The Bom should be publicly visible (if you have a Digi-Key account)
https://www.digikey.ch/classic/RegisteredUser/BOMBillOfMaterials.aspx?path=1&exist=1&id=851820
If not, here is the CSV export
https://dl.dropboxusercontent.com/u/46882396/635025735730186949__851820.csv
Note: I did not search for the cheapest possible BoM, I took the exact part as gbulmers BoM when possible and the first potentially compatible one I found for the rest.
To not measure the additional noise an active analog sensor introduces, I've breadboarded only a simple setup this time: 9 voltage dividers tied to Pins 3-11, AV-, AV+ or Vcc on the Orone and Maple Minis, respectively. The default sampling time of 55.5 was used.
https://dl.dropboxusercontent.com/u/46882396/adc_benchmark.pdf
conclusion: Maple (AV+) performs best (no surprise), Orone (AV+,Vcc) slightly worse (still good enough for me) than Maple (Vcc).
As two boards only are not really representative, somebody may want to verify, here the files to do so: https://github.com/ventosus/maple_adc_benchmark
ventosus - What were the values of the resistors in the resistor divider you used for the ADC noise test?
ventosus - Great. I just wanted to know if the values were low enough to get less than the theoretical 1/4 of LSB error according to the equation on page 76 of the datasheet. I think your resistor dividers meet the impedance requirement at all sample rates.
Maximum source output impedance for less than 1/4 LSB error = 1.5/(14megahertz*8picofarad*ln(2^14)) - 1kiloOhm = 380Ω
Output impedance of your voltage divider with two 180Ω resistors = 180/2Ω = 90Ω
Other things I've found to screw that up: noisy voltage reference or power supply, external noise (RFI), or noise injected into the ADC pin's trace from ground return currents from digital section of the uC or other components that might be in your circuit that share a ground return path.
gbulmer
Moderator
I could bring the 'effective' input voltage (after the two diodes on Vusb and Vin, i.e. at C1) out to a thru-hole pad in the lower right corner. That could be used to power an external voltage regulator. That could be anything folks want, e.g. an ultra-low-noise source with lots of decoupling. Then simple experiments to measure noise performance might be 'self contained' (powered from that pin), and hence require less test equipment.
That signal path could also be used to avoid the voltage drop across the Vin diode, reducing the minimum input voltage by 0.36V, for anyone expert enough to need it and know how to use it.
I could also add the av+ output on an extra thru-hole pad on the lower left (I don't want it on its Maple-mini position as I've explained elsewhere). Easy access to av+ might give access to more information about noise.
While I'm at it, I could bring Vusb (before the diode D1) to a further thru-hole pad in the top right. That would satisfy Crenn's requirement for access to that 5V voltage for LCDs.
After all, its the same cost to make the PCB, so I could try to make it more useful.
gbulmer - I also like the idea of having the 5V from USB available. Are the EAGLE files for the Orone available? Might I take a look?
ventosus - Another potentially revealing experiment regarding the ADC noise is to fire up a bunch of PWM outputs or anything digital, fast, and fairly asynchronous to the ADC measurements, and look at the ADC noise. The results of this kind of experiment were one of the reasons we went with a 4-layer PCB.
okie, earlier in the thread. https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0
gbulmer
Moderator
I've pushed a design based on 8mil track/8mil space board with the extra two voltages brought out to pads.
I've also increased the separation between one edge of the ADC inputs, and other signal tracks.
It's in https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0/Orone-mini-S8H-v0r001
There is also a copy of ventosus Digikey BoM.
gbulmer
Moderator
The two extra voltages pins on Orone-mini-S8H-v0r001 are:
- 'raw Vusb' (the voltage on the USB socket), and
- the pre-regulator voltage at C1 (about 4.7V when connected to USB). This pin could also be used as an alternative to Vin, and avoid the voltage drop from the diode between Vin and the regulators, though you'd need to be careful as a reversed voltage would damage C1.
I now think it should be Vusb after the resettable polyfuse, rather than the voltage on the USB socket.
The 'raw Vusb' voltage is not as robust as 'Vusb->Polyfuse', and 'raw Vusb' has very little advantage.
It'd be straightforward to bring 'Vusb->Polyfuse' to a header pin in the bottom right.
