rf traces

J

Jamie Morken

Guest
Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?

cheers,
Jamie
 
"Jamie Morken" <jmorken@shaw.ca> wrote in message
news:Mcxle.1492706$6l.1293797@pd7tw2no...
Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?

cheers,
Jamie
Click to expand...
They are transmission lines: it is for the input and output matching. The
data sheet will give more details.

Ken
 
Ken Taylor wrote:
"Jamie Morken" <jmorken@shaw.ca> wrote in message
news:Mcxle.1492706$6l.1293797@pd7tw2no...

Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?

cheers,
Jamie


They are transmission lines: it is for the input and output matching. The
data sheet will give more details.

Ken
Click to expand...
really? its a 4-layer pcb, assume 1.6mm thickness. if 0.4mm between top
layer and 0V plane, then

t/h = 35um/0.4mm = 0.088
w/h = 0.254mm/0.8mm = 0.636

M.A.R. Gunston gives Zo = 87 ohms (or thereabouts) for FR4.

this suggests that:
1) I have no idea exactly how wide that trace is,
2) nor do I know what the top-to-0V separation distance is

but suggests the track *should* be wider than 10mils. thinner (or
thicker) Cu has bugger all effect.

for 50 Ohms, 0.4mm spacing and 35um Cu, want W/h = 2 so 0.8mm wide
traces = 31mils or so.

zooming in, I see 1" = 170mm, trace = 2mm wide, so 2/170 = 11.8mils, IOW
Jamie wasnt far off. Perhaps the layer stackup is such that there is a
VERY small gap between the trace and 0V? more likely the PCB layout is
just wrong.


Cheers
Terry
 
On Fri, 27 May 2005 04:18:52 +0000, Jamie Morken wrote:

Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?

cheers,
Jamie
Click to expand...
I am WAY too lazy to look at the board. Here are some thoughts. The
most orthodox way to deal with the trace widths is to choose a stackup
and trace width so that you get the desired impedance (50 Ohms). For
surface layer traces, the only thing that really matters is the distance
to the ground (or power) plane and the trace width. The copper thickness
has a small effect also. It is certainly possible to create a stackup such
that a 10 mil trace has a 50 Ohm impedance. I have done this. You end up
using a fairly small gap between signal and plane, and a fairly large gap
between plane and plane, assuming that the board is 62 mils overall.

If Maxim didn't use 50-Ohm traces, there could be a few possible
explanations. It could be because they don't know any better or don't
care, or they could have something up their sleeve. I have to assume that
they know what they are doing, so I'll rule out the notion that they
don't know any better.

They might not care about the impedance if the traces are very short.
Afterall, if a trace is only 0.05 lambdas, then it doesn't really matter
if the impedance is right.

Another possibility is that they use traces which are a little bit too
narrow (high impedance) to compensate for the parasitic capacitance of
the pads. I don't know if this really works, but I have heard people
advocate it before. If you are really interested, you can go find the
formulas for pad capacitance, and model the traces as lossless
transmission lines and simulate it using spice or something similar. You
could do 16 simulations for 4 different capacitances, and 4 different
trace impedances. It might be just as easy to calculate the input
impedance using a spreadsheet, since you are only using one frequency.



T1
_______________
---+--------) )-----+-----+
= C1 --------------- = C1 |
| | \
GND GND / R1
\
/
|
GND

This is the setup when power is coming in from a connector to a device
on the board. C1 is the capacitance of the connector pad, C2 is the
capacitance of the receiving device pad, and R1 is meant to model the
input impedance of the receiving device. If you have reason to believe
that the input impedance is not 50 Ohms resistive (for example if you
have a spice model or listed package parameters), then replace R1 with
a more accurate impedance, Z1. T1 is the trace modelled as a transmission
line.

If you are transmitting off board, then you could just sort of turn it
around.

Have fun.

--Mac
 
Jamie Morken wrote:
Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?
Click to expand...
If there is GND on the same layer, how far away
is it ? The closer, the lower the impedance of
the narrow trace.

Rene
--
Ing.Buero R.Tschaggelar - http://www.ibrtses.com
& commercial newsgroups - http://www.talkto.net
 
Rene Tschaggelar wrote:
Jamie Morken wrote:

Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?


If there is GND on the same layer, how far away
is it ? The closer, the lower the impedance of
the narrow trace.

Rene
Click to expand...
no ground on the top layer. The PDF Jamie pointed to has all the artwork.
 
Mac wrote:
On Fri, 27 May 2005 04:18:52 +0000, Jamie Morken wrote:


Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?

cheers,
Jamie


I am WAY too lazy to look at the board. Here are some thoughts. The
most orthodox way to deal with the trace widths is to choose a stackup
and trace width so that you get the desired impedance (50 Ohms). For
surface layer traces, the only thing that really matters is the distance
to the ground (or power) plane and the trace width. The copper thickness
has a small effect also. It is certainly possible to create a stackup such
that a 10 mil trace has a 50 Ohm impedance. I have done this. You end up
using a fairly small gap between signal and plane, and a fairly large gap
between plane and plane, assuming that the board is 62 mils overall.
Click to expand...
looks like you need a W/h of about 2, so a *very* thin gap - IOW, 5 mils
or so.

