Upload your .asc file (and any library or model files that are not
included in the LTspice installation) to our Temp directory and we might
be able to help.

If there is more than one file, zip them together (.zip, please; NOT rar
or 7z or gz or ...) No need for any .raw, .net, or any other files. And
definitely no useless image files (.jpg or .png or whatever.) They don't
simulate at all :-)

Donald.
--

Adding a bit more to what Donald already wrote:

What we need are your schematic (.asc file), ALL symbols (.asy files) that didn't come with LTspice, and ALL SPICE models that didn't come with LTspice.? Without these, we can't open your schematic to see what's in it.? Do not include the output files (.raw, .log, or .net unless it's a SPICE model).

As you should know already, the place to upload is the group's "Temp" directory.? The link to it is on the group's main page.? Navigate to that directory first before clicking the "+New" button to start the upload.

If you insist on pictures, they should be uploaded to the group's "Photos" section.? Keep in mind that (1) we can't simulate a screen shot, and (2) with the schematic and models, everyone here can see the results so we probably don't need a photo.? They rarely help.

Please do not use "third party" file storage websites.? This group has its own File and Photo areas.? Use them.

I think you wrote that your simulation worked before, and then it doesn't work right anymore.? I wonder if you have some idea what you changed.? SOMEthing must have changed.? Don't assume that you used the standard settings.??How long ago did you have the working simulation?

Andy

I don't know if this helps -- but there are files already in our group for the TPS43060.? Perhaps the TPS43060 and TPS43061 are similar?? Look in this folder:

Files / z_yahoo / Files sorted by message number / msg_115005
/g/LTspice/files/z_yahoo/Files%20sorted%20by%20message%20number/msg_115005/

I think one of the problems with that model was double {{curly braces}} in TI's model.? That doesn't make sense for LTspice.

Andy

I have uploaded the files to the Temp folder. No pictures included, with the provided files you can do your own simulation runs anyhow.

cedrichirschi.21, I downloaded and ran your simulation.

It 'works'.? However, my results apparently differed from yours.? And it has those "errors" in the error log.

The output voltage V(out) overshoots twice to >4.7 V, then stabilizes at 3.48 V and stays there.? It reaches that by 1 ms, which apparently differs from your result which shows it exceeding 12 V.

The circuit you uploaded is not the same one in your screenshot.? There may be only a few differences, but they could be significant, and anyway the screenshot doesn't show hidden properties which might be there in the schematic.? (That's why we need actual .asc schematics, not screenshots.)

Could you repeat your simulation with the same circuit you uploaded to this group?? Before running it, also go to the Control Panel > SPICE tab, and click "Reset to Default Values", just to be sure that you really have the original un-altered settings.

It might actually be meaningless to do anything now with this simulation until the "errors" in the models are corrected.? Some model errors can be ignored because they don't affect the results, or have only a minor effect.? However, in this case I suspect the effects of these errors are too much to ignore.

Those errors would have been there when you ran this simulation before too.

Andy

FYI, when a SPICE model is poorly made or has math errors, it can force the simulator towards extreme voltages and currents.? This can cause those spikes you saw.

Behavior of components in SPICE models should be continuous in both value and derivative.? Many models are not.? Many models, including those from respectable IC manufacturers, have abrupt discontinuities (due to things like IF() statements in formulas) and they can make the simulation go haywire.

Andy

cedrichirschi.21,

Hmm, I need to modify what I wrote before.? If I re-run your simulation, I get different results after the first one.? One of mine even looks similar to your screenshot (png file).

Most SPICE simulations should simulate exactly the same every time -- unless there is an explicit random source (unlikely).? However, some models or simulations do behave a little randomly, which I don't understand.? It has been suggested in this group (but never confirmed) that LTspice has a tiny amount of randomness built-in, which helps prevent it from being stuck when something like a singular matrix comes along.? (Simulated circuits tend to be ideal and exactly balanced.??The randomness nudges it slightly, letting it get past the problem point.)

Andy

开云体育

This randomness may be inherent in the routine that adjusts the time-step around discontinuities. The finite bit-depth can result in at least an LSB variation between different runs. It could be much larger, but the probability would be a steeply-decreasing function of variation size.

cedrichirschi.21,

Hmm, I need to modify what I wrote before.? If I re-run your simulation, I get different results after the first one.? One of mine even looks similar to your screenshot (png file).

Most SPICE simulations should simulate exactly the same every time -- unless there is an explicit random source (unlikely).? However, some models or simulations do behave a little randomly, which I don't understand.? It has been suggested in this group (but never confirmed) that LTspice has a tiny amount of randomness built-in, which helps prevent it from being stuck when something like a singular matrix comes along.? (Simulated circuits tend to be ideal and exactly balanced.??The randomness nudges it slightly, letting it get past the problem point.)

Andy

cedrichirschi.21,

I edited the TPS43061 model file to remove all bad instances of the {{double curly braces}}, and remove the unused Td parameter.? I will upload it soon.? It eliminated all the errors.? But the behavior seems similar.

I am puzzled why the switching outputs from the TPS43061 to the CDS86330Q3D never switch when the output voltage stabilizes.? Is that expected?

The amount of overshoot seems to depend on the size of the load resistor.? More load -> less overshoot.

When the Enable pin goes negative, it is for less than 10 picoseconds.? I think it's in the part of the simulation where LTspice struggles, perhaps fighting with bad model formulas.? The timesteps become very small there, less than a femtosecond.??After the output stabilizes, the simulation proceeds much much much faster.

Andy

John wrote, "This randomness may be inherent in the routine that adjusts the time-step around discontinuities. The finite bit-depth can result in at least an LSB variation between different runs."

Sorry, but I am not buying it.? For what reason would LTspice add an intentional 1-LSB or few-LSB variation in the timesteps?

Andy

开云体育

It's not intentional, it's inevitable. Just think what happens, or so we are told. LTspice hits a large difference between sample x and sample x-dt,? where dt is the time-step, so it backs up to sample x-ndt, where n might vary? at the LSB level and tries again with a smaller dt; how much smaller might vary at the LSB level. There is inevitably at least an LSB uncertainty about the digital rendition of any quantity.? If the quantity is itself small, the LSB uncertainty is relatively big.

John wrote, "This randomness may be inherent in the routine that adjusts the time-step around discontinuities. The finite bit-depth can result in at least an LSB variation between different runs."

Sorry, but I am not buying it.? For what reason would LTspice add an intentional 1-LSB or few-LSB variation in the timesteps?

Andy

The nice thing about digital computers, is that they always give us the same results to the same calculations with the same inputs.? There is no possibility of having a different answer, unless either the inputs differ, or an intentional random difference was added to the calculation.? One LSB difference doesn't just happen on its own.

There can be an LSB of uncertainty between an analog quantity and its digital representation.? Or between an exact calculation (with infinite resolution) and a calculation with limited resolution.? But when I ask you to add integers 4 + 6, you'd better always get an answer of 10, and not 9 or 11 (= 10 +/- 1).

FYI, when LTspice needs to back up, it backs up to the previously saved good point.? Then it makes the timestep smaller.? With SPICE2, it made the timestep 1/8 what it was, but LTspice seems to use a different scaling.? Regardless of what that scale number is, there is no reason for it to be 1/8 sometimes, 1/7.9999999999999 sometimes, and 1/8.0000000000001 sometimes (starting from the same point), unless LTspice intentionally gives it that randomness.? It won't just happen because of round-off errors.? It'll be the same every time, because that's how math works on a digital computer.? Same inputs through same calculations --> same results, down to the very last bit.? Even rounding off a calculation is the same every time.

Andy