mc34063 buck converter as per ON datasheet

[GregaryB]

I have created the attached buck converter circuit in multisim 12 as per the ON datasheet for MC34063.

But the god damned thing wont work. The datasheet says it should output 5V but in fact it outputs only a few millivolts.

I cannot get these bloody devices to work on my bread board either - my buck converter outputs 3.5V when the calculations say it should output 6V.

I am at a total loss to understand what the hell it is I am doing incorrectly.

Can some one please make the attached multisim circuit work, as the datasheet says it should, so that perhaps I can see what it is I am doing incorrectly.

[Tayyab_R]

Hi GregaryB,

I was able to get the simulation working. The problem is that when working with oscillator's in spice, it takes time for them to actually get to a state where they are working. This time can be really significant based on the complexity of the circuit. What you can do is add another source like a function generator in the circuit to jump start the oscillator. Refer to the KB below:

http://digital.ni.com/public.nsf/allkb/D47BBE254EBF9A1D86257A5C00507BCB?OpenDocument

Attached is the working circuit. Just open the switch when you see the 25V reading.

Hope this helps.

[GregaryB]

Actually I solved that problem myself.

It only arose when I used the MC34063ADG device that came with Multisim.

I ended up finding a spice model of a MC34063A device on the ON Semiconductor website and managed to successfully create my own user device.

When I use this in place of MC34063ADG, the circuit behaves exactly as the datasheet says it should.

So I can only assume that MC34063ADG is not a standard device that the datasheet I have describes or this device in Multisim has been created incorrectly.

[Tayyab_R]

Hi GregaryB,

Can you post the working circuit. I want to check the working model.

[GregaryB]

This is the circuit with the new component I added. Just change it to the MC34063ADG - the pin arrangement is the same.

[derliin]

Hi,

I have a similar problem with boost converter.

I am trying to simulate boost converter from onsemi datasheet , I made the circuit exactly like in the datasheet but  it dosent work.

I am using multisim 13 .

I think I have some properties wrong but i cant figure it out. I´m not expierienced in multisim.

Help would be appriciated.

Aleksander.

[PB79]

For a MC34063 you can use a following Spice3 model (verified in LTSpice and NI Multisim 13):

.SUBCKT MC33063__DEF_3__4 1 2 3 4 5 6 7 8

*exempt 20030227 20395 -30736294
*BY KEHINDE OMOLAYO 2-20-03
*TERMINAL ID
*SWITCH COLLECTOR=1 SWITCH EMITTER=2 TIMING CAPACITOR=3 GND=4
*COMPARATOR INVERTING INPUT=5 VCC=6 IPK SENSE=7 DRIVER COLLECTOR=8
.MODEL DMC34063 D (CJO=2P N=0.05)
.MODEL QSWITCH NPN BF=75 CJC=2P IS=3E-9 RB=1 RC=0.45 RE=0
+ VJC=.75 VJE=.75 VJS=.75
E1 10 0 5 4 1
R1 4 5 10MEG
V1 20 0 PULSE 0 2
E2 11 0 3 4 1
*B1 13 0 V=1M/(ABS((27.475-195M*V(12))+(36.002+244M*V(12))*V(9)-(302.302+651M*V(12))*V(9)^2)+1F)
B1 13 0 V=1M/(ABS((27.475-195M*V(12))+(36.002+244M*V(12))*V(9)-(302.302+651M*V(12))*V(9)**2)+1F)
E3 12 0 6 4 1
E4 9 0 6 7 1
R2 6 7 10MEG
*B2 14 0 V=1M*((-10.765-151M*V(12))+(45.344+864M*V(12))*V(9)-+(35.99+1.378*V(12))*V(9)^2+(8.341+839M*V(12))*V(9)^3)
B2 14 0 V=1M*((-10.765-151M*V(12))+(45.344+864M*V(12))*V(9)-+(35.99+1.378*V(12))*V(9)**2+(8.341+839M*V(12))*V(9)**3)
*B4 15 0 V=V(9)>0.32 ? V(14) : V(13)
B4 15 0 V=IF( V(9)>0.32, V(14), V(13) )
C1 19 0 10P
*B5 16 0 V= V(20)<1 ? 2 : V(24)>1 ? 2 : V(19)>1 ? 0 : 2
B5 16 0 V= IF( V(20)<1, 2, IF(V(24)>1, 2, IF( V(19)>1, 0, 2 ) ) )
R3 16 17 150
C2 17 0 10P
*B6 18 0 V=V(20)<1 ? 0 : V(24)>1 ? 0 : V(11)<(1.083-1.239*V(29)) ? 2 : V(17)>1 ? 0 : 2
B6 18 0 V= IF( V(20)<1, 0, IF( V(24)>1, 0, IF( V(11)<(1.083-1.239*V(29)), 2, IF(V(17)>1, 0, 2 ) ) ) )
R4 18 19 150
D1 4 3 DMC34063
D2 3 6 DMC34063
C3 11 31 1N
*B7 4 36 I=V(17)>1 ? -(224.4U+2.359U*V(12))*0.77 : V(15)*0.77
B7 4 36 I=IF( V(17)>1, -(224.4U+2.359U*V(12))*0.77, V(15)*0.77 )
C5 23 0 10P
*B9 21 0 V= V(20)<1 ? 2 : V(17)>1 ? 2 : V(26)>1 ? 0 : 2
B9 21 0 V= IF( V(20)<1, 2, IF( V(17)>1, 2, IF( V(26)>1, 0, 2 ) ) )
R5 27 26 150
C6 26 0 10P
*B10 27 0 V=V(20)<1 ? 0 : V(17)>1 ? 0 : V(10)<1.25 ? 2 : V(23)>1 ? 0 : 2
B10 27 0 V=IF( V(20)<1, 0, IF(V(17)>1, 0, IF(V(10)<1.25, 2, IF(V(23)>1, 0, 2 ) ) ) )
R6 21 23 150
*B12 33 0 V=V(11)>(1.148+184.6M*V(29)) ? 2 : 0
B12 33 0 V=IF( V(11)>(1.148+184.6M*V(29)), 2, 0 )
R13 33 24 10K
C8 24 0 10P
Q1 8 30 25 QSWITCH
Q2 1 25 2 QSWITCH
R15 25 2 100
D5 2 30 DMC34063
G1 2 30 26 23 5M
R16 2 4 10MEG
R23 31 28 1M
*V6 28 0
V6 28 0 0
*V7 36 3
V7 36 3 0
B13 29 0 V=I(V6)/(I(V7)+866.8M*I(V6))

 .ENDS

To get a proper results in NI MultiSim 13 you must also remember to set custom simulation (suggested by Infineon  for a power electronics):

ABSTOL= 1nA (maximum current accuracy)
CHGTOL= 1pC (maximum charge accuracy)
ITL1= 150 (maximum number of iterations for DC analyses without initial
conditions)
ITL2= 150 (maximum number of iterations for DC analyses with initial
conditions)
ITL4= 500 (maximum number of iterations for transient analyses time
steps)
RELTOL= 0.01 (relative accuracy of voltages and currents)
METHOD: GEAR

This combination works OK for a MC33064/MC34063/NCV3063/NCV3064 buck converter, but not for a boost topology.

However for SMPS design I strongly recommend LTSpice (much faster, works with buck and boost topology without any convergence errors like in NI Multisim and there is no problem with various MC34063 models).

Regards,

PB