HL2 Beta5 Update

[Steve Haynal]

Hi Group,

I've made a first cut at a the new board to board interconnect for the HL2 and 5x10cm companion card. As a reminder, we plan to use a single row 0.1 inch spaced vertical male header on the HL2 and another on the 5x10cm companion card. These headers are right at the edge of each board such that when the boards abutt they form a dual row vertical male header that can be shorted with standard jumpers, custom boards, etc. This vertical approach conserves area on both the HL2 and companion card.

For a base build, I went with a 1x20 pin header on each board. 1x40 breakable headers are common and one would only need one of these headers. Also, for shorting the two boards together, 2x20 female connectors such as this are also quite common. One can just short the pins on this connector to make a 2x20 jumper or use it in a small custom board. 20 also has many divisors so combinations of smaller headers (10, 5, 12, 8) can also be used. 

The first hole is centered 8.5mm from the side of the HL2 with the PA and 1.25mm in from the back edge. Starting with this hole, the 20 signals are:

GND

RF2 Signal

GND

GND

GND

RF3 Signal

GND

GND

GND

RF1 Signal

GND

GND

Internal TR (raw FPGA signal)

CN8 FPGA input

External TR (relay driver)

I2C SDA2

I2C SCL2

3.3 V

AIN1

AIN2

There is also an overlapping 5x2 footprint for ribbon cable connection to other companion cards. The footprint is set back slightly from the back edge to allow connection of the ribbon cable even if in a 10x10cm enclosure. The pin out of the ribbon cable counter clockwise is:

I2C SDA2

I2C SCL2

3.3 V

AIN1

AIN2

GND

GND

CN8 FPGA Input

Internal TR (raw FPGA signal)

External TR (relay driver)

Github has the latest schematic and PCB layout. Please refer to those for exact details.

Note that there are two FPGA signals provided, the internal TR and CN8 FPGA input. The internal TR does not use a relay driver as I want to expose the true FPGA signal. When used with companion cards that have the TR switch on the companion card, the internal TR is not needed as there is no relay on the HL2. This signal can then be repurposed for other uses. The CN8 FPGA input is also there for potential need/use on a companion card. Since these signals are meant for inside-the-same-enclosure use by the companion card, there is no protection. Don't connect anything to them if you don't have a need. The external TR signal, also on both connectors, is meant to drive a relay and is always switched with HL TX/RX operation.

I am working up the back side of the HL2. I will extend this 20 pin connector with a footprint for another 12 pins. These additional pins will be power (various voltages), ground as well as a few spares that can be manually wired to other free signals on the HL2 if needed. Again, these are only there for future use since the space exists. Don't use a longer connector unless you want to use these additional signals. A 20-pin connector is the minimum needed.

I've done some planning and think I can fit a 5.5/2.1mm barrel power connector on the front as well as replace CN4 with a stereo jack for CW key input. This should help make the 5x10cm layout easier as there are fewer required connectors. Since Jim thinks he can fit the HPF on the 5x10cm board, I will not add it to the HL2 unless Jim is unable to fit it.

Below is a picture. This is a first cut, so please provide any feedback soon. There is more work planned and expected.

73,

Steve

KF7O

[Sebastien F4GRX]

Hello

I find this arrangement very interesting. It also allows for stacking two boards!

Sebastien

Le 02/10/2017 à 06:32, Steve Haynal a écrit :
> Hi Group,
>
> I've made a first cut at a the new board to board interconnect for the HL2 and
> 5x10cm companion card. As a reminder, we plan to use a single row 0.1 inch
> spaced vertical male header on the HL2 and another on the 5x10cm companion
> card. These headers are right at the edge of each board such that when the
> boards abutt they form a dual row vertical male header that can be shorted
> with standard jumpers, custom boards, etc. This vertical approach conserves
> area on both the HL2 and companion card.
>
> For a base build, I went with a 1x20 pin header on each board. 1x40 breakable

> headers <https://www.pololu.com/category/134/0.1-2.54-mm-male-headers> are

> common and one would only need one of these headers. Also, for shorting the
> two boards together, 2x20 female connectors such as this

> <https://www.pololu.com/product/1037> are also quite common. One can just

> <https://lh3.googleusercontent.com/-V3gImLEDDyQ/WdHAWC8ttgI/AAAAAAAAA3Y/9fz2BCs9jT0w-PiZoYJOwoo0LkDqcv9wQCLcBGAs/s1600/hl2bb3.png>
>
>
>
>
>
>
>
>
>
> --
> You received this message because you are subscribed to the Google Groups
> "Hermes-Lite" group.
> To unsubscribe from this group and stop receiving emails from it, send an
> email to hermes-lite...@googlegroups.com
> <mailto:hermes-lite...@googlegroups.com>.
> For more options, visit https://groups.google.com/d/optout.

[Alan Hopper]

Hi Steve,

if you go for the barrel connector, can there be some way to fit a on/off switch to the case for those that like such things? It could be as simple as just a couple of holes along the +ve trace from the barrel and, between them, a point where the trace can be cut or a 0ohm link removed. Alternatively a jumpered header could be fitted. The holes/header could possibly be shared with an option to supply power to the board directly.

I like the idea of plugging rather than soldering the filter board, it makes it much easier to support in the long term if it is to be mass produced. Dealing with returns that have been soldered and unsoldered would be a pain.

73 Alan M0NNB

[James Ahlstrom]

Hello Steve,

On Monday, October 2, 2017 at 12:32:03 AM UTC-4, Steve Haynal wrote:

The first hole is centered 8.5mm from the side of the HL2 with the PA and 1.25mm in from the back edge.

This all looks excellent, but I measure the first hole at about 9.2 mm from the edge. 

Jim

N2ADR

[Steve Haynal]

Hi Sebastien,

Yes, I like the idea of being able to stack too. When I add the stereo jack to the front, I will try to accommodate ad single row stackable header there too so that there is support on both ends of the board.

73,

Steve

KF7O

[Steve Haynal]

Hi Alan,

There is no room on the exposed edges for a switch, but are you suggesting an internal power switch? A footprint option for that may be possible. With a barrel connector it should be easier to "switch" but plugging/unplugging the connector. I saw some discussion about removing the power switch on the next Hermes board...

73,

Steve

KF7O

[Steve Haynal]

Hi Jim,

Sorry, I looked at the numbers for the center of the ground surface mount pad there. If you right click on that through hole pad in KiCAD, and then select edit the pad, it will display the exact location. The y position is 130.74mm which is 140-130.74 = 9.26mm away from the edge.

73,

Steve

KF7O

[Alan Hopper]

Steve,

yep, an just an internal point that a switch could be connected to, it is not important to me, I just thought if easy it was a nice option.   I would definitely like to keep an internal power connection for some of the case options I have in mind.

73 Alan M0NNB

[Steve Haynal]

Hi Group,

Below is a picture of how the mounting holes will probably be positioned in the beta5. Note how the mounting hole at the corner near the ethernet jack will be recessed to make room for the 5.5x2.1 mm barrel jack. Since my primary goal is for HL2s to be used with the target enclosure for proper heat sinking of the PA, the mounting holes will usually not be used and so I am not very concerned. For those wishing to use mounting holes, it is usually a custom build so this configuration can be handled. Please let me know if anyone has concerns.

For the barrel jack, I am considering these part numbers, all which can be accommodated with the same footprint and are commonly available in China:

PJ-002A

PJ-002B

https://www.adafruit.com/product/373

aliexpress1

aliexpress2

Note that this footprint support connectors with both 2.1 and 2.5 internal diameter pin. The footprint I will create will accommodate the widest seen pins and and minor variation (.1 or .2mm) of pin placement. Please let me know if anyone has concerns.

