Newbie question - basic simulation with amplifier AD620 which necessitate hours to be performed

phl_FR · Nov 30, 2023

Hi !

I'd like some help to debug my simulation, please.

I've probably made a mistake because when I launch the simulation, the calculation lasts hours instead of a few seconds.
I've been trying for hours to understand what is wrong but I still haven't found the reason of this problem.

Here on the screenshot, I've used the following parameters :
signal input : sin wave of 1V amplitude, 0V DC and 50 Hz frequency ;
the gain is supposed to be G = 2 (1+ 49,4K/49400).

Thanks in advance.

eTech · Nov 30, 2023

Hi

1. Edit the ad620.cir model file.

Find this line (approx #112):
L1 45 46 1E-6

Change to:
L1 45 46 1E-6 IC=0

2. Add a small serial resistance to all voltage sources (100m ohms).

3. Be aware the value specified for a sine voltage source is a Peak value. To specify an RMS value, specify the product of the Peak value multiplied by 1.414.

danadak · Dec 1, 2023

Regards, Dana.

phl_FR · Dec 20, 2023

Thank you very much eTech and danadak.

I've applied the advices. I think I have understood the goal of writing "IC=0" in the circuit file : it sets an initial condition and may reduces substantially the iterations that LTspice computes.
Dealing with the serial resistance 100 ohms with the voltage source : is it usefull for simulation ? I imagine it usefull in case of short circuit, but I'm not sure.

The answer of danadak made me smile because the final prototype's goal is to associate the AD620 (amplifier) to a AD536 (a chip which convert a signal in a RMS value.

My association of the 2 circuits on LTspice has generated errors that I have never been able to solve.

I'll try to study it again in the following days.

alec_t · Dec 20, 2023

phl_FR said:
the serial resistance 100 ohms with the voltage source

No. 100m (100 milliOhms).

Tony Stewart · Dec 20, 2023

This is wrong

This is correct = 2

If you want to input 1Vrms then specify 1rms not 1 which is pk.

Tony Stewart · Dec 20, 2023

Specifying a realistic Rs for any voltage source makes sense when significant voltage drop is expected from load pulses and valid initial conditions for V(C) and I(L) for transient startup, but has no effect on steady state.

Roff · Feb 3, 2024

eTech said:
Hi

1. Edit the ad620.cir model file.

Find this line (approx #112):
L1 45 46 1E-6

Change to:
L1 45 46 1E-6 IC=0

2. Add a small serial resistance to all voltage sources (100m ohms).

3. Be aware the value specified for a sine voltage source is a Peak value. To specify an RMS value, specify the product of the Peak value multiplied by 1.414.

View attachment 143484

When I initially ran the sim, without your recommended changes, I got a couple of random spurious large voltage spikes. After making the changes, it ran great. Just for grins, I removed the 100mohm resistors, and it still runs great.
I'm not saying it's not a good idea. Just sayin'.
I did have to start saving data at around 30us to avoid a large negative output spike at startup.

crutschow · Feb 4, 2024

Tony Stewart said:
If you want to input 1Vrms then specify 1rms not 1 which is pk.

Is there a way to do that besides multiplying the specified source voltage by √2?

crutschow · Feb 4, 2024

phl_FR said:
Here on the screenshot,

Normally the assigned pin numbers on the schematic part symbol are for the part package, not node numbers in its model file.
The function for each pin is also usually shown.

Roff · Feb 4, 2024

crutschow said:
Normally the assigned pin numbers on the schematic part symbol are for the part package, not node numbers in its model file.
The function for each pin is also usually shown.

This happens when you instruct LTSpice to automatically create a symbol from the .cir file. I encountered the same thing when I first ran the sim, so I modified the symbol. See attached files.

Tony Stewart · Feb 4, 2024

crutschow said:
Is there a way to do that besides multiplying the specified source voltage by √2?

No not on the generator for LTspice, although Falstad supports it directly.
But it supports it on MEAS. command.

.MEASURE -- Evaluate User-Defined Electrical Quantities
the .MEAS statement operates over the entire range of data. The types of measurement operations that can be done over an interval are

Keyword	Operation performed over interval
AVG	Compute the average of <expr>
MAX	Find the maximum value of <expr>
MIN	Find the minimum value of <expr>
PP	Find the peak-to-peak of <expr>
RMS	Compute the root mean square of <expr>
INTEG	Integrate <expr>

Tony Stewart · Feb 4, 2024

"Automatic Symbol Generation
When editing an ASCII netlist that contains subcircuit definitions, you place the cursor on the line containing the name of the subcircuit, right click, and execute context menu item "Create Symbol." For most users, this is the only method you should ever consider for adding third-party models defined as subcircuits since all the details are handled for you."

