Hi I am working on developing a bluetooth PCB using the BGM121. I have a few hardware design questions as well as tuning questions. I plan on using the internal antenna.
An RF engineer answered some of my earlier questions, but I had some followup questions and was unable to ask him them due to his busy schedule.
Due to the application of the device, we would like our design to be around 10-11mm x 10-11mm in size. The range can be short (<15m).
The questions are as follows:
1) You mentioned that the trace width to maintain 50 ohms a 4 layer standard PCB from advanced circuits was 17mil using this calculator https://www.eeweb.com/tools/microstrip-impedance. However, when I enter the specs from advanced circuits for a standard 4 layer board I do not get this. I get something closer to 30 mil. In addition, the calculator that you sent does not include spacing from the ground place around the trace. The calculator that I used to get 30 mil was AppCAD by http://www.hp.woodshot.com/. What am I doing differently than you to get this difference in trace width?
2) You mentioned that adjusting the width of the antenna loop on the BGM121 does not affect the frequency/impedance of the signal coming out of the rf_out port or the internal antenna. The datasheet mentions that changing the width of the antenna loop is used to tune up or down the frequency of the rf signal depending on which direction you shift the loop. If this does not affect the frequency/impedance of the rf_out port signal or the internal antenna, what causes this frequency shift. Also if the frequency/impedance does not change from the rf_out port how can you use a VNA to tune the antenna?
3) How do you use a VNA to quantitatively know how much to adjust the antenna loop to minimize power loss?
4) Can you tell me if there are flaws in the following logic: The standard output impedance from the rf_out port is 50 ohms. We have to make a trace that has 50 ohm impedance from the rf_out port to the U.FL connector. Depending on various factors when the BGM121 module is placed on a PCB, the impedance of the rf_out port can shift from 50 ohms to something slightly different. Since the trace to the U.FL connector is 50 ohms impedance if the rf_out port is giving a signal that is not 50 ohms there is reflection and power loss. When we adjust the antenna loop to “tune” the module, we try to get the impedance of the rf_out port to be 50 ohms. When it is 50 ohms, on the VNA we will see that there is very little power loss. This is the logic that I used until you mentioned that the rf_out port impedance does not change when you adjust the width of the antenna loop. If that is the case, how is it possible to use a VNA to tune the antenna?
It looks like you are referencing a conversation that took place in a different community forum page. If so can you provide the link for context?
You state right away that you are using the internal antenna for your design and not the external antenna and that you are primarily concerned with tuning the internal antenna. You are also connecting a U.FL connector for the purpose of this tuning exercise and are concerned with making the trace to the U.HL matched to 50 ohms. Additionally you expressed some confusion as to the procedure for tuning the on board antenna.
The best way to facilitate the antenna tuning is described in the KBA titled, https://www.silabs.com/community/wireless/bluetooth/knowledge-base.entry.html/2017/01/10/antenna_tuning_forb-R5av
This KBA also contains links to you tube videos providing more guidance for tuning your antenna:
Naturally you should also follow the guidelines given in the datasheet for the BGM12x.
First note that you should tune the antenna in the finished / completed product enclosure. Be sure to include any batteries, magnets, plastics, metal parts, screws, etc., basically everything that the customer will get in the final product. Otherwise you will potentially be tuning the antenna for a configuration that is different than your intended product if any of the above are placed close to the BGM12x after the tuning effort. These things can detune your antenna if not including during your antenna matching exercise.
To facilitate the S11 measurement I generally recommend placing an 0402 component pad in your PCB design to make the connection between pins 4, 2G4RF_ANT_IN and 5, 2G4RF_PORT. Normally the component will be a 10 pF or a 0 ohm resistor but for the purpose of using a VNA you will remove the component and add a semi rigid coaxial cable (pigtail) to the pad connected to pin 4 in order to make your S11 measurement of the antenna impedance. It sounds like you have placed a U.FL connector instead which aligns better with the KBA I referenced above but note the U.FL itself and the trace to the U.FL may introduce some impedance which would need to be calibrated out for accurate S11 measurement. The process for this calibration may vary depending on the VNA you are using, but would be the same as is done for using the pigtail.
Ultimately, the antenna tuning effort is PCB artwork dependent, so you should plan on iterations of the antenna loop dimensions. This means you will minimally make one more spin of the PCB. Your questions regarding the use of the VNA indicate you are not familiar with the use on one and so it may be advisable to simply build up a panel of PCBs with each instance having a different antenna loop dimension. In this way the proper matched artwork is found not by measurement with the VNA but by RF performance testing and simply choosing the best performing artwork. You should not take this step until you have resolved any other hardware placement questions in your product design so as to avoid any issues with detuning the antenna in your final layout and / or product enclosure.