To make room for the barrel connector, the ethernet jack will have to be moved down by 1.0 to 1.5 mm. This can be done without moving most of the ethernet components and with just some minor rerouting. It will impact CN4 used for CW key. CN4 will be replaced with a stereo jack with a 12.0mm width footprint which is slightly less than the room allocated for a full 2x4 ribbon cable connector (including connector not just pins). The two remaining IO from CN4 not used by the stereo jack will most likely be combined with those in CN5 in a 2x5 header. For the stereo jack, I am considering the following parts, again commonly available in China:

SJ1-352xng

adafruit

mouser

aliexpress1

I know there are some connectors that are not quite as wide, 10.2mm versus 12.0mm, but I'd like to go with the more commonly available part as I think I have the 1.8mm of space. Again, please let me know of any concerns.

73,

Steve

KF7O

[Steve Haynal]

Hi Group,

I have hopefully finalized the back connections. The first 20 pins covering the RF and most important signals for a companion card remain the same as last week. I did extend the connector by another optional 14 pins. Also, there is room on the back for an additional and optional power barrel connector footprint. I expect people to use the power connector by the Ethernet, but this is available for other builds. The barrel connector footprint also supports the same terminal block we've been using for power, but rotated 90 degrees.

A few more changes are planned. There will be some prototyping area (3x4) added near the spare signals on the additional 14 pin connector. The slow ADC block will be moved slightly to center it better and provide additional ways to connect to the analog inputs. A 6x1 connector for the mod to control power by Taka will be added to the top. Hopefully I can route the enable signals to this connector.

There are 4 spares on the optional 14 pin extension. The ideas is that some of the free FPGA signals at various spots on the HL2 can be hand wired to these spares in case we ever need more signals for the companion card or prototyping area.

The signals on the back starting with the pin at the RF connector end are:

GND

RF2 Signal

GND

GND

GND

RF3 Signal

GND

GND

GND

RF1 Signal

GND

GND

Internal TR (raw FPGA signal)

CN8 FPGA input

External TR (relay driver)

I2C SDA2

I2C SCL2

3.3 V

AIN1

AIN2

----- Start of optional 14 pins

3.3 V

3.3 V

GND

GND

Vsupply

Vsupply

Spare1

Spare2

Spare3

Spare4

Vexternal

Vexternal

GND

GND

Included is a screenshot. Github, including the .pdf schematic is updated. Refer to that for exact details.

73,

Steve

KF7O

 

[James Ahlstrom]

Hello Steve,

On Sunday, October 8, 2017 at 10:28:31 PM UTC-4, Steve Haynal wrote:

Hi Group,

I have hopefully finalized the back connections.

You probably know this already, but I was surprised to find out that a 20-pin female will not fit next to a 14-pin female.  If you want to use the extra 14 pins, you must use a 34-pin female header to join the boards.  For two female headers I have, one almost fits, but the other has a side wall 0.12 inches measured from the last pin.  Also, if 34 male pins are installed on the HL2 and you only need 20 pins, a 20-pin female will not work unless it is chosen to have a narrow side wall.  Separating the 20-pin from the 14-pin can fix this, but I doubt it is a real problem.  I just thought I would mention it.

Jim

N2ADR

[Steve Haynal]

Hi Jim,

You are right. I just tried with some PPTC062LFNB 6x2 headers I have on hand and there is just under .2 mm of extra width. I think a 34-pin female header will be hard to find. 2x13 are common as they are used on the RPi. I can convert that hole in between the two headers to a ground which may be skipped. So, those wanting to use the extension can use 2x20 and 2x13 headers and skip one hole, or a 2x34 if they can find one. Does that sound okay?

73,

Steve

KF7O

[James Ahlstrom]

Hi Steve,

Yes, that sounds okay to me.

Jim

N2ADR

[Steve Haynal]

Hi Group,

The components at the top of beta5 are pretty much finalized. I was able to route the power enable for the 3.3V and 1.8V regulators to DB9. This is to make the power on/off mod done by Taka and of interest to Alan easier to do. Those wanting to implement this mod can remove J24 and then enable power with jumper between pins 5 and 6 of DB9 or run wires from DB9 to whatever board they want to control power. A 6x1 connector is common due to Arduino use. The two 2x1 power taps for 3.3V and 1.8V have been moved to DB9 to make room for the enpwr routing. Git hub is updated. A picture of this portion of the layout below. The links on the website, including to the schematic dated 10/15/2017, are up to date. Now it is time to rework the front for the barrel connector.

73,

Steve

KF7O

 

[Steve Haynal]

Hi Group,

I've been working on the updated front IO of beta 5 and have a floor plan and implementable wire plan that I like. I wanted to share it before I do detailed routing for any feedback. As a reminder, a priority of beta 5 is improved front and back IO based on what we have learned. This includes tight interfacing to a 5x10cm filter board at the back, power moved to the front so that the unit can be easily tested without companion cards, stereo jack for CW and external switch for the 1.8V and 3.3V supplies. Since I had to do some major changes to the front to put in the power connector and stereo jack, I took this opportunity to make overall improvements. Only the IO on the periphery has changed. The core Ethernet, FPGA, ADC, Power, RF blocks all remain the same as what has been tested in beta2 and beta3.

Below is a picture of the new front floor plan. Starting at the top, there is the primary barrel power connector. This is the larger 5.5mm OD discussed. I have identical size/shape part numbers for 2.1 and 2.5 ID, but will probably go with the 2.1mm ID. I have both parts in hand and have physically checked that they can fit in the target case. One concern was that the main power pin will be within 4 mm of the side edge and touch the lip that is on the bottom of the target enclosure. I've checked this and it will not touch the lip.

Next is the ethernet jack. This is as in beta2 and beta3 except it has been moved down 1.5mm to make more room for the power connector.

The four LEDs have been moved to the center of the front and are now all on the top of the PCB. This will provide some distance between LEDs and make them easier to distinguish from a distance. I sometimes confuse LEDs on my beta2/3 as the two pairs, one on top and one on bottom are very close.

Right behind the LEDs is a single expansion connector. Several connectors have been combined into this 10x2 standard 0.1inch connector. It provides access to 6 2.5V FPGA IO, 4 3.3V LED FPGA IO, 2 3.3V I2C IO used with the Versa Chip, and 2 3.3V inputs used for CW on the stereo jack. This is 14 IO total. There will also be 2.5V, 3.3V and GND. The signals on this connector are not meant to be used outside of the enclosure and hence they are unprotected connections to the FPGA. This connector is meant for companion cards like Taka's keyer/codec card, or for more advanced 10x10cm filter companion cards the are placed directly above the HL2. One can connect to this DB1 via a standard 10x2 ribbon cable (the size of the female ribbon cable connector is considered and will fit) or Arduino stackable-style headers. Two 10x1 stackable headers may be used, or one 10x1 and two 6x1 headers (extra ground pins at each end). These are commonly available sizes used with the Arduino. This connector will not be stuffed in an assembled build but may be installed later by the owner.

Farther behind DB1 is DB12. This is another internal-only use connector that provides two LVDS pairs and two grounds. The primary purpose is to provide a high speed synchronized data link with another HL2 board in the same target case for RX and TX diversity/synchronization/MIMO use. The connector is centered such that it will align with another HL2 board and common straight 3x2 stackable headers may be used to connect the two.  Twisted pairs may also be used. This connector is still a standard 0.1 inch type so that these FPGA signals may also be used for general purpose IO if desired. There are 2 2.5V input and 2 2.5 output. This connector will not be installed in an assembled build.

Next on the front are the external clock output and input edge-launch SMA connectors. By default, these connect to external input and output on the Versa clock IC respectively. The primary purpose is to synchronize many HL2s. One HL2 will be configured as master. It produces a master clock that is fed to the next HL2. All subsequent HL2s are configured as slaves. A slave synchronized to the input clock but also passes the input clock to the output. In this way, many HL2s can be daisy chained and synchronized. Software receiving the packets will look at a clock stamp to combine data from the exact same moment in time.

