Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

How to decide how many layers you need in PCB application?

Status
Not open for further replies.

g_iftah

Junior Member level 3
Joined
Sep 26, 2004
Messages
28
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
Israel
Activity points
235
PCB layers

hi...evry one......

does any one know how do you decid how many layers you need in an application.

lets say for start that it has anlog and digital parts....
 

binu G

Advanced Member level 2
Joined
Jan 9, 2003
Messages
501
Helped
12
Reputation
24
Reaction score
3
Trophy points
1,298
Location
Bangalore
Activity points
3,780
PCB layers

if there are multiple voltages then how the layer stack up is designed.
how the ground layers are distrubited in this case.

binu g
 

g_iftah

Junior Member level 3
Joined
Sep 26, 2004
Messages
28
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Location
Israel
Activity points
235
Re: PCB layers

i am sorry didnt quit anderstand you....

i have 5V input and 3.3 after converter and regolator+
i have anlog part sach as codec and microfone + bluetooth baseband controler+digital cpu.....

i am thinking somting like 5 layers am i rigth or can you make less??
 

binu G

Advanced Member level 2
Joined
Jan 9, 2003
Messages
501
Helped
12
Reputation
24
Reaction score
3
Trophy points
1,298
Location
Bangalore
Activity points
3,780
Re: PCB layers

g_iftah

Normally the layer stackup is even number.

Binu G
 

House_Cat

Advanced Member level 4
Joined
Feb 21, 2002
Messages
1,371
Helped
406
Reputation
812
Reaction score
98
Trophy points
1,328
Location
USA
Activity points
16,416
Re: PCB layers

does any one know how do you decid how many layers you need in an application.

lets say for start that it has anlog and digital parts....


You decide how many layers you need depending on what you are trying to do with the circuit. You might need only a single sided board for a simple project, or you might need 4, 6, 8, 10, etc. layers for more complex circuitry.

The number of signal layers and the number of planes are each used in symetric pairs in a multilayer board. For multilayer boards, in general, you typically would have a ground plane, and a power plane. The power plane can be split to supply more than one voltage. These two plane layers would typically be in the center of your stackup.

The next layers out from the center would be signal layers. Critical signals would be run on the layer adjacent to the continuous ground plane - the trace width and the distance between the signal layer and plane would be chosen to give you the desired impedance for the signal traces. Less critical signals such as display traces, relay control, etc. could be on the layer adjacent to the power plane layer.

Analog and digital traces would be laid out such that they are separated physically, and do not share any areas of the adajcent plane. The reason for this is to avoid having shared signal return paths which could couple noise from digital to analog circuitry. Try to visualize each signal path as a complete loop consisting of the trace on the signal layer, and the return part of the loop through the adjacent copper on the plane.

Additional planes, and signal layers, would be added in pairs as needed to accomplish the desired routing.

There is no cookbook answer - you use your engineering knowledge to figure out what will give you the best results for your project - signal by signal.
 

    g_iftah

    Points: 2
    Helpful Answer Positive Rating

cube007

Full Member level 6
Joined
Mar 12, 2002
Messages
386
Helped
16
Reputation
32
Reaction score
5
Trophy points
1,298
Location
Australia
Activity points
3,477
PCB layers

The number of layer depends on different things: Speed of the signals, device packages, space for placing the devices. For example if you are using a BGA you will need at least 4 to 6 layers. The less space you have for placing your devices the more layers are needed. For digital high speed designs you will need proper power planes.
 

yangvic

Member level 2
Joined
Jun 24, 2004
Messages
50
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
323
PCB layers

You can refer your main chipset's application note.Sometimes it will discuss this.
 

tennad

Junior Member level 1
Joined
Mar 15, 2003
Messages
15
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Activity points
122
PCB layers

A table you can refer to
pin_density signal_layer PCB layer
>1.0 2 2
0.6-1.0 2 4
0.4-0.6 4 6
0.3-0.4 4 8
0.2-0.3 6 10
<0.2 8 >14

PCB density = PCB square(sq inch)/(pin sum./14)
 

amjad

Full Member level 5
Joined
Dec 29, 2002
Messages
274
Helped
9
Reputation
18
Reaction score
5
Trophy points
1,298
Activity points
2,291
Re: PCB layers

Number of layers depends on how much design complexity is the circuit, and how much signal layers required to complete the routing of nets and number of planes for power and gnd separations irrespective of the board area required for laying the component placement .

Also board thickness is considered before deciding the number of layers that the thickness can accomadate .
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top