Hermes-Lite2 Beta4 Draft Release

[Steve Haynal]

Hi Group,

I've made some draft releases for beta4. Please take a look at these files and let me know if you find anything questionable. The final beta4 release should happen this weekend.

Schematic:  https://github.com/softerhardware/Hermes-Lite2/blob/master/hardware/hl/hermeslite.pdf

Standard Build BOM: https://github.com/softerhardware/Hermes-Lite2/blob/master/hardware/hl/bom/bom.standard.pdf

Assembly House BOM: https://github.com/softerhardware/Hermes-Lite2/blob/master/hardware/hl/bom/bom.assembly.pdf

Gerbers will be released this weekend. GitHub is up to date, including KiCAD files.

Beta3 to Beta4 Change List:

** R55 now 120 Ohms to not overdrive PA.

** To adjust LED bright and connect to 3.3V supply, R30,R31,R32,R33 now DNI, R133,R134 now 270Ohm, R131,R132 now 10K.

** Added 4.7K R95 and R101 to properly switch PE4259.

** Added FB22 to reduce noise on slow ADC U13.

** Converted B118 to Q6 power decoupling and moved near Q6 to reduce noise on temperature readings.

** To increase accuracy and range, temperature and current analog signals are routed directly to slow ADC U13. R111 converted to J30 JNC. B95 to C91 100pF. R108 to 270Ohm. B93 to C90 100pF. R109 to 1K.

** As U18 will perform better for FWD/REV power on filter board, U18 and surrounding components now DNI. Can still be included if desired. R104,B67,R103,D10,R113,R115,B117,R114,D11,R116,U18,B96 now DNI.

** Since B62152A4X30 core for T3 may conduct if enamel coating of wire degrades, FEP or PFTE wire of AWG24 is specified on schematic.

** Added vias to bypass ain1 and ain2 on U18 opamp.

** B106 moved slightly to make more room for nut and bolt near LDMOS devices.

** Assembly BOM specifies no substitutions for filter caps to avoid 10M power drop.

73,

Steve

KF7O

[James Ahlstrom]

Hello Steve and Group,

On Wednesday, September 20, 2017 at 1:47:28 AM UTC-4, Steve Haynal wrote:

** As U18 will perform better for FWD/REV power on filter board, U18 and surrounding components now DNI. Can still be included if desired. R104,B67,R103,D10,R113,R115,B117,R114,D11,R116,U18,B96 now DNI.

As it stands, the AIN1 and AIN2 signals from CN7 go nowhere.  I think U18 should be removed, and AIN1 and AIN2 connected directly to U13 with only a bypass capacitor and no resistor to ground.  If the diode circuit is wanted, it must be placed on the filter board.  A resistor to ground is a problem because the usual diode detector has a high output impedance.  Even if an op amp is used, it cannot drive a capacitive load without a series resistor, and a resistor to ground at U13 will create a voltage divider.  So there is nothing left except a bypass capacitor from U13 pins 1 and 4 to ground.

Jim

N2ADR 

[Steve Haynal]

Hi Jim,

As discussed previously, beta4 is just minor changes from beta3 for those waiting for a board to build. I do not want to remove U18 on beta4 as that is making a major change in my opinion. If you check the KiCAD PCB layout and read the other point in that post:

** Added vias to bypass ain1 and ain2 on U18 opamp.

there are vias in place to jumper and bypass U18, so ain1 and ain2 on CN7 do go somewhere. U18 will be removed in the future and I don't expect beta4 builders to stuff U18.

73,

Steve

KF7O

[James Ahlstrom]

Hello Steve and Group,

On Wednesday, September 20, 2017 at 1:47:28 AM UTC-4, Steve Haynal wrote:

Hi Group,

I've made some draft releases for beta4. Please take a look at these files and let me know if you find anything questionable. The final beta4 release should happen this weekend.

