开云体育

Hi Dave,

1- I've upload the Kicad project as a zip file.
2- I also upload a PDF showing this part of the schematic and layout with different zoom levels in case you can't download or open the Kicad project.
3- The manufacturer (TE Connectivity) suggest a 3 element matching network (as pictured in the datasheet) to compensate for the final mounting conditions (plastic case). I've implemented what they suggest, leaving the pads unpopulated. I tried soldering only a series inductor. I used SimSmith software to simulate the required value.
4- For all the tests you've requested me, I've populated the series element with a 0 ohm resistor.
5- I'm in the process of modifying the schematic and layout. As a real amateur, I mixed up the transceiver pinout with a different model. When I came to fully assemble one of the boards, I realized it would have never worked.
The schematic I attached is the modified version I'm working on. I haven't moved the antenna or modified the ground plane dimension nor its shape. only the position of the LoRa module and the transmission line shape.

6- WOW ! Huge findings tonight ! I moved the ferrite decoupled coax AFTER the matching circuit, right at the antenna. Look at the pdf I have attached. The results are in the last 4 pages.
Essentially, Even with the PCB mounted in its case, the VSWR stays relatively acceptable under all across the full ISM bandwidth from 902 to 928. The response is more flat and "clean".
This suggests me there is something wrong with the transmission line in the section where there is a ground plane.

Thank you so much once again for all your dedication helping me

Nicolas

1- Would you recommend to clean all 3 elements of the matching network, as
I don't know which component will go where ?

Can you send me a schematic of the matching network? Possibly I can figure
it out. Is the matching network from the supplier or derived from you VNA
measurements?

I'm annal, but could you give me a clean S11 measurement from 902 through
928 MHz (the entire ISM band) of the unit in its case. Clearly the
dielectric of the plastic case is strongly affecting the behavior of the
antenna.

Looking at your previous postings, I can only conclude the antenna designer
developed that out of the plastic case. I seriously doubt he/she evey
evaluated the result that is published in the plastic case. I base that on
the relatively good S11 outside the case only requiring a single 10 nH
series inductor against the relatively poor S11 when inside the case.

Yet another request: Measure and send to me an S11 measurement of ONLY the
antenna. Attach the ferrite decoupled coax at the point on the PCB where
the transmitter energy is connected directly to the antenna with no
intervening components. I wat to determine how the antenna behaves both
inside and outside the plastic case.

2- If you look at the trace between the components, you'll see I made the
trace the same width as the pad. Is this a good idea ? The pad's center to
center is 4mm. The trace 0.9 wide, with a surrounding ground plane and via
fencing I treat it as a coplanar wave guide and the rest of the trace and
clearance are in accordance with that. The idea behind making the trace
between the component is to avoid width bumps.

Since these low power "transmitters" are pretty insensitive to SWR (or
reflection coefficient), I believe you did the right thing by keeping the
trace width the same as the pad for the series inductor. Of course, this
avoids an impedance bump in the path to the antenna.

3- Is my via fencing overkill putting them shoulder to shoulder ? Would a
1/10th of 1/4 wave spacing be enough for a coplanar wave guide ?

We typically use 1/10 spacing between the vias. However, that is not the
free space spacing but the spacing within the dielectric, Vp. Vp in a
dielectric goes as the reciprocal of the SQRT of the relative dielectric
constant of the dielectric medium. Since you are using FR-4, in round
numbers, the dielectric constant would be {SQRT [avg(3.8 and 4.8)]}^-1 =
{SQRT [4.3]}^-1 = 0.482. This multiplied by the free space spacing will
give you the "in-dielectric" spacing.

Yes, the via "fence" is always recommended to confine fringing fields from
propagating throughout the dielectric.

4- Could you suggest me a type of inductor in particular that would
appropriate in the 0603 package for what I'm doing ?

Typically, these days as a result of the cell phone and WiFi industries
operating up to and including 5 GHz, most of these parts are OK for the 900
MHz ISM band and through the 5 GHz ISM band. However, I still recommend
cleaning any copper from under the SM inductors and/or capacitors.

BTW, Yesterday I took a reading with the board flat outside its case. I had
installed 2 ferrite in a row along the cable. I had a VSWR of 1.19:1 all
across the bandwidth from 900 to 930MHz which is better than the spec
sheet. If only I could get below 2 while in its case...

