IR2110 simulation problem is pspice

Maji · Apr 27, 2019

IR2110 simulation problem in OrCad Pspice

Hello everyone!

I was trying to simulate for some time an H bridge inverter driven by two IC circuits "IR2110", but i can't seem to go through it.
And since I'm new to this whole simulation things, i couldn't have any idea what do i have to change and how should i proceed to figure out the solution to this error

The error problem goes as the following:

Code:

Resuming Simulation with the following settings
RELTOL = 0.0086


INTERNAL ERROR -- Overflow, Convert

ABORTING SIMULATION"

It seems that a lot of voltages/ currents aren't converging :

Code:

Convergence problem in transient analysis at Time =  184.8E-09
         Time step =  97.34E-18, minimum allowable step size =  100.0E-18

  These voltages failed to converge:

    V(N02921)                 =    70.48mV  \    70.63mV
    V(X_U3.g1)                =     14.70V  \     14.82V
    V(X_U3.d1)                =     50.08V  \     50.20V
    V(X_U3.s1)                =  -149.08mV  \   -31.01mV
    V(X_U3.s2)                =   -56.36mV  \    61.72mV
    V(X_U3.g2)                =     14.71V  \     14.83V
    V(X_U3.d2)                =     42.51V  \     42.63V
    V(X_U3.21)                =     50.08V  \     50.20V
    V(X_U3.c)                 =     42.51V  \     42.63V
    V(X_U3.a)                 =     14.71V  \     14.83V
    V(X_U3.b)                 =     42.51V  \     42.63V
    V(X_U3.d)                 =    -13.09V  \    -12.97V
    V(X_U4.g1)                =   219.44mV  \   265.36mV
    V(X_U4.s1)                =  -392.64mV  \  -346.72mV
    V(X_U4.s2)                =  -392.56mV  \  -346.64mV
    V(X_U4.g2)                =   221.92mV  \   267.84mV
    V(X_U4.a)                 =   221.94mV  \   267.86mV
    V(X_U5.g1)                =     14.37V  \     14.40V
    V(X_U5.d1)                =   321.38mV  \   351.89mV
    V(X_U5.s1)                =   -34.04mV  \   -3.538mV
    V(X_U5.s2)                =   -30.32mV  \   189.94uV
    V(X_U5.g2)                =     14.35V  \     14.38V
    V(X_U5.d2)                =    17.55mV  \    48.05mV
    V(X_U5.21)                =   321.38mV  \   351.89mV
    V(X_U5.c)                 =    -14.62V  \    -14.59V
    V(X_U5.a)                 =  -283.14mV  \  -252.63mV
    V(X_U5.b)                 =     14.35V  \     14.38V
    V(X_U5.d)                 =     28.69V  \     28.72V
    V(X_U6.g1)                =   597.40mV  \    -1.527V
    V(X_U6.d1)                =     15.65V  \     13.53V
    V(X_U6.s1)                =   597.56mV  \    -1.527V
    V(X_U6.s2)                =   597.56mV  \    -1.527V
    V(X_U6.g2)                =   596.95mV  \    -1.528V
    V(X_U6.d2)                =     15.65V  \     13.53V
    V(X_U6.21)                =     15.65V  \     13.53V
    V(X_U6.c)                 =     15.65V  \     13.53V
    V(X_U6.a)                 =   596.96mV  \    -1.528V
    V(X_U6.b)                 =     15.65V  \     13.53V
    V(X_U6.d)                 =    -14.46V  \    -16.58V
    V(X_D1.4)                 =    76.30mV  \    74.64mV

  These supply currents failed to converge:

    I(X_U1.V_MD4_RS_V1)       =    -2.090A  \    -2.085A"

The circuit i'm trying to simulate :

the netlist :

Code:

