GPS Impedance matching

[sekharareddy]

gps+trace+impedance

Hello All,

I have a GPS module and i'm going to place it on a test board which contains this GPS module,matching circuit(to be finalised) and antenna.

Can anybody suggest me how to proceed on this for finding out the matching component values? also how can I ensure that these two are matched perfectly?
Assume that I dont have the impedance values of either GPS module or antenna.

 

[GVVIN]

checking impedance match in pcb

use a 50 ohm coaxial cable and connect

Do you have a network anlayser ?
If you have measure both antenna and GPS module and do matching.

both the modules will be 50 ohms I guess , so there will not be any ned to match , just connect.

 

[sekharareddy]

difference+gps+impedance

If I connect the cable(Assume that GPS module and anttenna were assembled)in between GPS module and antenna and measure the impedance of antenna, is it correct procedure?I assume the power from NW anlayzer will enters into GPS module also.

 

[GVVIN]

Measure them seperately. antenna to NA and GPS to NA (Network Analyser)

Hope GPS module does not support active antenna. (with LNA) else use a Dc block at NA port.

you are right,may be default 0dBm of NA will drive GPS LNA into saturation. you can reduce the power from Network anlayser and do the measuremnt of GPS

Still I feel external matching wont be required.

Regards
GV

 

[sekharareddy]

When the GPS module and antenna were already assembled on the board,how can we measure the impedance separately?

I think Impedance matching is required because,the antenna was placed on a PCB with different dielectric thickness and different PCB ground plane dimensions from the one suggested by antenna manufacturer.In this case definately we observe some variation in antenna performance.

 

[RF-OM]

You can measure impedance right on the board with end-launch - short piece of 47mils semiridgit coaxial cable. After NA calibration you need to use Port Extension (but not electrical delay) to move calibration plane further away on the distance equal to electrical length of end-launch. Check the manufacturer data sheet, find the dielectric constant and it will allow you to determine how many ps you need to add to the Port Extension. It may be roughly about 7 ps per mm length.Good check of the calibration is to use Smith chart and check open short points with end-launch connected. Especially open test will show you how good is your calibration is. When you measure two impedances it is easy to use any simulator or matching software to calculate the match. I am using matching tool in LINC2 RF simulator, this is the fastest and easiest from what I know.

P.S. What is very important is to keep open central wire of the cable as short as it possible, in any case not longer than 0.5mm.

Best regards,
RF-OM

 

[sekharareddy]

Hello RF-OM,

Thanks for the reply.
This procedure is looking accurate.At present as I have some time,I wanted to fabricate a Calibaration PCB which contains an Open trace,short and load(50Ω) with length equal to the length of the trace on my actual PCB.
Then after calibration with those trace on test PCB,I'm planning to carry the measurements on my actual PCB.
Can you suggest me any care to be taken for the procedure which I have proposed?or If you think any problem with this method kindly suggest me.

 

[GVVIN]

Hi Sekhar,

I have one doubt. What is your application. Usually GPS antenna is mounted external and connected to GPS module, say if used in car. if you keep the antenna inside your lab you wont be getting enough signal from satellite to find the position or whatever.

You said you are going to mount antenna on to a PCB, Are you in the process of designing antenna ??

Regards
GV

 

[sekharareddy]

Hi GVVIN,

Our application is we have developed our own GPS module and we have some Geo helix antenna and Patch antennas.
We want to develop test boards for our GPS module with various avilable antennas and do the impedance matching for all the cases.

 

[RF-OM]

To sekharareddy,

Your idea is absolutely right. You need to have a few boards each for one of the SOLT calibration procedures. The only question is what is your frequency range? You know that calibrations kits are very expensive and it is because they made to work precisely in wide frequency range. If your application is only for GPS, or about 1500 MHz it is not so hard to build calibration boards. However, there are some points to consider. All traces must be really 50 Ohm, better to use coplanar wave guide than microstrip. SHORT one should be really short and here CPW is much better. Shorting must be done for both sides of the connector’s central pin and despite CPW via to ground plane must be place around. Via diameter about 15 mils is good and the spacing about 30 to 50 mils should be okay. Distance from via center to edge of CPW ground is about 2 via diameters or 30 mils. What is extremely important it is to solder the central pin of connectors along all the length. This is the tricky case because PCB manufacturers often want to stop copper about 0.25 to 0.5 mm (10 to 20mils) from the edge of the board. This will completely kill you standard. Never use SMA connectors designed to install vertically. Use only horizontal end-launch SMAs, desirable those that eliminate unsoldered part of the central pin to be hanging in the air. Footprint for chosen connector is also important. All the traces and ground planes must go to the very edge of the board! Just imaging those 20 mils of the central pin is sitting in the air. It is about 0.5 nH of inductance, which is about 3 Ohm at 1 GHz or about 5 Ohm at GPS frequency. It is not so good standard for calibration if it has series connected 5 Ohm reactance for each of connectors. All board must be kept as small as it possible (RF part of course, there may be empty space for convenience), except the THRU one. This board must have the length which is corresponds to the real one. The 50 Ohm load standard is also very tricky. It is better to install two resistors 100 Ohm each for both sides of the central pin to the CPW ground. The 0402 size should be okay for GPS frequencies. Pay special attention to the robustness of the boards. Very often they are under the stress from cable tension and develop some micro cracks or may be broken. Install stiffeners, but be careful not to damage the ground plane under them. Finally, it is good idea to check your standards with TDR.