Regarding your question about the microstrip impedance calculators, you should work with a calculator that can give you results for co-planer waveguide traces. The reason is we strongly recommend using ground plane on the top layer around your RF traces. A best practice rule for this is to have minimum spacing between the RF trace and the ground pour of about 10 mils and of course use plenty of stitching vias along the edges of the ground pour surrounding the RF trace.
Let us know if the KBA linked above along with the videos mentioned do not answer the questions you have asked here.
Thank you and best regards,
What are your questions?
For addressing the main concern of tuning the BGM12x antenna, please completely review the KBA I provided the link to, as well as the sub linked videos, as they provide the answers for the concerns you described in the paragraphs 2, 3 and 4. Hence my responses are general given the KBA and videos are quite good and provide a thorough description of what a designer needs to do to accomplish this task. If there are sections that are not clear or for which you have questions about, I can help to answer those questions but you need to let me know the specific area of concern.
Some clarifications I will make regarding paragraphs 1, 2, 3 and 4:
Paragraph 1. you state, "1) You mentioned that the trace width to maintain 50 ohms a 4 layer standard PCB from advanced circuits was 17mil using this calculator https://www.eeweb.com/tools/microstrip-impedance."
I believe this to be incorrect guidance. I have been in consultation with the support engineer you have been interfacing since your earlier portal cases and I do not recall this conversation. I don't believe either of us would have recommended that particular calculator due to the co-planer wave guide calculation is not available. Furthermore, you need to have knowledge of the FR4 material, layer stack thickness, copper thickness, etc to use as input for the most accurate result. Assuming this is regarding the 50 ohm trace between the U.FL and the antenna port, any resulting impedance mismatch impacting the S11 measurement of the internal antenna should be able to be addressed through the VNA measurement calibration process. Again, as I stated in my prior response, I would recommend not using the U.FL connector and instead use the component footprint pad that is attached to the pin 4 or the BGM12x for your S11 measurement. Note that if the U.FL is used only for conducted characterization measurements, it does not need to be matched to 50 ohms if kept less than 1 cm long.
Paragraph 2 seems to indicate a misunderstanding. Adjusting the antenna loop does not impact the impedance of the RF_OUT port, but it does impact the impedance of the antenna port. The U.FL is meant to be used for an external antenna use case or for conducted characterization of the RF_OUT port if needed for evaluation purposes. It is not meant to be used for antenna impedance matching, but it can be if the disconnecting components used to select between the antenna port or the external port are placed in layout in such a way as to facilitate this measurement. Looking at a design you submitted in a portal case, I can see that your layout is not done in a way to facilitate an easy S11 measurement of the antenna port. Again, I recommend using a pigtail on the component pad attached to pin 4 of the BGM12x instead of trying to use the U.FL connector. If you use the U.FL connector, you must somehow keep the RF_OUT port pin disconnected from the measurement, otherwise you will be measuring the RF_OUT port and the antenna port at the same time which of course will not help you at all. Again, closely review the KBA and associated videos for clarification on this subject. Another point of clarification here, be sure to not have the component populated for the U.FL at the same time as the antenna port component is populated when shipping this in production as the U.FL trace and connector will act as a branch circuit and detune the antenna to some degree.
Paragraph 3. The KBA and associated videos assume the designer has knowledge of the VNA instrument being used. However it is understood this is a specialized piece of test equipment for which you may not have experience with. Since the VNA is a critical component in the antenna tuning process there are a couple of options for you. One, reach out to the VNA vendor for guidance on S11 measurements and cable / path calibration. Two, go with the suggestion I made earlier to build iterations of the design (using a panelized PCB layout) with different antenna loop dimensions and choose the best RF performer.
Paragraph 4. See all of the above but especially note the RF_OUT port should not in any way be part of your antenna port S11 measurement. So the question here is are you tuning the on-SIP antenna or an external antenna? it sounds like you have matched the U.FL connector trace to 50 ohms, which is good, but did you have the antenna connected to it? Even so, the RF_OUT port should not be part of this measurement.