A second use for these connectors is for those wishing to use a very precise external clock. One can feed a precision clock into CL1 and then use the Versa to generate the exact frequency required by the AD9866. Note that that VCO option has been removed as I don't have any interest in testing that. Instead the Versa PLL will generate an small variations in frequency required.

The 2 SMA connectors also have dual optional uFL surface mount connectors. This is to support some experiments I have in mind with FPGA clock recovery, direct clocking of the AD9866, etc. In a default assembled build, CL1 and CL2 (SMA) as well as CL7 and CL5 (UFL) will not be stuffed. They can be installed later by an interested user. The link to the UFL connector says they can be hand soldered.

Finally, there is the stereo jack connector. We can configure how this is used in software. There are only two inputs here (no output possible from the FPGA). Various combinations of CW/PTT/Keyer should be possible. Since these signals are also connected to DB1, a companion card can intercept these signals and do additional processing. The stereo jack is located at the bottom as only 2 wires need to be routed.

The front mounting holes are recessed symmetrically now to make more space at the very front.

73,

Steve

KF7O

 

  

 

[Steve Haynal]

Hi Group,

The new front IO has been routed. Github and the schematic on www.hermelite.com have been updated. Hopefully we are just a couple of weeks a way from a small (5-10 units) group buy for beta5...

73,

Steve

KF7O

[PA3GSB]

Hi Group,

I did a quotation at elecrow for pcb and assembly order.

Defined a version 2 of the radioberry, smaller dimension, hoped for cheaper components.... but the price  at elecrow is now AD9866BCPZ $53.00  (also after asking twice).

Second disappointment was the MOQ of 60, a week ago  the MOQ was 1 for the cyclone 10 LP FPGA.

73 Johan PA3GSB

RF ADC DAC

AD9866BCPZ

N

IC401

64-VFQFN EP

64

1

$53.00

RF ADC DAC

AD9866BCPZ

N

IC401

64-VFQFN EP

64

1

$53.00

[Steve Haynal]

Hi Johan,

That is very interesting. Perhaps it was harder than expected for them to build the HL2 and hence the higher prices. The HL2 bid is on the github site. As you can see, the AD9866BCPZ was a lower price but they did quote >$50 for the Cyclone IV FPGA which is almost twice as much as from Digi-Key. I did not question them on this quote as the total price was low. I suspect that they normally quote high for the largest part on the board as their way to make profit. Also, although I requested the AD9866BCPZ, the assembled boards used the AD9866BCP (small lead content). Some states in the US still allow that. Maybe they know that the EU is much stricter and hence are quoting for a true AD9866BCPZ. The Cyclone 10 LP may be a new enough FPGA that they can't yet source it in small quantities there. 

I also received a similar but slightly higher quote from www.makerfabs.com. You may want to try them or another assembly house in China. See the assembly tab on www.pcbshopper.com. 

For another assembly order from www.elecrow.com, we sent a parts kit. They describe that their web page. You may want to do that for the FPGA and AD9866. This was for another project, not the HL.

73,

Steve

KF7O

[Steve Haynal]

Hi All,

Github is updated with the latest beta5 work, including schematics. Tonight I removed B69 B71 B76 B79 and replaced these with 0 ohm resistors on my beta3. I measured low and PA power output and all looks as before. These 4 DC-blocking capacitors (or jumpers) around the PE4259 devices will be removed. The jumpers were only for testing.

73,

Steve

KF7O

[Steve Haynal]

Hi Group,

Github and www.hermeslite.com are updated with the latest beta5 work. I've added optional Ufl connectors in all the places that I think they may be useful and where they were easy to add. I am revisiting raising Vpa as I see a bit more distortion on TX with my beta3 compared to my beta2. Alan and Jack also mentioned this. I am also looking at the power supply glitches that Claudio reported.

There has been some offline discussion with Jim regarding the 10x5cm companion filter board. I'd like feedback on these two design decisions:

*** Include or do not include HPF for >=3.4MHz on the main HL2 board. I have the PCB area and FPGA signal to do this. The change would switch a single HPF in and out of just the RX chain using two PE4259s. Jim was also able to include the HPF on his board, but it is still on the combined TX/RX path so requires 5W capable relay switching as well as control signaling to remove it during TX. Some pros for having this HPF filter on the main HL2 board are that you can use smaller and less expensive parts/switches in the RX path only, and it will be available and beneficial to those wishing to use the HL2 just for receive. Most of the garbage causing ADC overload appears to be at frequencies at the lower end of the spectrum, so having the ability to attenuate these should be valuable for RX. Some cons are having PE4259s in the RX chain. They may naturally attenuate at the lowest frequencies and also have a charge pump switching frequency that shows up at ~950 Khz. See this post for measurements of these birdies. Also, it seems like a cleaner division to have the minimal necessary filtering on the HL2 (only reconstruction, antialiasing filters) and all other filtering on a dedicated filter companion card.

*** Include or do not include the K2 TR relay on default assembled builds. There will always be the option to have the TR on the main HL2 board, but in the last assembled run the user had to hand install this part. The thinking was that companion filter cards may want to cover TR switching, especially if fast PIN diode switching is used. It is hard to remove K2 from the HL2 board as there is so much ground plane in that area that heating the board becomes difficult, but it is easy to install it. In the latest schematic, one would have to remove J14 and reinstall it as J1, then install the K2 relay to enable onboard TR switching. Jim's board does not take over TR switching but relies on K2 being present. Some pros for default onboard TR switching with K2 are that it can simplify the requirements for a companion filter card. Some cons are that it complicates handling of the RX paths, as the main RX path now must also be combined with TX, and the alternate RX input for VNA use must also be routed short distances (5-10cm) and can create a branching stub on the overall RX path.

73,

Steve

KF7O

[Sebastien F4GRX]

Hello,

Since our opinion is asked, my vote is to:

- "have the minimal necessary filtering on the HL2 (only reconstruction,

antialiasing filters) and all other filtering on a dedicated filter companion

card.". Please keep that board as SDR as possible instead of attempting to build
a HAM radio only HF transceiver.

- do not install the relay, since it's easy to install but hard to remove. is it
possible to install small (0603) 0R resistors or decoupling capacitors in a SPDT
configuration to avoid the stub effect of the alternate RX path?

73's de Sebastien

Le 30/10/2017 à 06:57, Steve Haynal a écrit :
> Hi Group,
>
> Github and www.hermeslite.com are updated with the latest beta5 work. I've
> added optional Ufl connectors in all the places that I think they may be
> useful and where they were easy to add. I am revisiting raising Vpa as I see a
> bit more distortion on TX with my beta3 compared to my beta2. Alan and Jack
> also mentioned this. I am also looking at the power supply glitches that
> Claudio reported.
>
> There has been some offline discussion with Jim regarding the 10x5cm companion
> filter board. I'd like feedback on these two design decisions:
>
> *** Include or do not include HPF for >=3.4MHz on the main HL2 board. I have
> the PCB area and FPGA signal to do this. The change would switch a single HPF
> in and out of just the RX chain using two PE4259s. Jim was also able to
> include the HPF on his board, but it is still on the combined TX/RX path so
> requires 5W capable relay switching as well as control signaling to remove it
> during TX. Some pros for having this HPF filter on the main HL2 board are that
> you can use smaller and less expensive parts/switches in the RX path only, and
> it will be available and beneficial to those wishing to use the HL2 just for
> receive. Most of the garbage causing ADC overload appears to be at frequencies
> at the lower end of the spectrum, so having the ability to attenuate these
> should be valuable for RX. Some cons are having PE4259s in the RX chain. They
> may naturally attenuate at the lowest frequencies and also have a charge pump
> switching frequency that shows up at ~950 Khz. See this post

> <https://groups.google.com/d/msg/hermes-lite/tUdCDAMf7Tw/ftC8TYy3BgAJ> for

> --
> You received this message because you are subscribed to the Google Groups
> "Hermes-Lite" group.