There is one more good opportunities to use such homemade boards. You can make small board that have two connectors and 50 Ohm loads. All traces are the same as on the test board. Then you measure S-parameter file (s2p) for input connector, then for output connector and save them. After these calibration procedures you measure your device under test (DUT) and save S-parameter file. After this you may use RF simulator or special calculator (for example in LINC2 RF simulator) and de-embed connectors and traces from test board S-parameter files. This will allow you to have pure S-parameter file for your device with test conditions what you need, not those that vendor provided.

I hope this information will be helpful.

Best regards,
RF-OM

Added after 8 minutes:

To GVVIN,

Your concern about antenna is right, but today's GPS receiver has sensitivity well below -165dBm (yes, close to kTB). A couple of years ago I participated in GPS chip design and this chip worked very well in the lab. Mass production receiver worked well under the seat in the car. I believe there should be no problem now.

Best regards,
RF-OM

 

[sekharareddy]

Hello RF-OM,

Thanks a lot for the elaborate explanation.I impressed the way of explanation you have given.

As my operating frequency is 1575.42Mhz,I think i can go for the calibration PCB i'm planning.But I'm plannig to make OPEN,SHORT and LOAD on same PCB.Will it creates any difficulties?

Also Can you suggest me any Passive Patch antenna(manufacturer) with Minimum Ground plane requrement(on test PCB)?

 

[RF-OM]

Yes, you can place all your calibration standards on one board, especially if you use CPW. Just keep upper ground plane width at least three to five CPW central trace width and good via.

Sorry, I did not understand your second question about Minimum Ground Plane requirements. If it related to PCB I can help you, if it more related to antenna it is better to ask somebody else, for example Azulykit. I know him as a good antenna engineer. I know antennas, but it is not my area and I am not the best person to ask questions about antennas.

Best regards,
RF-OM

 

[GVVIN]

https://www.delorme.com/byUse/gpsmodules/images/DeLorme_Antenna_RF_Design.pdf

 

[RF-OM]

Thanks a lot GVVIN for this link. It is interesting and definitely helpful. I just have some doubts that they provided right recommendation about CPW. Indeed CPW is very good, but when it has ground under the trace the dielectric loss may be higher. It depends on substrate properties, but in general, there may be a good compromise between substrate thickness and dielectric losses. On the CPW picture we may see that there is some space to adjust width of the CPW slots. It can be easily checked with field solver like Polar Si9000. If sekharareddy need it I can check CPW configuration with Polar Si9000, but I need to know substrate data (material, Er, loses, thickness, desirable trace width). One more point: they probably overestimated CPW effect on GPS receiver performance. The difference in CPW design at 1.575GHz may change implementation loss for about 1 dB (if we keep line short). It is only 26% and hardly noticeable. But accuracy in design is important and we need to consider all factors.

Best regards,
Rf-OM

 

[sekharareddy]

Thanks for GVVIN and RF-OM, for your continous support.

To RF-OM,

Actually we are palnning go with 4layer FR4 material(1mm) with the following stackup.Can you suggets me the CPW structure for this? some guidelines to be followed while doing the routing?

 

[RF-OM]

To sekharareddy,

Your picture shows substrate thickness 0.21mm and material is FR4 with half oz copper (18um). Considering Er=4.5 your CPW will have trace width of 0.36mm and slot width of 0.33mm. The width of ground strips on top side must be at least 1mm, better at least 1.5mm. There must be via row along each of ground strips. Via may be any diameter in 0.25 - 0.5mm range and via space about 2 to 3 via diameter should be okay. You need to check Er with board manufacturer, they must keep Er=4.5.

I hope it help,
RF-OM