Pulse generator (Impedance control help) - Page 1
Forum section: electronics / projects

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 01, 2018, 10:17:30 pm
content: Happy new year to anyoneI want to build a good pulse generator, with really fast edges, the schmit oscillator of "w2aew" is good, and pretty fast too, but is made at mid air, so I have maked a pcb to have a better stability, I want to use this component from Fairchild "NC7SZ14M5X" on the paper seems very good, all the other parts are SMD 0805, MLCC (NP0) and some thick resistor film for limiting the current at the end of the schmit triggers. I have designed the pcb to have the same lenght of traces and the traces are placed to have less possibile parasitic effect. I have ordered the components all made by the same producer, with the same tollerance and the same temperature coefficent. the pcb is made of FR4-standard Tg 104c with 1oz of copper, thickness 1.6mm).(I have used a SMA connector)The question is, Am I doing something wrong? Can I improve something?

author: rhb
author_rank: Super Contributor
timestamp: January 01, 2018, 11:03:18 pm
content: Study the one Leo Bodnar designed and sells. There's a long thread here:https://www.eevblog.com/forum/projects/yet-another-fast-edge-pulse-generator/msg1251589/#msg1251589And the classic by Jim Williams is covered here:https://www.eevblog.com/forum/projects/jim-williams-pulse-generator-is-still-strategic-military-or-dual-use-technology/msg1329248/#msg1329248

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 02, 2018, 07:27:08 am
content: Quote from: rhb on January 01, 2018, 11:03:18 pmI have thought to the adcmp572 too, but I can't solder it for it's package (yea..it's possibile with a soldering iron but it will be messy) I was reffering to my board, I am doing something wrong? Is worth what I have done?

author: rhb
author_rank: Super Contributor
timestamp: January 02, 2018, 04:03:17 pm
content: What is the signal path? You mentioned lots of parts choices, but didn't post a layout. The layout is the killer for fast edges. Read the digital black magic books by Graham and Johnson.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 02, 2018, 08:57:43 pm
content: Quote from: rhb on January 02, 2018, 04:03:17 pmA screen of the pcb will be good? Want the list in particular of all the parts choiches?And..hey, thank you very much for the title of this books, was somenthig that I was searching!

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 03, 2018, 12:16:21 pm
content: I have designed a new schematic with the ADCMP580, I feed the input signal with a schmit oscillator (10Mhz, using two NC7SZ14M5X) the 13th pin connected to -5V connected with a cap to pin 15 (to gnd) the output is grounded with a 50ohm resistor (because I have 1Mohm Z oscilloscope), the -5V rail is created with a LTC660CS8. The schmit oscillator is connected to +5 through a voltage divider, feeding 3V (the input of the ADCMP580 can only accept +3V and -2V. Vtp pin is feeded by 1.5V using a voltage divider. I have also used a power divider to have a trigger signalThis is the oscillatorhttps://imageshack.com/a/img922/3489/NMzr2K.png

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 04, 2018, 03:26:27 pm
content: First layout of the new board (It can be smaller, but I don't have an hot blow air gun, so Ill' not solder properly the components if the will be too much close)https://imageshack.com/a/img923/3610/VUswoC.png

author: capt bullshot
author_rank: Super Contributor
timestamp: January 04, 2018, 03:35:33 pm
content: I don't understand the purpose of the many white dots spread around the board ...Anyway, this may work in the sense "it may give you some weird pulse output", but for sure not in the sense of "clean pulse with fast rise time". You'll need a good ground plane and very short and/or impedance controlled traces from the ADCMP580 output to the connector.And I don't see any of the necessary decoupling caps around the ICs.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 04, 2018, 07:16:53 pm
content: Quote from: capt bullshot on January 04, 2018, 03:35:33 pmDon't ask me why there are that dots..don't knowFor the caps my bad..I've done another layout, with a good ground planeOverall:https://imageshack.com/a/img923/9678/hIgiCj.pngBottom only:https://imageshack.com/a/img923/4848/H30Vfl.pngTop only:https://imageshack.com/a/img922/3553/gn1UpZ.png

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 04, 2018, 07:37:06 pm
content: All C1 are decoupling caps

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 04, 2018, 07:57:11 pm
content: Added two plates to solder DC(With dec. cap) , dec. cap at usb VCC and R7 termination for the output (forget)Top only:https://imageshack.com/a/img922/9158/sbXS4P.png

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 04, 2018, 08:42:22 pm
content: Advices?

