Newbie in RF with a Crazy Project, a Few Questions - RF Cafe
Post subject: Newbie in RF with a crazy project, a few
Unread postPosted: Mon Sep 13, 2004 3:42 pm
Joined: Mon Sep 13, 2004 2:37 pm
I am working in my thesis
project which at the moment consists in a Ultra Wide Band (UWB)
Impulse radio Tx.
The idea is implement and test a simple UWB
Impulse transmitter using available RF components. So far, a first
system design simulation with ADS 2003C using SRD diodes to generate
very short impulses has been carried out succesfully. Now I have
to move to the circuit level and PCB design.
I would want to
know suggestions to start the Layout. I thougth to use the ADS Layout
tool to make the PCB, but my first impression is that it will be
a hell to place SMD components such as voltage regulators, amplifiers,
attenuators, filters, etc... I dont know if there are libraries
for the schematics parts and footprints for the layout.
I was thinking to use Orcad Schematics/Layout or other similar tools,
and once the PCB layout is ready, export it to the ADS and simulate
Do you know if it is possible to do this codesign
using a Layout tool to generate the PCB tracks and simulate back
Do you think that this procedure is correct? If not,
what tools do you suggest I should use?
Thanks in advance,
Unread postPosted: Tue Sep 14, 2004
You should separate between the
RF layout to the layout of other parts of your circuits (for example
as you mentioned voltage regulators etc).
The right way from
my experience to do this task is to simulate the layout of critical
RF sections in ADS or other RF CAD tool, and to be accurate as much
as possible in the definition of the layout parameters i.e: Substrate
type, er, Tand, thickness etc. This helps a lot to get accurate
results. You can export the layout from your PCB tool to ADS (using
DXF format or similar) and then simulate the layout structure and
see the effect of your layout on the circuit performance. By this
trial and error you can reach to the optimal layout of your circuit.
Once you have reached to the optimal layout you can transfer it
back to the PCB tool and this would be your final layout on the
The impact of the layout on the circuit goes hand
in hand with the increase of the frequency, this is especially right
for getting the optimal miter, diamaeter of vias etc.
first step to start with is of course to calculate the track width
for obtaining the desired Zo. You can do it with LineCalc, which
is an excellent tool for many RF structures (microstrip, stripline
etc) and you can synthesize and simulate physical structures and
see the electrical outcome and vice versa.
All after all
RF PCB layout requires some epxerience and CAD tools can be a good
way to predict various phenomenas but you should jump to the water
and gain this experience this is the best way to learn.
luck, and keep us posted.
Unread postPosted: Tue Sep 14, 2004
Thank you very much for your help Itay.
moment I am learning how to export Orcad Layout Plus designs to
DXF format, so I can import them in ADS afterwards.
sure I will have a lot of questions soon. Thanks for sharing your
Unread postPosted: Tue Sep 14, 2004 10:44 am
You have two circuits here, the RF and the DC. You will
hve to design chokes between them to keep them separate, that can
be tricky for UWB but any approach that considers interactions will
be immensly more complicated so forget about that.
you planning to do with ADS, obviously you have done a nonlinear
network simulation? ADS can create a Layout from this network with
some effort but so can OrCad. It would be difficult to layout the
DC part of the circuit with ADS. I think ADS is the qurikiest layout
editor of all the major simulators, I also think OrCad is the best
of the PCB tool I have used.
In practice, I send the DXF
to our PCB layout group. The generate the schematics and goto layout.
I just approve the final design.
Post subject: new questions
Thu Sep 30, 2004 6:10 am
Mon Sep 13, 2004 2:37 pm
friends, I am here again to kindly ask for your help. First, thank
for the previous feedback. I succesfully exported a DXF test file
and imported it in ADS.
Non-linear simulations with ADS were
succesful, so I spent the last weeks working on schematics in Orcad
Capture. In addition, I have worked on the footprints for the layout.
My design uses 2 Minicitcuits RF amplifiers, 3 RF switches, a 100MHz
oscilator, a few PI attenuator built using resistors, a few PECL
drivers, and connectors, etc. I designed the power supply for this
circuits with 3 Voltage regulators (+7, +5,-5).
Now I am
working on the layout, and I have the following questions:
The UWB pulses have a frequency spectrum from more or less 3
1. What kind of substrate should I use?
many layers do you suggest?
3. how can I distribute the power?
4. Which SMD resistors do you suggest for this application? Where
can I find the models for them in order to simulate at least the
5) I am using SMA connectors for the whole design,
but I dont know if it is correct for the output, is it?
Unread postPosted: Thu Sep 30, 2004
I am happy to hear that
your project is going well. To answer your questions:
What kind of substrate should I use?
Well this is all depends
on your frequency range, which as you stated is between 3-6GHz,
for this I highly recommend the RO4350 (ROGERS) family of substrates
which have repetitive and accurate Er of 3.48 and low losses (low
Tand). You should define the paramaters of this substrate in the
simulations of transmission lines and critical paths.
How many layers do you suggest?
Since you stated that your
design consists of 3 kind of circuits: Power, logic and RF, I would
suggest using 6 layers in the following order:
Top (RF layer
with all the RF componenets and related power supplies)
Voltage supplies layer
Logic signals layer
layer (in this layer place the PECL drivers and related power supply)
Make sure that your GND layers are complete, use 1 Oz copper
clading for each layer. the RF traces in the top layer should be
free of solder mask at this frequency range to minimize insertion
loss. Put plated via holes near each pad of componenet that is connected
to GND, stitch the edge of the board with as many via holes as you
can to form a good GND connection and to prevent bouncing of the
RF signal. the distance between the via holes should be less than
I would recommend using shielded cans for isolation
between the blocks and preventing radiations and spurious signals
from one block to the other. The diamater of the via holes should
be 10 mil.
3. how can I distribute the power?
wide traces in the power supply layer plane to ditribute the supplies
to the components. then you will connect each supply as close as
possible to the device through a plated via hole. The diamater of
the via holes for power connection should be between 12-16 mil.
4. Which SMD resistors do you suggest for this application?
Where can I find the models for them in order to simulate at least
the critical paths?
It all depends on the power levels your
application is using. I assume that 0805 would be enough. 0805 are
built for 1/8W, 0603 are built for 1/16W. calaculate the power levels
No need for simulating the resistors as their
parasistics start to effect above 10GHz.
5. 5) I am using
SMA connectors for the whole design, but I dont know if it is correct
for the output, is it?
It is the best choice. However there
are many vendors for SMA connectors. Y ou should do some checks
and find the best for your application. Some of the popular companies
are M/A-COM, Huber-Suhner etc.
I hope this helps. Please
keep in touch I will be keen to help you with your project.
subject: Thanks Itay!!
Unread postPosted: Fri Oct 01, 2004 5:51
Joined: Mon Sep 13, 2004 2:37
I am happy
to receive your answer. Thank you very much for your suggestions
and ideas, they are very valuable. I am going to work on the layout
these days and will post any news.