Power planes, ground cutout and guard traces

Hi experts,I'm designing a mixed signal board where the analog part is very criticalso noise and disturbances has to be minimized. I have three questions foryou:1) All the board is powered with LDOs and between regulators' output andpower planes I'm about to place 0 Ohm resistor to be able to disconnect onerail at a time in case of unwanted short due to production error. Does thishave counter effects? I mean having a wide power plane under loads anddecoupling capacitors connected with a narrow path (the resistor) toregulators output.2) Analog and digital parts share the same ground. In the common groundplane I would insert a cut out between the two parts and make the twogrounds (actually the same) connection under the ADC. Just to be clear:analog part is in upper right corner, digital one in lower right corner andADC in the left side and so the ground plane make a sort of C. Doing thisway some digital traces (switching eventually at tens of MHz) in innerlayers would cross the ground cutout (I can't move  or remove them). Couldthis approach add more noise instead of reducing it? Would you suggestbetter techniques?3) On top and bottom layers I have space to insert guard traces betweenanalog and digital parts in order to reduce crosstalk. What do you think isthe best way to accomplish this (leave trace floating, grounding it, howmany vias)?Thanks a lot,Michele
michele.manotti 5 years 10 months 17 days

4 answers


The best answer


You can select the best answer for current question!
Answered byhan.guobing 5 years 10 months 10 days
Hi Michele and Danny,Just one comment.Be careful about the guarding traces, which may cause extra resonance,especially when one end is open/floating.If you use guarding traces, it's recommend to ground them at both ends andbetter add one GND via every wavelength/10.Thanks,Robin2014-11-05 18:00 GMT+08:00 Danny Damhave :> Hi Michele,> 1) There is no "0 Ohm resistors". Some are closer to "0" than others but> expect a voltage drop.> Consider to design a special footprint with a short track between the> pads, keep the component not mounted> and cut this track for debugging and mount one of the better "0 Ohm> resistors" when needed.> 2) Be very carefull with cutouts, they increase crosstalk to nearby traces> a lot because of the large loop they introduce.> 3) Bogatin and Simonovich has written an excellent paper "Dramatic Noise> Reduction using Guard Traces with Optimized Shorting Vias".> But be aware that this paper and most other advices about guard traces are> based on a 50ohm (or close) environment. Maybe your sensitive analog traces> are high impedance> traces and then the conclusion is different and you will probably get more> from guard traces.> Best regards> Danny Damhave> Damhave Systems ApS>>>> On 05/11/2014, at 10.24, Michele Manotti > wrote:>> > Hi experts,> > I'm designing a mixed signal board where the analog part is very critical> > so noise and disturbances has to be minimized. I have three questions for> > you:> >> > 1) All the board is powered with LDOs and between regulators' output and> > power planes I'm about to place 0 Ohm resistor to be able to disconnect> one> > rail at a time in case of unwanted short due to production error. Does> this> > have counter effects? I mean having a wide power plane under loads and> > decoupling capacitors connected with a narrow path (the resistor) to> > regulators output.> >> > 2) Analog and digital parts share the same ground. In the common ground> > plane I would insert a cut out between the two parts and make the two> > grounds (actually the same) connection under the ADC. Just to be clear:> > analog part is in upper right corner, digital one in lower right corner> and> > ADC in the left side and so the ground plane make a sort of C. Doing this> > way some digital traces (switching eventually at tens of MHz) in inner> > layers would cross the ground cutout (I can't move  or remove them).> Could> > this approach add more noise instead of reducing it? Would you suggest> > better techniques?> >> > 3) On top and bottom layers I have space to insert guard traces between> > analog and digital parts in order to reduce crosstalk. What do you think> is> > the best way to accomplish this (leave trace floating, grounding it, how> > many vias)?> >> > Thanks a lot,> >> > Michele> >> >> > 
Answered byistvan.novak 5 years 10 months 10 days
