Help with layout High voltage converter MC34063 for Nixie tubes  - Page 1
Forum section: electronics / projects

author: matb
author_rank: Regular Contributor
timestamp: March 01, 2022, 04:56:09 pm
content: Hi everyone,some time back I posted about a high voltage power supply based on a NE555 to power 6 nixie tubes.That design had lots of negative remarks that the NE555 is not an IC made for such a task.So now after searching on Dave's channel I found his Nixie Tube playlist and that he was usinghttps://threeneurons.wordpress.com/nixie-power-supply/hv-supply-kit/which is the design I used (NK02) but I'm going for CMS parts only.Can you tell me if my layout seems good and if the components I chose are rated for such a task ? Also if the potentiometer seems wired correctly I am a bit confused by him.It will be my first power supply design feel free to critique it.The idea for the moment is just to get the power supply working, then I will create a PCB that will have the clocks and all the circuit to control them.Thanks for your input.Farnell numbersEdit :C1 680p 50Vhttps://fr.farnell.com/en-FR/avx/08051a681jat2a/cap-680pf-100v-5-c0g-np0-0805/dp/2280662?ost=2280662C2 680µ 35Vhttps://fr.farnell.com/en-FR/rubycon/35trv680m12-5x16/condensateur-680-f-35v-cms/dp/2535794C3 0.01µ 100Vhttps://fr.farnell.com/en-FR/avx/08051a681jat2a/cap-680pf-100v-5-c0g-np0-0805/dp/2280662?ost=2280662C4 2.2µ 400Vhttps://fr.farnell.com/en-FR/vishay/mal215299601e3/cap-2-2uf-400v-alu-elec-smd/dp/3288157?ost=3288157C5, C6 100n 50Vhttps://fr.farnell.com/en-FR/kemet/c0805c104z5vactu/cap-0-1-f-50v-y5v-0805/dp/2581082?ost=2581082C7 330p 250Vhttps://fr.farnell.com/en-FR/vishay/vj0805d331kxpaj/cap-330pf-250v-10-c0g-np0-0805/dp/2134071?ost=2134071C8 10n 50Vhttps://fr.farnell.com/en-FR/samsung-electro-mechanics/cl21b103kbannnc/cap-0-01uf-50v-mlcc-0805/dp/3013470?ost=3013470C9, C10 100n 250Vhttps://fr.farnell.com/en-FR/tdk/c2012x7t2e104k125ae/cap-0-1-f-250v-10-x7t-0805/dp/2525156?ost=2525156CR1 MC34063ACD-TRhttps://fr.farnell.com/en-FR/stmicroelectronics/mc34063acd-tr/dc-dc-conv-100khz-soic-8/dp/2463925?ost=2463925D1, D3 1N914https://fr.farnell.com/en-FR/on-semiconductor/1n914bws/diode-small-signal-100v-sod-323f/dp/2453274?ost=2453274D2 ES3Jhttps://fr.farnell.com/en-FR/on-semiconductor/es3j/diode-rectifier-3a-600v-do-214ab/dp/2101176?ost=2101176F1 2A 125VDChttps://fr.farnell.com/en-FR/littelfuse/0451002-mrl/fuse-2a-125vac-vdc-very-fast-smd/dp/2383274?ost=2383274L1 100µH 2Ahttps://fr.farnell.com/en-FR/bourns/srr1280a-101m/inductor-100uh-2a-20-power/dp/2374166RLQ1 SST2907AHZGT116https://fr.farnell.com/en-FR/rohm/sst2907ahzgt116/transistor-pnp-60v-0-6a-sot-23/dp/2706710?ost=2706710Q2 IRF740https://fr.farnell.com/en-FR/vishay/irf740aspbf/mosfet-n-400v-10a-d2-pak/dp/8657815?ost=8657815R1 1khttps://fr.farnell.com/en-FR/te-connectivity/crgh0805j1k0/res-1k-5-0-33w-0805-thick-film/dp/2331796?ost=2331796R2 475khttps://fr.farnell.com/en-FR/panasonic/erjp06f4753v/res-475k-1-0-5w-0805-thick-film/dp/2312266?ost=2312266R3 392khttps://fr.farnell.com/en-FR/panasonic/erj6enf3923v/res-392k-1-0-125w-0805-thick-film/dp/2303829?ost=2303829R4 13.7khttps://fr.farnell.com/en-FR/panasonic/erjp06f1372v/res-13k7-1-0-5w-0805-thick-film/dp/2326695?ost=2326695R5 4.02khttps://fr.farnell.com/en-FR/panasonic/erjp06f4021v/res-4k02-1-0-5w-0805-thick-film/dp/2312246?ost=2312246R6 TC33X-2-203Ehttps://fr.farnell.com/en-FR/bourns/tc33x-2-203e/trimmer-pot-20kohm-25-1turn-smd/dp/2321852?ost=2321852R7 10khttps://fr.farnell.com/en-FR/te-connectivity-neohm/crg0805f10k-10/res-10k-1-0-125w-0805-thick-film/dp/3399587R8 0805 1 ohm 125mWhttps://fr.farnell.com/en-FR/multicomp/mcwr08w1r00ftl/res-1r-1-0-125w-0805-thick-film/dp/2447598R9 0.22ohm 1Whttps://fr.farnell.com/en-FR/multicomp/mcww25xr220ftl/res-0r22-1-1w-2512-thick-film/dp/2696053?ost=2696053R10 100ohmhttps://fr.farnell.com/en-FR/multicomp/mcwf08p1000ftl/res-100r-1-0-25w-0805-thick-film/dp/2694094?ost=2694094

