
If you re-pour the power planes, a relief is made around each via on the power planes.
This relief should be large enough to prevent shorting. The amount of relief is controlled by the via-to-copper or the pad-to-copper clearance you set in your design rules. If you are having PADS remove unused pads on internal layers, it's the via-to-copper clearance you need to worry about. Keep in mind that vias are normally drilled slightly oversize to allow for the plating to bring them back to nominal size. Also, alignment of drilled holes to the copper artwork can't be exact. Also, the drill bit tends to wander slightly off of normal to the board surface. The thicker your board, the more error it can cause. You must allow enough relief around the holes to account for all these errors.
Final_Clearance = Design_Clearance - 1/2 * Drill_Oversize - Drill_Position_Tolerance - Drill_Wander_Tolerance
You only require a couple of mils of final clearance after you've accounted for all the manufacturing tolerances if you are designing for low voltage.
Inquire from your PCB vendor what tolerance they hold on drilled holes or their copper-to-drill clearance. They may specify it as several parameters like I've described it or they may lump them all together. Take the manufacturer's number then add how much additional tolerance you are comfortable with.
If you are not removing unused pads, the important clearance is your pad-to-copper clearance, but you must set your via pad sizes based on the PCB vendor's tolerances to avoid pad breakout.
It would be best to submit a service request for Mentor Support to help out on this issue.
If you can use Blind vias to GND plane ,you will get solid power plane on another planes with other layers.
Thanks and Regards
It's true you can use blind vias and if the ground plane is adjacent to the side on which the part is mounted you avoid vias on all the other internal layers, but you need to make sure you understand the manufacturer's capability and cost for blind vias and how to specify them to the vendor.
Thanks for all the reply to my question.
Retrieving data ...