3
\$\begingroup\$

I love Nixie tubes so I decided to build a Nixie clock.

I am a beginner. I have one successful design that electronics SE helped me design.

That PCB was based on through-hole components and an Arduino.

Now I decided to try a SMD design (and I think way more complicated than the previous one.)

This design is based on an NE555 as that is the simplest one I could find online. This PCB is just to test the power supply generation and the drive of one Nixie tube IN-14. It is not the final circuit.

Here is the design:

Input voltage +12V

Input voltage +12V

+170V generation

+170V generation

PCB without ground plane

PCB without ground plane

PCB with ground plane

PCB with ground plane

Picture of PCBA

enter image description here

What I know / found out:

  • I miscalculated the +9V LM317 resistors, it should be 1620 ohm and I soldered 1500 ohm.
  • Footprint of the fuse is way off, I soldered a wire to short it
  • C12 should be 100uF as per datasheet recommanded circuit
  • C14 is a 4.7u 400V aluminium capacitor (should have been 470uF.)

What is happening:

My power supply is showing a short circuit. I wire +9V@1A (current limited) on the +9V test points as the +9V generation doesn't work.

Using a very scientific method (my fingers) I feel that Q26 (IRF740) is getting very hot.

Checking with my multimeter shows no short on any of the components (continuity mode) +9V and ground are not shorted when the power is off.

Is the +9V generation a must or can I feed the +12V to the NE555 circuit?

Can you guys see a problem in the design, maybe the choice of the components?

Farnell codes :

[EDIT] Probe on pin 3 of NE555DR (sorry don't have a USB key right now):

Oscilloscope capture

[EDIT] I went and checked the OUT frequency before and after the diode, that's where the issue comes I guess:

Here is the probe before D9 1081180:

Probe before D9

Here is the probe after D9:

Probe after D9

[EDIT] Continued troubleshooting here's new infos:

Desoldered D9 and powered the circuit: no changes I'm losing the 555 frequency after the diode.

Resoldered D9, desoldered Q25 and powered the circuit: no changes, same as before.

When I power the power supply at 9V and allow a little bit of current it instantly goes to something like 5V (instead of 9V) so I guess that's another proof that something is wrong somewhere.

\$\endgroup\$
10
  • \$\begingroup\$ Probe between 555 pins 1 (GND) and 3 (Out) for <1s; if pulses are visible on the screen then the 555 is working. Could the MOSFET pin-out be different than the footprint? \$\endgroup\$
    – rdtsc
    Jan 27, 2022 at 20:49
  • \$\begingroup\$ NE555 farnell code is 3121192 \$\endgroup\$
    – Mat
    Jan 27, 2022 at 21:08
  • \$\begingroup\$ I have 29kHz on pin 3 30mV \$\endgroup\$
    – Mat
    Jan 27, 2022 at 21:14
  • \$\begingroup\$ Q26 getting a little hot (potentially even enough to feel very hot to the touch, since that would only be about 50~60 °C or so) is no surprise; if it's getting extremely hot (enough to boil water) you may have a problem. \$\endgroup\$
    – Hearth
    Jan 27, 2022 at 21:21
  • \$\begingroup\$ I mean I'm limiting current to 1 amp i guess if I put 3/4A it's going to go in flames ? \$\endgroup\$
    – Mat
    Jan 27, 2022 at 21:22

1 Answer 1

3
\$\begingroup\$

30mV pulses on the 555 pin 3 indicate that either Q25 or Q26 are mis-wired, shorted, or wrong type; and/or R41 is a very low value. But something after the 555 pin 3 is misbehaving; should be seeing 9V pulses.

This does run in simulation:

555 Boost Driver

Note that I drew this with power input on the left and output on the right. This is the "conventional" way of drawing schematics, flowing from left to right.

Also note there is some significant ringing on the MOSFET gate around 0v in this simulation (not shown here.) Simulations are only so-good; suggest measuring this after the main issue is found to see what really happens there. And I had to change D8 to a (random) different type; the closest LTspice has is the ES3B and that was limiting output to ~100V.

If you feel like giving this a try with LTspice, here is the .asc file:

