Hello

You don't have to make a symbol.
You can use the opamp2 symbol supplied with LTspice.
The opamp2 symbol is in the opamps section in the component selector.
After you place the opamp2 symbol on the schematic, change the symbol "value" attribute to OPA1611.
Make sure the OPA1611.LIB file is in the same folder as the schematic.
Add the directive .lib OPA1611.LIB so LTspice will know where to find the model file.

See attached Test Circuit.

View attachment 221808

Can you use the .asc I'm enclosing to see if it works as it should? It takes longer than it should to make it run. Please replace the existing opamp with the OPA1611. Please do tell me if you need any other file. Look at how fast the results show running with the LT1115.

 

Hi

I made some changes to the sim shown in rectangular boxes. I assumed you wanted 35VDC with 2Vpp@1khz ripple.
It looks like both opamps begin to oscillate at about 200ms. I had to increase R6 to ~100 ohms to get the OPA1611 to converge, but then it would no longer regulate.

 

Hi

I made some changes to the sim shown in rectangular boxes. I assumed you wanted 35VDC with 2Vpp@1khz ripple.
It looks like both opamps begin to oscillate at about 200ms. I had to increase R6 to ~100 ohms to get the OPA1611 to converge, but then it would no longer regulate.

View attachment 221850

How do you get that oscillation, and why I do not see it?

On the regulator I need 30v at the output.

If you can send to me, even if zipped, the files I need to run the regulator with the OPA1611.

There's a guy at the official Jung regulator thread that is using the OPA with excellent results.

 

How do you get that oscillation, and why I do not see it?

On the regulator I need 30v at the output.

If you can send to me, even if zipped, the files I need to run the regulator with the OPA1611.

There's a guy at the official Jung regulator thread that is using the OPA with excellent results.

What is he using for R6 with the OPA1611?. If I change R6 to 1k it regulates nicely at 30Vdc.

The schematic you posted is missing model files.
You have the same schematic I have, just make the changes I showed in boxes.
You need to run the simulation longer.....about 1.5 sec to see it regulate.

 

Do I get to do anything else besides renaming the pins?

You can draw lines, circles, ellipses, arcs, move pins, move lines , ........

 

What is he using for R6 with the OPA1611?. If I change R6 to 1k it regulates nicely at 30Vdc.

The schematic you posted is missing model files.
You have the same schematic I have, just make the changes I showed in boxes.
You need to run the simulation longer.....about 1.5 sec to see it regulate.

View attachment 221875

OK, how I adjust to 1,5 sec to see it regulate?

This the official and superproven circuit:

https://diyaudiostore.com/products/super-regulator

Can't go from 10 to 1K. It's not in the schematic.

Please, no changes, except for OPA1611. Any other change is not allowed, except to adjust output values.

Getting to use OPA1611 I what I need to do. With stability.

 

OK, how I adjust to 1,5 sec to see it regulate?

Change the .tran statement to

.tran 0 1.5 startup

"startup" tells LTspice to ramp up all voltage sources from 0v

This the official and superproven circuit:

https://diyaudiostore.com/products/super-regulator

I couldn't find the schematic showing the OPA1611.

Can't go from 10 to 1K. It's not in the schematic.

Please, no changes, except for OPA1611. Any other change is not allowed, except to adjust output values.

Getting to use OPA1611 I what I need to do. With stability.

I recommend you speak with TI regarding the OPA1611 model.

 

No, the original project does not include the OPA1611. They suggest AD825 and AD817.

But recent tests from one user suggest the OPA1611 as providing better specs. As you can plug in and try different types, it's worth a try. I'm just trying to simulate it first.

Pleas read this regulators comparison test.

https://linearaudio.nl/sites/linearaudio.net/files/v4 jdw.pdf

At the end, Walton centered on four specific opamps, the best being the AD797, which has instability issues, and the OPA134.

As I mentioned above, I couldn't make the OPA134 work either. Same family as the OPA1611.

So my question on this thread is for someone to show me how to make the OPA1611 or OPA134 to work with this .asc file.

And TI will not help you solve these issues, or LT.

 

hi carl,
As a check I have downloaded and unzipped the @eetech00 zip file, post #24, it works OK.
Have you tried the download.?
E

 

hi carl,
As a check I have downloaded and unzipped the @eetech00 zip file, post #24, it works OK.
Have you tried the download.?
E

There's no zipped file in post # 24

 

Woops!
It is post #19.

 

Well, I moved the files to a working and tried .asc file of the regulator, I think I managed to make it work, even if I had to wait a long time for calculations, and the psrr were similar to most, not as good as the AD797.

Now I wonder: how do you do or is it possible to convert any op-amp into a part like those listed in LT's directory?

 

hi,
If you have to wait a long time there must be a problem in your system.
On my two PC's the simulation is almost instantaneous.

Use the method described by eetech00, using OPOPA2 symbol as a template, post #19 again.

E

 

hi,
If you have to wait a long time there must be a problem in your system.
On my two PC's the simulation is almost instantaneous.

Use the method described by eetech00, using OPOPA2 symbol as a template, post #19 again.

E

No, the problem is in the model. If the model is fine the response is always instantaneous. I know a model is not right when it takes longer to simulate.
This happens on my PC, on my laptop and on my wife's laptop.

 

And TI will not help you solve these issues, or LT.

But they will tell you if the model is good and if the part is compatible with your design.

 

But they will tell you if the model is good and if the part is compatible with your design.

Where?

 

Where?

TI Tech support forum

 

hi carl,
A quick way that works for me.
Change the .lib extension to .net
Open it with LTSpice.
Highlight subckt OPA1611 in the net listing

Left click and select Create symbol...
It will create a yellow box.
If you don't like the yellow box, open the asy file and re build the symbol,,, do NOT erase the pin names just the box outline to suit a common OPA/
E

Added my version of the symbol,,, change the extension from .txt to .asy


BTW: The symbol can be found in the Auto Gen file under the F2 key

THANK YOU SO MUCH