author: capt bullshot
author_rank: Super Contributor
timestamp: January 05, 2018, 09:48:31 am
content: Try to make the ADCMP to connector trace shorter, and place a ground plane on the top side also. Can't tell you anything but a guts sense about controlled impedance, but this trace looks it could be wider for this purpose. Find yourself layouts with controlled impedance paths as an example of what it should look like.Try to make the traces from your decoupling capacitors shorter and bring the cap as near as possible to the ADCMP chip.Don't route the capacitors and the traces "away" from the small logic chips.Didn't check your schematic anyway, you could give it a try now and maybe do corrections and improvements next step. The schematic using the logic chips as oscillators isn't very readable caused by the symbols you made. Better use correct logic gate symbols and clean up the signal path if you want others to be able to read the schematics. The way you've done it looks OK if it's a one shot and for your personal purpose only, but you won't understand it anymore next year ...Building such a fast edge pulser isn't a one step and finished process.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 05, 2018, 12:13:30 pm
content: Quote from: capt bullshot on January 05, 2018, 09:48:31 amThank you for the advices, ill do rhis improvment tomorrow, I know that is something very difficult to built, I made several layouts, I think that could be better if also add a power plane on the bottom (switching the ground pland on the top avoiding via for decoupling caps(Also O have the schematic for this)

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 12:42:28 am
content: Quote from: capt bullshot on January 05, 2018, 09:48:31 amToday I have made a new layout, reducing all gaps, the signal traces, and adding other stuffOverall:https://imageshack.com/a/img923/7664/bqb1dQ.pngBottom:https://imageshack.com/a/img923/6348/58OA42.pngTop:https://imageshack.com/a/img924/4724/e5sumn.png

author: capt bullshot
author_rank: Super Contributor
timestamp: January 06, 2018, 10:34:46 am
content: Looks like there's missing some traces? VCC isn't connected, is this a 2 layer board, or did you place these traces into the internal layers of a 4 layer board?Otherwise: looks good, maybe you want to add some more vias to connect the top and bottom GND planes near the GND pads of the capacitors and ICs.Try to move the ADMCP output termination resistor (R7) as close as possible to the IC. The output pulse trace doesn't look impedance matched to me, but I can't help you here. It's out of my scope, never done this in own designs, some basic formulae exist for common PCB materials, you might find some examples of impedance controlled tracks here in the forum in other pulse generator threads. Otherwise: keep this track very very short and controlled impedance does matter less and less. Your layout still leaves room to move the SMA connector closer to the ADCMP chip.In general:If you place traces through a plane, the plane gets split or slotted (as you can see for the top layer). Having a solid plane on the other side of the board and placing vias along the traces helps bridging the gaps, basically useful when you only have a 2 layer board and need to place traces through an otherwise solid plane.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 11:56:06 am
content: Quote from: capt bullshot on January 06, 2018, 10:34:46 amThe bottom plane is the vcc plane and all the VCCS are connected to it, the 7 vias that you see are for the VCC on the bottom plane (VCC)Unfortunally is prdtty zoomed, the connector is only 1.02 cm from the ADCMP (isn't that short otherwise, but I have to solder all of them with the iron) I have tried to keep VP trace (in) and Q (out) of the same lengh (they are exactly 1.02mm) and even the trigger is of the same lenght, all the decoupling cap are more or less (I 've tried my best) at the same distance from the ADCMPI think that will become inpractical to have shorter gaps, cuz for the soldering method I will use (iron)If you have more advices, Ill be very happy! (Ill move R7 closer)

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 12:02:42 pm
content: The board is 5×5cm

author: capt bullshot
author_rank: Super Contributor
timestamp: January 06, 2018, 12:19:31 pm
content: OK, you've got GND on top layer and VCC on bottom.Well, it should work, as the only critical part is the power supply and output side of the ADCMP chip.But, doing so breaks up the GND plane in a lot of smaller and poorly connected sub-planes, which is not optimal. I'd recommend bridging the slots (where the traces route through the top layer plane) by placing a via to bottom, a short trace to the other side of the slot and a via back to top. It's redundant in the sense of ERC / DRC, but helps a lot with higher frequency stuff.For example, the plane around the output connector is quite separated from the rest by the trace from U30 to R2 / R3. Bridging this trace at a few places would improve this. Another place where I'd put a bridge is across the trace from R10 to U1.If it was my design, I would have placed GND planes on both sides, routed as few as possible traces on the bottom and used vias to bridge these traces by placing them along the traces, maybe one per 5mm or so.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 12:35:32 pm
content: Quote from: capt bullshot on January 06, 2018, 12:19:31 pmI think that having VCC on bottom and GND on top is better on a 2 layer board, and appling your idea of the vias to connect the segmented zones of the top plane (VCC) it should be just perfect, I hope that someone can help me with the impedance control, giving me advices. Also with this metod Ill have 400pF of capacitance between the layers. Thank you for this trick, Ill post another layout today!