Version 4
SHEET 1 1084 680
WIRE 384 -368 -224 -368
WIRE 704 -368 464 -368
WIRE 784 -368 704 -368
WIRE 896 -368 848 -368
WIRE 960 -368 896 -368
WIRE 1008 -368 960 -368
WIRE 704 -336 704 -368
WIRE 368 -256 -96 -256
WIRE 464 -256 368 -256
WIRE 496 -256 464 -256
WIRE 608 -256 560 -256
WIRE 656 -256 608 -256
WIRE 896 -256 896 -368
WIRE 1008 -256 1008 -368
WIRE 368 -208 368 -256
WIRE 608 -208 608 -256
WIRE -224 -192 -224 -368
WIRE -96 -192 -96 -256
WIRE 464 -160 464 -256
WIRE 544 -160 464 -160
WIRE -224 -80 -224 -112
WIRE -96 -80 -96 -112
WIRE 368 -80 368 -128
WIRE 608 -80 608 -112
WIRE 704 -80 704 -240
WIRE 896 -80 896 -192
WIRE 1008 -80 1008 -176
FLAG -96 -80 0
FLAG 704 -80 0
FLAG -224 -80 0
FLAG 368 -80 0
FLAG 608 -80 0
FLAG 896 -80 0
FLAG 1008 -80 0
FLAG 960 -368 VOUT
SYMBOL voltage -96 -208 R0
WINDOW 123 0 0 Left 0
WINDOW 39 24 124 Left 2
SYMATTR InstName V1
SYMATTR Value PULSE(0 9 1m 1n 1n 10u 34.483u 420)
SYMATTR SpiceLine Rser=10
SYMBOL sym\\nmos 656 -336 R0
SYMATTR InstName Q26
SYMATTR Value IRF740
SYMBOL pnp 544 -112 M180
WINDOW 0 60 64 Left 2
WINDOW 3 57 37 Left 2
SYMATTR InstName Q25
SYMATTR Value 2N2907
SYMBOL voltage -224 -208 R0
WINDOW 123 0 0 Left 0
WINDOW 39 24 124 Left 2
SYMATTR InstName V2
SYMATTR Value 9
SYMATTR SpiceLine Rser=1
SYMBOL ind 368 -352 R270
WINDOW 0 32 56 VTop 2
WINDOW 3 5 56 VBottom 2
SYMATTR InstName L1
SYMATTR Value 100µ
SYMATTR SpiceLine Ipk=1 Rser=0.16 Rpar=53868.3 Cpar=0 mfg="Bourns, Inc." pn="SRU1048-101Y"
SYMBOL diode 496 -240 R270
WINDOW 0 32 32 VTop 2
WINDOW 3 0 32 VBottom 2
SYMATTR InstName D9
SYMATTR Value 1N914
SYMBOL res 352 -224 R0
SYMATTR InstName R41
SYMATTR Value 1k
SYMBOL schottky 784 -352 R270
WINDOW 0 32 32 VTop 2
WINDOW 3 0 32 VBottom 2
SYMATTR InstName D8
SYMATTR Value UPSC600
SYMATTR Description Diode
SYMATTR Type diode
SYMBOL cap 880 -256 R0
SYMATTR InstName C9
SYMATTR Value 1µ
SYMATTR SpiceLine V=400 Irms=0 Rser=0.0252581 Lser=10.4595n mfg="Würth Elektronik" pn="890283326009CS WCAP-FTBP 22.5 x 26 x 17 x 8.5" type="Box"
SYMBOL res 992 -272 R0
SYMATTR InstName RL
SYMATTR Value 100k
TEXT -32 -152 Left 2 ;Simulated 555 output
TEXT -42 -304 Left 2 !.tran 15m startup uic
\$\endgroup\$
6
  • \$\begingroup\$ Thanks for the simulation I guess I should start to learn this software. The voltage never stabilize or it's because you stop the soft or didn't implement the Q24 circuit ? \$\endgroup\$
    – Mat
    Jan 28, 2022 at 7:10
  • \$\begingroup\$ Right, this is just a bare-bones test to see how the gate pulsing section works. It could be expanded with the entire circuit, but this will slow it way down and the results may not represent actuality very well. \$\endgroup\$
    – rdtsc
    Jan 28, 2022 at 14:44
  • \$\begingroup\$ I downoladed LTSpice 17 and wanted to try your circuit, the IRF740 is missing from the available nmos. I tried adding it in standard.mos but with no luck could you share your config ? .model IRF740 VDMOS(Kp=3.1089 Rs=0.0048 Rd=0.4166 Rg=0.91 Vto=4.5 Lambda=0.001 Cgdmax=1218p Cgdmin=15p Cgs=1300p tt=533n Is=2.41E-09 N=1.401 Rb=0.013053 M=0.452 Vj=0.36 Cjo=1424.39pF mfg=STmicro Qg=35n Ron=0.48 Vds=400) \$\endgroup\$
    – Mat
    Jan 30, 2022 at 9:13
  • \$\begingroup\$ Hmm, that's identical to what I have so it should be working. Try right-clicking Q26 and pick a different MOSFET. \$\endgroup\$
    – rdtsc
    Jan 31, 2022 at 13:07
  • \$\begingroup\$ Picking another one works like the 2N7002, the results are not what I expect but it works I can't see the IRF740 in the list very strange Can you share your standard.mos file if that's possible so I can try it out ? \$\endgroup\$
    – Mat
    Jan 31, 2022 at 13:16

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.