[Graeme Jury]

Hello Steve and group,

I would favor raising Vpa even though there is not a lot of voltage headroom on the transistors. Trying to get good linearity with low voltage is challenging.

My preference is to have all filtering other than anti aliasing and voltage smoothing etc. on the dedicated filter board. This raises the options for users of the HL board including VLF and transverter operation.

Unless it is required to transmit below the HPF frequency is there any real need to switch it? Perhaps it can be permanently in circuit unless its insertion loss is too high.

I have not had any problems with noise from the PE4259's in practice. The tiny output from them is swamped by my band noise and with an aerial on I can't find the bias generator signal from them.

It is true that most of the ADC overload comes from bottom of the band signals and is cleaned up beautifully with the HPF filters but without the anti aliasing filter I think that FM broadcast would also have shown as a problem in many locations.

I vote not to have the relay mounted on the assembled board. My 10 x 10 cm board has a separate Tx and Rx chain with a diode Tx/Rx changeover switch on the output. It would mean removing the relay if fitted in order to pair with my filter. There are others who are designing filters also with separate TX and Rx paths.

My companion filter board is being built as a universal board which can be used with any exciter project and my intention is to convert my HiQSDR to an identical I2C output as that used by HL and use it on that project too but its primary design is for HL compatibility and will be modified if necessary to fit the HL final design.

Finally congratulations on the HL progress and the great job you are doing on it and ditto for the other contributers.

73, Graeme zl2apv

[James Ahlstrom]

Hello Steve and Group,

My filter board requires the K2 T/R relay to be installed.   But I think the user should install it.  Since it is easy to install and hard to remove, it should not be installed by default.

But I don't think the user should be required to remove and install SMD parts, especially 0603.  The jumper J14 connects K2 pin 8 to pin 9.  We can remove J14, and instead require the user to either install the relay, or install a wire jumper between pin 8 and 9 of K2.

Installing J1 is more of a problem.  Ideally there would be two through-hole pads and the user would install a wire jumper between them.  But there is not much space available.  But there are problems with the Rx path sharing RF2 and RF3 that we should look at first.  It is problematic to use both RF2 for receive and also RF3 simultaneously.  I may be confused here, but Steve is moving our discussion to the list to get more input.

Jim

N2ADR

[Dani EA4GPZ]

El 30/10/17 a las 09:43, Sebastien F4GRX escribió:

> Hello,
>
> Since our opinion is asked, my vote is to:
>
> - "have the minimal necessary filtering on the HL2 (only reconstruction,
> antialiasing filters) and all other filtering on a dedicated filter companion
> card.". Please keep that board as SDR as possible instead of attempting to build
> a HAM radio only HF transceiver.

Hi Sebastien and all,

As I see it, the HL2 is already a transceiver intended for HF. It has a
5W HF PA which shouldn't so useful to drive a transverter for VHF & up.
The only thing that the HL2 needs to be perfectly usable as an HF
transceiver is either a lowpass filter board or an external PA including
lowpass filter such as the Hardrock-50. My current everyday HF rig is an
HL2 beta2 and a Hardrock-50.

Of course the HL2 can have many other uses: VNA, transverter driver,
etc, but as I see it, the main intended application is a QRP HF
transceiver which can work more or less out-of-the-box (perhaps as a kit
with the user having to install some through-hole parts).

This being said, I don't necessarily like the idea of having the PE4259s
in the RX path. The benefits of the HPF in comparison to the problems of
the Peregrine switches can depend on the RF environment and whether the
user wants to use the HL2 on LF or MF.

73,

Dani.

[mall...@orange.fr]

32,46 € at fr.farnell.com by 1 (6 en stock).

[James Ahlstrom]

Hello Steve and Group,

Just to complete my thought on J1, I think J1 should be replaced by a PCB trace, and J14 should be eliminated.  I don't think the extra load of having RF3 (the optional Rx input) connected to the empty relay terminal 10 is significant.  With this change the rules are as follows:

If you choose not to install the T/R relay K2, you must install a wire jumper from pin 8 to 9 on the through-hole relay pads.  This permanently connects the power amp to RF2 for Tx and RF3 is already connected and ready for Rx.

Or you can install the T/R relay K2.  In this case all Tx and Rx signals pass through RF2 and the T/R relay.  No connection is allowed to RF3.

Note that it is never possible to make a connection to both RF2 and RF3 simultaneously if the T/R relay is installed because they are in parallel for Rx, and the cables or connection will double load the Rx path.  My filter originally brought out RF3 to the back panel, but Steve pointed out that this was an error.  If we want RF2 and RF3 to both be available, we would need an extra PE4259 and FPGA pin to switch the Rx input of the AD9866 between RF3 and the T/R relay.  Or we could use the other half of K2 to switch RF3 to the AD9866 for Tx.

Is there a use for transmitting through RF2 while simultaneously receiving on RF3?  Does Pure Signal need this?  If it is needed, I have a problem because my filter requires the T/R relay.

Jim

N2ADR

[Steve Haynal]

Hi Jim and Group,

The thinking behind having surface mount J1 and J14 is to simplify assembly. It is easier to ask the assembly house to install another 0603 jumper (since they are already in the BOM) than to install a wire. I think we can keep both J1 and J14 but have the board assembled with just J1 installed. Those wishing to use K2 then just need to install it. Those wishing to not use K2 then install a wire jumper between pins 8 and 9 of K2. Furthermore, those wishing to not use K2 and concerned about the extra load on the RX line can also remove J1. Finally, future assembled builds without K2 are possible by having the assembly house install J14 and not J1.

The INTTR signal on the back connector is now the output of the NUD3124 device. It can still be used as a 3.3V logic signal, even without K2 installed if a resistor is installed between pins 1 and 12 of the K12 footprint instead. It can drive larger loads such as relays on a companion card. It is possible to have finer control over when INTTR switches. There is a control bit already in use so that it switches always with PTT or only when PA is enabled. So, my current thinking on the use of INTTR and EXTTR are:

INTTR: Drives K2 if present. Also available as TR signal for companion cards and should be used by companion cards when a TR signal outside of the MCP23008 is required. Can be set to always switch with PTT, or only switch with PTT when the PA is enabled.

EXTTR: For external PA use only. Always switches with PTT. No pull up as the external PA will define this and it may be 5V (Hardrock 50) or 12V. Available for companion card use provided equivalent behavior is again provided for an external PA. For example, an additional NUD3124 device on the companion card after EXTTR is used by the companion card.

I'm not sure it is an error to route RF3 (optional RX) to the back on your filter board, but I do wonder about the extra loading. At 5cm or 0.5% of lambda at 10m, it is not enough to have much of a RF stub effect. It adds about 6pF of capacitance. I'm not sure about the general noise pickup. Having the HPF on RF2 in parallel with RF3 when trying to use RF3 may be the bigger problem. Here are the options I see:

• Route optional RX3 to the back for VNA and Transverter use
• Normal PA mode (RF2 for TX/RX) This has slight loading from the RF3 route provided nothing is connected externally to RF3. We are probably fine if nothing is connected to RF3.
• VNA/Full duplex transverter mode 1 (RF1 for TX, RF3 for RX) This may suffer from loading on RF3 by RF2 also being in the RX state, especially from the HPF filter. This can be avoided by making INTTR switch with PTT in this mode, but then you will have possibly lengthy constant current drain from keeping K2 engaged.
• VNA/Full duplex transverter mode 2 (RF1 for TX, RF2 for RX) Similar to Normal PA mode. RF3 is actually not needed in this mode. This mode is potentially dangerous if RF2 is accidentally left in PA TX mode. For a VNA connection, there is the risk of damaging T1 or the PE4259 switches. For a full duplex transverter connection, there is risk of damaging the RX out of the transverter. I was reading about various transverters and VNAs in amateur radio use, and this potential danger may be comparable to what others normally face and hence may be acceptable.
• Don't route optional RX3 to the back
• Normal PA mode as above.
• VNA/Full duplex transverter mode 2 as above.
• Include TR switch on companion card, post filters. Route RX3 to this TR switch. TR switching and RX loading is then similar to HL2.

