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.
a) Up to 1 GHz you can still use normal FR4 PCB. (I used this with good results up to around 1.6Ghz for GPS amplifiers) Don't use the 64mil thickness, go for 32mil or so.
b) Short tracks. Use the correct width to match 50Ohm, mitered corners etc.
c) Good groundplane's
d) Plenty of vias, especially the ones next to microstrip lines.
e) Don't use groundplane under osc tank circuits. (Variation in temp can cause capacitance to vary)
f) Follow application layout guidelines where possible.
g) Keep coils/inductors at right angles to each other when they are closely spaced.
h) When crossing tracks, on layers, cross at right angles for minimum interference between them
i) Thin long tracks radiate, short thick ones less so.
j) Keep tracks away from each other by at least 1.5 times the thickness of your pcb for minimal coupling.
This is a few things that I can quickly think of. Other members might add on to this.
1.) a matching circuit (L and C) from the antenna pad to the antenna pin of your GPS module - micostrip design
2.) perfect ground condition - plenty of vias on the Antenna PAD and ground pins of gps module (as small as possible)
3.) never use square pads for Antenna input pin as the sharp edges could also act as an "antenna"
4.) FR4 - better dielectric constant
what is the purpose of the vias along microstrip? is there any guidelines for the vias, eg separation between vias, separation between via and microstrip, size of via etc.
The purpose of the vias around the microstrip is to "stitch" the gnds together. At higher frequencies, the gnd potential can vary depending on the distance between vias. As a rule of thumb, I keep the gnd via spacing to less than 1/8 wavelength of my highest frequency.
1. Shield clock, noisy signals
2. Partition your block.
3. Simulate your circuit.
4. Calculate trace width before layout.
5. Be careful with different power supply ground return.
In general, all high speed/RF/microwave design guidelines need to be taken into consideration.
In pcb routing, whether for low or high frequency, keep the following in mind:
[1] avoid bends at all cost if you can. Straight conductors are "balanced" structure in 1 sense, and contain the signal well. Signals' balance become disturbed at bends, and give rise to radiation. Research had been done to see the effect of various bend type on microwave & RF losses.
[2] Keep the ground plane below the high frequency traces intact. At high frequency, the return current flows directly beneath the signal trace, in the opposite direction. For example, if the RF ground in the RX RF path is "open", it can cause 3-5 dB drop in BER, as what I have experienced in a Bluetooth headset product.
[3] Ok, you like to impose the frequency range in questions. I only use the expected highest frequency of operation in calculating the trace width of RF trace, generally 50 ohm. No such things as using wider arbitary width in higher frequency. You have to calculate them. For Bluetooth, I use a frequncy of 2.5GHz for calculating the trace width, taking into the account of the pcb stackup design.
In typical RF PCB designs some of the tracks need to be much wider than others. Additionally, in some cases, if the RF designer has laid out the PCB with no concern for thermal effects, that may lead to 'tombstoning'. It is possible that there will be components (typically passives) which have a track of, say, 0.007" entering at one end, and 0.020" exiting from the other. Components with different size tracks entering and exiting is a prime example of how 'tombstoning' or 'billboarding' can occur, and is something that the manufacturing engineer must watch out for. Different track widths affect impedance and matching the size of the track to the correct impedance (say 3mm for 50W lines on FR4 ) is important for circuit performance. This type of track is commonly called a microstrip line, and will typically have a ground plane directly underneath it.
**broken link removed**
Personal suggestion on PCB layout for 10MHz - 2GHz
If anything wrong, pls correct me or append any different ideas
1. Stages should be lined up, rather than snake around
2. Ways to prevent RF leakage to DC or control line which address more on wireless performances : Use RF bypass capacitor near IC package and series resistors with resistance level close that of DC line.
3. Input and Output signal tracks should be far apart as possible in case of instability or interference.
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.