author: matb
author_rank: Regular Contributor
timestamp: March 04, 2022, 09:43:13 am
content: I made a through-hole breadboard prototype that is kind of working.I am getting a ~3Hz 150V that is falling rapidly but I guess that's because it's a breadboard prototype.I can show you an oscilloscope screen of that if that helps but that's not my point.My point is that I would like to go CMS for this power supply.

author: Ian.M
author_rank: Super Contributor
timestamp: March 04, 2022, 12:02:05 pm
content: Lets see your prototype. Solderless breadboards don't much like 1.4A pulsed currents - you probably need to assemble the inductor, MOSFET and input reservoir cap on perfboard, with supply and ground connected first to the perfboard, and then jumpered across to the breadboard.Also please explain "CMS parts".

author: matb
author_rank: Regular Contributor
timestamp: March 04, 2022, 12:08:59 pm
content: I will have to go to a PCB anyway and my tests on the breadboard are working enought that I want to build the schematic in a PCB.The only thing keeping me from ordering the design in message #1 is that I'm not sure the layout will work, neither if it will be capable of going to the range of +170V DC. For the moment I have all through-hole components to be able to test the design with the breadboard but my goal is to replace the through-hole components to only SMD components (sorry bad translation CMS → SMD)

author: Ian.M
author_rank: Super Contributor
timestamp: March 04, 2022, 01:07:00 pm
content: You should decrease the C1 L1 Q2 loop area and also put 100nF ceramic in parallel to C2 to reduce the HF impedance. The easiest fix for your layout would be to swap the positions of C2 and CR1 + Q1 and associated parts.Have a play with this LTspice sim of a boost converter very similar to your proposed circuit. I've added current limiting so it wont flux-walk into saturation and destroy itself if overloaded. Its also got a startup delay circuit to allow the initial charging current through the inductor of the output capacitor to decay.

author: matb
author_rank: Regular Contributor
timestamp: March 04, 2022, 01:34:06 pm
content: Wow thanks a lot that really helpful. The startup delay is a very good addition to the schematic.Just to be sure the R1, C8 and R2 of the spice model is the current limiting ? C6, R5 and D3 is the delay as written.What is the current limited to ?What is the I1 ? Variable resistor ?If I remember correctly MLCC capacitors should be doubled in the case of failure (IIRC Dave said that in some videos) what do you think should C2, C8, C5, C6 be MLCC or another type of capacitor ?