I can go with any of these options for the first versions of your companion card. I expect we will learn and refine over time.

I've also thought about using the other half of K2 to switch RX. Every scenario I've thought of so far requires keeping K2 engaged when RF3 is used. I don't like the idea of sinking that much current (~50mA) for possibly extended periods of time. Maybe there are scenarios I missed?

From a manufacturing and cost perspective, I don'l like having both through hole and surface mount versions of the same relay. The surface mount versions are 50% more expensive. Builders and assembly houses will have to buy both. This adds an extra line to the BOM. We don't realize as much economy of scale savings. This is something I am willing to work on after we prove your initial filter design. I can redo the layout with through hole relays.

One purpose of RF3 was for PureSignal feedback if needed. No one has done any real experiments and I'm not sure if it is needed. There is now a U.Fl connection on the RX line that can be used for this if every desired, so I'd say RF3 is not essential.

73,

Steve

KF7O

[Alan Hopper]

Hi Steve, Jim and Group

I don't think I fully understand all the options here but pure signal will definitely work better if the rx signal read during tx is a clean sample of the pa output and not just the cross talk from earlier in the chain.  I think it is important to keep the option of feeding a signal into rx during tx

 especially with external PAs.  A quick test with my beta3 showed a 60db increase in received signal level between pa on and off which indicates that there is enough cross talk after the pa to swamp the earlier stuff so nothing extra should be needed for use without an external pa. With full power carrier an lna gain of 16 gave almost full adc range. If I understand things correctly, this means at the lowest gain of -12 a sample from a pa could be 28db over the crosstalk from the internal amp, I believe pure signal can have a useful effect with this.  Maybe without the trx relay fitted the crosstalk would be lower?

73 Alan M0NNB

[James Ahlstrom]

Hello Steve and Group,

I now understand your thinking on J1 and J14.  Installing only J1 is a good solution.  I will change my logic to use INTTR as the NUD3124 output.  I will route EXTTR directly to a connector on the back panel.  I will change all relays to through-hole parts and reroute the board accordingly.

My current thinking is to make no connection to RF3.  But I will wait for feedback from other users before I make everything final.  There is still an issue with VNA mode, but I will do my rerouting first and report back with any remaining issues.  But it seems the design for beta5 is all but final.

Jim

N2ADR

[James Ahlstrom]

Hello Steve and Group,

Here is my remaining issue with VNA.  The RF1 is the RF output for the VNA.  If I lack RF3 (optional Rx input) I must use RF2 for VNA input.  But RF2 goes through the Rx and Tx filters, so I must set all filter relays to pass-through for VNA use.  I checked the foreign (non-Quisk) program HamVNA with Wireshark, and it sets filters to 0x00.  I suspect other VNA software does the same.  So I must have filter bits 0x00 specify pass-through.  This must be a general feature of all filter boards that support VNA.  Quisk can set any filter bits it wants, but the issue is support for foreign VNA programs.

This is not a problem for me, and I can design the filters so 0x00 passes RF2 through the seven relays to the antenna connector for VNA use.  The open-short-load calibration hopefully will account for the reactance in the relays.  I can leave the HPF relay default in-line to save the relay current on Rx if I invert the I2C bit.  So my issue is solved.

Jim

N2ADR

[in3otd]

Hello,
I too don't understand all the options, a diagram with all the possible variants/connections would be nice, hi.

Regarding the TX crosstalk to the RX, I've tried desoldering the K2 relay RX pin to see how much the crosstalk changed:

with the K2 pin 10 desoldered the levels are about 10 dB lower. The RX levels are relative, not in dBm, the noise floor was at about -126 dB.
The solder around the relay pin was removed from with a manual desoldering pump and since the pin is quite smaller than the PCB metalized hole it did not make contact anymore - likely some very small capacitance between the pin and the thru hole still remains but I didn't really want to desolder the whole relay.

73 de Claudio, DK1CG / IN3OTD

[James Ahlstrom]

Hello Alan, Steve and Group,

If we want to accommodate Pure Signal and feed an Rx signal into HL2 while using Tx, we could go back to the idea of switching the Rx path to the AD9866 with the other half of the T/R relay K2.  In this case, the AD9866 Rx input is RF2 when K2 is not energized, and RF3 when it is.  So on Tx, the Rx path is RF3 as required by Pure Signal.

This can also be used by VNA.  If the VNA bit (address 0x09 bit 23) is set, the power amp is turned off and K2 is turned on but EXTTR remains off.  Then the VNA input is RF3, and the state of the filter relays no longer matters.  VNA does not require this, but it seems it might be a cleaner solution.

This scheme only applies if K2 is installed.  If it is not, the filter board will have to supply its own switching.  It also requires redesign of J1 and J14, and requires the firmware to pause RF output to allow time for K2 to switch so no power is fed into the Rx path.  I am not really sure if this is a good idea or not, as the extra internal pickup from the 5 cm path to the back panel may add internal pickup that swamps the signal applied to RF3.  Steve also objected to the current drain, but this is only incurred for VNA.  For Pure Signal K2 must switch anyway.  So I am undecided about this.

Jim

N2ADR

[Steve Haynal]

Hi Jim, Claudio, Alan and Group,

This thread may be a little confusing as Jim sent me his latest schematic and layout a few days ago and much of his discussion is how his companion card will interface with the HL2. Jim, can you share your latest work with the group? I don't have your schematic library so can not create a clean .pdf.

Regarding better PureSignal support, we really need to start experimenting with it more, both with the basic HL2 and with Jim's companion card. What I've been trying to do is make sure the HL2 has some form of accommodation for PureSignal with and without an external PA.  More details later.

Jim, I thought about your suggestion to use the other side of K2 to switch RX on RF3, but would rather not for the following reasons:

* People are concerned about pickup of internal TX when they want to apply PureSignal based on the output of an external PA. Routing yet more RX through K2 will increase this pickup. Claudio's data shows increased pickup when just using K2 as is. J1 is included so that it can be removed for those who want to reduce this pickup. For even less use of RX board trace and less potential crosstalk, RF5 (uFL) can be installed and B81 removed. This assumes that no K2 is used.

* For any additional TX feedback to RF3 for improved PureSignal, I anticipate taps with high impedance. This means the tap can be left in place and in parallel during RX through default RF2 and shouldn't have a large effect.

* For VNA use, it is still possible to "disconnect" the RX line from default RF2 by engaging K2. Current draw during VNA use doesn't bother me, but for transverter configurations I am worried about having to engage K2 for long times. (I'm not a transverter user, so those with more experience, please speak up.)

* The routing is tight in that area and would become pretty messy if I were to try this modification.

73,

Steve

KF7O

[Steve Haynal]

Hi Jim,

The firmware knows when it is in VNA mode. If this becomes an issue, we can create a default filter setting when in VNA mode. The standard Hermes VNA programs are pretty dated and I am not sure there are many users. VNA is such a specific application that I am fine with having the HL2 VNA mode only compatible with Quisk or other apps written specifically for the HL2 VNA.

73,

Steve

KF7O

[James Ahlstrom]

Hello Steve and Group,

OK on not using K2 to switch RF3.  And here is the latest schematic of my filter board Rev E.  The PCB layout is not done.  The filter board requires that the T/R relay K2 is mounted on the HL2 board.