I would like to propose additional changes.  Connector RF2 is the SMA RF output.  I would like to change the footprint to accept a 3-pin 0.1 inch right-angle header while keeping the SMA.  There are already 5 through holes in RF2, and I am not sure what they are for.  Perhaps for soldering on a pigtail.  The pin header needs 3 holes on 0.1 inch centers with a diameter of 1.00 mm located 4.02 mm or a bit less from the rear edge of the card.  This is an easy fit.  The other two SMAs on the back edge should be changed too.  The idea here is to slide in the filter board or any other board, and connect it without soldering.  And if vertical pin headers are installed instead, a 3-wire cable with the center hot and the two outer grounds is not a bad transmission line.

Connectors CN11 and CN12 should be moved slightly so their pins line up on a 0.1 inch grid.  They are separated by 0.213 inch and can not be accessed with a 1x4 connector.

Nothing has been done with the power connector CN2, and I really don't have any ideas to propose.  My only thought was to move to a Molex connector of the sort used on computer motherboards.  As for a power barrel, I think the 2.1 mm is more common than a 2.5 mm, but it might be that neither will fit at the front of the HL2 on the PCB.  I found a 2.1 to 1.7 mm power adapter at circuitspecialist.com, but it is currently unavailable.  I was going to add a power barrel to the filter board, but it seems odd that the HL2 main board would not have a power connector.  I personally have no problem with a panel mount 2.1 mm power barrel on the front panel with a cable to a Molex at CN2.

Jim

N2ADR

[Takashi K]

Hi Steve,

Does not Beta 4 have any Rx HPF with PE4259 ?

73, Taka  ji1udd

[Steve Haynal]

Hi Taka and Group,

I think there is some confusion regarding beta4 as we've been discussing beta4 changes and later changes at the same time. Several people have expressed a desire to order boards and build a HL2, but there are a few known problems with beta3. So I proposed making a beta4 that just fixes issues found in beta3 so that they would have less work. I don't intend to build a beta4 as it will be so similar to my beta3. I want to keep the number and scale of the changes small so that I lower the risk of introducing a bug.

Some changes I see for after beta4 are:

* Consider moving power supply connector to front and replace with a barrel connector. I am ordering a selection of barrel connectors to see how they fit and feel.

* Try to add RX-only single switchable HPF to give more headroom to ADC.

* Rethink back connections for better interfacing to 10x5cm companion cards. I am ordering a selection of single and dual row connectors to again see how they fit and feel.

* Remove U18. Consider what to do with the space. Now I am leaning towards using this space for both a ribbon cable connection to a companion card and separate single row right angle connectors for connection to a companion card that will require little space on the companion card.

* Consider if a stereo jack for a CW key can be put on the front. Replace CN4 with a jack, then expand CN5 to 5x2 connector with two additional IO?

* Consider use of UFL connectors in some locations.

If there is no interest in the currently planned beta4, I can skip it and move on to the other changes and call that new board beta4 in a few weeks.

73,

Steve

KF7O

[Steve Haynal]

Hi Jim,

All the RF connectors already accept a 3 pin 0.1 inch header via the 3 pins closest to the edge. One hole is larger as this footprint also accepts 3 pins of a standard vertical SMA connector. The larger hole does not matter for the header as it will be soldered in place. I just checked with a 3 pin header. It sounds as if you want the 3 pins farther from the edge. I can add a sixth hole so that the second row can also accept a 3 pin header. The center line for this will be 3.91 mm from the edge.  

Actually, CN11 and CN12 already do accept a 4x1 0.1 inch header easily. I just checked. I'm not sure where your 0.213 inch comes from, but if I measure center to center between adjacent holes of CN11 and CN12 on KiCAD, it is 2.86mm. This is only .32mm more than 2.54mm and small enough error that the header still fits easily. I will adjust one so the separation is exactly 2.54mm.

