Continue to Site

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.

Register Log in

How to calculate 50 ohm line, need reality check please

Status
Not open for further replies.
Nora

Nora

Advanced Member level 4
Joined
Mar 31, 2006
Messages
115
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,296
Location
My garage, USA
Activity points
2,292
Hello-
I'm using a few different microstrip calculators, but when I draw my trace, the suggested width (2.9mm) seems huge.
Calculator here: https://ncalculators.com/electronics/microstrip-impedance-calculator.htm
The transmission line needs to be 50 ohms as it connects directly with a 50 ohm matched impedance IC, of which the leads are around 0.4mm

I'm using FR4 and this is a 2-layer board
dielectric constant er is 4.5
strip thickness is 1 oz copper, 0.035mm
dielectric height is a standard 2 layer board, it is 1.6mm
I need a Z0 of 50 ohms

What am I doing wrong?

I was also told that 50 ohm transmission lines on 2 layer boards would need to be much thicker than the same 50 ohm t-line on 4 layer boards. Can anyone confirm this?
Thank you,
Nora
 

That sounds about right. 50 and 75 ohm microstrips on a 2 layer 1.6mm FR4 PCB are wide. The widths on a 4 layer are considerably smaller depending on the exact layer stackup.

Keith
 

try putting some copper plane under you 50 ohm impedance line in bottom side this will reduce trace width but for 2 layer boards trace width will be thick compared to multilayer boards.
 

I assumed the underside of the trace was ground for microstrip. I don't think it is a microstrip line otherwise - simply a piece of wire dangling in space.

Keith
 

keith1200rs said:
That sounds about right. 50 and 75 ohm microstrips on a 2 layer 1.6mm FR4 PCB are wide. The widths on a 4 layer are considerably smaller depending on the exact layer stackup.

Keith
Click to expand...

Thank you for replies.
The IC pin that I'm going to is 0.3mm in width. Can I still use a 2 layer board and narrow down the trace to connect to the pin?
If I use a trace that "fits" mechanically on a 2 layer board, it is 0.46 mm and the Z0 is 113 ohms.

What happens when the impedances are mismatched so greatly?
 

You have to narrow down your trace at IC pin you do not have any other option for that but try to keep it as short as possible.

Impedance mismatch will imapct your design if you are using it for high speed designs but for boards with very low working frequncy it would not be of much effect.
 

Anonymous_Ricky said:
You have to narrow down your trace at IC pin you do not have any other option for that but try to keep it as short as possible.

Impedance mismatch will imapct your design if you are using it for high speed designs but for boards with very low working frequncy it would not be of much effect.
Click to expand...

Frequency is 900MHz. I should work with a 4 layer board then, right?
 

I would suggest go for 4 layer board if cost is not the main issue as at 900 MHz 4 Layers will give you better result.
 

At 900 MHz, it's no problem to have the trace tappered at the last 2 mm or so. You can also make coplanar strips with ground. It's particularly suggested if the pins next to the 50 ohm pin are ground pins anyway. If you can use a small ground separation, e.g. 100 µm, you come near to 50 ohm for a small trace.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top