This is why I'm requesting measurements of both the antenna only inside and
outside the case with your ferrite decoupled coax leading to the VNA.
Recently, I've had a couple of (paid) jobs where the plastic case
significantly altered the behavior of the intended antenna. You're not
alone, be rest assured.

We are finally touching on the design "gotcha's" regarding PCB design at ?W
frequencies. Possibly we should take this off the nanovna group. But,
it's still good information for those unfamiliar with these techniques.
Please let us (I'm one of the moderators of this group) if this thread bugs
anyone. It's good information for everyone concerned and certainly touches
on applications of the NANOVNA and any VNA.

Dave - W?LEV

On Thu, Mar 20, 2025 at 12:53?AM Nico via groups.io <nicolassimard=
[email protected]> wrote:

Dave,

Thanks for the hint.
1- Would you recommend to clean all 3 elements of the matching network, as
I don't know which component will go where ?
2- If you look at the trace between the components, you'll see I made the
trace the same width as the pad. Is this a good idea ? The pad's center to
center is 4mm. The trace 0.9 wide, with a surrounding ground plane and via
fencing I treat it as a coplanar wave guide and the rest of the trace and
clearance are in accordance with that. The idea behind making the trace
between the component is to avoid width bumps.
3- Is my via fencing overkill putting them shoulder to shoulder ? Would a
1/10th of 1/4 wave spacing be enough for a coplanar wave guide ?
4- Could you suggest me a type of inductor in particular that would
appropriate in the 0603 package for what I'm doing ?

BTW, Yesterday I took a reading with the board flat outside its case. I
had installed 2 ferrite in a row along the cable. I had a VSWR of 1.19:1
all across the bandwidth from 900 to 930MHz which is better than the spec
sheet. If only I could get below 2 while in its case...

Thanks,

--

*Dave - W?LEV*


--
Dave - W?LEV

Dave,

Thanks for the hint.
1- Would you recommend to clean all 3 elements of the matching network, as I don't know which component will go where ?
2- If you look at the trace between the components, you'll see I made the trace the same width as the pad. Is this a good idea ? The pad's center to center is 4mm. The trace 0.9 wide, with a surrounding ground plane and via fencing I treat it as a coplanar wave guide and the rest of the trace and clearance are in accordance with that. The idea behind making the trace between the component is to avoid width bumps.
3- Is my via fencing overkill putting them shoulder to shoulder ? Would a 1/10th of 1/4 wave spacing be enough for a coplanar wave guide ?
4- Could you suggest me a type of inductor in particular that would appropriate in the 0603 package for what I'm doing ?

BTW, Yesterday I took a reading with the board flat outside its case. I had installed 2 ferrite in a row along the cable. I had a VSWR of 1.19:1 all across the bandwidth from 900 to 930MHz which is better than the spec sheet. If only I could get below 2 while in its case...

Thanks,

Yes. When I commented "clean" the copper from beneath the inductors, I
imply no copper beneath the component(s).

Yes, that will introduce a slight impedance bump in the line. However,
even a bit of solder will do much the same. This becomes even more
critical with increasing frequency. Consider the length of even a small SM
component. Both the lands on the PCB to mount the device and the "bulk" of
the component contribute an impedance bump. Be thankful you're working at
915 MHz! My radio astronomy preamps are a challenge at even 1.42 GHz and
becomes worse as I go upward in frequency.

Dave - W?LEV

On Wed, Mar 19, 2025 at 2:09?AM Nico via groups.io <nicolassimard=
[email protected]> wrote:

Dave,

That's very interesting. That is what I came across the datasheet of the
capacitors I bought. Look at the picture, I think that's what you're
talking about. Unfortunately, it is not mentioned in the inductor
datasheet.

I tried it out tonight. Unfortunately, The match get worse (no as worse)
but in the same direction as when I've put the inductor. I didn't have an
18 gauge on hand though, only 22AWG.

When you say "clean" the ground plane, do you mean that below the
footprint occupied by the inductor, there should have no ground plane in a
"copper at all" beneath it ? In this case, doesn't it creat a return path
discontinuity for the transmission line ? I've attached a picture for
clarity.

Thanks

--

*Dave - W?LEV*


--
Dave - W?LEV

Dave,

That's very interesting. That is what I came across the datasheet of the capacitors I bought. Look at the picture, I think that's what you're talking about. Unfortunately, it is not mentioned in the inductor datasheet.

