Hi!
I'm designing a two layer analog small signal pcb, with ground plane on bottom an ground pours on top.
The connection between top and bottom layer ground plane is made via thermal pads at the opamps... nothing more...
As an audio design it is designed to reproduce frequencies between 20hz and 20khz....
The questions are:
¿what parameters define the separation between stitching vias?
¿the signal frequency?
¿the opamp bandwidth?
¿how can i calculate separation?
¿should i follow the perimeter between signal traces?
¿faraday cage stitching around the pcb perimeter?
The only thing i have more or less clear about this subject is that it is important to to stitch isolated ground pours or thin traces at opposite sides...
to avoid create antennas..
¡¡I hope this will be of interest of everyone!!
¡thank you for your help!
Jay X
I'm designing a two layer analog small signal pcb, with ground plane on bottom an ground pours on top.
The connection between top and bottom layer ground plane is made via thermal pads at the opamps... nothing more...
As an audio design it is designed to reproduce frequencies between 20hz and 20khz....
The questions are:
¿what parameters define the separation between stitching vias?
¿the signal frequency?
¿the opamp bandwidth?
¿how can i calculate separation?
¿should i follow the perimeter between signal traces?
¿faraday cage stitching around the pcb perimeter?
The only thing i have more or less clear about this subject is that it is important to to stitch isolated ground pours or thin traces at opposite sides...
to avoid create antennas..
¡¡I hope this will be of interest of everyone!!
¡thank you for your help!
Jay X
Hi,
It seems a difficult matter....
For example if i have a top ground pour area ( a peninsula a polygon...) in between traces, placing 1 via in each of the corners of the polygon would be ENOUGH??... to tie this ground pour to the bottom ground plane...
¡this is the question!...
To stitch or how to stitch...🙂
It seems a difficult matter....
For example if i have a top ground pour area ( a peninsula a polygon...) in between traces, placing 1 via in each of the corners of the polygon would be ENOUGH??... to tie this ground pour to the bottom ground plane...
¡this is the question!...
To stitch or how to stitch...🙂
A ground plane isn't a good idea in an audio circuit for a couple reasons.
In a digital circuit a plane is used to add capacitance to the power traces. In an audio circuit this can lead to oscillation.
Ground paths need to we well thought out to control ground loops. Each section of the amplifier should have a ground trace return to a star ground. There can only be one possible path for grounds to follow, otherwise there is a loop, and noise/problems can follow.
A ground plane can act as an antenna and pick up noise. If an Faraday cage is desired it should be built with a separate ground than audio ground. Interference from other sources should be isolated from the audio circuit, not injected into the main audio ground. The cage would likely be better connected to chassis ground and kept isolated from audio completely.
In a digital circuit a plane is used to add capacitance to the power traces. In an audio circuit this can lead to oscillation.
Ground paths need to we well thought out to control ground loops. Each section of the amplifier should have a ground trace return to a star ground. There can only be one possible path for grounds to follow, otherwise there is a loop, and noise/problems can follow.
A ground plane can act as an antenna and pick up noise. If an Faraday cage is desired it should be built with a separate ground than audio ground. Interference from other sources should be isolated from the audio circuit, not injected into the main audio ground. The cage would likely be better connected to chassis ground and kept isolated from audio completely.
At signal levels I do not believe you need the top pours at audio frequencies...It is used for RF for a different reason.
But if you do then I believe that you do not need significant stitching...one per inch still connects at 20KHz.
I believe that ground planes are required for good signal reference throughout the circuit. This also has to do with the EMI world where a trace is an antenna and pickup of RF fields is proportional to the height above a ground plane. So if your victim trace is further away form its' ground reference it will pick up more signal than if it was a circuit boards' thickness away from the ground plane.
However, jwilhelm does have a point about possible oscillation using ground planes. This comes into play with the capacitance between a high impedance signal node and the ground plane. I have read in some data sheets that the ground plane be eliminated beneath the +/- input pads of SMT op-amps. Some op-amps even require a guard ring around their inputs. One aspect of this is to have any high impedance point occupy as small a surface area as possible...feedback resistors should be close to the high impedance node and allow the low impedance drive to have the longer path.
Hope that helps.
Ground planes can work for high precision analog, but you do have to take a few things into consideration. The good part is that, if board capacitance is significant, it can always be compensated for with another capacitance, either manually added to the circuit, or by some other part of the PCB's capacitance. The good part is that, since the board geometry is stable, dependent upon the layout geometry, this can be compensated for fairly precisely and repeatably.
I'm glossing over this, since no particular circuit is in question, but I'm designing a high precision circuit on a 4 layer board, and stray shunt and feedthrough capacitances can be calculated, and in my circuit, compensated for with a little extra work.
I also feel that a low noise analog ground can be done very well using a ground plane, often better than with a pile of star traces and a magic node, since you're using more of the copper instead of etching it away into longer, more inductive and more resistive strips. Of course, one needs to prevent bad interactions, but often, where the sub circuits are located can control this, possibly also with a few judicious cuts in the various planes. Think of where the currents start and where they end up, and try to find ways to make some of these cancel, as close to each other as possible. Nasty currents can be sequestered using some cuts to the foil, which I find better than just star grounding everything offensive; at least within each little isolated foil area, the foil has a low impedance.
Best of luck!
I'm glossing over this, since no particular circuit is in question, but I'm designing a high precision circuit on a 4 layer board, and stray shunt and feedthrough capacitances can be calculated, and in my circuit, compensated for with a little extra work.