Upon running

also

Located in AD620.asy was
SYMATTR ModelFile C:\Users\rmaxh\AppData\Local\LTspice\lib\sub\ad620.cir

which resulted in error above shown below

XU1 N001 0 N003 N004 out 0 N002 N005 AD620
V1 0 N004 12
V2 N003 0 12
V3 N001 0 SINE(0 10m 1k)
RG N002 N005 49.4k
R2 out 0 10k
.tran 0 10m 30u 100u
* G-1
* RG =
* 49.4k
.lib C:\Users\rmaxh\AppData\Local\LTspice\lib\sub\ad620.cir
.backanno
.end

Tony Stewart · Feb 4, 2024

Weird!!

- any load more than +25 uA causes a glitch and makes the sim. crawl really slow.

Change RG or R2 load > 25uA , same result. some are 0 risetime glitches

eTech · Feb 6, 2024

Roff said:
When I initially ran the sim, without your recommended changes, I got a couple of random spurious large voltage spikes. After making the changes, it ran great. Just for grins, I removed the 100mohm resistors, and it still runs great.
I'm not saying it's not a good idea. Just sayin'.
I did have to start saving data at around 30us to avoid a large negative output spike at startup.

But they shouldn't be removed. All supply voltage sources have some resistance.
Just sayin'

Roff · Feb 8, 2024

Tony Stewart said:
"Automatic Symbol Generation
When editing an ASCII netlist that contains subcircuit definitions, you place the cursor on the line containing the name of the subcircuit, right click, and execute context menu item "Create Symbol." For most users, this is the only method you should ever consider for adding third-party models defined as subcircuits since all the details are handled for you."

Upon running

View attachment 144380

also

View attachment 144382

Located in AD620.asy was
SYMATTR ModelFile C:\Users\rmaxh\AppData\Local\LTspice\lib\sub\ad620.cir

which resulted in error above shown below

XU1 N001 0 N003 N004 out 0 N002 N005 AD620
V1 0 N004 12
V2 N003 0 12
V3 N001 0 SINE(0 10m 1k)
RG N002 N005 49.4k
R2 out 0 10k
.tran 0 10m 30u 100u
* G-1
* RG =
* 49.4k
.lib C:\Users\rmaxh\AppData\Local\LTspice\lib\sub\ad620.cir
.backanno
.end

Hi Tony,
The zip file, as you apparently know, contains AD620.cir and AD620.asy. I created the .asy file for my own convenience, so the schematic would make more sense to me. I posted what I had done as an explanation to crutschow about the weird AD620 symbol in the OP's schematic.
I'm sure you know that you could have edited AD620.asy to modify the SYMATTR line to reflect the location of YOUR AD620.cir file.
In retrospect, I should have let crutschow continue to wonder why the symbol was weird. It would have saved both you and me a lot of time.

Tony Stewart · Feb 8, 2024

Roff said:
Hi Tony,
The zip file, as you apparently know, contains AD620.cir and AD620.asy. I created the .asy file for my own convenience, so the schematic would make more sense to me. I posted what I had done as an explanation to crutschow about the weird AD620 symbol in the OP's schematic.
I'm sure you know that you could have edited AD620.asy to modify the SYMATTR line to reflect the location of YOUR AD620.cir file.
In retrospect, I should have let crutschow continue to wonder why the symbol was weird. It would have saved both you and me a lot of time.

Thanks, no sweat for me on the edit to make it work.
But why does it simulate oscillations this low threshold of load current?
That seems wrong.

Roff · Feb 9, 2024

Tony Stewart said:
Thanks, no sweat for me on the edit to make it work.
But why does it simulate oscillations this low threshold of load current?
That seems wrong.

I don't understand. The input is a 1 kHz voltage source.

Tony Stewart · Feb 9, 2024

Roff said:
I don't understand. The input is a 1 kHz voltage source.

What do you not understand from https://www.electro-tech-online.com...ate-hours-to-be-performed.165576/post-1447684 ?

try attached Run for 1 minute

Roff · Feb 9, 2024

Tony Stewart said:
What do you not understand from https://www.electro-tech-online.com...ate-hours-to-be-performed.165576/post-1447684 ?

try attached Run for 1 minute View attachment 144447

OK, now I see the glitches when I run the sim. They didn't show up with the value of Rg that I was using.
It's obviously a problem with the behavioral model.

Newbie question - basic simulation with amplifier AD620 which necessitate hours to be performed

New Member

Well-Known Member

Well-Known Member

New Member

Well-Known Member

Well-Known Member

Well-Known Member

Well-Known Member

Well-Known Member

Well-Known Member

Well-Known Member

Attachments

Well-Known Member

Well-Known Member

Attachments

Well-Known Member

Well-Known Member

Well-Known Member

Well-Known Member

Well-Known Member

Well-Known Member

Attachments

Well-Known Member

Similar threads

Privacy & Transparency

Privacy & Transparency