Printed Circuit Board Next Revision

[Steve Haynal]

I have captured PCB development tasks on the github issues list prefixed with PCB.  https://github.com/softerhardware/Hermes-Lite/issues

This thread is to discuss these issues, add/remove issues, discuss what the next PCB revision should have, and find out if anyone wants to volunteer to design the next PCB revision.

[Dave Miller]

After I learn Kicad I am happy to do some work on the PCB.
I have 20 plus years designing PCB's and use Altium in day job so I should be able to figure Kicad out make some contributions.
I have looked over the issues on Github and see there are a couple of nice easy issues to get my feet wet in Kicad.

When I loaded up Kicad and the boards I noted a few errors messages about libraries not found that I need to sort out.

So if there are no other volunteers I will work away and make some of the simple changes as I start up the learning curve.

Dave
VE7PKE

[Steve Haynal]

I added the following to the PCB README:

## Additional Documentation ##

Analog Devices made a AD9866 evaluation board which is a helpful reference. The schematic is [here](http://www.analog.com/static/imported-files/eval_boards/AD9865_66_Schematics.pdf) and the layout is [here](http://www.analog.com/static/imported-files/eval_boards/AD9865_66_Layout.pdf).

Schematics and documentation for the BeMicro SDR can be found [here](http://www.alteraforum.com/forum/archive/index.php/t-30731.html)

## Assembly Experiences ##

I tried three assembly methods. At first, I thought I'd use an inexpensive stencil from OshStencils, solder paste and my infrawave toaster oven. I could never get the proper (minimum) amount of paste on the pcb because the large thermal via opening in the stencil under the AD9866 caused too much paste to be pushed under the stencil on to some pins. I scrapped this plan and went with hot air. (I have a $80 smt rework station that includes hot air. You can find them on e-bay or amazon.) I was eventually able to get hot air to work by following techniques you can find on youtube videos. The AD9866 moved around quite a bit. This prototype has problems that at different gain settings for the ADC I see excessive noise. I think I fried it during assembly. The last technique and the one I would recommend would be to slightly tin the AD9866 pads and thermal pad on the PCB with a regular iron and regular solder. Care must be taken to not use too much solder. Then, place the AD9866 and use a toaster oven to solder it in place. I then placed and soldered all the other components by hand. I choose a minimum size of 0805 to make this easy. It may be possible to place and solder the other SMT components along with the AD9866 in the toaster oven too. 

I think the last technique is within reach of most hams. You can buy an old toaster oven at a thrift shop for under $5. You can buy an oven thermometer at Wal-Mart for around $5. 

The AD9866 also requires baking at a low temperature for 24 hours to remove moisture. I also did this in the toaster oven but used too high a temperature on my first prototype. (Maybe that is why it didn't work.) With the oven thermometer, this is no problem.

## PCB ##

 * http://oshpark.com

 * http://www.hackvana.com

 * http://seeedstudio.com

 * http://elecrow.com

 * http://smart-prototyping.com

## PCBA ##

 * Seeedstudio will do PCBA if you use their open parts library

 * smart-prototyping will do PCBA and source parts for you

 * Bittele

 * http://www.myropcb.com

 * Many companies on alibaba

## Stencils ##

 * http://ohararp.com

 * http://www.oshstencils.com

[Steve Haynal]

A good article on grounding in mixed signal PCB design is http://www.analog.com/library/analogdialogue/archives/46-06/staying_well_grounded.html

I also added two PCB issues that came up during discussion with KL7NA:

* There is no flooded ground plane in vacant space on the component and solder sides. I had intended to do this but forgot.

* There may be some signals that cross over from one ground plane to another. This should be examined and care taken that signals are always referenced to one ground.

[Steve Haynal]

Two issues with using the KiCad files that have come to my attention through private emails:

* Older versions of KiCad complain about an origin error when attempting to open the pcb file. The pcb file is a text file, so just remove the offending line reported in the error message and try again.

* An OS X user has had problems with case-sensitive names in OS X that are not case-sensitive on other operating systems. I used KiCad 2014-01-02 BZR 4600 on Linux. You'll probably have the best luck on Linux with that version.

Has anyone done any work on a next PCB revision? I am currently very busy ramping up with my new job. I may do a next PCB revision in the fall if no one else has.

[george....@gmail.com]

Hi Steve,

I have included a 'trimmed' version of your Hermes-Lite schematic. I do not have a new version of Kicad and I was only able to extract a partial schematic from your package. I normally use the Linux open-source gEDA / PCB for my board work and create a gEDA schematic.
I address a few of the issues in your TODO list.