I also feel that a low noise analog ground can be done very well using a ground plane, often better than with a pile of star traces and a magic node, since you're using more of the copper instead of etching it away into longer, more inductive and more resistive strips. Of course, one needs to prevent bad interactions, but often, where the sub circuits are located can control this, possibly also with a few judicious cuts in the various planes. Think of where the currents start and where they end up, and try to find ways to make some of these cancel, as close to each other as possible. Nasty currents can be sequestered using some cuts to the foil, which I find better than just star grounding everything offensive; at least within each little isolated foil area, the foil has a low impedance.
Best of luck!
Throw the stiching vias down randomly, especially at corners.
Nearly all low level analogue boards I work on have ground pours and full ground planes, stitched together, don't do silly routed star type grounds ever (do starpoints and separate power/isolated grounds).... do route some sensitive signals as balanced pair routing.
The stitching vias placed randomly supress planar resonances and avoid antenna structures.
look up stuff on precision analogue layout. Removing the ground from under op-amp pins is a requirement with some circuits and devices, used it twice in the last 10 years (could dig out the devices, high speed op-amps on a high speed analogue test card for high resolution sensor, not audio frequency range so I would not worry).
Planar capacitance supply capacitance etc. where to begin....power supply delivery is a whole topic on its own, lets just say for digital sections you would use limited power planes over a ground plane, for analogue supplies you want to use wide traces (that's the basics, there is noise coupling mechanisms to consider as well as other factors).
Basically keep it simple, avoid silly spiders legs style start grounds.
Nearly all low level analogue boards I work on have ground pours and full ground planes, stitched together, don't do silly routed star type grounds ever (do starpoints and separate power/isolated grounds).... do route some sensitive signals as balanced pair routing.
The stitching vias placed randomly supress planar resonances and avoid antenna structures.
look up stuff on precision analogue layout. Removing the ground from under op-amp pins is a requirement with some circuits and devices, used it twice in the last 10 years (could dig out the devices, high speed op-amps on a high speed analogue test card for high resolution sensor, not audio frequency range so I would not worry).
Planar capacitance supply capacitance etc. where to begin....power supply delivery is a whole topic on its own, lets just say for digital sections you would use limited power planes over a ground plane, for analogue supplies you want to use wide traces (that's the basics, there is noise coupling mechanisms to consider as well as other factors).
Basically keep it simple, avoid silly spiders legs style start grounds.
Hi all!
What i did in my last layout (2 layers). It is 100% analog audio design with linear opamps NE5532, LM833, DRV134 OMRON G5V RELAYS, linear dual psu.
1. All signal traces and power traces are on top even if this forced me to place wire jumpers, and all traces are 0.8mm wide.
2. My ground plane is free of traces...(except two very short.. in a feedback path).. i will try to re-route...
3. All the thru hole pads with copper in between each pad
4. Pad clearance (distance to ground plane) 0.3mm
5. I use sprint layout software for layout my boards... it has an "X ray mode" so you can check if top layer traces cross with anything on the bottom layer...
So i checked that below each trace on top layer, there is only copper on the bottom layer.
Regarding stitching, so i just have to "pepper" some vias.... and this not only for thin "antennas like" areas, but also for larger areas...
¿What is is the usual via size for stitching?
thanks a lot!!
What i did in my last layout (2 layers). It is 100% analog audio design with linear opamps NE5532, LM833, DRV134 OMRON G5V RELAYS, linear dual psu.
1. All signal traces and power traces are on top even if this forced me to place wire jumpers, and all traces are 0.8mm wide.
2. My ground plane is free of traces...(except two very short.. in a feedback path).. i will try to re-route...
3. All the thru hole pads with copper in between each pad
4. Pad clearance (distance to ground plane) 0.3mm
5. I use sprint layout software for layout my boards... it has an "X ray mode" so you can check if top layer traces cross with anything on the bottom layer...
So i checked that below each trace on top layer, there is only copper on the bottom layer.
Regarding stitching, so i just have to "pepper" some vias.... and this not only for thin "antennas like" areas, but also for larger areas...
¿What is is the usual via size for stitching?
thanks a lot!!
Many opamps and power audio ICs have thermal pads now. These are usually grounded, and the pads are thru-hole, sometimes a grid of thru-holes. Frequently at least a section of fill on both top and bottom is required to meet the requirements for the heatsinking copper area.
This means that PCB designers simply have to abandon the idea that ground planes on both sides are a no-no and focus instead on how to make them work, particularly since many of the reference designs in which these devices meet their data sheet specs already do so. We're all trying to cram more and more functionality into the same-size package.
Unfortunately amateur enthusiasm tends to slide past the necessity for meaningful test of a layout in audio and the unfortunate necessity to sometimes pay for a respin. The layout is the design in many respects, and even teams of peer-reviewing engineers only discover unwanted interactions after the fact sometimes.
Stitching is what you do on a slow Friday afternoon.
This means that PCB designers simply have to abandon the idea that ground planes on both sides are a no-no and focus instead on how to make them work, particularly since many of the reference designs in which these devices meet their data sheet specs already do so. We're all trying to cram more and more functionality into the same-size package.
Unfortunately amateur enthusiasm tends to slide past the necessity for meaningful test of a layout in audio and the unfortunate necessity to sometimes pay for a respin. The layout is the design in many respects, and even teams of peer-reviewing engineers only discover unwanted interactions after the fact sometimes.
Stitching is what you do on a slow Friday afternoon.
Regarding bottom terminated components (thermal pad packaging) here are some notes I sent someone recently when they queried my use of thermal vias in the actual thermal pad, may be of interest.
another worthwhile link regarding analogue layout.... there is plenty more.
http://www.x2y.com/filters/TechDay0...log_Designs_Demand_GoodPCBLayouts _JohnWu.pdf
another worthwhile link regarding analogue layout.... there is plenty more.
http://www.x2y.com/filters/TechDay0...log_Designs_Demand_GoodPCBLayouts _JohnWu.pdf
- Status
- Not open for further replies.