author: Ian.M
author_rank: Super Contributor
timestamp: March 04, 2022, 02:14:25 pm
content: Yes, R1, C8 and R2 is the current limiting. Place the current shunt resistor R1 right next to the inductor, and the other parts next to the chip. C8 and R2 provide leading edge blanking, so the current limit doesn't trip on induced transients. Current limiting is explained in T.I'sSLVA252B "Application of the MC34063 Switching Regulator", section '1.3 Current Limit'. The limit trips when the Ipk sense pin (7) is approx. 330mV below Vcc, so in this case 1.5A. The peak will exceed the trip point a bit as once tripped it has to charge the timing capacitor to the oscillator's upper threshold, so you may need to increase R1 experimentally to reduce the limit. Due to poor availability of sub-one ohm resistors in anything other than E12 series values, you may also want to add pads for an extra resistor in parallel with R1 to allow you to trim the peak current upwards.N.B. the SLVA252B stated minimum sense resistor of 0.2 ohm can be ignored, as you are using an external switching transistor with much higher current capability. Use whatever comes out of the design equations when you plug in your inductor's saturation current, but do check the resulting peak wont violate your MOSFET's SOA at max. temperature.Double up (in parallel) the decoupling caps C2 and C5. C3, C6 and C8 can't sensibly be doubled - C3 and C8 are so small value they wont have very thin layers so are more robust, and C6 although nice to have is non-critical, as the IRF740 SOA curves show it can withstand over 20A for 10ms and at 12V in it will be RDS(on)limited so cant exceed that. If you are worried about the input capacitor or the MOSFET failing shorted, add a polyfuse in series with 12V in.

author: Ian.M
author_rank: Super Contributor
timestamp: March 04, 2022, 03:55:26 pm
content: I've just tweaked the design to add a voltage doubling rectifier. This may be advantageous for a number of reasons - it allows you to use a lower voltage MOSFET and lower voltage rectifier diodes (possibly 100V Schottkys) and also reduces the 'dead time' forced by the MC3x043A's 84% max duty cycle providing excessive time for diode conduction. Performance is very similar with a slight improvement in output current capability at the cost of four extra parts. Unfortunately the voltage ratio is still too high so the boost converter is still in discontinuous mode. To fix that you'd either have to switch to a controller with a significantly higher duty cycle limit and built-in support for continuous mode, or if sticking with the MC3x043A, use a tapped inductor or a tripler rectifier (to increase the minimum off time) and add considerable complexity to provide variable current limiting so it doesn't drop out of continuous mode at the anticipated minimum load current.The attached sim needs models from the one above - drop it in the same folder.

author: matb
author_rank: Regular Contributor
timestamp: March 05, 2022, 01:39:43 pm
content: Thank you for you kind work, I think I will keep the 170V_boost from response #6.I updated the schematic with a fuse and all the components added from the Spice design.Is the schematic.Added pieces are :Fuse F1 Farnell code 3771734 (not sure if this one specifically will be of any use I guess I will have to take a big 12V@6A wall-wart to have a real current in case of a shortC5, C6 100nF 50V #2581082C9, C10 100nF 250V #2525156R8, R9 0.22ohm 1W #2696053 (there is little choice for 0.20ohm on Farnell) one of the two will be unpopulated depending on resultsR10 100ohm 250mW #2694094C7330pF 250V #2134071 (there are no 320pF on Farnell is the 320pF to 330pF a problem ?)C8 10nF 50V #3013470Layout part :QuoteAs a lot of things have changed I tried to do that but I'm a bit confused by all of it, I shared the Kicad project if that is usefull for anyone.https://drive.google.com/file/d/1DNUuidlsC-wN83WO0X8EjcAWbsxcOnSK/view?usp=sharing(Seems like I can't share rar files directly)is the 3D modelis the rooting (but I actually didn't trace anything yet as I would like confirmation on the layout first)

author: Ian.M
author_rank: Super Contributor
timestamp: March 05, 2022, 02:47:31 pm
content: The fuse shouldn't be much over the peak inductor current, and it could even be a bit lower as the average inductor currents is under half that as the boost converter runs in discontinuous mode.R8||R9 gives 0.11 ohms, so Ilim is 330mV/0.11 ohms =3A, but your inductor says 1.6A, so unless its datasheet says otherwise you've got a problem!Watch the inductor and MOSFET smoke while the fuse stays cool!Sorry about the confusion. C2, *NOT* C1. The critical loop area is the input decoupling cap - inductor - MOSFET, and ground back to the input cap loop. Move C2, J1 and F1 outside the board outline and rip up associated tracks. Also rip up the tracks to the current shunt resistors, C5 and C6 and to the MOSFET gate. Slide everything round the IC over to the bottom right corner as-is. Bring C2 back onto the board next to the legs of the MOSFET, + to the right and put C5 and C6 right next to the input side of the current shunt. Route wide short tracks linking the caps, current shunt and inductor, then place the fuse and input connector back on the board and route those, then let autoroute sort out the rest.

