Thanks for uploading. I'll have a look.

Please upload missing symbols for: 1) INV_1 in cursed simulation speed.asc 2) BUF_1 in lots of HF Transdiode-noise.asc 3\) INV\_1 and AND\_2 in Transnoise and Cursed\.asc 4) INV_1 in waveform error2.asc 5) INV_1 in Transnoise.asc I have found and fixed the issues in Cursed.asc and Transdiode-noise.asc. More when I have the missing symbols. Thanks.

@andyfierman I also used logic gates from another library: [https://drive.google.com/file/d/16hG99W1_uuQrV6nsxCrqZAQxoO8jAkjZ/view](https://drive.google.com/file/d/16hG99W1_uuQrV6nsxCrqZAQxoO8jAkjZ/view) but i tested if the bugs in the circuits would still occur even if someone doesn't has those extra components. I tested that by installing LTspice on a different PC (also Windows 8.1) and the glitches do still occur, so it really doesn't matter if you have this external component library.

Ok, I'll carry on playing with your sim files.

@Krischna, I will post a link to some fixed or commented LTspice files shortly. In summary however, the basic problem you have with all the sims that you posted in your link (which seems to be extracts of the same basic big circuit) is that they have too many over simplified models of things like the diodes and using simple snap action switches for the MOSFET drivers. You also have a lot of spurious unconnected floating stuff. These are all things that make the simulator have to work very hard to solve the thousands of matrix equations to run the simulation. Things like huge dynamic ranges together with instantaneously switching edges are classic causes of fconvergence failure in any simulator. Adding diodes in series with the switches used to model the MOSFETs also complicates the simulation for no reason: MOSFET do not have series channel diodes. IGBTs behave like they do but not MOSFETs. MOSFETs have parasitic body diodes as you have modelled but using more realistic diode models may help convergence. Good call using the continuous function version of the MOSFET model switches though! A lot of the art of successful simulation is to spot what can safely be simplifed and what needs attention to detail and accurate modelling. Also recognising when to break a circuit up into sections and to model and simulate eaqch section standalone and then building simplified behavioural models of previous stages to feed into the next stage. Even using LTspice's ability to save outputs as .wav files and then use those as input table to PWL sources to drive as inputs to later sections. Getting a sim to run is as much about how you craft it in the first place as it is about actually running it and interpreting the results. I recommend you spend time reading the links I will post for you and that you join LTspice group on Groups.io (what was the Yahoo group). You also need to lower your expectations of what a simulator is capable of. All simulators are just glorified calculators and the quality of the results, like any program, depend on the quality of the information that you put in. In the case of simulators this is as much about how the simulation circuit is crafted as the skill and quality of the modelling. I do not know what other simulators you have used but in my experience you would actually have a much harder time getting any of the sims that you posted to run in most of the big name (and big money!) simulation tools. One of the reasons EasyEDA moved from Ngspice to LTspice is because people were spending too much time trying to get their sims to run and not enough time getting anything useful out of them (and we were spending a lot of time posting bug reports and trying to get models to run). Ngspice is an excellent simulator but it takes a lot of experience to get good results out of it and as such it is not a beginner friendly simulation engine. Here are some links to source of information about modelling and simulation that I think you may find helpful. The whole of the Help file for LTspice is sprinlked with useful hints and tips. And this is an absolute goldmine: Ltwiki.org Good section on convergence issues. See also the explanation of tripdt and tripdv faor a and B sources. LTwiki has some very useful stuff about using BI sources with a cap in parallel instead of BV sources to improve convergence. I use that trick a lot and there is a section about it in my tutorial here: [https://docs\.google\.com/document/u/1/d/1OWZVVFRAe\_2NW3WratpkA\_SGuHa5AcRow5ZRfvcoVTU/pub\#h\.3ygebqi](https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub#h.3ygebqi) You will find some useful insights in my tutorial anyway: just go through the whole thing and play with the examples: [https://docs\.google\.com/document/u/1/d/1OWZVVFRAe\_2NW3WratpkA\_SGuHa5AcRow5ZRfvcoVTU/pub](https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub) This is very useful for a number of tricks and tips: [http://www.beigebag.com/resources.htm](http://www.beigebag.com/resources.htm) And: [http://www.5spice.com/html/links-tutorials.html#Tutorials](http://www.5spice.com/html/links-tutorials.html#Tutorials) The manuals for SIMetrix have a lot of very good information and a few tips on modelling, in particular about convergence issues in spice: [https://help\.simetrix\.co\.uk/8\.4/simetrix/simulator\_reference/topics/introduction\_overview\.htm](https://help.simetrix.co.uk/8.4/simetrix/simulator_reference/topics/introduction_overview.htm) and this is a must have (and free!) book: [http://www.designinganalogchips.com/_count/designinganalogchips.pdf](http://www.designinganalogchips.com/_count/designinganalogchips.pdf) [http://www.designinganalogchips.com/](http://www.designinganalogchips.com/) BTW, did you know that Superspice and Micro-Cap (Spectrum soft) and both now freeware? [https://www.anasoft.co.uk/index.htm](https://www.anasoft.co.uk/index.htm) [http://www.spectrum-soft.com/download/download.shtm](http://www.spectrum-soft.com/download/download.shtm) Both sites have links to excellent articles and newsletters about modelling: [http://www.kevinaylward.co.uk/ee/index.html](http://www.kevinaylward.co.uk/ee/index.html) [http://www.spectrum-soft.com/news.shtm](http://www.spectrum-soft.com/news.shtm) [http://www.spectrum-soft.com/usernotes.shtm](http://www.spectrum-soft.com/usernotes.shtm)

This is worth reading too: [https://www.analog.com/media/en/technical-documentation/lt-journal-article/ltjournal-v24n4-01-df-spicedifferentiation-mikeengelhardt.pdf](https://www.analog.com/media/en/technical-documentation/lt-journal-article/ltjournal-v24n4-01-df-spicedifferentiation-mikeengelhardt.pdf)

@Krischna, Fixed or commented copies of your sim files are attached as a zip to this empty project: [https://easyeda.com/andyfierman/responses-to-everything-wrong-with-ltspice](https://easyeda.com/andyfierman/responses-to-everything-wrong-with-ltspice)