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 01:59:36 pm
content: Layout update-Improvement= R7 closer to ADCMP - Segmented zones of the top plane (VCC) connected by VIAS (1mm vias-1mm traces)Overall:https://imageshack.com/a/img923/9057/0l48GZ.pngTop:https://imageshack.com/a/img922/5496/vnoJCk.pngBottom:https://imageshack.com/a/img924/2947/4g5uro.png

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 02:04:46 pm
content: And what do you mean when you say that the ADCMP supply is critical? what should I do?

author: capt bullshot
author_rank: Super Contributor
timestamp: January 06, 2018, 03:07:50 pm
content: Layout: make the bridges as short as possible, try to connect all segments of GND around U1 together using such bridges, but don't split your VCC plane.The power supply is critical in the sense that the decoupling capacitors must supply the chip with a stable voltage while the current consumption of the chip has very fast spikes. So it is important that the capacitors are tightly coupled to the supply pins, and a solid ground plane exists. This applies in general to any fast chip, these can draw nanosecond current spikes while the outputs or internal nodes are switching. The conductors from the power source to the chip have a resistive and an inductive component, the very fast spikes cause high voltage drop across the inductive component. So you reduce the inductive component by keeping the supply traces (including GND) as short as possible to the source (or the next decoupling cap, they serve as the source in this heavily simplified model).Read the chapter Power/Ground layout and bypassing, page 12 of the ADCMP580 datasheet. You won't be able to fulfill this with a simple 2 layer board, but try to get near to it.Anyway, I guess the layout should work and give a better result than a flying wire prototype, but would not achieve what is possible with a impedance controlled multi layer board, so it is a good compromise for a first shot. Post your results.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 04:55:14 pm
content: Quote from: capt bullshot on January 06, 2018, 03:07:50 pmI don't want to waste money, for this project the total will be 80euro, not that much, but don't want to waste money (I know that electronic in a lot of cases can be a trial n' error, but want to limit it), and I want it to works very well (control impedance..eh..)In this layout I have added extra decoupling caps at the supply terminals (100uF tant), adjusted the lenght of the traces to connect the same plane, and add few of those vias near U1EDIT:Bottom:https://imageshack.com/a/img922/7081/Z0R7Je.pngTop:https://imageshack.com/a/img923/327/pxdT3z.pngOverall:https://imageshack.com/a/img924/9841/VK5bxw.png

author: capt bullshot
author_rank: Super Contributor
timestamp: January 06, 2018, 06:59:40 pm
content: I'm missing some as short as possible connections from the GND pins of all the C1 around U1 to the GND plane at the output connector. Maybe you place another horizontal GND trace with some via to top below U1, and remove the redundant one that appears to be underneath the upper pin of R7.Otherwise (except the controlled impedance trace) I don't see any more improvements.Be sure to check your schematics, anything done wrong with U1 isn't easy to bodge with this package, other mistakes can be easier corrected if necessary.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 06, 2018, 08:55:04 pm
content: Quote from: capt bullshot on January 06, 2018, 06:59:40 pmThe improvement was the 100uF tant cap near the supply pads (they were 100nF MLCC)Now I have made a square under U1 connecting each angle with a via to top plane (GND) filling the square with 2 mid traces. I Have also routed a trace between the central pad (It have a via) to a larger copper area, and in the central pad now there are connected all the gnd pins. I think that will help with redundancy.Also thank you very much for this support, I am very thankfull to youOverall:https://imageshack.com/a/img923/8075/CxUhOM.pngTop:https://imageshack.com/a/img924/9606/DHoKHz.pngBottom:https://imageshack.com/a/img923/5850/MWyKX7.pngAlso Ill check it hundreds of times before sending the order, I have to be sure that all is perfect

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 11:43:08 am
content: Quote from: capt bullshot on January 06, 2018, 06:59:40 pmI have made the schematic, if there is something wrong please tell me, I hope that this will be useful for someoneI have only few questions..I have a 1M input scope..so I need of 50ohm of impedence in output of the circuit, so R7 isn't necessarily because the sma connector is 50 ohm impedence right? the decoupler caps are also right?Schematic:https://imageshack.com/a/img922/6053/8lKQqe.pngOverall:https://imageshack.com/a/img924/4003/THbTkt.pngTop:https://imageshack.com/a/img922/4952/T4HroB.pngBottom:https://imageshack.com/a/img922/762/gehGiW.png