- 10dbm TX only
- 400ma regulator for the analog supply
- Dropped the PCI-E connector
- Dip-switch:  replace with a jumper block  OR hard wire selections
     mode = half duplex
     config =  ??
     pwr_dwn = ??
- SPI bus ?? do you use it, can it be feed to the FPGA bus
- The AD9866 reset is permanently powered.  Should it be controlled?

Do not fuss about the parts designation or values. I am more worried about the interconnects right now.

Regards
George

[Rob Frohne]

Hi Steve, et. al.,

I'm working on making a smaller PCB with only the necessary things on it in order to make it less expensive to get four layer boards from OHSPark.  I think T/R switching, PA, filters, etc. can be put on a two layer board later.  I plan to eliminate the PCI Express connector, the DIP switches, the extra output connector (IOUT_P), solve the heat problem with the regulator, replace the Mini-circuits transformers with hand wound, use edge launch SMA connectors, and an Alex connector, to provide T/R control and filter selection.  

I still need to decide on a power connector.  I would use a micro B USB connector, but USB ports only handle 500 mA and I want to power both the SDK and the Hermes Lite with one power cable to eliminate ground loops, and make connections easier.  Where is the signal on the BeMicro SDK that is pulled low to make it powered from an external power?

All this brings up some questions that I hope you can much more easily answer than I can reverse engineer.

1)  What are the power requirements?  It looks like about half an ampere for the AD9866, but the BeMicro SDK doesn't seem to have that data very easily accessible.

2)  There are several jumpers on the board.  Is there a reason not to make them traces?

   a) The SPI bus appears to go from connector P1 to P17.  I will replace it with traces.

   b) There is a jumper from P14 (VIN) to P13 (VIN).  Was there a good reason to have this a jumper instead of a board trace?

   c) The note about the jumper between P18 and P5 states, "The prototype requires a jumper from pad P18 to P5. This was to allow freedom regarding which FPGA pin is used for the clock. This should be routed. The clocks should all go to dedicated FPGA clock pins."  Does this mean I want a jumper to replace it or does CLOCK_OUT1 needs to go to the Connector CN1 pin 5, and not Pin 29?

   d) I assume P22 can be omitted.

3) What position did the switches at P16 end up needing to be in?

4) Are there any reasons to have any of the unused signals that went to the PCI Express connector go to anything other than an Alex connector?

5) Is there anything else I can omit, or any other good way to make the board smaller yet?

6) Since a number of us want to use the Hermes-Lite as a VNA, it seems to me that it might be good to consider terminations, so that regular reflection bridges can be used.  It seems that 200 ohms across the output transformer would be good.  If I put in a place for the resistor, it can be populated or not, depending on what our experiments yield.

Thanks,

Rob

KL7NA

[Steve Haynal]

Hello George,

Thanks for the nice schematic! Regarding the dip switch, you can connect all 3 signals to the default 0. These are power-up defaults. The settings like full or half duplex can be changed by software. The SPI is currently jumpered via the 2 4-pin headers. This was to support prototyping. It should be directly wired. See the hires picture for details. A free pin on the FPGA with pullup can be used for reset.

Good luck!

Steve

KF7O

[Steve Haynal]

Hello Rob,

I need to refer to my notes (not with me now) to give you good answers. I'll try to answer them this weekend.

Steve

[Rob Frohne]

Hi Steve, et. al.,

I got a little time to work on Hermes Lite yesterday and this afternoon.  I have a schematic of a reduced board.  It has some issues that I need to answers for at present.  Steve, I'm hoping you can give it a quick look and at comment on my issues, as well as review what I did.  I'm still waiting on power requirements to determine what connector to power it with.  I'm attaching the schematic file here.

Thanks & 73

Rob

KL7NA

[John Marvin]

Rob,

I've been meaning to ask about this, but forgot about it (I wish reply by email wasn't disabled). What do you mean by saying adding T/R switching, PA, filters, etc. can be put on a two layer board later? Are you thinking that the basic board would be a four layer board, but you would need to add a separate two layer board to make a rough equivalent to a Softrock Rx/Tx Ensemble? If so, I'm not in favor of that idea. Sure it might make the 4 layer board a little cheaper, but am I mistaken in thinking the cost of a "better" four layer board would be cheaper than the combination of having a smaller 4 layer board plus the cost of a 2 layer board? Even so, if the cost isn't significantly higher I would think the convenience of one board would be worth it.

