Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic 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.

Register Log in

How to decide of number of layers

Status
Not open for further replies.

arm_learner

Member level 2
Joined
Jan 6, 2004
Messages
42
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
322
Could anyone tell me how to decide the number of layers?

:)
 

flatulent

Advanced Member level 5
Joined
Jul 19, 2002
Messages
4,629
Helped
489
Reputation
980
Reaction score
150
Trophy points
1,343
Location
Middle Earth
Activity points
46,689
For low frequencies two will work. For higher frequencies four is the minimum to pass EMI tests. From there it is the number of interconnects. Once you get into the ECL range and use differential pairs, you put them on inner layers between two ground planes.
 

gam

Advanced Member level 4
Joined
Mar 25, 2004
Messages
115
Helped
8
Reputation
16
Reaction score
4
Trophy points
1,298
Activity points
1,158
It really depende on the application, the cost restriction and complexity involved and of course the frequency wether it is Analog or Digital or mixed circuit.

If you specify more maybe we can help with suggestions
 

arm_learner

Member level 2
Joined
Jan 6, 2004
Messages
42
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,288
Activity points
322
gam said:
It really depende on the application, the cost restriction and complexity involved and of course the frequency wether it is Analog or Digital or mixed circuit.

If you specify more maybe we can help with suggestions
My PCB is for 200MHz and digital circuit only.
Thankz~~
 

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
3,782
for 200MHz u should go for atleast 4 layer, and may add up depending upon the net density.
 

mrcube_ns

Advanced Member level 1
Joined
Apr 10, 2002
Messages
452
Helped
48
Reputation
96
Reaction score
34
Trophy points
1,308
Location
Europe
Activity points
3,814
Contact firms who will make your PCBs and ask them how many layers they can make so thats max num of layers which you can apply.

In my country its 2 layers max.


Mr.Cube
 

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
3,782
mrcube_ns said:
Contact firms who will make your PCBs and ask them how many layers they can make so thats max num of layers which you can apply.

In my country its 2 layers max.


Mr.Cube
8O only two layers. so how u do highspeed design ckts

binu g
 

EEHardware

Advanced Member level 4
Joined
Apr 1, 2004
Messages
105
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,296
Activity points
719
signal speed, ref layers need, and crosstalk... etc.
 

ouli1

Newbie level 3
Joined
May 11, 2004
Messages
3
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
10
I guess it's tightly depend on your voltage levels used.
If the most of voltage levels are the same one, you can use 4layers.
And if you need wire a lot of transmission lines to compensate impedence, maybe you need 6 layers. You can try and error.
Good Luck.
 

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
16,422
The number of layers in a circuit board are determined by:

1. Are you going to control impedance? If so, then you need a continuous reference plane adjacent to the controlled impedance signal layer.
2. The number of layers should be even, and the core and prepreg dielectric thicknesses should be balanced. Odd number of layers, or unbalances thicknesses, in a stackup generally result in warping and/or cupping in the finished board.
3. Are there critical traces that need to be isolated from other signals? If so, you may need to dedicate a layer to them.
4. Are there multiple power supplies? If so, you may want to include a split power plane to distribute the power. The split plane should be adjacent to a continuous ground reference plane. High speed/critical signal traces should not be adjacent to the splits, because the return path will be interrupted.
5. Will the frequencies used tend to radiate from the board? If so, you may need to flood the outside layers with grounded copper. The signal layers would then be internal, and you would still need to consider 1-4 above.

As you can see, there is no cookbook answer - it depends on what you are trying to do (this is also called "engineering").
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top