Dear all,The screen shots shows the ground vias in negative and positive planes of a BGA package. Here some of vias are fully voided due to different net and the antipad of via. But the tool indicates it was connected in negative plane and not connected in positive. I have still doubt that whether it is connected to plane during fabrication in nagetive plane? How can i connect these vias? Is it possible using traces? And which one is best-positive or negative-to set the plane? Seeking correct answer.Thanks,Shiva.
And one more question. What's the differnce between positive and negative plane whether it's power or ground?Thanks.
I feel your better off using positive planes, you can see on the screen what you going to get when you go to gerber / ODB++. The difference between positive plane and negitive plane is in thinking like photographic film. The negitive is the opposite of what the positive (photo) will look like. The signal layers are made as positives.
The isolated connections on negative planes that are formed by the joining of anti-pads was an old problem in Allegro which was corrected some time ago. Basically, a new DRC check was added to check for these island conditions and by default the check is off. Go to Setup > Constraints > Modes and turn on the "Negative plane islands" check so you receive the same results for negative and positive planes.
Hope this helps,
Hello Mike,I have set as you told and got DRC. But my doubt is, how can i connect the seperated or island same net vias? Is it ok as rboquette told, that is set the planes to possitive? In positive planes, it's possible using traces. Please let me know further details.Regards,Shiva.
It is certainly OK to use positive planes instead of negative planes to get the result you are looking for. Negative planes are driven using the anti-pad definition inside of your Via padstacks while positive planes clearances are driven the DRC Clearance to the copper pad by default but you have the option to use the anti-pad to drive positive planes as well.
It most but not all cases the fabrication vendor would like a larger clearance on plane layers to prevent possible plane shorts. This could occur on planes where you have a large mass of copper that tends to shift during processing and also on plated thru hole location which need to be drilled larger to meet the hole size requirements once the holes are plated. I would confirm with the fabrication vendors that you use on what minimum clearance (anti-pad) is required on plane layers and adjust the anti-pad in you padstacks and/or the DRC Clearance to shapes accordingly to avoid any fabrication issues.
You could use positive planes and then add traces to connect all the islands, which would take a lot of your time, but as I said previously it may be in your best interest to consult with your fabrication vendor that your company uses in the hopes that they are OK with reducing the clearance so copper planes can flow the BGA pin fields without being broken up.
Here is a couple images of a small BGA with a slightly modified pin escape to allow the planes to flow to the inner power and ground vias. This can also be a solution to your plane break-up problem you are seeing. It is best to plan ahead during the beginning stages in the design on how you are going to get multiple powers planes connected up. I highlighted GND green and the 4 Powers different colors to illustrate what I have done.