I'm just thinking that perhaps this is penny wise and pound foolish, but you know the costs better than I do. Can you put some approximate cost numbers on this? We're obviously trying to keep costs down, but I think we still want a board that is roughly equivalent to a Softrock RX/TX ensemble in functionality, i.e. 0.5 -1 watt (or even a little more) PA, T/R switching (either relay or diode switching), and the ability to put a bandpass or low pass filter on the board. A user can choose to populate that part and restrict the output range (similar to a RX/TX) or not put it on and rely on an external filter setup or the filters in an external amp. Personally I would prefer to have one board with the flexibility to populate certain features, but that is going to take more time to design the board. So many features of Hermes are 90% or more in the fpga and only require minimal external hardware to support.

There are a variety of other simple feature that can be added for very little cost by  not populating through hole components and connectors, but providing the surface mount parts (i.e. PTT out, PTT in, Paddle/Key input, etc.). Users can then decide to populate the parts they require. Even providing the pads for more expensive surface mount components that are not populated might make sense (e.g. a TXCO).

I think it would be worth discussing some of these features before rushing to produce the next board. Does that make any sense?

John
AC0ZG

[Rob Frohne]

Hi John,

Yes, at present I'm working on a version of Steve's board without all the debugging connectors, features that Steve included "just in case he needed them".  I agree that eventually the board needs to be like the Softrock, having higher power, band specific filters for RX and TX, with functionality to be used as a VNA as well.  However, at this point, there are still a number of development issues that are unresolved, and untested.  See Steve's issues list.  In my experience, it takes several revs to get to the place you wish to be.  At this point, there are some blocks to continued large scale production, like the limited availability of the BeMicro SDK, so this version of the board will probably inherently have a limited supply.  And I have to admit, I'm picking low hanging fruit.  I actually prefer having a BeMicro SDK and the add on board, because my major goal in amateur radio anymore is learning, and that setup is better for learning than a full fledged transceiver with all the bells/whistles.  It is what is used to develop the full product, but it isn't the finished product.  Look how long and how many revisions were needed to produce the existing Softrock line of kits.  

As to the cost, I suspect I could get enough PCB's for interested developers, so that the cost using sampled parts for the connector and modem IC would be about $75 for the small circuit board and BeMicro SDK.  I'm not interested in kitting units, but I should be able to send out a limited number of PCBs that are excess to my needs to others who want to help develop/experiment with Hermes-Lite.

Your comments about other features that you would like to have available are very helpful.  It appears that I need to but a few more GPIO pins on a connector on the board to allow experimentation with Keyers, and other features I haven't thought of yet.  A TCXO could be wired into the Si510 pads, but I suspect that people who want high class features like that will want a regular Hermes.  Some more brain storming on what I should include would be excellent.  

Thanks for the note!

73,

Rob

KL7NA

[Steve Haynal]

1. The signal to connect/disconnect power is PWREN1# and PWREN2#. The details are on page 7 of the BeMicro SDK schematic. There is a PWREN# (pin 4) on the BeMicro connector. Currently, I have added a jumper to the BeMicro to pull PWREN low. I do this not to connect the two 5V supplies, but to fool the FT245RQ. I must then also connect power and ground to the USB connector as well as the SDR. (If there is no "true" USB connection, I believe the FT245RQ detects this and prevents the BeMicro SDK from functioning.)

If I were to redesign this, I would have a jumper for PWREN# on the daughterboard and also tie the 5V digital supplies between the SDR and BeMicro. (Currently they are disconnected in the prototype, but with a test pad for experimentation.) Then, you could put the jumper on to pull PWREN# low and power everything through the SDR power with no need or noise hassles of a USB connection. You can also remove the jumper and power the BeMicro via standard USB for quick programming iterations. You will need to be able to power the BeMicro via standard USB for the initial boot and programming of the EEPROM.

I measure 230-240 mA at 4.86 V for the BeMicro SDK when running 2 receivers. I think this is close to the maximum you will see. You probably should add some margin.

By the way, the NCP111/ST33TG regulators will not handle >10V input. I almost fried my prototype by connecting it to 13V. Also, they burn a lot of power in heat. I saw them being used in either the Hermes, HiQSDR or AD9866 demo board, and just went with them. Some sort of low-noise switching supply design might be better. The BeMicro does this. 

