Hi, From your public project https://easyeda.com/hetashrim/New_Project-P4ECOMJHF, It is too complex for simulation. EasyEDA hasn't such spice simulation model. In this case , you need to build a PCB and do some test with real components.

Hi, Thank you for your reply. Is there any other alternative that you can suggest me? For example, can I download the Spice model of the IC from EasyEDA? Regards,

@dillon Hello, Now, I mainly want to see the waveforms of IC DS90C401 through simulation. I am getting same errors for that too. Is it not possible to simulate this particular IC on EasyEDA as you mentioned or I have made some errors with the connections? Could you please help me out again? Thanking you.

@dillon Sorry I forgot to attach the link. https://easyeda.com/editor#id=qic6oGYg9 This is the schematic of that IC. Regards,

Hi Hetashrim, Welcome to EasyEDA. It may be possible to simulate your circuit in EasyEDA but there are several steps to take before that can happen. Analog Devices do supply spice models for the AD8201, AD8332 and AD8333 devices. However, we have not included them in our library and have not tested them in EasyEDA for ngspice compatibility. We can do this but for models of this complexity it make take some while. You also need to be aware of how a spice model is associated with a schematic symbol. It is possible to map the model onto the symbol you have used but it is more usual in spice simulation to create and use simplified symbols that, for example, do not show the multiple ground or supply pins that are on the physical package. Unfortunately there are no publically available models for the TI DS90C401 device. However, we have a fairly crude behavioural model of an LVDS transmitter. For more information, please see this thread: https://easyeda.com/forum/topic/Compatible_IC_models_and_How_to_include_the_model_to_IC-9jhfBXUSQ For more information about simulation in EasyEDA, you may also like to have a look at: https://easyeda.com/Doc/Simulation-eBook/

@andyfierman Hello Andyfierman, Your post was really helpful. The LVDS transmitter you have created also seems perfect for my application. No IC manufacturers have spice models for it. In fact, this is the first time I could actually see the waveforms of LVDS on a simulation software. Thank you so much for sharing the model you built. The main problem is that I need to simulate the LVDS driver alongwith AD8333 to proceed with my project. Now that I can use this LVDS model, if somehow I can also import spice model of AD8333 and simulate, it will be like a blessing :) Is there a possibility that I can import or associate a new model to these schematic symbols based on their spice files on EasyEDA platform? Kindly share any further suggestion/help you have to guide me. Best regards,

Hetashrim, 1) First I recommend you start off by reading the whole of: https://easyeda.com/Doc/Simulation-eBook/Device-models.htm#Device-models and: https://easyeda.com/Doc/Simulation-eBook/Schematic-symbols-prefixes-and-pin-numbers.htm and getting your head round the examples. 2) Then you need to download a copy of the AD8333 spice model from AD: http://www.analog.com/media/en/simulation-models/spice-models/ad8333p.cir Open it in a text editor to see how many pins it has, what they are called/numbered and in what order they are. Then **Create a new Spice Symbol** for it so that the number of pins and spice pin order matches that of the spice subckt model. 3) Draw a schematic of the simplest possible test jig using the new symbol for the device. Do not try anything fancy because if it fails to run (and it probably will) then it can be a nightmare to debug (and it probably will). 4) Import the spice model into your schematic. The easiest way to import a spice model is simply to copy and paste it into your schematic as described here: https://easyeda.com/Doc/Simulation-eBook/Schematic-symbols-prefixes-and-pin-numbers.htm#For-SUBCKT-defined-models 5) Set up a simple transient simulation and try running it. AD models are not brilliant: I have had trouble even getting some of their basic opamp models to run in ngspice and these are a bit more complex! Your sim will probably fail but if you can't figure out why, don't worry. Just post back here and I'll try to debug it. If you're new to simulation you probably need to work through the eBook and play with copies of the examples first to get the hang of it. :)

@Hetashrim, A very quick look at the AD8333 model shows that it uses the IF(x,y,z) function which is not available by default in ngspice (which EasyEDA uses for the simulation engine). Therefore you would have to add a `.func` statement to your copy of the AD8333 model, to include the EasyEDA IF() function. The IF() function: `.func ifx(x,y,z) {ternary_fcn(x, y, z)}` is described here: https://easyeda.com/editor#id=9lR8qICUc For more see: https://easyeda.com/Doc/Simulation-eBook/Functions.htm#Functions There may be other ngspice incompatibilities in the AD8333 (and AD8332) models: I haven't had chance to look at them in detail yet.

@andyfierman Hi Andy, Wow, thank you so much for the detailed guideline :) It will help a lot. I will surely follow these steps and try my best to get it done. Once again, thank you.