Please note that grounding a shield trace at both ends vs only one end shifts theresonance frequencies of the guard trace from quarter-wave to half-wave, whichis a factor of two increase.  With today's rise times it is usually still not enough.Empirical data shows that to avoid excess ringing, the round trip delay betweenadjacent grounding vias should not be more than the rise time of the main signal(s).Assuming 100ps rise time, adjacent grounding vias should be closer than one thirdof an inch or less than one centimeter.Regards,Istvan NovakOracleOn 11/12/2014 2:19 AM, Han, Guobing wrote:> Hi Michele and Danny,> Just one comment.> Be careful about the guarding traces, which may cause extra resonance,> especially when one end is open/floating.> If you use guarding traces, it's recommend to ground them at both ends and> better add one GND via every wavelength/10.>> Thanks,> Robin>> 2014-11-05 18:00 GMT+08:00 Danny Damhave :>>> Hi Michele,>> 1) There is no "0 Ohm resistors". Some are closer to "0" than others but>> expect a voltage drop.>> Consider to design a special footprint with a short track between the>> pads, keep the component not mounted>> and cut this track for debugging and mount one of the better "0 Ohm>> resistors" when needed.>> 2) Be very carefull with cutouts, they increase crosstalk to nearby traces>> a lot because of the large loop they introduce.>> 3) Bogatin and Simonovich has written an excellent paper "Dramatic Noise>> Reduction using Guard Traces with Optimized Shorting Vias".>> But be aware that this paper and most other advices about guard traces are>> based on a 50ohm (or close) environment. Maybe your sensitive analog traces>> are high impedance>> traces and then the conclusion is different and you will probably get more>> from guard traces.>> Best regards>> Danny Damhave>> Damhave Systems ApS>>>>>>>> On 05/11/2014, at 10.24, Michele Manotti >> wrote:>>>>> Hi experts,>>> I'm designing a mixed signal board where the analog part is very critical>>> so noise and disturbances has to be minimized. I have three questions for>>> you:>>>>>> 1) All the board is powered with LDOs and between regulators' output and>>> power planes I'm about to place 0 Ohm resistor to be able to disconnect>> one>>> rail at a time in case of unwanted short due to production error. Does>> this>>> have counter effects? I mean having a wide power plane under loads and>>> decoupling capacitors connected with a narrow path (the resistor) to>>> regulators output.>>>>>> 2) Analog and digital parts share the same ground. In the common ground>>> plane I would insert a cut out between the two parts and make the two>>> grounds (actually the same) connection under the ADC. Just to be clear:>>> analog part is in upper right corner, digital one in lower right corner>> and>>> ADC in the left side and so the ground plane make a sort of C. Doing this>>> way some digital traces (switching eventually at tens of MHz) in inner>>> layers would cross the ground cutout (I can't move  or remove them).>> Could>>> this approach add more noise instead of reducing it? Would you suggest>>> better techniques?>>>>>> 3) On top and bottom layers I have space to insert guard traces between>>> analog and digital parts in order to reduce crosstalk. What do you think>> is>>> the best way to accomplish this (leave trace floating, grounding it, how>>> many vias)?>>>>>> Thanks a lot,>>>>>> Michele>>>>>>>>>
Answered bydd 5 years 10 months 17 days
Hi Michele,1) There is no “0 Ohm resistors”. Some are closer to “0” than others but expect a voltage drop.Consider to design a special footprint with a short track between the pads, keep the component not mountedand cut this track for debugging and mount one of the better “0 Ohm resistors” when needed.2) Be very carefull with cutouts, they increase crosstalk to nearby traces a lot because of the large loop they introduce.3) Bogatin and Simonovich has written an excellent paper “Dramatic Noise Reduction using Guard Traces with Optimized Shorting Vias”.But be aware that this paper and most other advices about guard traces are based on a 50ohm (or close) environment. Maybe your sensitive analog traces are high impedancetraces and then the conclusion is different and you will probably get more from guard traces. Best regardsDanny DamhaveDamhave Systems ApSOn 05/11/2014, at 10.24, Michele Manotti  wrote:> Hi experts,> I'm designing a mixed signal board where the analog part is very critical> so noise and disturbances has to be minimized. I have three questions for> you:> > 1) All the board is powered with LDOs and between regulators' output and> power planes I'm about to place 0 Ohm resistor to be able to disconnect one> rail at a time in case of unwanted short due to production error. Does this> have counter effects? I mean having a wide power plane under loads and> decoupling capacitors connected with a narrow path (the resistor) to> regulators output.