2a. The SPI bus from P1 to P17 should be wired as traces on the pcb. These connectors can be removed. They were included for flexibility during prototyping, but the FPGA SPI works find.

2b. The jumper from P14 to P13 supplies voltage to the +5V plane for the output amplifier in the AD9866. It is a jumper on the prototype to provide flexibility on what, if any, this voltage is. R6, which was just a wire in the prototype, is included because of discussion on pages 30 and 31 of the data sheet, under "IAMP CURRENT-MODE OPERATION." It says, "The transformer should be specified to handle the dc standing current, Ibias, drawn by the IAMP. Also, because Ibias remains signal independent, a series resistor (not shown) can be inserted between AVDD and the transformer's center-tap to reduce the IAMP's common-mode voltage, Vcm, and reduce the power dissipation on the IC." I used a 0 Ohm resistor for R6 but was careful to adjust my 5V supply to just bellow 5V. Also, I determined the minicircuits device could not handle this standing current, and wound my own transformer. 

Since you are using the medium output power path on the AD9866, be sure to read the section "IAMP CURRENT CONSUMPTION CONSIDERATIONS" on page 32 of the datasheet. It appears possible to exceed the device power dissipation limit, but maybe not with only the OUT_N.

2c. Regarding clocking, there are dedicated clock inputs on the FPGA, which appear on signals P1,P2,P35,P36 of the BeMicro connector. The clkout1 of the AD9866 should not connect to P12 (a generic IO) on the BeMicro connector, but should instead route to P1 (pin 1, test pad 5) of the BeMicro connector, which is a dedicated clock input. My prototype had routed to both pins, which is extra load on the clock. I never used the P12 input except for some early testing.

In full-duplex mode, "The AD986 acts as the master, providing RXCLK as an output clock that is used for the timing of both the TX[5:0] and RX[5:0] ports." (datasheet pg. 24) In my current prototype, rxclk is connected to a general I/O on the FPGA (signal P13, pin 31). This signal is a ~147 MHz clock in full-duplex (2x the 73.768 MHz) and more thought should be given to it. (It may be one of the reasons for the noise I saw when experimenting with full-duplex.) My guess is that it should be carefully routed to an FPGA dedicated clock output. Signal P54 (pin 52) for example. I don't know off the top of my head, but I'd read the relevant sections of the Cyclone IV documentation and figure out the best thing to do. You want to use a FPGA pin capable of general I/O for half-duplex operation, and one that can drive a fairly high-speed clock when in full-duplex mode.

2d. Yes, P22 can be ommitted. CLKOUT1 is the recommended output clock to use. 

3. The DIP switches pulled all 3 signals low. The various modes are described on page 19 of the datasheet. This makes half-duplex the default, but you can still switch to full-duplex by writing configuration registers via the SPI.

4. You may want to use 4 of the unused pins for a MAC/IP serial EEPROM as in the original Hermes. In the current Hermes-Lite RTL, the MAC address is hardcoded, and the IP can be hardcoded or set to use DHCP. Changing the hardcoded values requires recompilation with Quartus II. There is room on the BeMicro SDK EEPROM for these values, and eventually I'd like to use that, but it requires some work. The easiest would be to match the Hermes exactly with an extra serial EEPROM. Refer to their schematic. 

Also, you may want to expose at least a few of these pins to pads or a simple header for experiments.

5. I can't think of anything else that can be removed. I see you still have just two regulators. How are you planning to address the excessive heating I saw with the AVDD_ADC/AVDD_DAC/CLKVDD regulator? One way is to add a third regulator that drives only AVDD_ADC. 

6. "The nominal differential input impedance of the RxPGA input appearing at the device RX+ and RX− input pins is 400 Ω//4 pF (±20%) and remains relatively independent of gain setting." (pg. 33 of datasheet) I had planned to better match this impedance in a next pcb layout by using the solder side as a ground plane for these traces (nothing in between). Right now the trace impedance is much lower. Regarding terminiation resistors, I haven't thought much about this, and am no expert in this area, so do what you think is best.

[Steve Haynal]

Hello Rob,

You may find more detailed answers for some of the questions on your schematic in my previous post.

3) You will want to have a trace for P18-P5. This is a dedicated clock. It should not go to P12 (pin 29) as in the prototype. I see that your schematic reflects this.

4) Yes, see the early post.

5) Yes, if you want to power the BeMicro from the SDR. Also, see the early post about PWREN# to do this.