author: NiHaoMike
author_rank: Super Contributor
timestamp: March 05, 2022, 04:20:40 pm
content: You'll have a much easier time starting with a flyback or "flyboost" (boost + flyback) design, which won't have the extreme duty cycle problem.

author: matb
author_rank: Regular Contributor
timestamp: March 05, 2022, 05:06:20 pm
content: So the fuse should be rated for what 1.3A ?Just noticed the inductor info is even more wrong it's a 1.3Ahttps://fr.farnell.com/en-FR/multicomp-pro/mp002851/inductance-de-puiss-100uh-blind/dp/3370508https://www.farnell.com/datasheets/2918522.pdf. There is no mention of peak current what should I expect x2, x3 ?So doing the calculations Ilim = 330mV / 0.22ohm = 1.5Amps so still too much I should go for a 1.3A = 330mV / 0.25ohm right ?There is no 0.25 in stock at Farnell if I take 1.375A = 330mV / 0.24ohm is it still in tolerance ? Or another solution is to take 2 x 0.5ohm ?What should be the power dissipation of the current shunt resistor(s) ?is the new layout after I followed your instructions, does that seem right ? (I have not rooted yet all the traces just the caps, current shunt and inductor.

author: Ian.M
author_rank: Super Contributor
timestamp: March 05, 2022, 06:24:02 pm
content: The inductor datasheet says:QuoteA 25% drop in inductance is well onto the knee of the B-H curve, and personally I'd prefer not to exceed 95% of that current, to allow a bit of margin for other component tolerances. If you are staying with that inductor you'd be designing to slightly over 1.2A peak with a 0.27R shunt and could fuse at the peak current as the average input current is significantly lower. Do put in a realistic value for the 220uF input capacitor's ESR and check its RMS ripple current during the load pulse, then make sure your cap is rated for that.Depending on the output power you need, you may need a beefier inductor.https://fr.farnell.com/en-FR/bourns/srr1280a-101m/inductor-100uh-2a-20-power/dp/2374166RLlooks like a likely candidate - it has 2A saturation current so would be fine running with a 1.8A current limit.The layout is much improved but still looks a bit funny round the current sense resistors, with too narrow tracks to the inductor and C2.The input current ramps from 0 to Ilim over at most 84% of the whole cycle. Although it is possible to calculate the RMS power, its far easier to sim it - increase the pulsed load current till the output starts to droop, so you know the boost converter is working flat-out, then Alt-click R1 in the sim to plot the power dissipated in it. Select the time period corresponding to the load current pulse and ctrl-click the title of the power waveform to get the average power, I'm getting approx 127 mW so if it was a single resistor, a 1/4W resistor would probably be suitable. You've got two shunt resistor footprints so the total power is split between them and you can choose values to get closer to what you actually want e.g. 0.47R || 0.56R gives 0.256R though if I wanted 0.25R I'd probably start with a single 0.27R resistor capable of handling the total power, then put a much smaller footprint 3.3R resistor in parallel to trim down to 0.25R. As the 'trim' resistor carries less than a tenth of the current, its dissipation will be negligible. Apart from saving needing to order so many large package high dissipation SMD resistors, the smaller 'trim' resistor footprint also eases layout.

author: matb
author_rank: Regular Contributor
timestamp: March 07, 2022, 07:50:02 am
content: Ok let's go with the 2A one, going with 1.8A, R = 330mV / 1.8A = 0.183ohmThen I replace for exemple R8 to a 0804 footprint and I can try multiple values, this ref is a 0.18ohm 5% so I should not need a second resistor, correct ?https://fr.farnell.com/bourns/crl1206-jw-r180elf/res-couche-epaisse-0-18r-5-0-25w/dp/2328140As 330mV / 1.8A = 0.183ohm and 330mV/0.18ohm = 1.83AQuoteI will update the pcb traces and R8 footprint to be a 0805 during the dayAbout the fuse would this one work as expected ?https://fr.farnell.com/en-FR/littelfuse/0451002-mrl/fusible-2a-125vac-vdc-tres-rapide/dp/2383274From my understanding I would have 2A (well 1.8A) being drawn max so according to the datasheet the opening time should not happen ? Or after 6 hours ? I'm confused by that.% of Ampere | Rating Ampere Rating | Opening Time100% | 1/16 –15 | 4 hours, Minimum200% | 1/16 –10 | 5 sec., Maximum| 12 –15 | 20 sec., Maximum