Moving the power connector is something for after beta4 in my mind. Again, beta4 is a small delta from beta3 just satisfy some who want a board now. As previously discussed, I want a power connector on the HL2 to facilitate testing by the assembly house without the need for a filter card. If you look at DigiKey, the number of connectors they have for each size are:

158 5.5mmx2.5mm

112 5.5mmx2.1mm

33 3.4mmx1.0mm

27 3.4mmx1.3mm

so 5.5mmx2.5mm does seem to be more common. I am ordering a selection of barrel connectors to see how they fit. I may be motivated enough to nudge the ethernet jack on the layout to make enough room available.

I am also ordering various 1.27 and 2.54 mm spaced single and dual row right angle connectors to think about how to connect to a companion filter card easily. I'd like a method like single row that does not take much room on the companion card. I am thinking about just using the extra space from freeing U18 to support both a 0.1 inch 2x4 (or larger) ribbon cable connector as well as a right angle single row on the edge for companion card connection. So stay tuned as the board to board interconnect may change.

73,

Steve

KF7O

[Steve Haynal]

Hi Group,

I've made additional changes to beta4:

** Better tie off for unused op amps in U18.

** Added C92 22uF right at T3 for better Vpa filtering.

** Added 6th hole to SMA footprint to support setback right angle 3-pin 0.1 inch connector.

** Nudged CN12 closer to CN11 to align exactly to 0.1 inch grid.

Github and the .pdf schematics are up to date. I will generate Gerber for review tomorrow evening.

73,

Steve

KF7O

[Takashi K]

Hi Steve,

For the relationship between HLv2 and the supported filter boards,
The following my understanding is right?

           HL      RxHPF
           size     on HL     official supported filter board (device and protocol)
V2b4  10x10    No      Graeme's 10x10 (ATMEGA328,1byte code for LPF/HPF)
V2.1   10x10    Yes     Jim's 10x5 (MCP23008,1byte code for LPF) and Graeme's

> ** Nudged CN12 closer to CN11 to align exactly to 0.1 inch grid.

If V2b4 does not support jim's and there is no special reason, please keep the current CN12 location on V2b4 for my 10x10 filter board. but It's not strong request.

73, Taka  ji1udd

[James Ahlstrom]

Hello Steve,

This all sounds excellent.  I was just rushing to finish my filter board so I could test the new SWR bridge.  But I can just make a small board with only the SWR bridge, connect it to my current filter board, and test that way.  The final board can wait until the interface to the HL2 main board is final.  I will probably pass on beta4 and wait for beta5.

Jim

N2ADR

[Steve Haynal]

Hi Taka,

The change in position is so small it should still be in tolerance for your board.

This is still HL2.0. There will be betas until there are no more significant changes and then it will be called 2.0.

73,

Steve

KF7O

[Steve Haynal]

Hi Group,

I've uploaded gerber files at https://github.com/softerhardware/Hermes-Lite2/tree/master/hardware/hl/gerber

They are also attached as .zip. You can use http://gerbv.geda-project.org/ to view them. Please let me know if you think there should be any changes. I will post a final version this weekend.

73,

Steve

KF7O

[Takashi K]

Hi Steve,

I understood that beta 4 is temporary and does not become final version.

Most people might wait for beta5 / final version if not so far.

73, Taka  ji1udd

[James Ahlstrom]

Hello Group,

On Thursday, September 21, 2017 at 12:21:40 AM UTC-4, Steve Haynal wrote:

I am also ordering various 1.27 and 2.54 mm spaced single and dual row right angle connectors to think about how to connect to a companion filter card easily.

I measured a 2.54 mm right angle single, and it takes 14 mm total width.  This is painful on a 50 mm board even if the space is split with the HL2.  We have more space vertically, so I was thinking about using vertical pin headers for the RF connectors.  Three pins on the HL2 and the corresponding pins on the companion boards could be connected with 2.54 mm jumpers.  This puts the pin headers close to the edge, but there is also a 5.08 mm jumper here.  We could also place two 3-position right angle pin headers back to back, join them with jumpers, and solder them down to the RF pads like a SMD.  Just a thought.