6) I may not understand this question. I had separate connections for various power and grounds to experiment with reducing noise. I ended up not needing them to be separate.

7) Yes, you will want to pull it high. Currently the FPGA is clocked via the AD9866. You can get into the situation where the FPGA has no clock if reset is low. There is another clock on the BeMicroSDK that should be used for reset stuff, but currently it isn't.

8) P39 is a signal to the PCIE connector in my schematic. I don't know why it is grounded in your schematic.

9) I wouldn't use P35 (pin6) as a connection to the alex spi. It is a dedicated clock input and might need to be reserved. The other available FPGA pins should be fine. P1, P2, P35 and P36 can be dedicated clock inputs.

[irbsu...@yahoo.co.uk]

Hello Rob,
I think your approach is the right way to go. Right now I think the priority should be to produce some prototypes that can be used to fully evaluate the performance of the AD9866, then add the bells and whistles later if it looks like a winner, which based on Steve's tests it looks good. I am very keen to do lab measurements / on-the-air tests and do a comparison against a 'full' Hermes. I would be pleased to help support you with your design and if there is anything I can do, whether that be checking schematics / layouts or help with the design etc, please let me know. I would definately be interested in building up a board.
This could be a real pivotal project in the world of low cost sdr!
Andrew
G4XZL

[Rob Frohne]

Greetings All,

Thanks Steve for the great data.  This is how my progress has gone so far.  There are some still unresolved issues below, some that I haven't got to yet and some that I'm not savvy on, and any/all comments on them are very welcome.

On 05/04/2014 03:55 PM, Steve Haynal wrote:

1. The signal to connect/disconnect power is PWREN1# and PWREN2#. The details are on page 7 of the BeMicro SDK schematic. There is a PWREN# (pin 4) on the BeMicro connector. Currently, I have added a jumper to the BeMicro to pull PWREN low. I do this not to connect the two 5V supplies, but to fool the FT245RQ. I must then also connect power and ground to the USB connector as well as the SDR. (If there is no "true" USB connection, I believe the FT245RQ detects this and prevents the BeMicro SDK from functioning.)

If I were to redesign this, I would have a jumper for PWREN# on the daughterboard and also tie the 5V digital supplies between the SDR and BeMicro. (Currently they are disconnected in the prototype, but with a test pad for experimentation.) Then, you could put the jumper on to pull PWREN# low and power everything through the SDR power with no need or noise hassles of a USB connection. You can also remove the jumper and power the BeMicro via standard USB for quick programming iterations. You will need to be able to power the BeMicro via standard USB for the initial boot and programming of the EEPROM.

Done.

I measure 230-240 mA at 4.86 V for the BeMicro SDK when running 2 receivers. I think this is close to the maximum you will see. You probably should add some margin.

By the way, the NCP111/ST33TG regulators will not handle >10V input. I almost fried my prototype by connecting it to 13V. Also, they burn a lot of power in heat. I saw them being used in either the Hermes, HiQSDR or AD9866 demo board, and just went with them. Some sort of low-noise switching supply design might be better. The BeMicro does this. 

Where do you get the data that they won't work over 10 V?  The On Semi ones say 20 V in the datasheet.  I do agree they will burn a lot of power at 13.8 volts, something around five watts.

At this point, I don't want to put any kind of a switching regulator on the board, even a low noise one.  I would rather waste some power, than have the possibility of more noise.  What I presently have is a third regulator for CLKVDD.  I couldn't find the data you seem to have that pin 35 of the AD9866 is the ADC supply, and pin 40 is the DAC one, but there was some nice data in the AD9866 data sheet about the amount of current each part of the circuit draws.  U2 (the analog supply) seems to be the one overheating so I put in another separate regulator for the CLKVDD which draws about a quarter of the total current (107 mA), but is rather constant over the separate modes, whereas some of the others vary with settings.  The regulators are protected so that they won't dissipate too much power; you just have to heat sink them more, according to the datasheet.

2a. The SPI bus from P1 to P17 should be wired as traces on the pcb. These connectors can be removed. They were included for flexibility during prototyping, but the FPGA SPI works find.

Done.

2b. The jumper from P14 to P13 supplies voltage to the +5V plane for the output amplifier in the AD9866. It is a jumper on the prototype to provide flexibility on what, if any, this voltage is.

Done.