There are seven filters and seven relays labeled Band1 to Band7.  Bands 1-6 are low pass transmit filters.  Band7 is the 3 MHz high pass Rx filter.  To place a filter in line, you write a one to the I2C interface.  Most bands will use the HPF plus a low pass filter, so the I2C byte will be 1001000 or 1000010, etc.  But the HPF must be switched out for 160 meters, so the I2C byte is 0000001.  The I2C byte 0000000 specifies that all filters are bypassed, and then RF2 just connects to the back panel through the relays and SWR bridge.  The HPF is always switched out with the INTTR signal during Tx  to avoid the filter loss and to protect the 0805 filter components.

When no relays are energized, the bands 1 to 6 are bypassed, but the HPF is in-line.  So a logic inverter is used for band 7.  Therefore, byte 0000000 activates the HPF relay, and 1001000 activates only the LPF relay.  This was done because the HPF will remain in-line most of the time for typical use, and I wanted to save the relay current of 45 ma at 3.3 volts.

I do not see a need for separate Rx and Tx filters for this board.  If you want to scan with multiple receivers, just declare a "Scan" band that specifies a filter 1000000 for 3.5 MHz and up (no relay current) or 0000000 for 100 kHz to 30 MHz (one relay current drain).  Of course, you must not transmit with these filters, so just change back to one of the HF bands for Tx.

I can still make changes, and would appreciate any comments on the design.

Steve, what is the part number of your stereo jack for the key?  If I can use the same one it will eliminate a line in the BOM.  My jack is SMD.

Jim

N2ADR

[John Williams]

Jim,

Have you given any thought to being able to jumper out your power sensing circuit so that one can be added after an outboard PA? I have not been paying attention to how you are connecting AIN1/2 at P12 to know if it can be done there. Perhaps just a couple of R0 jumpers where it is convenient to do so. What would be preferred is a 3 pin molex location that could be populated instead of the on board circuit.

I really like your board and plan to use it on my radio but prefer to have the power sense after my hardrock amp as it is on my HL1.

John - W9JSW

--
You received this message because you are subscribed to the Google Groups "Hermes-Lite" group.

To unsubscribe from this group and stop receiving emails from it, send an email to hermes-lite...@googlegroups.com.

[Graeme Jury]

Hello Jim,

I am interested to know how you are going to manage the switching of the filters in Quisk. Taking a case of wanting to scan say 80, 60, 40, and 30 M bands but transmit on 40 M band, you would need to send 0x00001000 with on Rx bit 6 = 0 switching in the 3 MHz HPF and bit 3 =1 switching in the 30/20 M LPF. Upon operating the Tx you would send 0x01000010 for bit 6 to switch out the LPF and bit 1 to switch in the 80 m LPF. This means that you need to send 0x00001000 on receive and 0x01000010 on transmit over the I2C line. I am interested in what you are proposing assigning to the band button e.g a transmit edit box and a receive edit box associated with each button where you can place the 2 different values or something similar. I keep in mind that you won't be wanting to affect the existing HiQSDR, softrock and and other users but still accommodate the need for HL to (possibly) have separate RX and TX I2C signals. If TX and RX signals are the same then existing users should not be affected and anyway won't be using I2C at this stage although I am already converting my HiQSDR to I2C so that my filters will be universal. I am not sure if you have looked at my I2C simulator where I have used checkboxes to set the bits visually but this is only one way of doing it. You would need the code off my github as the code posted was an early version and incomplete.

I like the logic and simplicity of your filter board and it is perfect for QRP but still excellent when used as a driver for a high power amplifier. I would also add that people who want more HPF's can add an external board and use the PTT signal to switch them out of circuit on TX or scan mode. To develop the logic to mate an HPF board would be very straightforward. Like John I also would like to be able to feed in the swr from an external amplifier and would be happy to solder jumpers to do so.

73, Graeme zl2apv

[Steve Haynal]

Hi Jim,

The jack I am using on the HL2 is the first from:

 For the stereo jack, I am considering the following parts, again commonly available in China:

SJ1-352xng

adafruit

mouser

aliexpress1

Even though it has extra pins, it is a very common and inexpensive jack and is footprint compatible with other jacks with fewer pins.

Why are you using a stereo jack for the external PTT? The footprint is pretty large. I think amplifiers such as the HardRock-50 use a RCA phono jack. Maybe those who use external amplifiers can weigh in on the preferred connector.

FB on your switching plans and ability to have just a single filter setting. I still plan to support both RX and TX filter settings via the two defined Alex bytes for HPF and LPF as previously discussed and hashed out on this list.

73,

Steve

KF7O

[Glenn P]

Jim,
I am not familiar with the topology you have used for the SWR detectors, eg D1 and D2.   Can you explain it pls.

What I am seeing is one section of the dual diode is providing a DC signal based on the level of the RF present and smoothed by the capacitor. What evades me is what is the 2nd diode in the pair for. It appears to be that the 2nd diode in the pair is 'shunting' that DC voltage to ground, via the 4k7 resistor.

Glenn
vk3pe

[in3otd]

Hello Glenn,
your analysis is correct, the important point is that both the rectified DC voltage and the shunting resistance provided by the second diode are temperature-dependent so the circuit provides a voltage which does not change (much) over temperature. A description of the circuit is in this article.

73 de Claudio, IN3OTD / DK1CG

[Glenn P]

Thanks for that info. Interesting idea.  Never come across it before.
Glenn
vk3pe

[James Ahlstrom]

Hello Glenn,

The reference given by Claudio is correct, and the circuit is mentioned in the data sheet for the HSMS-2825.  But a simpler way of understanding it is to look at it as a voltage divider.  We want to measure the voltage at L3.  The top of the voltage divider is a diode and resistor, and the bottom is another diode and an equal resistor.  So the op amp at the center of the voltage divider sees half the voltage at L3.  The key is that the diode drop in the two diodes is the same if the diodes are matched and the current is the same.  The HSMS-2825 is two matched diodes at equal temperature.  The current is the same if the op amp draws no current.  The current in the diodes is only microamps, so we need a quality op amp with picoamp bias.

Jim

N2ADR

[James Ahlstrom]

Hello Steve,

On Monday, November 6, 2017 at 11:42:26 PM UTC-5, Steve Haynal wrote:

Why are you using a stereo jack for the external PTT?

I used a stereo jack because I had room, and I thought the extra pin (the ring) might be useful if someone wanted to bring out another connection.  I can change to a phono jack if that is what people want.

 

FB on your switching plans and ability to have just a single filter setting. I still plan to support both RX and TX filter settings via the two defined Alex bytes for HPF and LPF as previously discussed and hashed out on this list.

I can add separate Rx and Tx filters to Quisk.  But please change the protocol document to show where the two settings go when you get a chance.

Jim

N2ADR 

[James Ahlstrom]

Hello John,

You can break the connection to the on-board power sensing by removing R12 and R15.  I will try to find room for a 2 or 3 pin header to connect AIN1/2.  Or I will provide a way to use P12.

Jim

N2ADR

[John Williams]

Thanks Jim, but on second thought, do you think it wiser to replicate your voltage sense circuit off-board and feed into your op-amp, vs directly into ain1/2 using my FR Sense board (schem attached). That way I would not have to supply an external voltage feed to the board.

Graeme - your thoughts?

John

--

[Graeme Jury]

Hello John,

I would be happy with Jim's solution and for the small cost feel that the power and swr monitoring components should be on board and simply isolated if using an external circuit. The majority of users, if the softrock usage is anything to go by, will be for a 5 watt stand alone unit probably used for whisper, FT8, JT65 or QRP etc. and will want the power monitoring incorporated. There will be a small percentage (which may be a large number) who will build up to a contest grade radio and of course they will want to monitor power and swr further up the chain which Jim's solution will allow.