Jim

N2ADR

[Glenn P]

I am following this thread on a casual basis only. So ignore if not relevant !!

But I have some Harwin brand connectors here that might be suitable for board to board. (not RF.) Right angle dual row type. 2 rows of 6.

They appear to have a part number of M20-9880606 although this may not be current.

glenn
vk3pe

[Steve Haynal]

Hi Glenn,

That female connector does have a small footprint compared to other dual row connectors I've seen. Thanks for sharing.

73,

Steve

KF7O

[Steve Haynal]

Hi Jim,

Yes, all the 2.54 mm right angle solutions I've seen take more space than I like. Also, 1.27mm female right angle connectors do not appear to be common.

I've been thinking along the same lines as you the past few days and also think we should go vertical.  A vertical male 2.54mm headers on the HL2 and vertical male 2.54mm headers on the companion filter card can be positioned close enough to the edge such that they create a dual header when assembled. I wanted to make sure www.elecrow.com supports holes this close to the PCB edge. I thought I had seen this design rule on the site once, but haven't found it again. There are holes at 1.5mm from the edge now on the HL2 and these would have to be moved to 1.2 to 1.3mm from the edge. I think it is doable. I like this solution for the following reasons:

* It saves space on both the HL2 and companion filter card. I will still have a ribbon cable connector on the HL2 for those wishing to design a 10x10cm filter companion card.

* Those wishing a permanent solution can just "stitch" the two board together with wires.

* The two boards can be easily combined (or separated) for some runs where we want a single board v2.1. The two layouts just need to be abutted and wires drawn in KiCAD.

* 0.1inch headers are common and inexpensive.

* Inexpensive shunt jumpers can be used for those wanting to change out companion filter card in a modular fashion.

* To avoid the pain of installing 10s of jumpers, we can fabricate a small PCB that has a female connector correctly jumpered. Such boards are small and can be panelized. The cost is very low. I did something similar for the Hermes-Lite1 CV ethernet "swizzle" board. I still have a drawer full of those boards.

73,

Steve

KF7O

[Steve Haynal]

Hi Group,

Hermes-Lite 2 beta4 is now officially released. See the new releases wiki page for more details. Any one interested in building or procuring a Hermes-Lite 2 now should use this release. I do not plan to organize any group buys for this release, but others are encouraged to do so. This is a good release which mainly fixes issues found in the tested beta3 builds. See the change list. Do not let my use of "beta" scare you. I use beta in the same way Google does as described in this article.

I am working on beta5. I hope to organize another group buy of 5 to 10 assembled beta5 units in November. The goals for beta5 include:

* Consider moving power supply connector to front and replace with a barrel connector. I am ordering a selection of barrel connectors to see how they fit and feel.

* Try to add RX-only single switchable HPF to give more headroom to ADC.

* Rethink back connections for better interfacing to 10x5cm companion cards. I am ordering a selection of single and dual row connectors to again see how they fit and feel.

* Remove U18. Consider what to do with the space. Now I am leaning towards using this space for both a ribbon cable connection to a companion card and separate single row right angle connectors for connection to a companion card that will require little space on the companion card.

* Consider if a stereo jack for a CW key can be put on the front. Replace CN4 with a jack, then expand CN5 to 5x2 connector with two additional IO?

* Consider use of UFL connectors in some locations.

* See how much testing elecrow is willing to do, and try to have them do at least some testing on the next assembled run.

* See if elecrow will ship directly to a customer.

73,

Steve

KF7O

On Thursday, September 21, 2017 at 9:03:21 PM UTC-7, Steve Haynal wrote:

Hi Group,

[Heikki Ahola]

Steve,

I am looking forward to the beta5 release and would like to join the anticipated group buy. 

73 de Heikki (OF2LZI/OH2LZI) 

[James Ahlstrom]

Hello Steve,

On Sunday, September 24, 2017 at 2:19:02 AM UTC-4, Steve Haynal wrote:

* To avoid the pain of installing 10s of jumpers, we can fabricate a small PCB that has a female connector correctly jumpered. Such boards are small and can be panelized. The cost is very low. I did something similar for the Hermes-Lite1 CV ethernet "swizzle" board. I still have a drawer full of those boards.

