Cheap 4 layer :
Seeed Studio Bazaar,Boost ideas,extend the reach
I tested, the boards are very good quality especially considering the prics. The cheap postage option is extremely slow though, you may prefer to select fedex/ups...
About your layout, there are too many holes in your planes. Putting many vias close together without the copper plane flowing between them creates voids in your plane. Look at the connector at the top, the copper flows between each pin, this is the way it must be done also between vias.
Remember one reason to use a plane is to give a short path to return currents. If the plane has slots, traces going over the slots will not have their return current under them, it will have to make a detour. Slot antennas are also efficient at radiating and picking up EMI.
It would be better to route all the analog output traces on top layer, directly from DAC to connector. This would remove most vias. Route differential signals as differential pairs (place differential directive in schematic and let Altium do the work).
Then, layer 1 is the DAC, layer 2 is ground plane. You did not put traces on ground plane layer, this is good. No need to use a polygon, use Altium's plane function in the layer stack manager, it is much faster to display.
Then, supplies. The pinout looks nicely organized. You can use polygons on the back of the board under the DAC for each supply voltage, with decoupling capacitors. For example supply polygons on layer 3, and a ground pour on layer 4, stitched to layer 2 ground with vias. One via per power pin to the copper pour on the inside of the chip footprint, immediately next to each one or two GND vias.
You can remove the rest of useless GND copper pour on all layers, and selectively add it back where it matters. If you have two copper planes they must be stitched with vias everywhere.
Then, digital IO.
You are using unshielded flat cable for your analog signals (nothing wrong with that although an extra GND wire between each diff pair would definitely help) and then routing the analog signals between planes (probably to shield them) ; on the other hand you use shielded coax for your digital siggnals but route them on top layer... kind of contradiction here.
The worst offenders regarding noise emissions will be your clock and I2S. You could route them on layer 3 between two ground planes (stitched), and via them to the DAC IO pins.
I am perplexed about the fashion of using these U/FL connectors. If you design both boards (dac/dsp), why not mate them edge to edge with edge connectors ? It is a practical way to get lots of pins for cheap and continuity of ground plane between boards.
I simply solder dual row 0.1" headers and female receptacles along the board edge.
Seeed Studio Bazaar,Boost ideas,extend the reach
I tested, the boards are very good quality especially considering the prics. The cheap postage option is extremely slow though, you may prefer to select fedex/ups...
About your layout, there are too many holes in your planes. Putting many vias close together without the copper plane flowing between them creates voids in your plane. Look at the connector at the top, the copper flows between each pin, this is the way it must be done also between vias.
Remember one reason to use a plane is to give a short path to return currents. If the plane has slots, traces going over the slots will not have their return current under them, it will have to make a detour. Slot antennas are also efficient at radiating and picking up EMI.
It would be better to route all the analog output traces on top layer, directly from DAC to connector. This would remove most vias. Route differential signals as differential pairs (place differential directive in schematic and let Altium do the work).
Then, layer 1 is the DAC, layer 2 is ground plane. You did not put traces on ground plane layer, this is good. No need to use a polygon, use Altium's plane function in the layer stack manager, it is much faster to display.
Then, supplies. The pinout looks nicely organized. You can use polygons on the back of the board under the DAC for each supply voltage, with decoupling capacitors. For example supply polygons on layer 3, and a ground pour on layer 4, stitched to layer 2 ground with vias. One via per power pin to the copper pour on the inside of the chip footprint, immediately next to each one or two GND vias.
You can remove the rest of useless GND copper pour on all layers, and selectively add it back where it matters. If you have two copper planes they must be stitched with vias everywhere.
Then, digital IO.
You are using unshielded flat cable for your analog signals (nothing wrong with that although an extra GND wire between each diff pair would definitely help) and then routing the analog signals between planes (probably to shield them) ; on the other hand you use shielded coax for your digital siggnals but route them on top layer... kind of contradiction here.
The worst offenders regarding noise emissions will be your clock and I2S. You could route them on layer 3 between two ground planes (stitched), and via them to the DAC IO pins.
I am perplexed about the fashion of using these U/FL connectors. If you design both boards (dac/dsp), why not mate them edge to edge with edge connectors ? It is a practical way to get lots of pins for cheap and continuity of ground plane between boards.
I simply solder dual row 0.1" headers and female receptacles along the board edge.
Have you considered using this pinout to enable using pressfit connectors with a flatcable ending in 2 DB 25 connectors?
http://tascam.com/content/downloads/products/220/DB-25_Pinout.pdf
I am extreamly impressed with our progress.
Even if suggestions like this could slow you down.