> > 2) Analog and digital parts share the same ground. In the common ground> plane I would insert a cut out between the two parts and make the two> grounds (actually the same) connection under the ADC. Just to be clear:> analog part is in upper right corner, digital one in lower right corner and> ADC in the left side and so the ground plane make a sort of C. Doing this> way some digital traces (switching eventually at tens of MHz) in inner> layers would cross the ground cutout (I can't move  or remove them). Could> this approach add more noise instead of reducing it? Would you suggest> better techniques?> > 3) On top and bottom layers I have space to insert guard traces between> analog and digital parts in order to reduce crosstalk. What do you think is> the best way to accomplish this (leave trace floating, grounding it, how> many vias)?> > Thanks a lot,> > Michele> > > 
Answered byken 5 years 10 months 17 days
Hi Michele, good questions.1. I guess I donâ??t see much issue with the 0-Ohm resistors, but as Danny mentioned, there will be some voltage drop, depending on the DCR.2. Thereâ??s still lotâ??s of debate on splitting analog and digital return planes. The trick with any design (split or not) is to trace the path of ALL high frequency return currents and make sure they donâ??t â??mingleâ? together in the return plane, which will cause noise coupling. Above all, donâ??t be crossing the gap between planes with high frequency clock (or other high frequency digital) traces. This not only presents a signal integrity issue, but will generate extreme amounts of common-mode currents, which typically flow out I/O cables and cause you to fail EMI.Gaps in return planes - yes or no? http://www.edn.com/electronics-blogs/designcon-central-/4429950/Gaps-in-return-planes---yes-or-no-You may also wish to check out Dr. Todd Hubings CVEL web site for more on PC board design: http://www.cvel.clemson.edu/emc/index.html Thereâ??s also a discussion on the same topic over at the â??EMC Troubleshootersâ? LinkedIn discussion group.3. Guard traces should be grounded at each end with ground vias distributed along the length. I, and several others, have written about this extensively.Guard traces - use â??em, or not? http://www.edn.com/electronics-blogs/the-emc-blog/4378148/Guard-Traces--Use-Em-or-Not-Cheers, Ken_______________________Kenneth WyattWyatt Technical Services, Inc.56 Aspen Dr.Woodland Park, COPhone: (719) 310-5418Email Me!  | Web Site  | Blog The EMC Blog (EDN) Subscribe to Newsletter Connect with me on LinkedIn > On Nov 5, 2014, at 2:24 AM, Michele Manotti  wrote:> > Hi experts,> I'm designing a mixed signal board where the analog part is very critical> so noise and disturbances has to be minimized. I have three questions for> you:> > 1) All the board is powered with LDOs and between regulators' output and> power planes I'm about to place 0 Ohm resistor to be able to disconnect one> rail at a time in case of unwanted short due to production error. Does this> have counter effects? I mean having a wide power plane under loads and> decoupling capacitors connected with a narrow path (the resistor) to> regulators output.> > 2) Analog and digital parts share the same ground. In the common ground> plane I would insert a cut out between the two parts and make the two> grounds (actually the same) connection under the ADC. Just to be clear:> analog part is in upper right corner, digital one in lower right corner and> ADC in the left side and so the ground plane make a sort of C. Doing this> way some digital traces (switching eventually at tens of MHz) in inner> layers would cross the ground cutout (I can't move  or remove them). Could> this approach add more noise instead of reducing it? Would you suggest> better techniques?> > 3) On top and bottom layers I have space to insert guard traces between> analog and digital parts in order to reduce crosstalk. What do you think is> the best way to accomplish this (leave trace floating, grounding it, how> many vias)?> > Thanks a lot,> > Michele> > >