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 11:44:27 am
content: This are the final results, if nothing is wrong Ill order all the necessarily this week, and as soon as possible Ill post all the results!

author: capt bullshot
author_rank: Super Contributor
timestamp: January 08, 2018, 12:03:18 pm
content: I've had another look into the ADCMP 580 datasheet:The IC is designed to drive a 50 Ohm transmission line and includes the back termination. So you won't use R7 in your circuit, but you've got to use a 50 Ohms feedthrough terminator at the end of the cable, just plugged into your scope scope. If you don't terminate the cable, you'll see all kind of reflections - if the scope is fast enough and the cable long enough.Leaving R7 in the circuit and using the 1M input will give you a different (worse) result, even if you connect the SMA directly (using only a suitable adaptor, no cable) to the scope.If you really want to see all these details (fast rise time, different terminations and their effects), you'd need a GHz scope, they usually have built-in switchable termination.Supplying the inverters from a voltage divider is a bit unusual, but I don't see an issue, should work.You don't need a decoupling cap at the -LE and HYS inputs, they might even disturb the IC, so remove them, or just do not populate.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 01:04:45 pm
content: Quote from: capt bullshot on January 08, 2018, 12:03:18 pmOh, there are very preacius advices! So ill remove the dec cap from hys and-le and also R7I was in conflict aboit ehat to do with R7, I know that the sma conmector was 50ohm so R7 was usless, but want to be sure, so sma connector and a feedthrough resistor on the input of the scope! Thanks for the advices!

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 01:11:28 pm
content: Quote from: capt bullshot on January 08, 2018, 12:03:18 pmThe decision to drive the ICs with a voltage divider come from the though tha putting a voltage divider on the trasmission line will added parisitic effectn tha will disturb the line (my thought) so is more simple to drive the Ics at 3V using a voltage divieder, without splitting the under plane using another plane attached to a 3V regulator

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 01:57:53 pm
content: This are the finished schematics and pcb layouts, I hope that someone will found this interesting or usefulSchematic:https://imageshack.com/a/img924/7074/KRxdqS.pngPcb overall:https://imageshack.com/a/img923/1192/WwWUhd.pngPcb top:https://imageshack.com/a/img922/1075/92gRXg.pngPcb bottom:https://imageshack.com/a/img922/4150/8OO7HO.pngI am very thankful to you Capt Bullshot because you have helped me a lotAs soon as possible I will assemble the unit and posts the results (I have a rigol 1054Z.. can't to that much at this level of rise times, but I will buy a GHz scope in the imminent present)If there will be any question I hope that someone will help meNia Debesis

author: capt bullshot
author_rank: Super Contributor
timestamp: January 08, 2018, 04:02:08 pm
content: Quote from: NiaDebesis on January 08, 2018, 01:11:28 pmUsing a voltage divider along the signal path would have been the usual way, and wouldn't have negative impact on your signal. Together with the ADCMP580's input termination, a single series resistor does the job. And you can use the NC7S series instead of the NC7SZ, these work from 2...6V Vcc and can be directly fed by 5V.Another issue with your schema is: The ADCMP 580 input termination (50 Ohm) places an additional load on the voltage divider, so the second 7SZ14 supply is reduced by that. For a approximate square wave, the input termination places 100 Ohm in parallel to R8-1.And usually this kind of oscillator is built using an unbuffered inverter (e.g. 'HCU04), not a schmitt trigger ('14). Should work anyway, this kind of circuit is quite forgiving.The ADCMP580 has quite high current consumption for the negative voltage, did you check the LTC660 is able to deliver that?

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 06:39:47 pm
content: Quote from: capt bullshot on January 08, 2018, 04:02:08 pm1) The NC7SZ14M5X can be drived with 5V, but the output will go from 0 to 5, and the ADCMP580 only accept 3V, so if I feed them at 3V the voltage will go to 0 from 32) Technically, If I remove the voltage divider, and feed the ic's directly to 5V, and add a parallel resistor of 120ohm to R10, should be fine? I ll have 2.9V I think3) I have chosen this type of Ic's because they are fast, my other options was the SN74LVC1G14DCKR in the same configuration (switiching the NC7SZ14M5X4 to SN74LVC1G14DCKR)4) According to the schematic from the negative supply it absorb 40mA more less, this supply go to 100mA so I am fine

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 07:08:54 pm
content: Quote from: capt bullshot on January 08, 2018, 04:02:08 pmPoint 2 schematichttps://imageshack.com/a/img924/7004/6ROQTN.png

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 08:55:46 pm
content: Quote from: capt bullshot on January 08, 2018, 04:02:08 pmAlso checking another time on the datasheet of the ADCM, is better to have input and output matching, and in this case (parallel solution) Ill have 85ohm input.. and the out is 50..

