after hours of faffing, if i change the transistors for 2N2222 transistors it seams to simulate every time.

the bug must be in the spice model or in how easy eda handles spice models and reports errors "Simulation Gatway Timeout" is defiantly not a helpful error message

"i made it public if it helps"
https://easyeda.com/editor#cmd=new_schematic,cmd_for_project=2b75c7513fbd421eb2629e4c5107ab0b



You have made a blank schematic sheet public.

It may help you to read and follow the instructions in:

https://u.easyeda.com/forum/topic/How-to-make-a-Project-public-and-share-the-links-to-it-9f006513b84b412580910905b0281d20



It may also help you to read the Simulation Tutorial (3) in (2) in:

https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a



where you will find extensive information about how to successfully start up simulations, in particular those involving symmetrical multivibrators such as your example.

one year on and this simulator still wont simulate a basic transistor, if i build a circuit with standard resistors from the "Commonly Library"
(side not, is "Commonly Library" not bad English, "Common Library" or "Common Components") ?
it simulates every single time but as soon as you introduce a 2N2222 from the same "Commonly Library" the simulator fails with "ERROR: Gateway Timout" 99% of the time you press simulate.

Please post a link to a public project so that it can be examined.

@andyfierman i sent you personally a link to the project JDND01818R1 about 10 hours ago when I posted the question
i think i did anyway anyway, it said invite sent

i have since worked out the problem is something to do with the value of the resistor at the NPN gate.
in the screenshot posted bellow R17 has a value of 1M and R18 has a value of 1K
if i change the value of R18 to 1M then the simulation files almost every time with meaningless error "Gatway Timeout"
it does not appear to fail if the NPN is actually in the schematic, only if there is a high resistance connected at the base of any 2N2222

There are two problems with your simulation.

One is that you have forgotten that 1MegOhm in Spice must be written as 1Meg and not 1M.

Please re-read the Simulation Tutorial for advice on this.

The other problem is with EasyEDA and I do not know what is causing it. Simulation in EasyEDA runs on LTspiceXVIII. If I recreate your simple Sim Test circuit: and run it in LTspice XVIII or export the LTspice netlist from your Sim Test schematic then it works fine (even with your 1 milliOhm base resistance).

So there is something wrong with how LTspice is being configured in EasyEDA.

Unfortunately, I have no control over that so I can only raise this as a Bug Report to EasyEDA Support.

thanks, i always thought m was milliOhm and M was megOhm, why would LTspiceXVIII make up there own rules to confuse people.
anyway, thank you, im glad to see its something in the LTspice configuration, not just me going mad.
i hope somone can work it out in the end.
are you saying there is a simple way i can export the data from EasyEDA sim to LTspice XVIII somwhere in order to test my circuits now?
i am running a ubuntu a computer, can i install LTspice XVIII and export the easyEDA data to that to run a simulation from EasyEDA schematic?

This is why I wrote and keep banging on about it being essential that people read all of the Simulation Tutorial before attempting simulation in EasyEDA. All these topics are covered in there and so it saves me writing the same stuff over and over again.

https://docs.easyeda.com/en/Simulation/Headings/index.html





"...why would LTspiceXVIII make up there own rules to confuse people."

These are not rules set by LTspice. They are rules set by Larry Nagel in the early 1970's when he wrote his PhD theses when he first created spice. It is possible that the units convention was derived from an earlier program called CANCER.

"are you saying there is a simple way i can export the data from EasyEDA sim to LTspice XVIII somwhere in order to test my circuits now?"

Yes.

File > Export Netlist > LTspice for This sheet

"i am running a ubuntu a computer, can i install LTspice XVIII and export the easyEDA data to that to run a simulation from EasyEDA schematic?"

Yes.

I too run Linux.

Install the most up to date stable version of WINE.
Download LTspice from here:

https://www.analog.com/en/resources/design-tools-and-calculators/ltspice-simulator.html



Just open the download file and WINE should install it OK.

Note: I am still running LTspiceXVIII. I have not tried installing LTspice24 yet.

You will need to do a little hand editing of the netlst to make it run properly in LTspice.

To help you get started, I have pasted an edited copy of the netlist from my test sim:

https://oshwlab.com/andyfierman/simulation-problem-240427

** Sim Test **
Q16 VM2 Q16_1 GND 2N2222
R21 VM2 VIN 1K
R22 Q16_1 VM1 1MEG
V3 VM1 GND PULSE(0 5 1M 1M 1M 10M 20M)
V4 VIN GND 20

** Using asterisks, I have commented out the lines below from
** the original EasyEDA Netlist:
*.SAVE VM2 VM1
*.tran 40m
*.inc standard.bjt

** Then I have added the lines below to keep LTspice happy
** about where it's models and libraries are kept and for
** consistency, put the tran statement where LTspice puts it
** in a netlist.

.model NPN NPN
.model PNP PNP
.lib C:\users\andy\Documents\LTspiceXVII\lib\cmp\standard.bjt
.tran 40m
.backanno
.end

"i hope somone can work it out in the end."

Me too, because I have no access to the running of LTspice for EasyEDA.

:)

https://en.wikipedia.org/wiki/SPICE

Seems to work OK now.

I have asked if the user error warning can be improved.

:)