author: Ian.M
author_rank: Super Contributor
timestamp: March 07, 2022, 08:43:50 am
content: The peak current is 1.8A, so as the average*is far less than that, and much of the current ripple gets smoothed out by the input cap, a 2A fuse will *NEVER* open in normal operation. Its only there to prevent tracks burning if a component fails.Tweak the sim to match your proposed circuit changes (e.g. new inductor's internal series resistance, and 0.18 ohm current shunt) and run it to check the shunt dissipation and average input current.* Strictly speaking, even though the current is mostly DC, for pulsing fusing currents at repetition rates much faster than the thermal time constant of the fuse or shunt resistor, you need the RMS average, not the mean.

author: matb
author_rank: Regular Contributor
timestamp: March 07, 2022, 09:09:56 am
content: On LTSpice I'm getting R1 (shunt) an average of 81mW, the max is 500mW so I guess I will take a 1W to be very large.Plotting I(V1) doesn't seem to work I'm getting log drawing from -44A to ~0A.I also can't seem to find the ESR of the input cap to replace the one on the simulation. It's not written in the datasheet neither on google (at least I haven't found it)

author: Ian.M
author_rank: Super Contributor
timestamp: March 07, 2022, 10:22:57 am
content: Did you increase the load current till the output starts to droop? The converter needs to be working 'flat out' where you measure the average input current and power dissipated in the shunt. Alternatively measure it averaging over >50 cycles (for <2% error) just before the converter shuts off on startup when it reaches 170V.I'm getting 735mA average input current (793mA RMS) and 226mA RMS ripple current in C1. If you link the cap you are considering, I'll see if I'm luckier than you finding its ESR! If you can afford the board area it may well help to put two caps in parallel for C1 to improve the ripple current rating, reduce ESR, and split the dissipation so they run cooler for longer life.I'm getting 145mW in R1, so a 1/4W part would run rather warm, but with the width copper tracks it should be connected to, should be OK, but >=1/2W would be a better choice.What about mounting holes, or are you planning to use it as a PCB mount module?

author: matb
author_rank: Regular Contributor
timestamp: March 07, 2022, 12:29:50 pm
content: Though I had linked all the components I only took a screenshot of the bom, I'm going to edit the first message to have clickable links but anyway here's the one :https://fr.farnell.com/en-FR/panasonic/eeehb1e221p/cap-220-f-25v-radial-smd/dp/9696830?ost=9696830QuoteYou're right I didn't add mounting holes as this will be a "standalone" pcb that will then connect to my other one with 2 wires. I guess I will add M3/M4 mounting holes and buy screws so the pcb is not flat on the desk.

author: Ian.M
author_rank: Super Contributor
timestamp: March 07, 2022, 12:46:12 pm
content: Seehttps://en.wikipedia.org/wiki/Dissipation_factorESR of EEEHB1E221P calculates out as 0.96 ohms, and as its only rated for max. 190mA ripple current it isn't particularly suitable for this application, as the AC component*of the current drawn by the buck converter is 528mA RMS. It won't however destroy itself as its ESR is too high for it to pass excessive ripple current.As Farnell lets you search with ESR as a parameter, why not do so for capacitors with adequate voltage rating and ESR under 0.5 ohms and see what comes out as in stock. You may have to go to a higher value (or use multiple capacitors in parallel) to get the ratings you want.* Method: Plot I(R1) or I(L1), select the time interval of interest, take the average and edit the trace expression to subtract it then you can take the RMS of the AC component, which will be the upper limit of the ripple current as ESR tends to zero.

author: matb
author_rank: Regular Contributor
timestamp: March 07, 2022, 01:39:16 pm
content: I updated the original post with the ref I have on hands, I will update the remaining components when I can access the schematic.Would this one be a good replacement ? 680µF 35V 0.074ohm 1.2A Ripple current AC (not the same size as the previous but no problem)https://fr.farnell.com/en-FR/rubycon/35trv680m12-5x16/condensateur-680-f-35v-cms/dp/2535794

author: Ian.M
author_rank: Super Contributor
timestamp: March 07, 2022, 01:48:37 pm
content: Looks good. One of the clues its likely to be suitable for a switched mode application is it has ripple current specs for higher frequencies and impedance @100KHz.