Best Regrads Bosse
http://tascam.com/content/downloads/products/220/DB-25_Pinout.pdf
I am extreamly impressed with our progress.
Even if suggestions like this could slow you down.
Best Regrads Bosse
Done, will be posting an update shot soon.
The cable I will be using is unshielded but it is a twisted pair and grounds are present on each end of the connector.
I've buried these lines onto L3 now, so they are now mostly covered by 2 GND planes, however the signal is on top layer from the resistor network to the chip.
These connectors are fairly cheap and they have a 6GHz rating as well and because their sub-miniature size offers a simple and cheap solution for RF signals. Also this is a great way for others to use these boards with their existing hardware.
I figured at first I'm going to stuff everything on a single board...
But then I thought a modular approach is an easier way for others to pick and choose what they want.
Thanks Bosse.
This board wasn't designed to directly interface anything as there isn't any kind of filtering or buffer on the DAC. In order to "protect" the DAC we need either a passive or active buffer which will be implemented on the Analog Output Board.
As far as the connectors there will be a wide variety of options available
PS:
Keep Posted I will be posting the new snapshots shortly
Your copper planes look much better.
SMD ceramic decoupling capacitors are nice because they are small, therefore have low inductance. Also they are cheap which allows you to put lots of them in parallel, which gives even lower inductance. Decoupling caps are all about inductance. Capacitance is a side effect.
However thay have low ESR which means paralleling ceramic caps of different values is prone to creating resonances.
These are the reason why Rule #1 of decoupling capacitors is, if a capacitor is connected to something through a long thin trace, the trace will have 10x more inductance than the tiny SMD cap, and therefore it will not be very useful. This is also true for C31.
These caps also look pretty small. Are they 0402 ? If you're going to hand solder those, you have my respects...
You could make a better placement of the caps like C3, C18, C19 and all the others, a bit closer to the chip, perhaps.
If the caps are more than 1.6mm away from the chip, that is the thickness of the board : they would then be better on the back side, connected by a via. This allows a copper pour for power on the back side, which is nice.
Consider C5 for example. The correct way would be to put a via inside the chip footprint to the AVDD puddle on layer 4, and all the capacitors on it. Here you use a long thin trace to connect C5 to the AVDD pin (making C5 useless), and this power trace also couples closely to the analog trace nearby, which will inject power supply current noise into the analog signal.
SMD ceramic decoupling capacitors are nice because they are small, therefore have low inductance. Also they are cheap which allows you to put lots of them in parallel, which gives even lower inductance. Decoupling caps are all about inductance. Capacitance is a side effect.
However thay have low ESR which means paralleling ceramic caps of different values is prone to creating resonances.
These are the reason why Rule #1 of decoupling capacitors is, if a capacitor is connected to something through a long thin trace, the trace will have 10x more inductance than the tiny SMD cap, and therefore it will not be very useful. This is also true for C31.
These caps also look pretty small. Are they 0402 ? If you're going to hand solder those, you have my respects...
You could make a better placement of the caps like C3, C18, C19 and all the others, a bit closer to the chip, perhaps.
If the caps are more than 1.6mm away from the chip, that is the thickness of the board : they would then be better on the back side, connected by a via. This allows a copper pour for power on the back side, which is nice.
Consider C5 for example. The correct way would be to put a via inside the chip footprint to the AVDD puddle on layer 4, and all the capacitors on it. Here you use a long thin trace to connect C5 to the AVDD pin (making C5 useless), and this power trace also couples closely to the analog trace nearby, which will inject power supply current noise into the analog signal.
Thanks peufeu,
Most caps on here are still 0603, while the polarized caps are 0608 and even that is plenty small for me.
I have a proper Hot Air Rework Station as well as the proper tweezers, Vacuum Pick-up Tool as well as working on a DIY Re-flow Oven.
I will be assembling these board by myself ( or my wife, since she thinks soldering is so much "fun" LOL )
C29, C30, C31 were a last minute thought and were added mainly as supply filtering and should have added a 1/10th value decoupling cap in parallel.
Again, part placement only on the 1 side of the board will make it easier to assemble.
Most caps on here are still 0603, while the polarized caps are 0608 and even that is plenty small for me.
I have a proper Hot Air Rework Station as well as the proper tweezers, Vacuum Pick-up Tool as well as working on a DIY Re-flow Oven.
I will be assembling these board by myself ( or my wife, since she thinks soldering is so much "fun" LOL )
C29, C30, C31 were a last minute thought and were added mainly as supply filtering and should have added a 1/10th value decoupling cap in parallel.
Again, part placement only on the 1 side of the board will make it easier to assemble.
