pspice changing time step issue

Do you have a load resistor on the circuit or is the two diodes the whole thing?

Spice sometimes gives wild results for circuits that won't work. With no load resistor, the Vout node is basically floating when the two diodes are off.

-------------O =A0Vout

I do have a load resistor.... and also grounds, would you expect a voltage spike in a circuit like this?

Hello,

You might reduce the minimum conductance (GMIN). Depending on the load resistance you can reduce it significantly. Also check your maximum step size. As this is 1us, it takes 3e6 steps to run the simulation.

Regarding the spikes. When you have a pulse source with 1us rise and fall times, you may reduce the maximum step size to below 1us (but this will cause long sim times when you run for 3s). Other option is increase the rise and fall times of your pulse sources and increase the step size also, this will speed up your simulation.

What type of diode do you use? Try another one (for example a 1n4148) and see what happens). Keep in mind that real diodes have capacitance. When the output is already 12V, you can get a spike via the diode that has been connected to the source that goes from low to high. So it may not be a simulation error.

When I have doubts about a circuit, I play with the max step size setting.

Best regards,

Wim PA3DJS

remove abc from the mail address.

-------------O =A0Vout

I keep getting errors like this now:

"ERROR -- Convergence problem in transient analysis at Time =3D .133 Time step =3D 72.00E-21, minimum allowable step size =3D

1.000E-18

These voltages failed to converge:

V(N902046) =3D 5.041uV \\ 2.644uV

These supply currents failed to converge:

I(V_V1) =3D 2.343mA \\ -5.677uA I(V_V2) =3D 2.354mA \\ 4.846uA

These devices failed to converge: X_D1.D1 "

How do I change the step size? I see maximum step size option, but no minimum... wouldn't I want to change the minimum step size to make the simulation run faster? Do you know what these errors mean? Thanks

"panfilero" schrieb im Newsbeitrag news: snipped-for-privacy@s12g2000prg.googlegroups.com...

Hello panfilero,

Please show your SPICE netlist, if you are interested in a helpful answer. It's the .net and the .cir file.

Best regards, Helmut

- snipped-for-privacy@s12g2000prg.googlegroups.com...

----------O =A0Vout

Hi Helmut,

Here's my netlist and .cir files... thanks for taking a look at this

• source Test_ X_D1 N899662 N901787 D120NQ045 X_D2 N900764 N901787 D120NQ045 V_V1 N899662 0

+PULSE 12 0 15u 1n 1n 1 2 V_V2 N900764 0 +PULSE 12 12 0 1p 1p 1 2

** Creating circuit file "Test_.cir"

** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:

• Profile Libraries :

• Local Libraries :

• From [PSPICE NETLIST] section of C:\OrCAD\OrCAD_16.0\tools\PSpice \PSpice.ini file: =2Elib "nom.lib"

*Analysis directives: =2ETRAN 0 3 0 =2EPROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*)) =2EINC "..\\SCHEMATIC1.net"

=2EEND

Newsbeitragnews: snipped-for-privacy@s12g2000prg.googlegroups.com...

Hi Helmut,

Here's my netlist and .cir files... thanks for taking a look at this

• source Test_ X_D1 N899662 N901787 D120NQ045 X_D2 N900764 N901787 D120NQ045 V_V1 N899662 0

+PULSE 12 0 15u 1n 1n 1 2 V_V2 N900764 0 +PULSE 12 12 0 1p 1p 1 2

Hello,

I have looked at your circuit and simulated it with LTspice.

It's quite normal to see the large voltage spike at the output, because your diodes have a few nano-Farads capacitance and you drive it extremely "hard" with your voltage sources (Trise=1ns, Ri=0Ohm). The junctiom capacitance is the reason for the voltage spikes. (SPICE model: CJO=11.509E-9) If you add a capacitor to the output, the spikes will become very small.

Best regards, Helmut

** Creating circuit file "Test_.cir" ** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:

• Profile Libraries :

• Local Libraries :

• From [PSPICE NETLIST] section of C:\OrCAD\OrCAD_16.0\tools\PSpice \PSpice.ini file: .lib "nom.lib"

*Analysis directives: .TRAN 0 3 0 .PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*)) .INC "..\\SCHEMATIC1.net"

.END

- snipped-for-privacy@s19g2000prg.googlegroups.com...

roups.com...

r.

I"ll try that, I really appreciate the help! Thanks

No I wouldn't.

What sort of diodes is it and what sort of spice?

Newsbeitragnews: snipped-for-privacy@s19g2000prg.googlegroups.com...

Newsbeitragnews: snipped-for-privacy@s12g2000prg.googlegroups.com...

Clarification: if 12V=Large the above is correct if 1000V= large this isn't what you were seeing

Most likely you saw 12V spikes.

Hello

We talked about a spike with 4V on top of the 12V DC.

Best regards, Helmut

PS: The rectifier has two 120A diodes 120NQ045.

Newsbeitragnews: snipped-for-privacy@s12g2000prg.googlegroups.com...

Hello,

When I look into your circuit, it seems a little bit unpractical:

You are using power diodes in combination with ps pulses. You might reduce the rise and fall times of your sources and add a load resistor (to ground for example). When the load resistance is not in the many Meg Ohms, you might reduce the GMIN parameter (it will probably default in the 1e-12 range).

This may help to converge the simulation process. Pspice reduces its time step until the specified accuracy is reached (with a certain minimum time step). When the iterative process does not converge, you get the minimum time step error.

Probably you will add inductances in the future. Inductances in combination with diodes are the key ingredients for convergence problems. Using realistic components by adding loss resistances and capacitances to inductors, helps to speed up your simulations.

Hope this helps a bit.

Best regards,

Wim PA3DJS

remove abc from the mail address.

Newsbeitragnews: snipped-for-privacy@s12g2000prg.googlegroups.com...

Small error, you should increase it (for example from 1e-12 to

1e-9).

best regards,

Wim

Newsbeitragnews: snipped-for-privacy@s12g2000prg.googlegroups.com...

I see no load device. What is up with the picosecond edges on V_V2?