.EXTERNAL OUTPUT Vin2
.EXTERNAL OUTPUT Vin1
X_U1         +15V VIN1 0 VIN2 0 N04951 N01620 N01238 +15V 0 N04893 IR2110
+  PARAMS:  T1=-40 T2=25 T3=125 V1=10 V2=15 V3=20 TONT1=90N TONT2=120N TONT3=170N
+  TONV1=140N TONV2=120N TONV3=100N TOFFT1=77N TOFFT2=94N TOFFT3=130N TOFFV1=115N
+  TOFFV2=94N TOFFV3=75N TONVDD1=125N TONVDD2=120N TONVDD3=115N TOFFVDD1=113N
+  TOFFVDD2=94N TOFFVDD3=72N
X_U2         +15V VIN2 0 VIN1 0 N02388 N02921 N02864 +15V 0 N03056 IR2110
+  PARAMS:  T1=-40 T2=25 T3=125 V1=10 V2=15 V3=20 TONT1=90N TONT2=120N TONT3=170N
+  TONV1=140N TONV2=120N TONV3=100N TOFFT1=77N TOFFT2=94N TOFFT3=130N TOFFV1=115N
+  TOFFV2=94N TOFFV3=75N TONVDD1=125N TONVDD2=120N TONVDD3=115N TOFFVDD1=113N
+  TOFFVDD2=94N TOFFVDD3=72N
X_U3         +50V N01021 0 BSC440N10NS3_L0 
X_U4         +50V N02423 0 BSC440N10NS3_L0 
X_U5         N02864 N03095 0 BSC440N10NS3_L0 
X_U6         N01238 N01859 0 BSC440N10NS3_L0 
X_D1         +15V N02921 SMBD7000/INF
X_D2         N01021 N04951 SMBD7000/INF
X_D3         +15V N01620 SMBD7000/INF
X_D4         N02423 N02388 SMBD7000/INF
X_D5         N03095 N03056 SMBD7000/INF
X_D6         N01859 N04893 SMBD7000/INF
R_R1         N04951 N01021  10 TC=0,0 
R_R2         0 N03095  1k TC=0,0 
R_R3         N02423 N02388  10 TC=0,0 
R_R4         N04893 N01859  10 TC=0,0 
R_R5         N03095 N03056  10 TC=0,0 
R_R6         0 N01021  1k TC=0,0 
R_R7         0 N02423  1k TC=0,0 
V_V1         +50V 0 50Vdc
V_V2         +15V 0 15Vdc
V_V6         VIN1 0  
+PULSE 10V 0V 0 0 0 0.00001s 0.00002s
V_V7         VIN2 0  
+PULSE 0V 10V 0 0 0 0.00001s 0.00002s
C_C1         N01238 N01620  1u IC=5V TC=0,0 
R_R8         0 N01859  1k TC=0,0 
L_L1         N05212 0  2mH  
C_C2         N02864 N02921  1u IC=5V TC=0,0 
R_R9         0 N05212  10m TC=0,0

I'm sincerely grateful for the the time you spent reading/helping on this thread!

fourtytwo · Apr 27, 2019

Your FET wiring is crazy and wrong!! I am not surprised with that awful symbol, is that what you get paying $$$$$ for Orcad ?
If I were you I would use a free simulator with decent symbols like LTspice and drop the expensive horrible Orcad

The next problem you will find is your 1K gate/source resistors, they are unnecessary and will kill the high side boost supply.

FvM · Apr 27, 2019

Convergence problems with SPICE simulators are just normal operation. They may happen with strongly non-linear circuits, but also due to circuit errors and floating nodes. In the former case, it's necessary to tune different transient analysis parameters.

I see a basic circuit error that may cause the problems, shorted half-bridges. You should at least try with a corrected circuit.

Maji · Apr 27, 2019

Thank you @FvM for your answer.
The simulation is finally working. the voltage output seems to be fine but there's no current in the load.
For the circuit, I just did the same one that i found in website from where i downloaded the ir2110 pspice model, I think there's a part that I didn't understand while trying to build the circuit!

FvM · Apr 27, 2019

there's no current in the load

What do you expect? Driving the H-bridge with 50 kHz, 50% duty cycle, there's only a small reactive output current.

Maji · Apr 29, 2019

well, besides the shorted half bridges error that you warned me about @FvM, and which i'm so grateful for, i figured out some parameters through the forum here and elsewhere, by changing values in the simulation options as it follows:

And all the other settings must be left unchanged
One another important thing is the 2 capacitors used, need to be well placed (node number 2 must be facing the upper side and the IC of each capacitor must be initialized to 5).
after doing this run a bias point simulation, and then a time transient simulation with a 1ms run to time (if you change it to 500us you need to change the ITL4 to 5 to have a total simulation)
As i wasted a lot of time trying to simulate these two ic's, i wanted to share this parameters with all of the people that might have to use it in the future saving them some of the effort.
Thank you so much for your help and have a great day!

Maji · Apr 29, 2019

Also the itl4 in the autoconvergence settings need to be changed to 100

Welcome to EDAboard.com

IR2110 simulation problem is pspice

Maji

Newbie level 3

Attachments

fourtytwo

Guest

Maji

FvM

Super Moderator

Maji

Maji

Newbie level 3

FvM

Super Moderator

Maji

Maji

Newbie level 3

Maji

Newbie level 3

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Connect with us

Online statistics

Forum statistics