Started on the buffer/filter circuit tonight.
Its based on the AD8672
The board will employ a 36 pin header on the input and 3 pin connectors on the output to connect to your favourite output connectors ( XLR, TRS, DB25, ETC )
Later revisions will have XLR, TRS and the later mentions DB25.
Its based on the AD8672
The board will employ a 36 pin header on the input and 3 pin connectors on the output to connect to your favourite output connectors ( XLR, TRS, DB25, ETC )
Later revisions will have XLR, TRS and the later mentions DB25.
Last edited:
More "modules"...
I pulled the connectors on a separate board again, using a pin header.
Also added 3 pin Hirose DF1B Series connector for either RCA or XLR connectivity.
Yes, its not as pretty as having all the connectors on a PCB but this is a BETA board and makes rear panel prototyping a lot easier when your trying to stick 32 XLR connectors on there plus your digital I/O's
Anyway...
Here's a quick peek
I'm still working on laying out the active filter board, but work is getting in the way yet again.
I pulled the connectors on a separate board again, using a pin header.
Also added 3 pin Hirose DF1B Series connector for either RCA or XLR connectivity.
Yes, its not as pretty as having all the connectors on a PCB but this is a BETA board and makes rear panel prototyping a lot easier when your trying to stick 32 XLR connectors on there plus your digital I/O's
Anyway...
Here's a quick peek
I'm still working on laying out the active filter board, but work is getting in the way yet again.
Well, quick update...
Finished the individual modules that will go onto the main board
These modules will be plugged in vertically onto the output board which will be a stretched out version of the above board and will go in-between the header and the output.
Like I said earlier...
Progress is slow but with work picking up steadily I have limited time and can work on this in the evenings now. DAC boards have been sent out a few minutes ago to the PCB manufacturer
Finished the individual modules that will go onto the main board
These modules will be plugged in vertically onto the output board which will be a stretched out version of the above board and will go in-between the header and the output.
Like I said earlier...
Progress is slow but with work picking up steadily I have limited time and can work on this in the evenings now. DAC boards have been sent out a few minutes ago to the PCB manufacturer
I still love your progress speed 
When can I get a complete set of modules for I2S inputs to the Tascam V25 interface?
I do not need to wait for the USB part as I can/thinking to use a dual Optical ADAT receiving interfaces to connect the 8 I2S signals for 16 outchannels
the current first step for card architecture will require 8 Buffer cards for 16 out channels?
Not that i won't be interested in the full USB functionality and to deploy more than 16 channels.
Best regards Bosse
When can I get a complete set of modules for I2S inputs to the Tascam V25 interface?
I do not need to wait for the USB part as I can/thinking to use a dual Optical ADAT receiving interfaces to connect the 8 I2S signals for 16 outchannels
the current first step for card architecture will require 8 Buffer cards for 16 out channels?
Not that i won't be interested in the full USB functionality and to deploy more than 16 channels.
Best regards Bosse
I still love your progress speed
When can I get a complete set of modules for I2S inputs to the Tascam V25 interface?
I do not need to wait for the USB part as I can/thinking to use a dual Optical ADAT receiving interfaces to connect the 8 I2S signals for 16 outchannels
the current first step for card architecture will require 8 Buffer cards for 16 out channels?
Not that i won't be interested in the full USB functionality and to deploy more than 16 channels.
Best regards Bosse
Hi Bosse,
For best channel separation each card only does 1 channel.
However SMD components are quite cheap and keeping everything single sided its easily re-flowed in a toaster oven, so assembly is fast and easy.
once the design of the DAC and its sub parts are finalised they are going out and they are going into the test phase.
If you want I can send a set of boards out for you to test out and give me some feedback.
Well...
Last night I started working out the regulator boards ( yes boards as the Analog and Digital sections will be fed by separate supplies).
They will be based on the new Analog Devices ADM7150 Ultra Low Noise / High PSRR LDO.
The power supply itself will be on a separate board.
It's going to be bipolar supply ( for the output board ) with 12V regulated positive and negative rails as well as a "sea of caps" and separate Analog and Digital feeds which again its not going to be nothing fancy.
I've been hunting caps for the power supply board to try and keep them all audio grade.
The power supply will be through hole where as the reg boards are SMT ( again spent quite a few hours to find Audio Grade SMD caps ( 10x10mm ). Also mostly every single one is decoupled with a second 1/10th size cap.
Well... I'm gonna go finish laying out the boards and post them up in a bit.
Last night I started working out the regulator boards ( yes boards as the Analog and Digital sections will be fed by separate supplies).
They will be based on the new Analog Devices ADM7150 Ultra Low Noise / High PSRR LDO.