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 08, 2018, 10:32:47 pm
content: The solution is maybe to use only one voltage divider? I don't know what to do at this point..I am stressedFor example using one SN74LVC1GX04DBVR, using 1K resistor 1M resistor, the 16pF caps and the 10MHz quartz, using only one voltage divider, is specified for partial power down..

author: capt bullshot
author_rank: Super Contributor
timestamp: January 09, 2018, 11:02:09 am
content: My suggestion regarding the voltage divider is this:Use logic gates that have a 5V supply (like the NC7S series, or a 74HCU04 which would be the best choice for an Xtal oscillator), and place a single resistor from the output of the second inverter to the ADCMP input.The ADCMP's internal termination resistor together with this external resistor forms a voltage divider. In this special case (signal is originating a few mm from the ADCMP input) no impedance match is necessary for the input.Edit: checked your new schematic, yes you've done it the exactly the way I mentioned. I'd just recommend to use the NC7SZU04 for the oscillator (left one) and the NC7SZ04 or NC7SZ14 for the buffer (right one).Looks like the R10 / R45 is shorted in you schematic.There's also no need to equalize track lengths around the oscillator. In case you build you generator with a differential output (both output pins of the ADCMP used), this would be the only point (the tracks from ADCMP to SMA connectors) where you'd equalize the track lengths.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 09, 2018, 11:50:51 am
content: Quote from: capt bullshot on January 09, 2018, 11:02:09 amYea but the problem is the power divider, tha goes on the trigger out, to have 3V in the resistor in the adcmp580 I have to put a parallel resistor of 120ohm to R10, to have 33ohm in series to the internal resistor pf the adcmp, having 3V, but this would increase the power in input of the adcm, having less power on the trigger out, so I think that will be better modifing r11 and r10 to be both 33ohm, so the power will be equal and the inpit voltage will be of 3V at the ends of the 50ohm internal resistor of the adcmpRight?

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 09, 2018, 12:05:04 pm
content: Quote from: NiaDebesis on January 09, 2018, 11:50:51 amPtherwise when I arrive at home Ill do another schematic, because in this way is confusing

author: capt bullshot
author_rank: Super Contributor
timestamp: January 09, 2018, 12:48:42 pm
content: There's no need to build a power splitter for the second inverters output. This is just a 10MHz signal running through short traces, this may be treated like DC in this context, there's no impedance matching required for the purpose of feeding the ADCMP and providing a trigger output. Loading the inverter with 50 Ohm is too much for this chip, so you'd anyway have to go for a higher impedance here.You don't need 3V input level for the ADCMP580, lower levels will also work fine.No, it's all way much easier:For example, set the inverting input to 0.25V (using the pull-up resistor and the built-in termination) and set the level at the non-inverting input to 0.5Vpp. This can be easily achieved by a 10:1 voltage divider (50 Ohm internal, and 450 Ohm series resistor). Use a 1k pullup for the inverting pullup to 5V, this gives you approx. .25V here.Then you could use the same resistor value (450 Ohm) in series with the trigger output SMA, this provides you with a 0.5Vpp signal into 50 Ohms and 5Vpp unloaded. This will be fine for triggering a scope.You can substitute the 450 Ohm resistors by a common value (like 470 or 430) with little to non impact on your circuit. The fast edge output waveform doesn't depend on the input matching of the ADCMP, only on the output signal layout and impedance matching.So just place a 1k resistor from 5V to VN (Pin 3) and a 470R resistor from Y (inverter output) to VP (Pin 2). And another 470R from Y to the trigger out SMA, that's all you need.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 09, 2018, 01:01:17 pm
content: Quote from: capt bullshot on January 09, 2018, 12:48:42 pmIsn't better to set the inverting input to 1.5 volt and feeding the non inverter input with 3V?I think that is more simpleOnly change R10 and R11 to 33ohm resistor and nothing more, and also replace the osc and inverter Chips woth what you mentioned before

author: capt bullshot
author_rank: Super Contributor
timestamp: January 09, 2018, 01:37:40 pm
content: Quote from: NiaDebesis on January 09, 2018, 01:01:17 pmIn general, yes. But the 33 Ohms place too much load on the output of the inverters, these are not able to drive this to the full output voltage and may be overloaded. So you've got to go for higher resistance values here.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 09, 2018, 04:46:47 pm
content: Quote from: capt bullshot on January 09, 2018, 01:37:40 pmhttps://imageshack.com/a/img923/493/20MqJf.pngSo know I think that is ok right?