I tried it out tonight. Unfortunately, The match get worse (no as worse) but in the same direction as when I've put the inductor. I didn't have an 18 gauge on hand though, only 22AWG.

When you say "clean" the ground plane, do you mean that below the footprint occupied by the inductor, there should have no ground plane in a "copper at all" beneath it ? In this case, doesn't it creat a return path discontinuity for the transmission line ? I've attached a picture for clarity.

Thanks

Since you are dealing with SM inductors, I remembered something I've
learned and practiced for a couple of decades. In mounting SM inductors it
matters how they are constructed internally. The suppliers do not publish
this data. As such, I have always required the PCB layout engineers clean
the "ground" plane from under any and all SM inductors. Depending on the
internal construction of the SM inductor, the close proximity of planes and
traces immediately beneath the inductor will alter its characteristics and
in-place inductance. Even on 2-layer boards at microwave frequencies, this
is a concern. I may even require cleaning the common plane and all traces
from any of the layers under the SM inductors.

Instead of using your 10 nH SM inductor, a 0.5-inch of AWG #18 solid copper
wire would yield something very close to your target inductor. Install it
between the pads intended for your SM inductor and make a very wide hairpin
out of the wire. Even a hair pin will introduce additional inductance over
a linear straight conductor, so you may require a bit less than
0.5-inches.

Dave - W?LEV

On Tue, Mar 18, 2025 at 2:56?AM Nico via groups.io <nicolassimard=
[email protected]> wrote:

Roger,

Thanks for the idea. I already tried sending them an email a while ago for
that exact request ! The phone is still ringing, nobody answered yet at the
other end ;( But I should throw the fishing stick once again using my email
address from the office, that would look more serious... I'll let you know.

In the meantime, I've conducted one more test tonight, with interesting
but a little disappointing results. arrrrgg, I'm missing the knowledge and
there may be something obvious I don't get. Maybe someone has the right
batteries to fit my torch !

I've cut on end of a 36" long RG316. I soldered it to the PCB. I
reinstalled the pcb in its case and made the cable going through a hole on
the underside. Straight out the box I wrapped the cable 3 times around a
Fair-Rite 61 material that has a 0.9" inside diameter. I connected this to
another 12" premade cable then to the VNA just to give me some length. That
is for sure, I took the time to calibrate OSL right before mounting all
that. BTW the load has been done a 50 Ohm 0603 chip resistor at 0.1%
accuracy spec (at 3$ a piece !!).

Picture 1 : Test setup (the same as all my other tests)
Picture 2 : Measurement in this condition (no matching network, only a 0
ohm resitor to pass through)
Picture 3 : Data from the VNA plotted in SimSmith,
Picture 4 : Expected reading (or close) after putting a 10nH in series.
Picture 5 : Actual reading I got after installing the inductor.

Every time I tried to correct/match the antenna it gave me horrible
results like that. There must be something obvious I don't see.

At the end, I do not expect to achieve the 1.5 VSWR flat as in the
datasheet. It is a personal project after all. But if I could at least
match it down to 2, I would be more than happy. This module will be
installed in my backyard and the receiver will be at less than 50 feet. It
is more a matter of learning new things. The one thing I want to avoid
though, is to make it work by pure luck without knowing why.

I'm searching for a needle in the haystack, can someone lend me a metal
detector please !!

Nico

--

*Dave - W?LEV*


--
Dave - W?LEV

Roger,

The only thing I can think of right now, may be in relation with the fact even though I ordered my inductor / capacitor design kit for RF, the test frequency of the inductors is 100MHz. The curve from the datasheet shows it is fairly flat up to 1GHz but right above the chart it is written "typical value". Maybe I should try out component specifically tested for 800MHz as you mentioned.

Nico

Roger,

Thanks for the idea. I already tried sending them an email a while ago for that exact request ! The phone is still ringing, nobody answered yet at the other end ;( But I should throw the fishing stick once again using my email address from the office, that would look more serious... I'll let you know.

In the meantime, I've conducted one more test tonight, with interesting but a little disappointing results. arrrrgg, I'm missing the knowledge and there may be something obvious I don't get. Maybe someone has the right batteries to fit my torch !

I've cut on end of a 36" long RG316. I soldered it to the PCB. I reinstalled the pcb in its case and made the cable going through a hole on the underside. Straight out the box I wrapped the cable 3 times around a Fair-Rite 61 material that has a 0.9" inside diameter. I connected this to another 12" premade cable then to the VNA just to give me some length. That is for sure, I took the time to calibrate OSL right before mounting all that. BTW the load has been done a 50 Ohm 0603 chip resistor at 0.1% accuracy spec (at 3$ a piece !!).