R6, which was just a wire in the prototype, is included because of discussion on pages 30 and 31 of the data sheet, under "IAMP CURRENT-MODE OPERATION." It says, "The transformer should be specified to handle the dc standing current, Ibias, drawn by the IAMP. Also, because Ibias remains signal independent, a series resistor (not shown) can be inserted between AVDD and the transformer's center-tap to reduce the IAMP's common-mode voltage, Vcm, and reduce the power dissipation on the IC." I used a 0 Ohm resistor for R6 but was careful to adjust my 5V supply to just bellow 5V. Also, I determined the minicircuits device could not handle this standing current, and wound my own transformer. 

Since you are using the medium output power path on the AD9866, be sure to read the section "IAMP CURRENT CONSUMPTION CONSIDERATIONS" on page 32 of the datasheet. It appears possible to exceed the device power dissipation limit, but maybe not with only the OUT_N.

I assume you meant page 42.  At 85 degrees C, you can dissipate 1.66 watts if you solder the thermal pad is soldered correctly and I get enough vias to a big enough ground plane.  Iamp is running at 5 volts and draws 100 mA max, so that is 0.5 watts.  TxDAC draws 60mA at 3.3 volts, so that is 0.2 watts.  The ADC draws 220mA at 3.3 volts, so that is 0.73 watts.  The clock draws 107mA at 3.3 volts, so that is 0.35 watts, and the digital part is 133 mA at 3.3 volts, which is 0.44 watts.  That is 2.2 watts total.  That is okay if you drop the ambient temperature for operation down by 13 degrees to 73 Celsius.  You can dissipate up to 5.5 watts if you drop down to 40 degrees C.  Unless I missed a really big current draw, I think we are okay.

2c. Regarding clocking, there are dedicated clock inputs on the FPGA, which appear on signals P1,P2,P35,P36 of the BeMicro connector. The clkout1 of the AD9866 should not connect to P12 (a generic IO) on the BeMicro connector, but should instead route to P1 (pin 1, test pad 5) of the BeMicro connector, which is a dedicated clock input. My prototype had routed to both pins, which is extra load on the clock. I never used the P12 input except for some early testing.

Done.

In full-duplex mode, "The AD9866 acts as the master, providing RXCLK as an output clock that is used for the timing of both the TX[5:0] and RX[5:0] ports." (datasheet pg. 24) In my current prototype, rxclk is connected to a general I/O on the FPGA (signal P13, pin 31). This signal is a ~147 MHz clock in full-duplex (2x the 73.768 MHz) and more thought should be given to it. (It may be one of the reasons for the noise I saw when experimenting with full-duplex.) My guess is that it should be carefully routed to an FPGA dedicated clock output. Signal P54 (pin 52) for example. I don't know off the top of my head, but I'd read the relevant sections of the Cyclone IV documentation and figure out the best thing to do. You want to use a FPGA pin capable of general I/O for half-duplex operation, and one that can drive a fairly high-speed clock when in full-duplex mode.

It looks like P54 is the other side of the differential output that is used to drive the Ethernet, which I think means it is off limits for us, because we need the Ethernet.  Perhaps we can use the one that goes to the MicroSD card, but that one doesn't seem to go to the connector.  I looked at the Altera Pin Planning Guide (which has the Cyclone IV data removed), the Cyclone IV Device Datasheet, and probably the most helpful the Quartus II Chapter 4 on I/O assignments.  At this point, I don't see a good way to connect this to a PLL_CLKOUT pin, but there may be other better options than the general purpose I/O pins.  I'm not familiar enough with this digital stuff to feel comfortable changing this.  Maybe someone with more savvy can have a stab at it.

2d. Yes, P22 can be ommitted. CLKOUT1 is the recommended output clock to use.

Done.

3. The DIP switches pulled all 3 signals low. The various modes are described on page 19 of the datasheet. This makes half-duplex the default, but you can still switch to full-duplex by writing configuration registers via the SPI.

Done.

4. You may want to use 4 of the unused pins for a MAC/IP serial EEPROM as in the original Hermes. In the current Hermes-Lite RTL, the MAC address is hardcoded, and the IP can be hardcoded or set to use DHCP. Changing the hardcoded values requires recompilation with Quartus II. There is room on the BeMicro SDK EEPROM for these values, and eventually I'd like to use that, but it requires some work. The easiest would be to match the Hermes exactly with an extra serial EEPROM. Refer to their schematic. 

Not done yet, but it seems like the right thing to do.

Also, you may want to expose at least a few of these pins to pads or a simple header for experiments.

Yes, I agree.  Not done yet though.