Interestingly you have independently developed the same circuit as I am using in my current autotuner and it works well for me. I think your board will be a really handy board for anyone to have in their shack for a number of general purpose uses. Glenn and I keep in regular touch and are building an identical autotuner each. Glenn has done some beautiful boards heavily based on the K3NG tuner and I was intending to pick up the power and SWR from the autotuner if it is close to my amplifier and HL but it may go up my mast in the end so not so sure.

On the issue of voltage supply, all my projects have an Anderson pole power input and I mount a pair of them in parallel so I can daisy chain other external devices to the parent device with short leads with Anderson poles at each end. I am looking at 150 mm long cases for HL so will have plenty of room for larger plugs, filtering or little daughter boards.

Jim, I guess you will be reading this and you have answered my question with your response to Steve. I thought you would probably be doing something like that.

A few more thoughts than you asked for John but we haven't caught up for ages and it is good to hear from you.

73, Graeme zl2apv

[John Williams]

Hi Graeme,

Good to hear from you. My circuit is copied from the Elecraft 20W autotuner. I chose it because the sensing inductors are so easy to replicate. I guess I will continue to use it. I do have to make a update to the board to fix a silkscreen issue. Otherwise it is working great. I will likely have another 10 boards done sometime so feel free to ask if you need one or more.

Can you share some of your autotuner info?

John

[James Ahlstrom]

Hello Graeme,

On Monday, November 6, 2017 at 11:23:50 PM UTC-5, Graeme Jury wrote:

I am interested to know how you are going to manage the switching of the filters in Quisk. Taking a case of wanting to scan say 80, 60, 40, and 30 M bands but transmit on 40 M band,

My thinking is that you would add a "Scan" band and button to Quisk.  This feature currently exists.  The 40 meter band would have filter 0b1000100 and the Scan band would have filter 0b1000000.  Then you scan by switching to the Scan band, and transmit on 40 by switching to the 40 meter band.  The switching can be done by pressing the band button, or it could be under program control.  But I understand that others want different Rx/Tx filters.

I am interested in what you are proposing assigning to the band button e.g a transmit edit box and a receive edit box associated with each button where you can place the 2 different values or something similar.

I have code to replace the "IO Bus" integers on the radio Bands screen with seven check boxes, one for each bit.  This is similar to PowerSDR.  Then I will add a second column of check boxes for receive.  I see that PowerSDR numbered the bit boxes from 1 to 7, but I don't know the order in the byte.  Mine are tentatively numbered from 6 to 0, left to right, most to least significant bit.

Jim

N2ADR

[James Ahlstrom]

Hello John,

On Tuesday, November 7, 2017 at 9:34:00 AM UTC-5, John Williams wrote:

Thanks Jim, but on second thought, do you think it wiser to replicate your voltage sense circuit off-board and feed into your op-amp, vs directly into ain1/2 using my FR Sense board (schem attached). That way I would not have to supply an external 

I am not sure what you mean.  You could remove L3, R6 and R7, and feed the forward and reverse RF from your sense board directly into my diodes.   But that would require two more RF connectors on the back panel.

Jim

N2ADR

[Graeme Jury]

Hello Jim,

Yes I would agree that the numbering of the checkboxes is the most intuitive to me and probably the others. I wonder if it would be possible to put the PTT signal on bit 8? It would not need a checkbox and can be ignored by filters which don't need the information but is a good way to convey the filters required by PTT state solely via I2C. Probably providing an 8th bit checkbox would be even more versatile but not strictly necessary.

I would be interested to know if you drop the RF before the PTT signal going from TX to RX and raise it after the PTT going from RX to TX or maybe this is done in the RTL but it could affect hot switching of filters so is an issue for me.

I am getting mixed results with my diode switched filters which I am intending to use on a post HL amplifier. The through loss is not an issue with bandpass losses around .2 to .3 dB but I am rectifying the RF to get reverse bias voltage and it affects the out of band response with signal level. I may have to develop an additional dc bias voltage around 50 volts or so and I really did not want to do this as things are getting too complicated. I'm thinking of going back to building crystal sets :-)

John and I have exchanged comments on an autotuner which in my case is going to be part of a Hermes-Lite suite to make a complete station and I suspect others are working on things also associated and will be interested in mating with the Quisk software but I will continue discussion in another thread so as not to hijack this one.

73, Graeme zl2apv

[James Ahlstrom]

Hello Graeme,

On Tuesday, November 7, 2017 at 1:50:14 PM UTC-5, Graeme Jury wrote:

 I wonder if it would be possible to put the PTT signal on bit 8?

That could be done by the firmware.  Quisk can not do it because of timing and reliability.

I would be interested to know if you drop the RF before the PTT signal going from TX to RX and raise it after the PTT going from RX to TX or maybe this is done in the RTL but it could affect hot switching of filters so is an issue for me.

This must be done in the firmware to avoid hot switching the relays.  Neither my filter board nor Quisk can do it.

Jim

N2ADR

[Alan Hopper]

Hi Jim, Steve, Graeme, Group,

Am I right in assuming we are using the J16 command from the pc to set 7 of the 8 i2c filter bits with the fpga adding the tx/rx signal and in future use Alex commands for extra i2c devices ? 

I've been pondering how to handle filters from the software with multiple receivers. Tx is simple whilst we are only transmitting on one frequency at a time.  Rx is quite tricky if we want to automatically open the perfect hole in the spectrum for the selected receivers. If we don't want to set up a large table for every combination, the software needs to understand what each bit does i.e. is it a lpf,bpf or hpf and what combinations are allowed. If further decoding is done on the filter bits in hardware things get complicated as the software can no longer associate a given bit with a filter so interpolating between settings becomes hard.  I've yet to come up with something that I can easily express in a user interface, it may be that for automatic operation a large table is created by the filter designer (or keen user) that can be loaded by the software.  Jim's filter is simple to allow for (turn off hpf if any rx is lower than 80m) but generalizing that to all possible filters is an interesting challenge.

Jim, your filter looks great to me and does everything I want for a qrp rig, I'm very keen to get an early one, both to test my sw and to have fun with.

73 Alan M0NNB

[Glenn P]

Thanks Jim, yes I was aware of the voltage divider formed by the two 4k7 resistors but didn't twig to the compensation idea.
It might be a good idea to add to that schematic that substitution of the following op-amp is not recommended.
glenn

[Glenn P]

John, the autotuner is based on the work by K3NG, who never did a PCB for the project. The original design is a fully balanced ATU.  . I got interested in the idea and decided to make  PCB's for it.  Nothing as small as that by Elekraft though. I made two versions with a common control PCB and SWR head, however these are unbalanced versions only.

I ended up making a ~30W version with the L&C switching on a 100x100mm PCB and a 100W version using 2 x 100mm square pcb's.   Control board and SWR boards are both 50x100mm although the SWR board could be made a bit smaller. The unbalanced version referred too was not proceeded with after some draft pcb's were made.

The reason for the PCB sizes was economics. 100mm square boards can now be had out of China for between $2 and $5 for 10 pcs. It used to be that 50x100mm were the cheapest size. Over 100x100mm the costs rise dramatically.

While the Elekraft is very elegant and small, it uses latching relays which tend to be expensive. I settled on standard relay types like K3NG used,  that are about US$1 each or so.

The ATU uses a standard Arduino  NANO board plugged into the control board which has a number of optional indicators. 16 LED's to show the L&C selections. Also the choice of several alpha/numeric displays from stand LCD modules through to TFT colour types although the latter was never instigated by K3NG.  TFT used is a Digole which is  a smart display and only requires simple commands be sent to it.

Graeme actually wrote the tune algorithm that K3NG used.

Attached is a bit of a draft summary with pictures. 