Picture 1 : Test setup (the same as all my other tests)
Picture 2 : Measurement in this condition (no matching network, only a 0 ohm resitor to pass through)
Picture 3 : Data from the VNA plotted in SimSmith,
Picture 4 : Expected reading (or close) after putting a 10nH in series.
Picture 5 : Actual reading I got after installing the inductor.

Every time I tried to correct/match the antenna it gave me horrible results like that. There must be something obvious I don't see.

At the end, I do not expect to achieve the 1.5 VSWR flat as in the datasheet. It is a personal project after all. But if I could at least match it down to 2, I would be more than happy. This module will be installed in my backyard and the receiver will be at less than 50 feet. It is more a matter of learning new things. The one thing I want to avoid though, is to make it work by pure luck without knowing why.

I'm searching for a needle in the haystack, can someone lend me a metal detector please !!

Nico

Nico,

After reviewing the data sheet that you posted earlier I see that Linx does offer customer support for this antenna. They state that they can supply PCB layout files and recommend matching network components. Since they are the designers of the antenna I suggest that you contact them and have them review your layout and see if they have any testing and matching network suggestions for you. Let us know how it works out for you with this project.

Roger

If I get you correctly, that is the "skin" current that gets radiated from
the antenna as pure RF ? If so, that remaining common mode current is
reflected back at the source and then "recombine" at the connector to be
read as "raised noise" or reflected power ? Can I see it this way ?

RF energy that is intended to be radiated from the antenna all reduces as
fields inside the coax. Fields between:

1) The inner surface of the outer shield, and

2) The outer surface of the center conductor.

The internal fields carry the RF power.

What is referred to as the common mode current travels on the outside
surface of the outer shield.

If I'm still correct, then the 2-3 turns around the ferrite will "trap"
this third wire current and give me a more accurate reading ?

A few turns through the toroid will not "trap" RF energy on the outer
surface of the shield, but it will prevent energy from the antenna inducing
current on the outer surface of the shield. As such, your coax will become
isolated from the assembly. Of course, there will be no effect on fields
internal to the coax. There will be a small amount of "trapping" due to
losses in the ferrite. Some ferrites are designed specifically for loss.

In the last test I did, I had wrapped one ferrite at each end of the cable
for 2 turns. When I put my hands on coax, I could see that I got almost no
" hand touching" effect on the VNA. Well, I want to thank you for this
advice because it really helped me.

Your result is just what we were striving for. There is little or no
interaction between the assembly/antenna and the outer surface of the
shield. Excellent!

Now, here are the inductors and capacitors I bought.

Wurth Electronics 0603 RF inductor designer's ket


RF and microwave 0603 capacitor kit


Excellent!

As for all the previous test I made in the last few days, each and every
time I tried to add a matching inductor and/or capacitor, it did not
helped. My measurement got to the other side of the spectrum. This leads me
to think that as exactly as you pointed out, my measurement accuracy is
distorted.

With a few turns through your toroids at each end of the coax, the impact
of the matching network may become more observable and not disturbed by
grabbing the coax.

I'll make some other testing with my smaller ferrite with 3 turns instead
of 2 as close as I can to the insertion point and get back to you with some
results.

I don't know much I can thank you enough for all the time you take helping
me out. It is truly appreciated.

Just glad to help and apply what I've learned over some 60+ years to help
others.

Dave - W?LEV


On Sun, Mar 16, 2025 at 6:17?PM Nico via groups.io <nicolassimard=
[email protected]> wrote:

@Roger And @Dave,

If I get you correctly, that is the "skin" current that gets radiated from
the antenna as pure RF ? If so, that remaining common mode current is
reflected back at the source and then "recombine" at the connector to be
read as "raised noise" or reflected power ? Can I see it this way ?

If I'm still correct, then the 2-3 turns around the ferrite will "trap"
this third wire current and give me a more accurate reading ?

In the last test I did, I had wrapped one ferrite at each end of the cable
for 2 turns. When I put my hands on coax, I could see that I got almost no
" hand touching" effect on the VNA. Well, I want to thank you for this
advice because it really helped me.

Now, here are the inductors and capacitors I bought.