Are folks okay with that change (Edit: as we used to say "silence is agreement")?
gbulmer
Moderator
I've added ventosus' Digi-Key BoM to github:
https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0/Orone-mini-BoM-v0r001
I've also changed the S8D variant (which is 6mil track & space & large C1 capacitor):
https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0/Orone-mini-S8D-v0r001
The Vusb pad exposes the voltage after the polyfuse.
The pads for the Vusb and pre-regulator voltage (Vx) are placed at the end of the original 20pin header. The intention is to make all PCB's match this pin-out
Ground and analogue ground copper pours have been slightly re-routed to improve ground flow left to right.
Edit: Updated 8mil track/space variant, Orone-mini-S8H, to match Orone-mini-S8D pin out and improve ground
https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0/Orone-mini-S8H-v0r001
Moved LED1 to make it easier to use 3mm LED.
Should I reconnect 'av+' to pin 1 of the J1 pin header in place of 3.3V from the larger voltage regulator?
It might give a slightly less noisy voltage source for the ADC. I could add a warning on the silk screen to tell users that 'av+' can only supply a small current at higher input voltages.
@gbulmer: I've cut the stencils for free on an Epilog laser cutter at the local FabLab http://luzern.fablab.ch
@all: I've built a second Orone Mini equipped with the STM32F303CC. As I want to program it with libmaple, I ended up creating an initial F3 port first ;-)
I'll create a new thread for the port, once I've pushed the code to github (which will be soon).
I use the built-in DfuSe bootloader to load code onto the chip, which works fine. I don't see the point of porting the maple Dfu loader to the F3, if there's already one built-in. I'd like to use that one.
However, with the present design of the Orones, I need to an external 1k5 pull-up resistor on USB-DP for flashish. As all pins (but the debug pins) are in input-floating mode at boot, the DISC circuitry is disabled at boot (so is the pull-up) and the DfuSe device will not enumerate.
To operate the built-in DfuSe bootloader without external pull-up, I followed others ideas to write some minimal boot-code which fires up the DISC circuitry and then jumps to the buitl-in boot-loader. Although the jump works fine, the internal boot-loader resets all pins (even if they're locked) once started and again cannot enumerate. I have not yet given up to get around this by software, but it may be only possible by a hardware mod, USB-DP being pulled-up at boot.
Or there may be another approach I have not seen yet?
gbulmer
Moderator
ventosus - Thanks for the info about the stencil. I'll try a similar route. Did you modify the DRC->Mask parameters?
" I've built a second Orone Mini equipped with the STM32F303CC ... "
Excellent!
"I use the built-in DfuSe bootloader to load code onto the chip, which works fine. I don't see the point of porting the maple Dfu loader to the F3, if there's already one built-in."
I am thinking along the same lines as you.
Originally I had planned on using either an ST-LINK/2 (e.g. the ST-LINK/V2 on an STM32FxDiscovery board) or a USB-UART cable to load the initial program. However, I decided to remove the need for that by bringing USB_DISC to a pad. It is just about available on the Orone-mini-S8A variant on a via connected to T1.
I've since modified the PCB to make access to USB_DISC easier. The two most recent designs (S8D which is 6mil track space, and S8H which is 8mil track and space) bring the USB_DISC signal to a proper pad on the 0.1" grid. This could be used to pull up USB resistor by pulling USB_DISC to ground. I would have liked to bring this to pad at the edge, but it is getting a bit tight, so it is interior to the board, labelled 'DISC' next to T1.
"minimal boot-code which fires up the DISC circuitry and then jumps to the buitl-in boot-loader. Although the jump works fine, the internal boot-loader resets all pins (even if they're locked) once started and again cannot enumerate"
It sounds like you are using ala42 technique for calling the built-in bootloader in system ROM. I had assumed that would work, so maybe ala42 can clarify. Have you got a JTAG debugger (e.g. an STM32FxDiscovery and gdb)? Can you see the code which resets the pins? Is it early enough in the bootloader that it can be skipped?
Edit: I've had as look at the PCBs. It is tight, and this may only be an option on the S8D (6mil track/space PCB), however I think there is enough space to get a ground pad next to the USB_DISC pad, on a 0.1" grid. So we could insert a 2 pin header, and USB_DISC could be shorted to ground with an ordinary 2 pin female jumper. Or the two holes (USB_DISC and Ground) could be wired to a button or switch.
You must log in to post.