author: capt bullshot
author_rank: Super Contributor
timestamp: January 09, 2018, 06:38:26 pm
content: Yes, looks OK

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 09, 2018, 11:27:46 pm
content: Quote from: capt bullshot on January 09, 2018, 06:38:26 pmNew pcb finally done, I hope that know Is all in the right place in right amountand end this project for know ahahSchematic:https://imageshack.com/a/img922/6245/bsxb5t.pngOverall:https://imageshack.com/a/img922/6796/5ap3fU.pngTop:https://imageshack.com/a/img922/7850/fqMVdc.pngBottom:https://imageshack.com/a/img922/77/xP4FAL.pngI have also flipped all the caps for reducing the risk fo cracking some of them when connecting the sma connectors, only precaution

author: capt bullshot
author_rank: Super Contributor
timestamp: January 10, 2018, 09:10:13 am
content: Yes, looks OK.IMO there's still room left to move the SMA output nearer to the ADCMP chip. This is the only place you can improve the output pulse with this design (the shorter the trace, the better).

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 10, 2018, 04:51:18 pm
content: Quote from: capt bullshot on January 10, 2018, 09:10:13 amNow the SMA connector is 3,4mm closer to the chip, is the max length that I can achieveTop:https://imageshack.com/a/img922/7513/QY4Oje.pngBottom:https://imageshack.com/a/img922/9607/hwKDMa.pngOverall:https://imageshack.com/a/img922/5841/8maIvM.pngIn your opinion is well designed?

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 10, 2018, 05:00:36 pm
content: EDITTop:https://imageshack.com/a/img923/772/J3oKGn.pngBottom:https://imageshack.com/a/img924/576/tTX7SF.pngOverall:https://imageshack.com/a/img922/2268/opy1zd.pngI have reduced VEE trace

author: capt bullshot
author_rank: Super Contributor
timestamp: January 10, 2018, 05:02:35 pm
content: Looks OK to me.

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: January 10, 2018, 06:49:30 pm
content: Quote from: capt bullshot on January 10, 2018, 05:02:35 pmTo be sure I've also gived a little bit gap between components (min gap 1.56mm) I' have increased of .50mm the distance from the ic of some decouplers..but I think that will be worth for signal integritySo..here we are, this are the final schematics and layout (I Hope..) I also hope that this thing will achieve very fast rise times and a have a flat top pulse (Is very..very difficult that this will happen..because is my V1.0..so, who knows, will test this soon as possibileOverall:https://imageshack.com/a/img922/8636/67Vx8U.pngTop:https://imageshack.com/a/img922/5893/Nm2huD.pngBottom:https://imageshack.com/a/img923/9691/Vut9vC.pngSchematics:https://imageshack.com/a/img922/8030/ry7pZF.pngThese are also the measure of decoupler tracesDistance of C1 to VCC Top ADCM (central pad to central pad, including the length of the via to VCC) 4.89mmDistance of C1 to VCC Top ADCM (central pad to central pad, including the length of the via to VCC) 4.76mmDistance of C1 to VEE ADCM (central pad to central pad, including the length of the via to VEE) 5.95mmDistance of C1 to VCC LTC660 (central pad to central pad) 3.81mmDistance of C1 to VN (central pad to ADCM to top of C1) 3.44mmDistance of C1 to osc and inv ic's (Including diagonal nodes) 5.3mmLength of I/O tracesOut length (central pad to central pad) 7.87mmIn length (central pad to central pad) 7.62mmTrigger lenght (central pad of sma, to central pad of top R11 plus the trace between down pad of R11 to first pad of R10) 8mm

author: moore
author_rank: Contributor
timestamp: January 18, 2018, 03:06:53 am
content: Just read through the whole thread, interesting to follow the development process. Did you get a chance to build and test one?

author: NiaDebesis
author_rank: Frequent Contributor
timestamp: June 05, 2018, 08:36:34 pm
content: Want to revive the topic, the project is in stop, because that was a difficult period, now I' ve ordered the pcb, I'll post the photo as soon as possible