I really like this idea, and there are several ways to proceed.  We could place 1-row male pins spaced 1.27 mm from the board edge, and plug in a 2-row female with a top jumper board on the pins.  But I am worried about getting the male pins perfectly vertical since it is hard to drop in the assembly and solder from the top.  We could place the 1-row pins a bit farther back from the edge and use two 1-row female sockets and a slightly wider jumper board.  We would solder the male pins as vertical as possible, mate the sockets, drop on the jumper board, and solder on the top.  Another variation is to use 2-row male pins and 2-row sockets with a jumper board.  The advantage here is that two-row pins are easier to get vertical, and the pins accommodate a ribbon cable if desired.  But there are 1-row ribbons too, so maybe that doesn't matter.  Some variation of this will certainly work at CN7.  I am less sure about the RF connection.  I never used pins at RF, but maybe it will work.

I see that the 5x10 cm filter board must have a design requirement that the CN7 connections are directly across from the HL2 CN7 so that it is easy to make a 10x15 cm HL2.1 board.

But I have come to believe that my idea of moving the 3 MHz HPF to the HL2 is a mistake.  This moves the high pass Rx filter to the HL2, but in the past we had designs with multiple HPFs.  For example, an 8 or 12 MHz HPF for 20 meters to remove foreign broadcast interference in Europe.  Graeme is working on a design with multiple Rx filters.  My previous 5x10 cm filter had a 3.4 MHz HPF on board, and I could go back to that.  But the Rx filter must be switched out for Tx.  So I am now thinking of a design with the T/R relay on the filter board along with a single Rx filter.  I think that makes for a cleaner interface with HL2.  But before recommending this change I will open a new topic about add-in boards in general so that we are sure we can accommodate boards that are not filters.

Jim

N2ADR

[Sid Boyce]

Hi Steve,
I'd like to join the group buy.
73 ... Sid.

On 24/09/17 07:32, Steve Haynal wrote:
> Hi Group,
>

> Hermes-Lite 2 beta4 is now officially released. See the new releases
> wiki page
> <https://github.com/softerhardware/Hermes-Lite2/wiki/Releases> for

> more details. Any one interested in building or procuring a
> Hermes-Lite 2 now should use this release. I do not plan to organize
> any group buys for this release, but others are encouraged to do so.
> This is a good release which mainly fixes issues found in the tested

> beta3 builds. See the change list
> <https://github.com/softerhardware/Hermes-Lite2/tree/master/hardware/hl/releases/hl2p0beta4>.

> Do not let my use of "beta" scare you. I use beta in the same way

> Google does as described in this article
> <http://www.slate.com/articles/news_and_politics/recycled/2009/07/why_did_it_take_google_so_long_to_take_gmail_out_of_beta.html>.

> I've uploaded gerber files atÂ
> https://github.com/softerhardware/Hermes-Lite2/tree/master/hardware/hl/gerber
> <https://github.com/softerhardware/Hermes-Lite2/tree/master/hardware/hl/gerber>
> They are also attached as .zip. You can useÂ
> http://gerbv.geda-project.org/ <http://gerbv.geda-project.org/> to

> view them. Please let me know if you think there should be any
> changes. I will post a final version this weekend.
>
> 73,
>
> Steve
> KF7O
>
>

> --
> 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

[Steve Haynal]

Hi Jim,

To make these two single headers straight, one can solder them as a pair. Connect the two single row male headers together with jumpers or female dual row connector, insert them into both HL2 and the filter board at the same time, then solder. This header will not be stuffed by the assembly house so different users can customize the back and front to their liking.

I think we should plan on a distance of 1.2 to 1.25mm from the edge so there can be a very small tolerance gap between the boards. The HL2 is already not exactly 10cm in length but just under that for similar tolerance reasons.