It contains links to the K3NG original information.

Glenn

[John Williams]

Glenn,

This sounds interesting on first blush. I will respond under another thread name so not to confuse the Beta5 topic...

John

[John Williams]

Glenn,

I am keenly interested in this approach. I run a doublet that is 130 ft long fed with 300 ohm twinlead. I have it fed to a balun in my shack that then goes unbalanced to a MFJ manual tuner. This may be a good test for the tuner as I can remove the MFJ and see how it does on this sort of aerial. I will take a look at the attachment.

John

[Glenn P]

Hi John
Thats about what I run here, although I used to have a 135' dipole with balanced feed, in the new QTH I am limited to around 120', also with balanced line. It's fed from ATU via a ferrite current balun.

Attached is a drawing of the ATU. Not shown is the SWR head.  For the lower power version the two 100mm square L&C boards are replaced with a single PCB. All else remains the same including the control board, sketch etc.

I hope this is not too far off the subject. Perhaps we should have another thread.

Glenn

[Graeme Jury]

Hello John,

With the 300 ohm feeder assuming it is matching the antenna it may be better to use a balanced tuner. Glenn's design will still set up as balanced but of course more relays inductors and capacitors etc. required. I have attached my notes on the tuning algorithm so you can see where it fits in. This is the one used in my current tuner not the K3NG tuner which also works well. I will dig up some more info and if you want a real in depth study of Stockton bridges have a look here where Jeff has done an amazing job of analysing the bridge.

This should get you reading for quite a while.

73, Graeme zl2apv

[James Ahlstrom]

Hello Alan,

On Tuesday, November 7, 2017 at 3:01:24 PM UTC-5, Alan Hopper wrote:

Am I right in assuming we are using the J16 command from the pc to set 7 of the 8 i2c filter bits with the fpga adding the tx/rx signal and in future use Alex commands for extra i2c devices ? 

My current understanding is that Quisk and PowerSDR etc. will store a seven bit value for Tx and a 7 bit value for Rx for each band.  When the band is changed, the two new 7 bit values are sent to the HL2.  The firmware will write either the 7 bit Rx or Tx value to the I2C interface based on the T/R state known to the firmware.  The eighth bit is currently undefined, but it could be that the firmware will write the T/R state in this bit.  But the T/R state is available as the INTTR signal on the interface connector, so I don't know why that is useful.

The 7 bit values are arbitrary and there is no requirement that each bit corresponds to a relay.  The value could be interpreted by a microcontroller on the filter board for example.  Quisk can add extra bands with arbitrary names such as Scan, Tom, Dick, Harry, etc.  So the bands don't have to be actual ham bands.

The Tx filter value is in the protocol document as address 0x00 bits 17 to 23 inclusive.  I don't know where the Rx value is.

Jim

N2ADR

[Alan Hopper]

Jim,

thanks, I understand the arbitrary nature of the data and the fact that the fpga controls the real time selection of tx/rx filter values. My real question is how we pass these values from the pc (you are in the unique position of filter board designer and sw creator so probably have the best handle on this). The tx filter address you refer to is what I called the j16(open collector) 7 bits. I currently change these depending on tx or rx but can see there might be sync issues with this.  I'm happy to live with 'not yet defined' for now :)

73 Alan M0NNB

[James Ahlstrom]

Hello Allan,

Yes, the address 0x00 bits 17 to 23 is the J16 open collector 7 bits.  I wanted to give a full description as documentation for others, so I guess I was a bit wordy.  Quisk reads the dictionary that gives the filter setting vs band only when the band is changed, and sends the data to HL2.  Yes, there are sync issues for Rx/Tx switching by Quisk that I think are unsolvable.  But Steve plans to do it in firmware.

Jim

N2ADR

[Takashi K]

Hi all,

I propose to support ALEX HPF / LPF and manual/auto selection.

I think this will allow HL2 to be used in combination with a variety of SDR software.

ALEX manual HLP/LPF selection bit is set to 0 by default.

So HL2 firmware selects suitable HPF/LPF  according to tx and rx1, (rx2) frequencies.

If ALEX manual HLP/LPF selection bit is set to 1, HL2 firmware select HLP/LPF according to ALEX HLP/LPF bits from SDR software.

My TRX firmware supports this (not uploaded it on my git yet). The idea is same as Hermes firmware. 

73, Taka  ji1udd

[Glenn P]

Jim,
On your schematic you have  a spare output on U1. (GP7)   If you change U2 to a ULN2803 you can utilise that pin and have a spare output pin for 'something'.
glenn
vk3pe

[James Ahlstrom]

Hello Glenn,

True.  But I chose the "LV" version because it is designed for low voltages like our 3.3 volts, and has much lower saturation voltage.

Jim

N2ADR

[Glenn P]

Fair enough Jim, I hadn't even noticed the LV suffix!.  They use an NFET in the output. Rather than the darlington of the std. chip versions.
glenn


glenn

[James Ahlstrom]

Hello Glenn,

That explains the lower saturation voltage.

I can bring out the eighth bit of the I2C (U1 pin 19) to a pad even if I have no spare relay drivers.  At least then it can be used for something.  Currently it is unconnected.

Jim

N2ADR

[Glenn P]

That would be good I think, Jim.

[James Ahlstrom]

Hello John, Glenn and Group,

I made some changes to the 5x10 cm filter board.  See the attached photo and schematic.  I had to change P2 back to 20 pins due to parts availability.  The longer 24-pin P2 connector was used to add another ground, so that is available at J3 if required.  I added a connector P9 to connect an external SWR and power bridge.  I changed the EXTTR connector J4 to an RCA phono to accommodate the HardRock-50 power amp.  All relays are now through-hole because they are less expensive.  The eighth bit of the I2C is available at P13.  This board is 4-layer, and everything is tested except for the I2C.  When I get my HL2 I will test I2C and the filter response.  There are some board errors I need to correct, and there may be changes in the filter values, but I think this is the final version.

Jim

N2ADR

[John Williams]

John,

Thanks for adding the external amp facilities. Count me in on your final version...

John - W9JSW

[Glenn P]

Very Nice work Jim.

Perhaps you might consider using a through hole trim pot in your revision. Cheaper and easier to get.

glenn
vk3pe

[Sid Boyce]

Hi Jim,
Great work again.
I'm interested in one of your boards when you next order.
73 ... Sid.

On 06/12/17 14:53, James Ahlstrom wrote:
> Hello John, Glenn and Group,
>

> I made some changes to the 5x10 cm filter board.  See the attached
> photo and schematic.  I had to change P2 back to 20 pins due to parts
> availability.  The longer 24-pin P2 connector was used to add another
> ground, so that is available at J3 if required.  I added a connector
> P9 to connect an external SWR and power bridge.  I changed the EXTTR

> connector J4 to an RCA phono to accommodate the HardRock-50 power

> amp. All relays are now through-hole because they are less
> expensive.  The eighth bit of the I2C is available at P13. This
> board is 4-layer, and everything is tested except for the I2C.  When
> I get my HL2 I will test I2C and the filter response.  There are some

> board errors I need to correct, and there may be changes in the filter
> values, but I think this is the final version.
>
> Jim
> N2ADR
>
>

> --
> You received this message because you are subscribed to the Google
> Groups "Hermes-Lite" group.
> To unsubscribe from this group and stop receiving emails from it, send
> an email to hermes-lite...@googlegroups.com

> <mailto:hermes-lite...@googlegroups.com>.

> For more options, visit https://groups.google.com/d/optout.

--
Sid Boyce ... Hamradio License G3VBV, Licensed Private Pilot
Emeritus IBM/Amdahl Mainframes and Sun/Fujitsu Servers Tech Support
Senior Staff Specialist, Cricket Coach
Microsoft Windows Free Zone - Linux used for all Computing Tasks