author: matb
author_rank: Regular Contributor
timestamp: March 07, 2022, 05:29:38 pm
content: I changed the inductor and C2, here is the schematic. I added mounting holes, changed R8 to 1 ohm and changed inductor + C2 to reflect changes.is the 3D modelis the pcb, thin traces are 0.25mm, medium 1mm and big are 3mmpcb_rev4_layout.PNG(56.1 kB. 1627x665 - viewed 88 times.) is the pcb layout with ground on bottomis the pcb layout without ground on bottomThere are no 0.18ohm in stock so I want with a 0.22 and a 1ohm. Rtotal = 0.18 = 1 / ( 1 / 0.22 + 1 / x) so x = 1ohm correct ? (calculated withhttps://www.digikey.fr/fr/resources/conversion-calculators/conversion-calculator-parallel-and-series-resistor)I updated the original post with the full bom and the kicad archivehttps://drive.google.com/file/d/1DNUuidlsC-wN83WO0X8EjcAWbsxcOnSK/view?usp=sharing

author: Ian.M
author_rank: Super Contributor
timestamp: March 08, 2022, 05:56:50 am
content: I suggest a few changes in the C2 C5 C6 area to improve grounding by removing the long slot in the ground plane and shortening ground connections. It also takes Vcc directly from the shunt resistor, as it should be. Move C5 and C6 slightly towards J1 to make space for the third ground via. Also put a top-side ground pour between the MOSFET source and C2 Gnd, and stitch it to the ground plane with extra vias. Sorry about the horrible edit in a paint package, I hope my intentions are clear enough!I also advise more clearance round the bottom right mounting hole. Having a MLCC capacitor (C8) that close to a mounting hole is problematic, especially as its long axis is oriented towards the hole, so it will be maximally stressed by the board flexing near the fixing.

author: matb
author_rank: Regular Contributor
timestamp: March 08, 2022, 07:17:21 am
content: is the 3d viewis the pcb rootingis the layout with ground pour

author: Ian.M
author_rank: Super Contributor
timestamp: March 08, 2022, 07:53:23 am
content: Better. Move the current sense track to R10 to run next to the +12V/Vcc track to the IC to minimize the loop area and thus noise pickup, and it woud be pretty good.However what's happened to the feedback track from junction(R3, R4, R5) to pin 5 of the IC? When you put it back in, move C3 next to the chip so it can filter noise pickup on the long feedback track.

author: matb
author_rank: Regular Contributor
timestamp: March 08, 2022, 08:03:58 am
content: You are right I missed that !I moved C3 next to the IC, R10 track is next to the +12V line and added the R5 → CII lineI also forgot the GND on pad R7, just added it.

author: Ian.M
author_rank: Super Contributor
timestamp: March 08, 2022, 08:26:32 am
content: Looks reasonable. If it passes DRC and ERC you could go to production. However, and this is only a minor nit-pick, I don't like the use of two identical connectors for 12V in and 170V out, and I don't like the inconsistent ground pin placement on them. Make one three pin, and you'll never blow it up by plugging the cables in the wrong ends!

author: matb
author_rank: Regular Contributor
timestamp: March 08, 2022, 08:32:14 am
content: Thank you very much for your help ! Finger crossed this will work first tryQuoteGround is always at the bottom but I'm going to write with the silkscreen where is what. You are right I will probably have one green and one blue or something like that to tell them appart.

author: Ian.M
author_rank: Super Contributor
timestamp: March 08, 2022, 08:39:02 am
content: J1 has ground on pin 1 and J2 has ground on pin 2. That's just asking for mistakes assembling the cables. Flip one of them!Personally, I'd use a three pin connector for J2 and omit the center pin (pull it out of the housing) as it gives better creepage and clearance distances for the high voltage + prevents mixups.P.S. please follow-up in this topic when you've got it built and tested.

author: matb
author_rank: Regular Contributor
timestamp: March 08, 2022, 08:48:57 am
content: You're right I didn't saw that I refered to the general disposition beeing left HV right LV.I will update the post once I receive and fill the PCBA that should be in almost 2 weeks. Thank you again for your kind help.

author: matb
author_rank: Regular Contributor
timestamp: March 22, 2022, 07:09:15 am
content: Hi everyone, I just received and assembled the PCB, it works very well (at least with no load).It goes from 129.7V up to 348V DC.Link for the imageshttps://imgur.com/a/dR0GDj0as I can't seem to share them here directlyI will share the Kicad project on my GitHub page soon and I will contact Threeneuron about it to see if he is interested.Thank you Ian.M for your helpI have yet to try my nixie tubes that arrived.