5. I can't think of anything else that can be removed. I see you still have just two regulators. How are you planning to address the excessive heating I saw with the AVDD_ADC/AVDD_DAC/CLKVDD regulator? One way is to add a third regulator that drives only AVDD_ADC.

It comes down to what is more expensive, I think, a heat sink or another regulator or two.  I haven't compared the costs yet.

6. "The nominal differential input impedance of the RxPGA input appearing at the device RX+ and RX− input pins is 400 Ω//4 pF (±20%) and remains relatively independent of gain setting." (pg. 33 of datasheet) I had planned to better match this impedance in a next pcb layout by using the solder side as a ground plane for these traces (nothing in between). Right now the trace impedance is much lower. Regarding terminiation resistors, I haven't thought much about this, and am no expert in this area, so do what you think is best.

Okay, I'll think about this more carefully.  I really would like a fairly good 50 ohm match on both RX and TX if it doesn't cause other issues.

I need to go to bed.  Thanks for the assistance, and for any comments you have time for on the issues I'm still pondering.

73,

Rob
KL7NA

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

[dean.f...@gmail.com]

Hi Rob,

I would certainly be interested in purchasing a board or two when the time comes, if spares are available of course. I have the parts from the original BOM and would just need to pickup any changes that I don't have on hand.

Thanks,

Dean

[Rob Frohne]

Okay Dean,

I wonder how many boards should I have made on my first batch....  I'm a bit worried about making a big order, because I almost never make a first batch without at least one mistake, or something to change next time. I am going to publish the design files, so you can always order from OHSPark and get three for about $40, assuming I can fit it in 5cm x  5cm which is the standard size for a small board for a number of board houses.  And by the way, I'm not in a great hurry myself, so I plan to order the boards from the slow guys (about three weeks) to save money.

If you want a bare board from the first batch, assuming it will cost about $10 shipped, send me a note to that effect.  That will help me determine how many to order.  And (Dean you can be the first one on that list.)  Unless you are interested in contributing to the development effort, I recommend waiting until the board is verified and corrected.  It will probably be a better board, and if there are more boards for that batch, they will probably be cheaper.

73,

Rob
KL7NA

--

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

-- 
Rob Frohne, PhD, PE
Professor
EF Cross School of Engineering
Walla Walla University
100 SW 4th Street
College Place, WA 99324
(509) 527-2075

[irbsu...@yahoo.co.uk]

Hello Rob,
I would certainly be interested in a pcb to experiment with please if you would be willing to post to the UK.

Regarding the Minicircuits transformers and the desire to replace them, I agree that they can be a problem to buy because of the MOQs etc but the prices can be quite reasonable especially in a group buy as we did for Hermes.
A possible alternative part might be a Coilcraft WBC8-1L which is 8:1 and goes down to 150kHz which could be an advantage.
It would be nice to have the option to fit a homemade one but winding a 9:1 can be a bit tricky so as a suggestion would it be possible to use footprints that would allow say the Minicircuits still to be fitted?
Thanks,
Andrew
G4XZL

[pascal.v...@gmail.com]

Hi Rob, I will be interested in a PCB as soon as a version will be verified, as I cannot be a great help in debugging. I already received the BeMico SDK....

Thanks and 73

Pascal

[Matt]

How many UK based people would be interested in an order of dev pcbs? I've used seeed studio before for PCB fab and was very cheap. Possibly cheaper than a group buy from US then shipping to UK?

Matt.

[Kaj Wiik]

I'm interested in a bare board. Good work!

Thanks,
Kaj OH6EH

[Steve Haynal]

Hi Rob,

I think I've done this without harm. You might want to ask an app engineer at Arrow.

73,

Steve

KF7O

On Wed, May 7, 2014 at 6:17 PM, Rob Frohne <rob.f...@wallawalla.edu> wrote:

Hi Steve,

I have another question for you.....

On 05/04/2014 03:55 PM, Steve Haynal wrote:

1. The signal to connect/disconnect power is PWREN1# and PWREN2#. The details are on page 7 of the BeMicro SDK schematic. There is a PWREN# (pin 4) on the BeMicro connector. Currently, I have added a jumper to the BeMicro to pull PWREN low. I do this not to connect the two 5V supplies, but to fool the FT245RQ. I must then also connect power and ground to the USB connector as well as the SDR. (If there is no "true" USB connection, I believe the FT245RQ detects this and prevents the BeMicro SDK from functioning.)