Wurth Electronics 0603 RF inductor designer's ket



RF and microwave 0603 capacitor kit



As for all the previous test I made in the last few days, each and every
time I tried to add a matching inductor and/or capacitor, it did not
helped. My measurement got to the other side of the spectrum. This leads me
to think that as exactly as you pointed out, my measurement accuracy is
distorted.

I'll make some other testing with my smaller ferrite with 3 turns instead
of 2 as close as I can to the insertion point and get back to you with some
results.

I don't know much I can thank you enough for all the time you take helping
me out. It is truly appreciated.

Nic

--

*Dave - W?LEV*


--
Dave - W?LEV

@Roger And @Dave,

If I get you correctly, that is the "skin" current that gets radiated from the antenna as pure RF ? If so, that remaining common mode current is reflected back at the source and then "recombine" at the connector to be read as "raised noise" or reflected power ? Can I see it this way ?

If I'm still correct, then the 2-3 turns around the ferrite will "trap" this third wire current and give me a more accurate reading ?

In the last test I did, I had wrapped one ferrite at each end of the cable for 2 turns. When I put my hands on coax, I could see that I got almost no " hand touching" effect on the VNA. Well, I want to thank you for this advice because it really helped me.

Now, here are the inductors and capacitors I bought.

Wurth Electronics 0603 RF inductor designer's ket


RF and microwave 0603 capacitor kit


As for all the previous test I made in the last few days, each and every time I tried to add a matching inductor and/or capacitor, it did not helped. My measurement got to the other side of the spectrum. This leads me to think that as exactly as you pointed out, my measurement accuracy is distorted.

I'll make some other testing with my smaller ferrite with 3 turns instead of 2 as close as I can to the insertion point and get back to you with some results.

I don't know much I can thank you enough for all the time you take helping me out. It is truly appreciated.

Nic

When you use a coaxial cable the RF current goes up and down the center
conductor and the inner surface of the coax shield. The reason I say inner
shield is that due to the "skin effect" the RF current only travels on the
surface of the inner surface of the shield and slightly below the surface.
The outer surface is effectively isolated and acts like a "third wire".

You are correct. A coaxial cable is really a 3-conductor topology for RF
energy.

1) The inner portion of the center conductor which only supplies
"bulk" to the conductor
and really does nothing for conducting RF energy.

2) The outer surface of the center conductor which conducts RF energy
(skin depth).

3) The inner surface of the shield which conducts RF energy (skin
effect).

4) The outer surface of the shield which only supplies "bulk" to the
conductor and really
does nothing for conducting internal energy. However, if not
correctly decoupled, may
carry common mode currents which distort antenna patterns and
introduce noise to the
receiving system (degrade receiver noise floor).

Now in your case you have the following. You have a microstrip
transmission line and only one side is connected to your helical radiator.
So what is the return path of the RF current? It is the ground side of the
microstrip which is connected to the ground plane. So your antenna
consists of the helical radiator and the other half is the transmission
line ground side and PCB ground plane. Both are radiating RF.

All correct.

When you connect your RG316 cable and nanoVNA the RF current flows on the
inner conductor and inner surface of the shield. The outer surface is
attached to the ground plane so it will radiate as well and is part of the
antenna system. When you wrap the coax around a ferrite you do not affect
the current flowing inside the coax - only the current on the outer shield
is reduced. The current flowing on the outer surface is known as "common
mode current" The common mode current reduction is due to the complex
impedance (R + X) of the inductor which is effectively in series with the
outer shield surface. If you google "braid breaker", "current balun" or
"RF Choke" you will find more info on this subject.

For your application I'd recommend a current choke consisting of 2 to 3
turns loosely spaced of your RG-316 on a small (1" OD or so) 61 material
ferrite toroid. Place this immediately at the connection of the coax braid
to the PCB with absolutely minimal pigtail.

Dave - W?LEV


On Sat, Mar 15, 2025 at 6:34?PM Roger Need via groups.io <sailtamarack=
[email protected]> wrote:

On Fri, Mar 14, 2025 at 08:39 PM, Nico wrote:

It took me a few reading of your two last replies but I think I got it.

If I

understand correctly, the shield of my coax is now integral part of the
antenna system as it is connected to the ground pad which is the antenna

and

system ground and also the ground plane. In this case then, how will I

ever

achieve an accurate reading ?

