4 layer PCB: third layer?! - RF Cafe Forums
Because of the high maintenance needed to monitor and filter spammers from the RF Cafe Forums, I decided that it would be best to just archive the pages to make all the good information posted in the past available for review. It is unfortunate that the scumbags of the world ruin an otherwise useful venue for people wanting to exchanged useful ideas and views. It seems that the more formal social media like Facebook pretty much dominate this kind of venue anymore anyway, so if you would like to post something on RF Cafe's Facebook page, please do.
Below are all of the forum threads, including all the responses to the original posts.
Post subject: 4 layer PCB: third layer?! Posted: Thu Jan 10, 2008 4:40 am
Joined: Thu Jan 10, 2008 4:05 am
I´m new to this forum and I hope you can help me with my question.
Acutally I´m desinging a rf-board with a 2.4ghz transceiver. I found some application notes from different suppliers and I found some differences regarding the layer build up of a four-layer-pcb:
- The first and fourth layer are almost everytime used for routing with covering copper (connected to ground) at the remaining space.
- The second layer is complete ground.
- Regarding the third layer I found a difference: One company suggests that the third layer is used for power routing and covering the remaining space with copper connected to ground. Another suggestion is to add a complete copper-area connected to VCC.
Are there any experiences that you can share with me/us? Should one of the options should be prefered (why?)?
Post subject: Posted: Thu Jan 10, 2008 3:03 pm
Joined: Thu Sep 25, 2003 1:19 am
I've always been told to route layer 3 with power and pour the remaining area with copper ground. ( for RF boards )
Post subject: Posted: Wed Jan 30, 2008 5:38 pm
Joined: Wed May 16, 2007 4:16 pm
In the past, I would make the first inner layer a ground plane and the second layer a power plane. I do it different now, and I think that the new way is better.
On the first inner layer, I create small power planes under the RF chips. If I need to expand them a little to cover the bias inductors, I will. Then I connect these separate planes using 40 mil traces to a single trace outside of the RF area that provides power. This distributed power method ensures that I am able to isolate power supplies at RF to eliminate problems with spurious radiation, unwanted oscillation, tec.
The important part is to leave the area under the discrete components open for the most part on the first inner layer. The only other thing I would do on that layer is to put a small ground plane under the RF switch if there is one.
Then, on the second inner layer (or layer 3 as you call it), put a solid ground plane under all of the RF circuitry. Stitch it to the top layer ground connections liberally with vias. Then, on the bottom layer, pour a ground plane under the RF section so that it fills all of the area not occupied by other traces.
So why put the ground plane on layer 3 instead of 2, which is the common wisdom today? Well, the answer is parasitic capacitance. The layer stackup used by different board manufacturers varies widely from one to another. So the gap between the top layer and the layer 2 can be smaller than you intend. If it is too small, you will get unwanted capacitance to that big ground plane which will make tuning your TX and RX paths a pain. You can of course try to specify the buildup and hope your manufacturer complies. But as things continually move to China, you are dealing with an unknown there.
So I say why leave it to chance. By moving the ground plane to the 3rd layer, you ensure that parasitc capacitance for any common layer stackup won't be a problem. Your circuits will be easier to tune and will work better, and you will have less problems moving your product to China for manufacturing.
More than 10,000 searchable pages indexed.