If I were to redesign this, I would have a jumper for PWREN# on the daughterboard and also tie the 5V digital supplies between the SDR and BeMicro. (Currently they are disconnected in the prototype, but with a test pad for experimentation.) Then, you could put the jumper on to pull PWREN# low and power everything through the SDR power with no need or noise hassles of a USB connection. You can also remove the jumper and power the BeMicro via standard USB for quick programming iterations. You will need to be able to power the BeMicro via standard USB for the initial boot and programming of the EEPROM.

It looks to me as if when PWREN2# is low it connects VCC (the +5V input from the USB connector on the BeMicro) to the +5V bus that powers the rest of the BeMicro and which is connected to the 80 pin connector, (pins 79-80), and so it connects the external power to the FT245R, and pull its RESET# low, making turning off the FT245R nicely as you describe.  However, what happens when someone removes the jumper and powers the board without the USB port of the BeMicro connected to the computer or other power?  The max ratings say that the voltages on the bidirectional data pins of the FT245R must be lower than VCC+0.5 volts, but VCC will be 0 volts.  The data pins are connected to the CPLD (EPM240ZM68C7N) and who knows what it might be putting on the data lines.  I'm probably worrying about nothing, but would feel more comfortable with your take on how dangerous this is.  I suppose we could make dire warnings in the documentation to not do this.

Any comments?

Thanks,

Rob

[Steve Haynal]

Hello Rob,

I agree that it may be a maximum rating, but it is interesting that they don't talk about using this regulator above 10V. My experience is that 13.8V is out of spec with my prototype. I currently use a 13.8 to 5 V buck regulator that I got for cheap on Amazon. I was curious if this was adding any noise to my setup so I removed it and hooked the SDR directly to 13.8V. The regulator for the analog supplies became too hot to touch within seconds and the radio did not work. I measured the output voltage from this regulator and it was significantly below 3.3 V (2 something). I tried several different variations but always with the same result. Perhaps now that you have 3 regulators in your schematic you will be able to push it up to 13.8V input. 

I like your idea of using a USB power supply, but have found significant noise differences in various USB power supplies. I think it would be nice if there was another power connection option, even just two through holes.

73,

Steve

KF7O

On Mon, May 5, 2014 at 10:39 PM, Rob Frohne <rob.f...@wallawalla.edu> wrote:

Thanks for the quick reply.  I don't really think you want to use a device like this to run at 13.8 volts, unless the current is minimal.   I think if it really is a maximum rating, it should me in the Makimum Ratings section, but I may be wrong.  Usually the notes you took as absolute maximum ratings are for the test they are printing the spec for, at least that is how I've always interpreted them.

My tentative plan is to use a micro USB connector for the power.  You can get chargers now that put out a couple of amperes, even though computer USB ports are limited at 500 mA.  Other options I've thought about a little are to just put terminal screw connectors, or perhaps a more specialized connector, like a barrel connector?

Thanks again Steve!

Rob

On 05/05/2014 10:23 PM, Steve Haynal wrote:

Page 3 of the regulator datasheet you link to:

3.3 V (Vin = 5.3 V, Iout = 10 mA, TA = 25 °C)

(Vin = 4.75 V to 10 V, Iout = 0 mA to 800 mA) (Note 4)

I read this as Vin should not be above 10V. 

73,

Steve

KF7O

[Rob Frohne]

Hi Steve,

Yes, the power dissipated in the regulator at 13.8 volts would be something on the order of 5 watts, and the regulators have thermal shutdown, so unless you are putting them in some special heat removing substance, running them at 13.8 is just plain crazy.  I doubt that it will work even with three regulators. 

I'll put in another power option.  I would like something that is keyed against reverse polarity, but then it has the same difficulties as the USB connector.  Perhaps I should put in a beefy diode to protect against reverse polarity, and then the question is should I put it in series (which will drop the VIN by 0.6 volts (.3 if I can find a good Schottky diode) if you use that connector, or should I put it in parallel, across the connector, which would stress the power supply, or should I just assume if you use the spare connector, you won't swap the polarity.

Rob

[Zl2APV]

Have you considered using an FET as a protection device? The FDT434P as a P channel FET for example has an on resistance of 0.05 ohms at 5 Amps so the voltage drop is negligible. Physically small and of course operating at saturation won't require any heatsinking.

73, Graeme ZL2APV

[irbsu...@yahoo.co.uk]

Matt,
Yes, I'm interested, definately one, maybe two.
Thanks,
Andrew
G4XZL