When you use a coaxial cable the RF current goes up and down the center
conductor and the inner surface of the coax shield. The reason I say inner
shield is that due to the "skin effect" the RF current only travels on the
surface of the inner surface of the shield and slightly below the surface.
The outer surface is effectively isolated and acts like a "third wire".

Now in your case you have the following. You have a microstrip
transmission line and only one side is connected to your helical radiator.
So what is the return path of the RF current? It is the ground side of the
microstrip which is connected to the ground plane. So your antenna
consists of the helical radiator and the other half is the transmission
line ground side and PCB ground plane. Both are radiating RF.

When you connect your RG316 cable and nanoVNA the RF current flows on the
inner conductor and inner surface of the shield. The outer surface is
attached to the ground plane so it will radiate as well and is part of the
antenna system. When you wrap the coax around a ferrite you do not affect
the current flowing inside the coax - only the current on the outer shield
is reduced. The current flowing on the outer surface is known as "common
mode current" The common mode current reduction is due to the complex
impedance (R + X) of the inductor which is effectively in series with the
outer shield surface. If you google "braid breaker", "current balun" or
"RF Choke" you will find more info on this subject.

--

*Dave - W?LEV*


--
Dave - W?LEV

On Fri, Mar 14, 2025 at 08:39 PM, Nico wrote:

It took me a few reading of your two last replies but I think I got it. If I
understand correctly, the shield of my coax is now integral part of the
antenna system as it is connected to the ground pad which is the antenna and
system ground and also the ground plane. In this case then, how will I ever
achieve an accurate reading ?

When you use a coaxial cable the RF current goes up and down the center conductor and the inner surface of the coax shield. The reason I say inner shield is that due to the "skin effect" the RF current only travels on the surface of the inner surface of the shield and slightly below the surface. The outer surface is effectively isolated and acts like a "third wire".

Now in your case you have the following. You have a microstrip transmission line and only one side is connected to your helical radiator. So what is the return path of the RF current? It is the ground side of the microstrip which is connected to the ground plane. So your antenna consists of the helical radiator and the other half is the transmission line ground side and PCB ground plane. Both are radiating RF.

When you connect your RG316 cable and nanoVNA the RF current flows on the inner conductor and inner surface of the shield. The outer surface is attached to the ground plane so it will radiate as well and is part of the antenna system. When you wrap the coax around a ferrite you do not affect the current flowing inside the coax - only the current on the outer shield is reduced. The current flowing on the outer surface is known as "common mode current" The common mode current reduction is due to the complex impedance (R + X) of the inductor which is effectively in series with the outer shield surface. If you google "braid breaker", "current balun" or "RF Choke" you will find more info on this subject.

@Dave :

Thanks, 1.86:1 was before I put the PCB into its final plastic case. Then within the case it jumped to 2.6. That's when I calculated the corresponding matching values. I've put an 8.2nHload inductor and a 3.9pF series capacitor. The resulting reading is on the 9th picture. It jumped the other way around. I think it has to do with what Roger says.

@Roger : It took me a few reading of your two last replies but I think I got it. If I understand correctly, the shield of my coax is now integral part of the antenna system as it is connected to the ground pad which is the antenna and system ground and also the ground plane. In this case then, how will I ever achieve an accurate reading ?

Thanks

Further addressing small values of inductance: There is really no need to
buy SM inductors which may or may not be apropriate. Small nH inductors
can easily be made of short lengths of appropriate single conductors. For
example and one I always remember is that AWG #18 solid copper wire
exhibits 18.1 nH / inch. The following calculator may be of use for this
purpose:



Dave - W?LEV

On Fri, Mar 14, 2025 at 8:51?PM Roger Need via groups.io <sailtamarack=
[email protected]> wrote:

Nico,

So you have two issues here...

Th first one is that you will have difficulty knowing what the impedance
is near the matching network because your measuring system is affecting the
results. That was the point of my previous post.

The second is that even if you knew precisely what impedance you are
trying to match inductors and capacitors at 916 MHz. will not have the same
values as they do at lower frequencies. An inductor will have series
resistance that increases with frequency and parallel capacitance. A
capacitor will have lead inductance. So you need to purchase components
that have been characterized at 900 MHz.

--

*Dave - W?LEV*


--
Dave - W?LEV

Nico,

So you have two issues here...

Th first one is that you will have difficulty knowing what the impedance is near the matching network because your measuring system is affecting the results. That was the point of my previous post.

