Newbie Help: Microstrip - Page 1
Forum section: electronics / projects

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 05:55:41 am
content: I bought a few V.KEL VK1097U7M3 GPS modules (10mm by 9.7mm size - so tiny!) and the datasheet calls for a 50 ohm microstrip at most 2.5cm long from the module to the antenna socket, with a "T circuit". What does that mean, and how should the board look like?BTW my go-to SMD part size is 0603 (even though I hand solder everything, 0603 is still okay to me.)

author: KJDS
author_rank: Super Contributor
timestamp: August 03, 2015, 08:54:48 am
content: Follow the instructions on page 11 of the datasheet. All the L1 choke so that the pad sits on the antenna feed line without making it wider. You'll need to chose one small enough that it doesn't make the antenna feed line wider.

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 12:06:47 pm
content: Quote from: KJDS on August 03, 2015, 08:54:48 amThat won't fit me as several parameters does not match my board house.Parameters from my board house:Copper cladding: 1ozBoard thickness: 1.6mmNeither matches the datasheet.

author: KJDS
author_rank: Super Contributor
timestamp: August 03, 2015, 12:34:26 pm
content: Quote from: technix on August 03, 2015, 12:06:47 pmThen you have a choice of a lot of careful design, verified on an EM simulator and then further work with adjustments when the board is tested to make it work, or chose a different board manufacturer.

author: tggzzz
author_rank: Super Contributor
timestamp: August 03, 2015, 12:35:31 pm
content: Quote from: technix on August 03, 2015, 12:06:47 pmSo change your board house or change your parameters. Some aspects of the latter are explained here:http://bfy.tw/17ZM

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 12:47:24 pm
content: Quote from: KJDS on August 03, 2015, 12:34:26 pmA calculator told me that I need 3mm traces based on what my board house does - too wide for the small module. Is there any way to compensate this: I don't want to go 4 layer (5x more expensive) or 0.8mm board (too thin to use reliably in vehicle mounted gear)Or please suggest a free EM simulator so I can do this supposedly quick and dirty simulation.

author: tggzzz
author_rank: Super Contributor
timestamp: August 03, 2015, 01:51:39 pm
content: Quote from: technix on August 03, 2015, 12:47:24 pmNot really; all possibilities are expensive!QuoteWhat theory or experience leads you to believe that? I would think a competent mechanical engineer would be able to get it to work; failing that I would expect supports could be over-engineered.

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 03:49:09 pm
content: Quote from: tggzzz on August 03, 2015, 01:51:39 pmThen can I do this: put all the RF stuff, including the GPS module itself, on a small 8mm thick daughterboard (probably in a can) and connect this daughterboard to the 16mm thick project board (which itself is a daughterboard to Raspberry Pi) using some other interface.Given the size of the module (about 10mm square) is it a good idea to have the daughterboard taking the footprint of a 24-pin 0.6in wide DIP chip alongside the DS3231 chip for auxiliary timekeeping, as well as an optional AMS1117-3.3 regulator? If so, I may even start selling this module (won't be cheap though).

author: LaserSteve
author_rank: Super Contributor
timestamp: August 03, 2015, 04:24:34 pm
content: HP APPCAD for the free trace simulator. It will not model the transimpedance segment from the module to the board, but it is a good start.Steve

author: Kalvin
author_rank: Super Contributor
timestamp: August 03, 2015, 04:29:24 pm
content: What happens if you just try to make as good match as possible, and accept the fact that the matching is not optimal and you will lose sone sensitivity?

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 04:36:27 pm
content: Quote from: Kalvin on August 03, 2015, 04:29:24 pmThe thing is if I go with a 0.65mm trace on 1.6mm board I got slightly 99.57 ohms of impedance. Is there any way to compensate this out (just crop the impedance in half, I think it won't hurt too much for the 0.5%-1% mismatch, and a few preferred numbers for resistors sits around this value)

author: Kalvin
author_rank: Super Contributor
timestamp: August 03, 2015, 04:44:10 pm
content: Quote from: technix on August 03, 2015, 04:36:27 pmYou cannot make it 3mm wide at all? Or could you make it narrower near the module an then make it 3mm wide for the rest of the PCB?