The power supply itself will be on a separate board.
It's going to be bipolar supply ( for the output board ) with 12V regulated positive and negative rails as well as a "sea of caps" and separate Analog and Digital feeds which again its not going to be nothing fancy.
I've been hunting caps for the power supply board to try and keep them all audio grade.
The power supply will be through hole where as the reg boards are SMT ( again spent quite a few hours to find Audio Grade SMD caps ( 10x10mm ). Also mostly every single one is decoupled with a second 1/10th size cap.
Well... I'm gonna go finish laying out the boards and post them up in a bit.
All done
I have pulled out the Enable pins to the edge of the board to a standard 2 pin header.
The reason for this being that you can either jumper it or let the MCU control the power sequencing.
The reason behind the 3 stages is simple:
AVDD, PLL & DVDD, IOVDD
And now for the eye candy:
PS:
I just realize I have forgotten the VIA's under the chip and adding them as we speak.
I have pulled out the Enable pins to the edge of the board to a standard 2 pin header.
The reason for this being that you can either jumper it or let the MCU control the power sequencing.
The reason behind the 3 stages is simple:
AVDD, PLL & DVDD, IOVDD
And now for the eye candy:
PS:
I just realize I have forgotten the VIA's under the chip and adding them as we speak.
The Schematic was a nightmare!
I just got it done, but I couldn't fit it on one sheet so had to break it up in 4 sheets:
Sheet 1 - Input header and Input Net Names
Sheet 2 - Buffer Modules 1 - 8
Sheet 3 - Buffer Modules 9 - 16
Sheet 4 - Output Connectors ( Same as last revision with DB25 and 16x 3 Pin headers )
Still have to lay out the boards, but its not gonna happen tonight as its already 1:15AM :/
I just got it done, but I couldn't fit it on one sheet so had to break it up in 4 sheets:
Sheet 1 - Input header and Input Net Names
Sheet 2 - Buffer Modules 1 - 8
Sheet 3 - Buffer Modules 9 - 16
Sheet 4 - Output Connectors ( Same as last revision with DB25 and 16x 3 Pin headers )
Still have to lay out the boards, but its not gonna happen tonight as its already 1:15AM :/
Today I sprung and bought the power supply transformers:
Antek
1 x AS-0512 - 50VA 12V Transformer
1 x AS-0505 - 50VA 5V Transformer
2 x CA-050 Steel Cover
Grand total of $101.50 with shipping to my door.
Not bad considering its overkill for what I need for the Analog and Digital Sections.
The 5V supply will be on constantly providing power to the MCU and other systems.
The Regulator board has the enable pins brought to the edge, so it can either be bypassed with a jumper to power or controlled via an MCU to turn them on or off.
This would allow the MCU to fully boot and voltage to stabilize before anything is powered up.
The 12V supply is mainly for the Buffers and it will have a switched AC supply.
Regulator for this is not going to be anything special... LM317/377 with a few audiophile caps in a CLCRC configuration and that's about it. It may sound crazy, but I'm biased towards Nichicon and Elna caps, but specially more towards the Nichicon MUSE and Nichicon KA Series.
Anyways...
Next week i will most likely get a chassis and start getting a few more things together and more parts ordered.
That's all for now
Antek
1 x AS-0512 - 50VA 12V Transformer
1 x AS-0505 - 50VA 5V Transformer
2 x CA-050 Steel Cover
Grand total of $101.50 with shipping to my door.
Not bad considering its overkill for what I need for the Analog and Digital Sections.
The 5V supply will be on constantly providing power to the MCU and other systems.
The Regulator board has the enable pins brought to the edge, so it can either be bypassed with a jumper to power or controlled via an MCU to turn them on or off.
This would allow the MCU to fully boot and voltage to stabilize before anything is powered up.
The 12V supply is mainly for the Buffers and it will have a switched AC supply.
Regulator for this is not going to be anything special... LM317/377 with a few audiophile caps in a CLCRC configuration and that's about it. It may sound crazy, but I'm biased towards Nichicon and Elna caps, but specially more towards the Nichicon MUSE and Nichicon KA Series.
Anyways...
Next week i will most likely get a chassis and start getting a few more things together and more parts ordered.
That's all for now
Last edited:
NOTE:
AS-0512 - 12VAC @ 2.1A / Sec. ( 5.3A in Parallel )
AS-0505 - 5VAC @ 4A / Sec. ( 11.5A in Parallel )
Digital Supplies will be fed from Secondary 1 of AS-0505
Analog supplies will be fed from Secondary 2 of AS-0505
The buffer section / headphone amp will be fed from the AS-0512
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.