If Maxim didn't use 50-Ohm traces, there could be a few possible
explanations. It could be because they don't know any better or don't
care, or they could have something up their sleeve. I have to assume that
they know what they are doing, so I'll rule out the notion that they
don't know any better.
Click to expand...
app notes are often written by the least skilled (usually the most
junior) "engineers"

years ago, I tried some IR 1200V 1/2-bridge gatedrivers. We destroyed
about 6 of them (2 demo boards) before giving up in disgust. 2 years
later some IR bigwigs came to see why we weren't buying them. When told
the sorry tale, they apologised profusely, and pointed out the pcb
layout was so bad that pretty much *all* of the demo boards blew up.
Didnt convince us to buy any though - too damn expensive.


They might not care about the impedance if the traces are very short.
Afterall, if a trace is only 0.05 lambdas, then it doesn't really matter
if the impedance is right.
Click to expand...
probably the case. especially since its a demo board, so doesnt have to
pass any sort of EMI tests.

Another possibility is that they use traces which are a little bit too
narrow (high impedance) to compensate for the parasitic capacitance of
the pads. I don't know if this really works, but I have heard people
advocate it before. If you are really interested, you can go find the
formulas for pad capacitance, and model the traces as lossless
transmission lines and simulate it using spice or something similar. You
could do 16 simulations for 4 different capacitances, and 4 different
trace impedances. It might be just as easy to calculate the input
impedance using a spreadsheet, since you are only using one frequency.
Click to expand...
slicing the pcb and measuring the top-to-mi1-layer spacing would be a
good start.

T1
_______________
---+--------) )-----+-----+
= C1 --------------- = C1 |
| | \
GND GND / R1
\
/
|
GND

This is the setup when power is coming in from a connector to a device
on the board. C1 is the capacitance of the connector pad, C2 is the
capacitance of the receiving device pad, and R1 is meant to model the
input impedance of the receiving device. If you have reason to believe
that the input impedance is not 50 Ohms resistive (for example if you
have a spice model or listed package parameters), then replace R1 with
a more accurate impedance, Z1. T1 is the trace modelled as a transmission
line.

If you are transmitting off board, then you could just sort of turn it
around.

Have fun.

--Mac
Click to expand...
Cheers
Terry
 
On Fri, 27 May 2005 17:53:29 +1200, Terry Given <my_name@ieee.org> wrote:



zooming in, I see 1" = 170mm, trace = 2mm wide, so 2/170 = 11.8mils, IOW
Jamie wasnt far off. Perhaps the layer stackup is such that there is a
VERY small gap between the trace and 0V? more likely the PCB layout is
just wrong.
Click to expand...
Have a look at the circuit diagram on page 3.
It gives the two track widths used (3.2mil and 5 mil), their lengths and
electrical properties - to the left of C8


Geo
 
"Jamie Morken" <jmorken@shaw.ca> wrote in message
news:Mcxle.1492706$6l.1293797@pd7tw2no...
Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?

cheers,
Jamie
Click to expand...
maybe its used as a 1/4 wavelength matching line ?

Colin =^.^=
 
Jamie Morken wrote:
Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?
Click to expand...
They want to present some specific impedance to the PA. That is, they
transform a nominal 50 Ohms on the output port to something else. You
can likely come close to computing what it *theoretically* should be
with the data they give.

However, there are some questionable areas when it comes to actual
physical builds.

1. They don't tell you if mask covers the traces, which does affect the
line Z.

2. They don't tell you the plating thickness. That 0.5 oz copper might
be up to around 1.5 mil thick by the time they are done with copper and
[other] plating.

3. There is probably around a ą1 mil etching tolerance (width) when the
fab is made. What this means is that for 5 mil and 3.6 mil (!) traces,
there is a high fractional tolerance in line impedance.


I think the design is a bit dubious for production units, so for eval
with it is also questionable if you're using the info to guess what
might happen in production.

I wonder how close this chip is to the max2242 I used a few years back.
 
On Fri, 27 May 2005 04:18:52 GMT, Jamie Morken <jmorken@shaw.ca>
wrote:

Hi,

In this eval board datasheet for the max2240 2.4GHz power amp:

"http://pdfserv.maxim-ic.com/en/ds/MAX2240EVKIT.pdf"

It shows the 50ohm RF input with a narrow (~10mil) trace, and also the
RF output is conducted through a very narrow trace. Could someone
explain why these narrow traces are used?

cheers,
Jamie
Click to expand...

10 mil wide microstrip on 6 mil FR-4 is just about 50 ohms.

John
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top