author: matb
author_rank: Regular Contributor
timestamp: March 22, 2022, 07:20:27 am
content: Just a quick question about the nixie tube. One of the pins is cut very very short but I can't deduce which one it is, seems like the comma pin ?The datasheet :https://tubehobby.com/datasheets/in14.pdfLink of the images :https://imgur.com/a/Cfrieay

author: Ian.M
author_rank: Super Contributor
timestamp: March 22, 2022, 08:15:32 am
content: Your photos aren't good enough to identify pin 1, the anode. If these ИН-14 tubes are pulls rather than N.O.S. its not unusual for an unused comma wire to be cut short. Unfortunately that doesn't help much as they have two commas, one either side of the anode pin. If the marking is ambiguous or missing, and you cant figure it out by peering through the glass to positively identify which pin connects to the anode, you'll have to determine it experimentally by probing with a high voltage supply and a suitable current limiting resistor. Work hands-off with clip leads so it doesn't bite!As you don't know which comma it is, I'd link the pins either side of the clipped one to be certain to get the anode and apply HT through a resistor, and ground a pin on the other side of the tube and see what digit appears. You can then count round to pin 1 and mark it.

author: matb
author_rank: Regular Contributor
timestamp: March 22, 2022, 08:21:31 am
content: You're right looking back the photos are very crappy, looking at it I think it is a comma pin so I will hook the ground and go around to see what is lighting up. Thanks again

author: matb
author_rank: Regular Contributor
timestamp: March 23, 2022, 05:49:06 pm
content: Ok so "final" post with a 10k resistor it works very well.The cutted pin is the left comma which is "disabled" in the spec it seems ?Anyway a big thanks to all of you, very great and friendly community

author: Ian.M
author_rank: Super Contributor
timestamp: March 23, 2022, 06:02:33 pm
content: What voltage drop are you getting across the 10K anode resistor?That gives you the digit current, which you *MUST* check against datasheet specs. as excess current is likely to cause sputtering damage and insufficient current can result in premature flickering failure, so its desirable to set it in the middle of the permissible range for the mode of operation you are using.

author: matb
author_rank: Regular Contributor
timestamp: March 23, 2022, 06:22:58 pm
content: I have 4mA drawn when a digit lights up on my power supply.Checking this datasheet :https://tubehobby.com/datasheets/in14.pdfthe max current seems to be 3.5mA but the +170V generated is not 100% performante so I will have to calculate the voltage drop you're right.

author: midasgossye
author_rank: Contributor
timestamp: April 10, 2024, 07:55:42 am
content: Hi all,I wanted to thank everyone here for their contributions to this Nixie HV supply. I used the schematic that was posted here as a basis to design my own HV PSU using parts available from LCSC.I got it soldered up yesterday and it is working perfectly. Happily driving digits of an IN-16 nixie tube:I want to upload the KiCad files and LCSC BOM list to a github and share it here for anyone interested, but I first wanted to ask if the contributors here are OK with me putting these up online since the design is their hard work. I will of course put a link to the forum thread and proper attribution.

author: Ian.M
author_rank: Super Contributor
timestamp: April 10, 2024, 12:00:29 pm
content: I'm fine with that.

author: reboots
author_rank: Regular Contributor
timestamp: April 10, 2024, 03:15:43 pm
content: This thread caught my eye, since I had built a clock (and a few other nixie projects) with my own implementation of Threeneuron's MC34063 design a little over ten years ago; details and design files at the link below. The clock has operated continuously and still works great. I'll have to review this thread with an eye toward updating the design, since people seem to have contributed quite a bit of refinement.http://reboots.g-cipher.net/time/

author: mariush
author_rank: Super Contributor
timestamp: April 10, 2024, 03:47:37 pm
content: How much current do you need for that nixie tube?There's MP6002 or MP6003 for example :https://www.digikey.com/en/products/detail/monolithic-power-systems-inc/MP6002DN-LF-Z/5292521There's an example in datasheet with a led driver boosting input voltage to 180v 20mA, you could easily adjust to 170v by changing the feedback resistors . See page 14, figure 8 :https://www.monolithicpower.com/en/documentview/productdocument/index/version/2/document_type/Datasheet/lang/en/sku/MP6002/document_id/1135