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

PCB Differential Pairs Impedance

Status
Not open for further replies.

kotshe

Junior Member level 3
Joined
Mar 18, 2008
Messages
30
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,503
Hi All ,

I'm trying to set Differential Pairs Impedance at 90 Ohm's For standard PCB FR4 of two layers , i'm trying to use Saturn PCB design , what I can't understand what is conductor Height .

I have

Base copper Weight = 18um
Plating thickness = 18um
Er = 4.6

But I cant understand what conductor Height is ?

Any help please
 

robertferanec

Member level 1
Joined
Jun 15, 2011
Messages
37
Helped
17
Reputation
34
Reaction score
17
Trophy points
1,288
Activity points
1,481
To calculate geometry for 90OHMs Differential pairs routed on 2 layer PCB (Differential impedance of Microstrips) you need to know: width of the traces, space (gap) between the traces, height of dielectric above return plane, trace thickness and relative permittivity of the dielectric. There are plenty Impedance calculators available, but I would recommend you to ask your PCB manufacturer. Your calculated track geometry may differenciate from the numbers provided by your PCB manufacuter.
 

kotshe

Junior Member level 3
Joined
Mar 18, 2008
Messages
30
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,503
FvM : I don't know if thats the sum of Weight and thickness , thats what i'm asking for ?

robertferanec :I'm asking with small PCB manufacturer , they are not helpful : they don't know what i'm asking for
 

androm

Junior Member level 2
Joined
Jun 6, 2011
Messages
24
Helped
5
Reputation
10
Reaction score
5
Trophy points
1,283
Activity points
1,419
I can be missing here something but is that possible to achieve a proper differential pair routing without a permanent return current plane? Don't you guys think the board should be at least 4-layer for microstrip case?
 

robertferanec

Member level 1
Joined
Jun 15, 2011
Messages
37
Helped
17
Reputation
34
Reaction score
17
Trophy points
1,288
Activity points
1,481
I agree androm, but maybe it is just a small breakout board with usb on the top and gnd on the bottom.
 

kotshe

Junior Member level 3
Joined
Mar 18, 2008
Messages
30
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,503
Robertferanec : could you please explain "height of dielectric above return plane" ? you don't mean width of PCB which is almost 1.6mm for standard PCB ? right ?
 

robertferanec

Member level 1
Joined
Jun 15, 2011
Messages
37
Helped
17
Reputation
34
Reaction score
17
Trophy points
1,288
Activity points
1,481
kotshe: you are right - 1.6mm. I don't use 2 layer PCB for impedance controlled tracks (minimum 4 layers as mentioned by androm). I was actually curious what the track geometry would be like for 1.6mm pcb and I did try to put some numbers here: PCB Calculator The results: width 2.5mm / gap 1.6mm :) (Zo = 55OHMs, Zdiff = 90OHMs)
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,489
Helped
14,050
Reputation
28,355
Reaction score
12,708
Trophy points
1,393
Location
Bochum, Germany
Activity points
276,162
You got a lot of answers to questions you actually didn't ask for. :smile: (although some of these questions may be relevant for your application as well)

Conductor height is simply the total copper thickness, and that's in fact the sum of the base copper and galvanic plating. The latter applies only for outer layers (or inner layers of a burried via process).

I understand, that you are designing a standard two layer PCB. In this case dielectric height, Er, copper height, possibly coating Er and thickness are the only relevant substrate parameters for trace impedance calculation. You'll notice, that the impact of copper height is limited for reasonable spacing numbers.

I further think, that the term "impedance control" doesn't apply here. It's just a PCB design for nominal trace impedance, without a tolerance specification or tests performed in PCB production.
 

kotshe

Junior Member level 3
Joined
Mar 18, 2008
Messages
30
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,503
Well following to what had been said before I can't acheive design impedance of 90 Ohms for two layers PCB( Trace width and gap are big)

I will explain my problem clearly and I would be happy to get suggestion from you :

I need to connect Two IC through cast5e (cable, impedance of 90 Ohm) I'm using RJ45 connector ? how can I keep Continuity of 90Ohm ?(for two layers PCB)

Do you think mid layers could solve the problem
 

robertferanec

Member level 1
Joined
Jun 15, 2011
Messages
37
Helped
17
Reputation
34
Reaction score
17
Trophy points
1,288
Activity points
1,481
kotshe: I believe cat5e is 100 ohms. what ICs you would like to connect?
 
  • Like
Reactions: kotshe

    kotshe

    points: 2
    Helpful Answer Positive Rating

kotshe

Junior Member level 3
Joined
Mar 18, 2008
Messages
30
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,503
UIC4102CP (USB extender) ,
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,489
Helped
14,050
Reputation
28,355
Reaction score
12,708
Trophy points
1,393
Location
Bochum, Germany
Activity points
276,162
Of course 90 ohm can be achieved in two layer PCB. You didn't yet tell, if you have a copper pour or void at the opposite layer. The USB common mode impedance specification would require a ground pour.

For 0.15 mm spacing, you get about 0.6 mm trace width. To further reduce the trace width, you can go for a "differential coplanar waveguide with ground" topology.





Apart from the basic feasibilty to implement USB impedances in a two layer PCB, there may be many reasons to use a multilayer, of course.
 
Last edited:
  • Like
Reactions: kotshe

    kotshe

    points: 2
    Helpful Answer Positive Rating

ea.arun

Full Member level 2
Joined
Apr 26, 2011
Messages
123
Helped
33
Reputation
66
Reaction score
32
Trophy points
1,308
Location
Chennai
Activity points
1,942
Kotsche:mid layers will definitely solve your problem(considering your copper thickness+tin plating thickness,Er etc).......
but you can try reducing the dielectric thicknes and increase the copper thickness to achieve the mentioned 90 ohm differential impedance(like 47mils from 62mils(1.6mm)) and achieve the same in 2 layers.....i have done the same but for a different impedance value....
unless it affetcs any mechanical or other parameters....
 
  • Like
Reactions: kotshe

    kotshe

    points: 2
    Helpful Answer Positive Rating

kotshe

Junior Member level 3
Joined
Mar 18, 2008
Messages
30
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,503
I can use ground pour at top and bottom layers. Could you explain more how can I achieve 90 Ohm ? if 1.6mm height of dielectric above return plane 2.5mm width and spacing 1.6 mm it's too big to use ....
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,489
Helped
14,050
Reputation
28,355
Reaction score
12,708
Trophy points
1,393
Location
Bochum, Germany
Activity points
276,162
The SMSC AN uses 1.2 mm substrate. But you get reasonable dimensions with 1.6 mm standard substrate as well, see above.
 
  • Like
Reactions: kotshe

    kotshe

    points: 2
    Helpful Answer Positive Rating

kotshe

Junior Member level 3
Joined
Mar 18, 2008
Messages
30
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
1,503
FvM : Thank you all , but I Guess I would go for FvM soluation seems to be the easy one to add Ground Polygon Pour (it's not considered as another layer and it would solve the problem).

---------- Post added at 14:43 ---------- Previous post was at 13:54 ----------

Final Request FvM could you please refer me to the calculator that you used .

Thanks A lot
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
47,489
Helped
14,050
Reputation
28,355
Reaction score
12,708
Trophy points
1,393
Location
Bochum, Germany
Activity points
276,162
I used Si6000 from polainstruments.com according to habbit. There's a number of free tools available as well.
 
Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top