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 04:53:21 pm
content: Quote from: Kalvin on August 03, 2015, 04:44:10 pmI can make it 3mm wide anywhere but right next to the pin on the module, which is only 0.8mm wide. If I used 3mm traces how to make that "T circuit" (or can I just forgone with it?)

author: Kalvin
author_rank: Super Contributor
timestamp: August 03, 2015, 05:04:32 pm
content: Quote from: technix on August 03, 2015, 04:53:21 pmIf the 0.65mm part of the trace is only few millimeters, you should be just fine like blueskull said above. Unfortunately my knowledge is too limited to say any specifics here. Possibly there are guys with more practical experience who can give you a ball-park estimate how good matching will be if you make the trace 3mm as long as possible and then pinch it to 0.65mm only for few millimeters.

author: Howardlong
author_rank: Super Contributor
timestamp: August 03, 2015, 05:18:03 pm
content: FWIW, rule of thumb for microstrip width on FR4 or similar substrate with ballpark Er~=4 is 2 * PCB thickness.Regarding whether or not to implement 3mm thickness, you could taper it if necessary over a couple of mm at the device's pad, but it'll be an impedance bump. Optimum IMHO would be to go to multilayer, that way you get rigidity and thin, impedance-matched traces.You might find that although your GPS modules may be very cheap, fabricating properly around them might make it more expensive especially for small runs. You might find that a slightly more expensive GPS solution, perhaps one with an integrated antenna, will mean you can get away with a $0.50 PCB. The same applies to supplying an appropriate antenna connector, that can end up being an expensive option on a low volume price sensitive device.Engineering isn't just about applying a few calculations, it's also about judging how and where to compromise. Just be aware that GPS implementations are weak signal and not a million miles away from the Shannon limit due to the fairly tight link margin: every compromise you stick in the sharp end will inevitably directly affect the end result.

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 06:02:05 pm
content: Quote from: Howardlong on August 03, 2015, 05:18:03 pmI cannot use those GPS with integrated antenna since the box will be placed under the hood of a vehicle (blocks GPS, but 3G will not suffer that much so that will be okay) or I will go with VK16U6 (which I already own one)Miltilayer boards are 5x as expensive so not an option at all, I cannot afford it. Daughterboards are cheaper in this sense actually - an 8mm thick daughterboard holding the GPS module, RF traces and local decoupling/filtering, and break all other pins out using some standard form factor like a 24-pin wide-body DIP (so I can reuse existing connectors like sockets for such DIP packages - cheaper)I want to place the antenna socket so close to the module that only a 3-5mm trace is needed. Does this allow me to forgone this microstrip entirely?

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 06:13:44 pm
content: Quote from: blueskull on August 03, 2015, 06:05:53 pmWhat is the maximum ratio of trace length to wavelength before I have to put RF effects into consideration? And will the GPS's reception be significantly reduced if I forgone microstrip for this 3-5mm trace?

author: Kalvin
author_rank: Super Contributor
timestamp: August 03, 2015, 06:24:40 pm
content: Quote from: technix on August 03, 2015, 06:13:44 pmIf the trace length is less 1/20 compared to the wavelength you are fine. If the trace length is approx. 1/10 compared to the wavelength you may be still fine, but you are definitely getting very close to the limit where you need to consider the trace as a transmission line.

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 06:48:32 pm
content: Quote from: Kalvin on August 03, 2015, 06:24:40 pmTried laying out using Eagle and a 5mm trace is easily manageable. So does that means I can rest the case and forgone the transmission line problem for now, since the trace is short enough not to be a problem?

author: Kalvin
author_rank: Super Contributor
timestamp: August 03, 2015, 07:17:40 pm
content: Quote from: technix on August 03, 2015, 06:48:32 pmAs blueskull already calculated the wavelength to be around 10cm on the FR4 PCB, the 5mm is close enough to the 1/20 rule-of-the-thumb. I would say that you should be ok with the tapered trace of 5mm in length (the shorter, the better), if you make the rest of the trace 3mm wide (50 ohms).

author: technix
author_rank: Super Contributor
timestamp: August 03, 2015, 07:19:28 pm
content: Quote from: Kalvin on August 03, 2015, 07:17:40 pmThe total trace length is 5mm (3mm width wont fit either at the chip or under the connector so the point is moot here)

author: Kalvin
author_rank: Super Contributor
timestamp: August 03, 2015, 07:23:38 pm
content: Quote from: technix on August 03, 2015, 07:19:28 pmOk. Just didn't quite keep up as the first post mentioned trace length of 2.5cm, so I thought you are still considering that option. Nevertheless, the 5mm trace should not be a problem.