Final note: Based on the portal reviews, it appears you have followed the guidelines and recommendations provided by the support team. If this is the same design, you should not need to re-tune the antenna unless you have a final product design not shown in the portal case that you believe is effecting your antenna match, such as a battery, magnet or metal part that is very close to the antenna. If this is not the case and your final design is clear of such RF obstructions, then we expect you will obtain the range you stated you need. Given you have discussed impedance matching the RF path to the U.FL, have you also done RF performance testing, both conducted and radiated? Comparison of these measurements will help you determine if you need the antenna to be re-tuned or not.
Again, let us know what is not clarified from these posts and from the linked KBA and videos.
Thank you and best regards,
Thanks for the response. The support engineer that I was referencing was Eric from Arrow Electronics that I talked to through a phone conversation. Aundrea Ehrlich from SiLabs connected me to him. However, since he is not an employee of SiLabs, there were some things that he was unable to answer.
The reason I earlier mentioned that you did not properly answer my questions is because of this paragraph in your first response:
"You state right away that you are using the internal antenna for your design and not the external antenna and that you are primarily concerned with tuning the external antenna. You are also connecting a U.FL connector for the purpose of this tuning exercise and are concerned with making the trace to the U.HL matched to 50 ohms. Additionally you expressed some confusion as to the procedure for tuning the on board antenna. "
I am not sure if it is a typo or not but I mentioned that I am using the internal antenna and not the external antenna and am primarily concerned with tuning the internal antenna. Can you clarify whether this is a typo?
Please read through all the questions before answering them as some of them are based on your first response and some are based on your second response so they may contradict a bit.
I have a few more questions:
1) In your first response, you state that you recommend that I use the component footprint pad to connect the VNA to using a semi-rigid coaxial cable (pigtail) Do you have a link to such a cable and would the end of this cable be able to soldered onto the 0402 component footprint?
2) In your first response, you mention that the pigtail cable should be connected to pin 4 (2G4RF_ANT_IN) in order for me to make the S11 measurement. The S11 measurement is a reflection coefficient if I am correct. When I connect the cable to pin 4, what signal is being transmitted for me to measure power loss from. I am a bit confused here for a few reasons. The KBA shows a VNA connected through a U.FL connector which is connected to pin 5 and pin 4 is left open (it is hard to definitively tell if this is the pin that the U.FL connector is connected to). Pin 5 is 2G4RF_RF_PORT so how would connecting a U.FL connector to that pin be used to tune the internal antenna? Are the internal antenna and that RF port pin somehow internally connected?
3) Based on your first response only: Why do you recommend that I use a pigtail connector to pin 4 instead of using a U.FL connector to pin 5. Originally I thought the reason for this was because of impedance that may be introduced through the trace between the U.FL connector and pin 5. However, since there would also be impedance in the coaxial cable to the VNA itself which would be present in both cases (using a pigtail cable to pin 4 and U.FL to pin 5) this would need to be calibrated out as you mentioned. You also mentioned that the calibration process for both the pigtail connector and U.FL is the same. If this is the case why does it matter that there is impedance in the trace to the U.FL connector? Can't this just be calibrated out?
4) From your second response: You mention that the impedance of the trace to the U.FL connector does not need to be matched to 50 ohms if I am only using it to measure conducted characterization measurements. What are conducted characterization measurements? Is the trace to the U.FL connector for the BRD4302A test board for the BGM121 module matched to 50 ohms.
5) From your second response: This question may seem a little contradictory to question #3 above. You mention that if I am using a U.FL connector, I must somehow keep RF_OUT port (pin 5?) disconnected. The point you make in the first post makes a little more sense now because I can now see the reason to why I should choose a pigtail connector over a U.FL connector - in order for me to connect the U.FL connector to pin 4 (2G4RF_ANT_IN) I need to go around pin 5 (2G4RF_RF_PORT) which is very difficult since the module also has to be placed near the edge of the board. The only way I can see doing this would be to remove a connector pad for pin 5 so it is not in the way. I have a couple important questions about this. In this KBA that you linked me (https://www.silabs.com/community/wireless/bluetooth/knowledge-base.entry.html/2017/01/10/antenna_tuning_forb-R5av) is this U.FL connector connected to pin 4 (2G4RF_ANT_IN) or pin 5 (2G4RF_RF_PORT)? If it is connected to pin 4, that makes a lot of sense based on your above responses, if it is connected to pin 5, I would like to know why.
