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

Plating Effects on Impedance of Traces

Status
Not open for further replies.
A

Anonymous_Ricky

Advanced Member level 2
Joined
Dec 26, 2006
Messages
516
Helped
88
Reputation
178
Reaction score
58
Trophy points
1,308
Location
India
Activity points
3,974
Hi All,

How does plating process effect the impedances of traces?
what will be the best Plating process?

T&R

Ricky
 

The plating process will lower the impedance of your trace. When calculating the trace impedance I always use the finished (after plating) copper thickness.
On a 50ohms SE trace the difference can be as much as 5 ohms (10%).

52ohms for a trace thickness of 18u and 47.9 ohms for a thickness of 35u.
 

you have higher losses when you use a nickel-gold plating on copper traces. But only in high frequency designs.
 

Thats plating on Pads, you dont plate traces (cost etc etc), you only plate pads to protect them from the envoironment before soldering. Generaly only outer layers get plated up during the through hole plating process, souse he finished copper wieght for your calcs.
 
That's often true, but for higher frequency designs you might not have soldermask on the traces, and so you would have to plate them.
 

Hi Marce,

Thanks for your Reply!
I would like to know can we prevent outer layer traces from getting plated during through hole plating. I have this doubt as plating is a process done before soldermasking so I think outer traces will get plated.
Or during my Impedance calculation I have to always consider outer trace plating.

T&R

Ricky
 

For high frequency signals, the current is mainly concentrated along the trace edges (many will argue but it's true). Not many realize this and they go through great lengths to use expensive mixed selective platings. The added copper has little effect on the total loss. Its biggest effect is it lowers the impedance. Most will be fine if you just start with 1/2 oz copper and go ahead and have normal plating and account for it in your impedance calculation.
 

I believe if you have a plane for the return current the highest density is actualy at the bottom of the trace, for the uninitiated we are discussing skin effect.
This argument is almost academic, as for most high speed digital designs (lets leave GHzs RF out of the equation for now) as you are best to run your traces as stripline on innerlayers so they are not gonna get plated. I have never employed any plating on traces or had to worry about solder resist for any HS digital design yet, and as said earlier I try to maximise stripline routing for high speed signals as the wave propagation is nearer to true TEM.
Very high GHz RF design is a different ball game...
 

So during plating for PTH pads my outer traces will also get plated and I have to consider plating in my calculations for impedance, Right?
Or PTH plating will be different from trace Plating?
 

yes, you really should consider the plating effects in your impedance calculation. check with your fabricator to give you what is typical. it seems every fabricator is a little different and i have seen ranges of 33um to 53um as the final thickness when starting with 1/2 oz copper

- - - Updated - - -

yes, you really should consider the plating effects in your impedance calculation. check with your fabricator to give you what is typical. it seems every fabricator is a little different and i have seen ranges of 33um to 53um as the final thickness when starting with 1/2 oz copper
 

Again why burrying all high speed signals on inner layers is becoming a popular technique.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top