author: rfeecs
author_rank: Frequent Contributor
timestamp: August 03, 2015, 07:36:23 pm
content: If really want to get obsessive over this you could download a free EM simulator:http://www.sonnetsoftware.com/products/lite/You put in your microstrip geometry and it calculates the S-parameters.

author: G0HZU
author_rank: Super Contributor
timestamp: August 03, 2015, 08:24:24 pm
content: Quote from: technix on August 03, 2015, 05:55:41 amIt seems a bit odd that it asks for microstrip because I would use grounded coplanar waveguide for something like this. I'd normally be using a multilayer board but you would design the GCPW spacings such that you achieve a workable (or ideal) centre conductor width. i.e. you have more control over the dimensions of your 50R transmission line this way.The other (highly relevant) advantage of this approach is that you will achieve much better isolation (less noise pickup) from interference from any nearby PCB traces. Make sure you use lots of via stitching around the device an also along the GCPW.I don't think it would be a good idea to try and have classic 3mm wide microstrip instead because you end up with a huge fat trace and also the problem of grounding the chip using via holes that are 1.6mm long. Also, the isolation performance will be worse. For good performance wrt tiny GPS signals you need to prevent any unwanted noise pickup at this sensitive place so you need to keep this trace short and ideally arrange it as GCPW. Looking at the pictures of it on google images I suspect that this chip is designed for GCPW because it appears to have a ground pin either side of the RF input pin. HTH

author: ywara
author_rank: Contributor
timestamp: August 04, 2015, 12:31:34 am
content: GCPW would theoretically allow you to use your different-sized board material. You would still need compensation at your transitions somehow.And everyone quoting the 1/10th or 1/20th wavelength rule of thumb: The rule is that below some threshold you can treat it as lumped elements, not neglect it entirely. Mismatches as short as a few thousandths of a wavelength are still significant.

author: rfeecs
author_rank: Frequent Contributor
timestamp: August 04, 2015, 12:59:14 am
content: The datasheet from here:http://www.vkelcom.com/soft.php(In Chinese)indicates using GCPW and shows an example using AppCAD with 0.8mm thick board. Using a 1.6mm board with a small discontinuity near the package shouldn't be a big problem if you scale up the dimensions. Again, you can do EM if you are concerned.From the picture on the front of the datasheet:

author: technix
author_rank: Super Contributor
timestamp: August 04, 2015, 03:31:05 pm
content: Quote from: rfeecs on August 04, 2015, 12:59:14 amWhat are the three small components? What is the circuit there?

author: technix
author_rank: Super Contributor
timestamp: August 04, 2015, 03:38:03 pm
content: Quote from: G0HZU on August 03, 2015, 08:24:24 pmQuick trip to GCPW calculator the gap between the 0.8mm RF trace and the ground plane (with via fences) have to be 0.11mm, which is just above the 4mil minimum trace distance of my board house. I am not sure if this will violate any design rules.

author: rfeecs
author_rank: Frequent Contributor
timestamp: August 04, 2015, 04:29:07 pm
content: Quote from: technix on August 04, 2015, 03:31:05 pmFrom the datasheet schematic, it looks like you have to inject bias into the RF input from the Vcc. So the shunt inductor and capacitor is probably doing that. The series inductor, shunt capacitor is probably tuning to tweek the input match, I'm guessing.

author: tggzzz
author_rank: Super Contributor
timestamp: August 04, 2015, 04:36:40 pm
content: Quote from: technix on August 04, 2015, 03:38:03 pmTry 1mm/0.2mm or 1.2mm/0.35mm and fiddle a little until you are satisfied.I presume you have checked what the maximum length of "incorrect" impedance stub you can tolerate. There are many easily found references that will give you a good starting point, and then you could even use LTspice (etc) and its transmission line models to givesomeconfidence in your understanding.

author: rfeecs
author_rank: Frequent Contributor
timestamp: August 04, 2015, 05:02:14 pm
content: Quote from: rfeecs on August 04, 2015, 04:29:07 pmLooking at the datasheet, I'm more confused. The block diagram in paragraph 5 shows one connection to the antenna, the schematic in paragraph 8 shows something different.The pinout description calls out VCC_RF "can be used for active antenna or external LNA supply" and there is another pin V_ANT/NC which is an input labeled "Antenna Bias Voltage": "Connect to GND (or leave open) if passive antenna is used. If an active antenna is used, add a 10 ? resistor in front of V_ANT input to the Antenna Bias Voltage or VCC_RF.So I have no idea.