Hello, I’m having trouble importing this lib file to Qspice. The model seems complex and for some reason not all the pins are being discovered:

Any thoughts on what I could do to fix it?

Hello, I’m having trouble importing this lib file to Qspice. The model seems complex and for some reason not all the pins are being discovered:

Any thoughts on what I could do to fix it?

Hi,

It seems that the terminals following the “+” are being ignored. Please modify “LMG3522R030.lib” as follows:

.SUBCKT lmg3522R030 VDD LDO_5V IN RDRV BBSW VNEG

+OC_B FAULT_B TEMP GND SOURCE DRAIN

should be changed to:

.SUBCKT lmg3522R030 VDD LDO_5V IN RDRV BBSW VNEG OC_B FAULT_B TEMP GND SOURCE DRAIN

+PARAMS: Temp_Celsius=160

This is a PSPICE model, so it’s possible that some modifications in the model file (“LMG3522R030.lib”) might be needed.

Ah thank you, that worked!

Looks like there may be more stuff to fix, ill keep looking into it:

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U112•X2” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U112•X2” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U121•X2” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U121•X2” – defaults assumed.

Didn’t find a model for “D_D1•X2” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_FAULT1_U111•X2” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_FAULT1_U111•X2” – defaults assumed.

MOSFET M1•X_UTOP_U_GAN_FET•X2 has L=1e-06 which is smaller than can is be realistically modeled with a level 1 equations.

MOSFET M1•X_UTOP_U_GAN_FET•X2 has W=1e-06 which is smaller than can is be realistically modeled with a level 1 equations.

Didn’t find a model for “DBREAK•XU3•X1” – defaults assumed.

Didn’t find a model for “DBREAK•XU3•X1” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X1” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X1” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X1” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X1” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U112•X3” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U112•X3” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U121•X3” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_ILIM1_U121•X3” – defaults assumed.

Didn’t find a model for “D_D1•X3” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_FAULT1_U111•X3” – defaults assumed.

Didn’t find a model for “D_D1•X_UTOP_U_FAULT1_U111•X3” – defaults assumed.

MOSFET M1•X_UTOP_U_GAN_FET•X3 has L=1e-06 which is smaller than can is be realistically modeled with a level 1 equations.

Didn’t find a model for “DBREAK•XU3•X4” – defaults assumed.

Didn’t find a model for “DBREAK•XU3•X4” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X4” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X4” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X4” – defaults assumed.

Didn’t find a model for “DBREAK•XU5•X4” – defaults assumed.

C:\WorkSpace\Welder\QSPICE_Example_Projects\LMG3522R030_Half_Bridge.qsch

Warning: Extending the PULSE() period of V_UTOP_U_PWM_TEMP_VRAMP1•X3 from 9.09e-05 to 0.0001818(9.09e-05 longer) so as not to be less than rise, fall, plus on times.

Warning: Extending the PULSE() period of V_UTOP_U_PWM_TEMP_VRAMP1•X2 from 9.09e-05 to 0.0001818(9.09e-05 longer) so as not to be less than rise, fall, plus on times.

Simulation process terminated.

Hm, my simulation seems to be crashing when I hit 350us(HV_PWR start up). Any thoughts?

LMG3522R030_Half_Bridge.qsch (95.3 KB)

ISO7710.txt (4.3 KB)

LMG3522R030_edit.txt (43.0 KB)

Hi,

Let’s start with a simple test.

It seems that we need to make some modifications to the model file, but it functionally works.

Hi,

I think that the EXOR used in the sub-circuit “MONOPOS_PS” should be modified, as “^” does not represent exclusive-or in QSPICE.

Fortunately, MONOPOS_PS is not utilized in the LMG3522 library, so I don’t think any modifications are necessary for it.

I experimented with a circuit where the ISO7710 was replaced by a PULSE signal source, and it worked fine.

However, with the ISO7710, I was unable to get the expected results.

More investigation needed!

[LMG3522R030_Half_Bridge_test3-2.qsch|attachment]

LMG3522R030_Half_Bridge_test3-2.qsch (822.4 KB)

LMG3522R030_Half_Bridge_test3-2.pfg.txt (1.3 KB)

BTW, does anyone know how to change the font size of the signal expression in the plot?

It may be related to the fact that this QRAW file is ballooning to 95GB? Maybe a memory leak somewhere:

Not sure on the font size, but agree it would be nice to be able to edit.

1 Like

Hi,

I didn’t realize that the QRAW file had ballooned to such a large size. Thank you.

You might have misunderstood the extremely slow simulation speed as a crash.

I noticed that the startup of the LDO_5V output was very slow with ISO7710, so I replaced the LDO_5V with a voltage source.

Although it works, the simulation speed is now extremely slow and the QRAW file size has reached 168GB!

The LMG3522R0330 model is designed for PSpice, so I’ll try running it on PSpice for TI.

Yeah the thing that made me realize it was a message from windows saying my pc was out of space.

I wonder if the LDO may really be that wimpy on the part itself.

Hi,

The results from PSpice for TI are as follows:

Data collection setting is “All but internal Subcircuits”.

I had misunderstood that the low side LDO_5V (V5V_L in the plot) was connected to VCC2 of the ISO7710. The startup of the low side LDO_5V (V5V_L in the plot) is slow, but it does not affect the operation of the ISO7710.

In any case, PSpice for TI completed the task in only 420 seconds, and the data size is 787.9MB.

Thanks El! I haven’t gotten the chance to work on this in a bit, but those are interesting results. I wonder if the reason for the simulation speed on Qspice is because of having to save all that data.

I was wanting to simulate a version of this circuit that had six switches in parallel but given all the data it ballooned to over a terrabyte and the simulation could not finish. it would be nice if there was a way to limit what data is saved.

There was a request and Mike implemented .save in Dec 2023.

Refer to HELP > Simulator > Command Reference > Limit Saved Data Traces (.save)

Feature Request: Reduce waveform data - QSPICE - Qorvo Tech Forum

Ah, didn’t realize I missed that. Thanks y’all!