The second is that even if you knew precisely what impedance you are trying to match inductors and capacitors at 916 MHz. will not have the same values as they do at lower frequencies. An inductor will have series resistance that increases with frequency and parallel capacitance. A capacitor will have lead inductance. So you need to purchase components that have been characterized at 900 MHz.

On Fri, Mar 14, 2025 at 04:00 AM, Nico wrote:

Look at the picture and zoom it (not zoomed it does not show up properly),
you'll see a blurred larger line around the feedline. This is the return path
or, the other half of the transmission line. This is a ground line attached to
the ground plane on layers 2 and 3. I was unsure on how to terminate it close
to the antenna attachment point, so I've just ended it close to it

Nico,

In your case the purchased helical is one half of the antenna. The other half is the "buried" side of the transmission line and the ground plane of your board. When making measurements of the antenna the outer surface of the shield of your connecting RG316 cable is now also part of the antenna. Grab the coax with your hand or attach a wire to the SMA connector nut on the VNA and you will see the SWR change. The situation is similar to what happens on a handheld radio transmitter where the operator is capacitively coupled to the radios antenna system.

You can try reducing the RF current on the coax cable with ferrites but you will not get rid of it entirely. And at this high of a frequency you will still have a considerable length of coax shield radiating until the ferrites.

The image that shows a SWR of 2.6 : 1 (the sixth image), all you need to do
is add an inductor in series to cancel the -j 45.6 ohms. At 916 MHz that
would be 7.9 nH.

In reality, 1.86 : 1 is not bad at all. For this sort of application, I'd
declare it complete.

Dave - W ?LEV

On Fri, Mar 14, 2025 at 3:05?AM Nico via groups.io <nicolassimard=
[email protected]> wrote:

Hi everyone,

No, I haven't abandoned yet ! I got my revised pcb (attached picture)
yesterday
1- Revised ground plane dimensions which I made the same as the test board
shown in the antenna datasheet.
2- Controlled impedance PREPREG material for the 4 layer PCB.
3- Revised feedline width for 50ohm target impedance
4- Revised return path width in adjacent layer
5- Fixed a jumper trace mistakenly placed in the feedline path.

I have calibrated O-S-L with a 0.1% 50ohms 0603 chip resistor soldered
directly on the end of the cable.
I have replaced my RG174 with a brand new RG316 36" extension from Digi-Key
I added a 6" piece of RG316 opened at one end and SMA connected to the
extension at the other.
I calibrated with everything attached to the VNA and finally soldered back
the open end right where the source swill be.
I have put 2 Fair-rite 61 ferrites on the cable, one at each ends.
I soldered a 0 ohm resistor to bypass the matching network

Picture 1 : New board front
Picture 2 : New board back
Picture 3 : Test measurement setup
Picture 4 : Antenna pcb feedline and return path
Picture 5 : Measurement with board laid on a wood plank (no matching)
Picture 6 : Measurement with board inside its plastic case (no matching)
Picture 7 : Calculated correction values from Sim Smith (High Pass)
Picture 8 : Installed L and C values (High Pass)
Picture 9 : Measurement with L and C installed

I think I have improved the antenna performance with the new board. Maybe
I have a better quality setup also. As you can see, once the board is
inside the box, it is not too bad. But unfortunately, I'm the kind of who
loves to chase perfection. Using the provided numbers from the nanoVNA, I
tried to compute some matching network values to better tune the antenna in
Sim Smith. I ordered 0603 inductor and capacitor dewsign kits at DigiKey.
Not those cheapy ones from Amazon. I installed L and C into my matching
network but as you'll see with the pictures, it did not helped at all.

1- Am I going too far, and should I stay with the values from the initial
measurements ?
2- What am I missing here ?
3- What would be your advices if I wanted to improve the response to
something close to like 2:1 VSWR ?
4- From here, I am really scratching my head...

--

*Dave - W?LEV*


--
Dave - W?LEV

Roger,

Thanks for this advice. I'll try it out tonight.

Look at the picture and zoom it (not zoomed it does not show up properly), you'll see a blurred larger line around the feedline. This is the return path or, the other half of the transmission line. This is a ground line attached to the ground plane on layers 2 and 3. I was unsure on how to terminate it close to the antenna attachment point, so I've just ended it close to it.

I'll post results tonight with a few turn of ferrite.

Nic

Do you have a trace inside the board to be the other half of the transmission line?

One turn through the ferrite is not enough. The impedance goes up approximately as the square of the turns.