I am also a bit confused because about a month and a half ago, I made a technical review quote from Silicon Labs. I asked for my design to be checked for bluetooth signal and whether my U.FL connector was placed correctly for me to tune the PCB afterward if the internal antenna's antenna loop needed adjustment. I was told that everything "looked good" other this: "If the trace width of the U.FL connector can be reduced such that you have GND pour covering the RF trace at the edge of the PCB along with vias, then that will be better for RF signal." In this PCB version that I got reviewed, the U.FL connector was connected to pin 5 (2G4RF_RF_PORT). Wouldn't that design not work for tuning the internal antenna then? Doesn't the U.FL need to be connected to pin 4 (2G4RF_ANT_IN)?
You are correct, I made a mistake and wrote external when i meant to say internal. Sorry for the confusion on this. I have edited the post to correct this statement.
For #1, please see the cable in this link: https://www.digikey.com/product-detail/en/taoglas-limited/CAB.058/931-1391-ND/5287277. You will need to calibrate the VNA to the point this pigtail attaches to the module. This often requires temporarily shorting the the junction of the pigtail connection to ground to make the calibration. The body casing of the semi rigid cable must also somehow be soldered to the ground of your PCB as close as possible to the RF path connection. Care must be taken when soldering the casing to make sure the cable conductor is not soldered to the antenna side RF pad until after the cable casing has cooled or you will likely damage the RF pad on the PCB. This is due to when the casing is soldered the entire assembly expands and the conductor lengthens out very perceptively, but if you solder the conductor at this time, then as the cable assembly cools and shrinks, the conductor shortens and will either break the PCB pad or will break the connection inside the SMA end of the semi-rigid.
For #2, The RF port and the antenna port are not internally connected. If you connect the VNA to the RF_PORT, then you are making an impedance measurement of the rF_PORT and conversely if you attach the VNA to the Antenna port then you are making an impedance measurement of the antenna. I agree it is hard to see in the pictures in the KBA but the only way to measure the impedance of the antenna is to connect to pin 4 antenna port.
For #3, yes either a pigtail or the U.FL connector can be used since neither are going to be connected during your production build but if you can successfully solder the pigtail to the antenna pad, you are more likely to have an accurate measurement. The pigtail is easier to calibrate and measure with as it has a better quality connection whereas the U.FL may not have good stability during this kind of measurement. I.e., if you move the cable side of the U.FL, you may see a significant impact on the VNA S11 measurement that you would not with the pigtail.
For #4, I have not looked at the BRD4302A board design files and so I do not know if the trace is matched to 50 ohms impedance or not. It really doesn't matter. My statement from the earlier post is, " Note that if the U.FL is used only for conducted characterization measurements, it does not need to be matched to 50 ohms if kept less than 1 cm long". What I am saying here is that for 2.4 GHz the path losses for a trace on your design which is not matched to 50 ohms but is less than a centimeter long are minimal. If the trace is a centimeter or longer, you need to match it to 50 ohms or you will potentially incur significant path loss.
Conducted characterization means you connect measurement equipment to the RF port of the radio through a cable to accurately observe the RF performance instead of taking OTA (over the air) measurements for both transmit and receive operation. You can use these result to confirm your actual TX power output, check EVM or confirm your RX sensitivity. conversely, you can also connect an external antenna to the U.FL connector and compare it's OTA RF performance to the on chip OTA RF performance.
For #5, as stated in my earlier post, the artwork for the U.FL is not optimally placed for measuring the antenna impedance. This is because the primary purpose for the U.FL is to provide an easy way to do the conducted RF characterization or to connect an external antenna. As such the guidance you received in the portal case was for those considerations and not for antenna tuning. You can still use the U.FL to measure the antenna impedance but you will need to solder a conductor in such a way as to not connect the RF_PORT pin. If you are able to accomplish this soldering task then why not instead place the pigtail onto the antenna side of the component that connects pin 4 to pin 5?
Hope this helps,
It looks like your question #4 regarding if the BRD4302A U.FL connector trace is matched to 50 ohms is answered in the forum you posted here: https://www.silabs.com/community/wireless/bluetooth/forum.topic.html/question_on_u_flcon-RUPn
Per the answer provided there, it is matched to 50 ohms.
We don't have a link to the coaxial cable with SMA male connector.
I am not sure how you are planning to connect your board with VNA, but I think that you would be using a RF cable.
The setup in our lab is as follows:-
VNA --> VNA port Adapter to SMA female connector --> RF cable with male to male connectors on both end --> female connector to cable --> test point on the DUT.
I don't know what is the type of adapter used by your test instrument. Usually the above setup is common and might be possible that it is applicable to your setup as well.