73,

Steve

KF7O

[James Ahlstrom]

Hi Steve,

On Wednesday, September 27, 2017 at 12:18:00 AM UTC-4, Steve Haynal wrote:

Connect the two single row male headers together with jumpers or female dual row connector, insert them into both HL2 and the filter board at the same time, then solder.

I thought soldering from the top might be a problem because the pads are covered by the plastic spacer on the pins.  And the bottom is not accessible.  But let's try it.

Jim

N2ADR 

[Steve Haynal]

Hi Jim,

I was thinking these headers would be soldered in when the two boards are out of the enclosure and the bottom is accessible. There may be a little bit of balancing and support required for the two boards, but I think it should be possible.

73,

Steve

KF7O

[Takashi K]

Hi Steve, Jim and Graeme,

I think that there is a possibility that HL2 with filter can be made small form factor even with stacked 10 cm x 10 cm board by using SMD parts and low profile relay or diode switch.

Have you already considered it?

73, Taka  ji1udd

[James Ahlstrom]

Hello Taka,

I am working on a 5x10 cm filter board using SMD parts and the same relay as the HL2 uses for T/R.  I will keep everyone posted on how it is going.

Jim

N2ADR

[Takashi K]

Hi Jim-san,

OK. Sorry to disturb you.

73, Taka  ji1udd

[Steve Haynal]

Hi Taka,

Are you thinking about stacking boards with something like these stackable headers? It should be possible, but I haven't given much thought to it. I think Graeme is working on a 10x10 cm board with diode switching. I'm hoping we can have the basic 5x10cm filter board that Jim is building available soon with the HL2beta5 run. That will provide a complete transceiver, but I hope to see other companion card options created.

73,

Steve

KF7O

[Takashi K]

Hi Steve,

FYI, I have almost finished making my stacked filter board. The total height is about 30mm.

I thought that if a thin stacked filter board is made using SMD parts and low profile relay or diode switch, HLv2 and filter board might be able to be put in 100 x 105 x 30mm enclosure.

73, Taka  ji1udd

[Steve Haynal]

Hi Taka,

Very nice! Will you share this design on github? Do you notice any RX difference when you have the aluminum over the HL2 versus no aluminum? Is the AD9866 still able to cool adequately?

73,

Steve

KF7O

[Takashi K]

Hi Steve,

> Will you share this design on github?

I have already uploaded my filter board materials on my git.
For LPF/HPF parameters, I'm  using Graeme's design on his git.

> Do you notice any RX difference when you have the aluminum over HL2 versus no aluminum ?

Please refer to the attached file. 

When I attached 50 ohms dummy load to ANT terminal of my filter board, I found Rx noise on around  0.9M, 1.9M and 2.8MHz.

I guessed it came from DC-DC converter. So I added AL shield, but it was not enouph effective.

The noise was from PE4259 for Rx HPF switch. This is known issue for you. But I have not remembered it.

> Is the AD9866 still able to cool adequately ?

I have not measured AD9866 temperature yet.

I think AL shield will be useful as a part of heat sink by using thermal conductor such as  Cool Staff tube type.

73, Taka  ji1udd

[Steve Haynal]

Hi Taka,

Thanks for the information. Why does the plot with no filter board and no shield (top) look the cleanest? Was there some difference in antenna connection? Does the filter board pick up the switching power supply noise better?

73,

Steve

KF7O

[Takashi K]

Hi Steve,

> Why does the plot with no filter board and no shield (top) look the cleanest?

I'm not sure. I thought that RF trace on filter board might work as small antenna.

I did simple shield test using a microwave oven. but it seems no difference.

> Was there some difference in antenna connection?

Even in case of connecting to my LW antenna, there is still PE4259 noise.

> Does the filter board pick up the switching power supply noise better?

I checked noise source on HL2 using small loop antenna (diameter about 20mm) connecting to RF3 input,

I did not find strong noise around DC-DC converter.

73,  Taka  ji1udd