@Hetashrim, See how you get on with this: https://easyeda.com/andyfierman/AD8333_test_jig-8WQK20JDV :)

@andyfierman You are the saviour :) It seems perfect. So now I can use this symbol alongwith the '.options' statement in my schematic? Many thanks for this wonderful help. :)

`So now I can use this symbol alongwith the '.options' statement in my schematic?` That's correct. Just search for the `AD8333` spice symbol (*not* the other AD8333 symbols with suffixes) using the **SHIFT+F** library search, (it is under the `User Component` tab) and place it into your schematic, replacing the symbol you used originally. Then paste in the `.options rshunt = 1.0e12` statement and a copy of the spice model from my example into your schematic, remembering to set them both to `text attribute > spice` If you need the AD8201 and AD8332 models, please post back, though at this stage I can't promise to be able to make them work in EasyEDA. :)

AD8021 model and symbol are good to go: https://easyeda.com/andyfierman/AD8021_test_jig-qKWw6FfPN Note that the `Logic Reference` and `notDISABLE` pins are not modelled.

@andyfierman Hi, All of my problems are solved now. I really cannot thank you enough.Thank you for your time and instant help. I will connect the circuit again using your models and post the updates to you. :) :) Best regards,

@andyfierman Hey I know I have already got a lot of favours but I have just one more favour to ask. Does EasyEDA have spice model for any of the LNA ICs. In AD8332 also, my main need is just LNA. Its quite okay if there is no such model. I can use two sources with 2.5V offset as you have used for your AD8333 model. But if you know any simulatable IC which gives LNA function, kindly suggest me. Thank you. :)

Looking at your original schematic, you are only using one channel of the AD8332 so I will try to fire up the AD8331 LNA model. Would that be OK?

@andyfierman That would be awesome actually. :)

AD8331 LNA stage only spice symbol, model and simulation: https://easyeda.com/andyfierman/AD8331LNA_stage_test_jig-3BNBzwu42 Sorted. :)

@andyfierman Great! Many many thanks Mr. Andyfierman for your support and help. I am really grateful. I will update you about how it goes. God bless you :)

If this all works for you, it would be great if you could tell eveyone via blogging, Facebook and Google+ etc., how wonderful you think EasyEDA is! # ***:*** **)** ...If it *doesn't* work for you, please tell us why or what you'd like us to improve. :) p.s. Don't forget, you can buy PCBs for your finished project direct from EasyEDA! > https://easyeda.com/Doc/Tutorial/PCBOrder.htm

@andyfierman I will surely post about this awesome software platform and its instant userfriendly support. I will also recommend it to all my friends. And if I find any further problem, I will post back to you. It was a wonderful experience. Thank you. :)

@andyfierman Hello, I have constructed my circuit using your models. But when I run the project, it gives some errors saying few parameters had to be ignored. I have divided my project into 2 parts, the first part which contains AD8331(LNA) works perfectly. But while running the whole project, simulation fails somehow. In the second part I have included LVDS and AD8333. When I tried to run only this document, it runs only for 1.6ns! Simulating only LVDS also works fine. https://easyeda.com/editor#id=kqPN9ljhe|wHBTN5nFX This is the link. Could you please have a look and guide me on why it runs only for such a small period or why it ignores certain parameters? Thanking you.

Could you clarify a couple of things? Are you running each of the two sheets separately using `Run the Document`? Or are you running the whole projects using `Run the Project`? It also looks like I have some fixing to do of the LVDS TX model. Sorry about that...

@andyfierman When I run the whole project using 'Run the Project', the parameters like trise and tfall are being ignored and I don't get any waveforms. But when I select 'Run the document' for the schematic containing LVDS and AD8333, I get waveforms but it goes only till 1.6ns. And its okay if you need some time to check the LVDS model. Please update us when you look into it. :)

@Hetashrim, Fixed it. I have fixed the typos in the LVDS and the AD8021 models so those warnings have gone. In your schematics, you have a couple of easy-to-make-but-harder-to-spot mistakes. 1) The differences between running a single sheet sim using `Run the Document` and running a multisheet sim using `Run the Project` take a bit of getting used to. `Run the Project` simulates the whole circuit represented on all the sheets in a project so - as you have correctly assigned - all the prefixes need to be unique. However you also need to check that all the netnames are consistent and this is where you have made a couple of minor errors. `Run the Document` simulates only the single sheet you have selected to run in a project. It then completely ignores anything in the other sheets in that project. Therefore if, for example, your power supply is on a sheet other than the one you have selected to run, then the selected sheet will have no power. And that is what had happened with your IQ sheet. There are no +/-5V supply sources on that sheet. Adding a pair of supplies to generate rails netlabeled as +5V and -5V, fixes the problem and it then runs OK using `Run the Document`. However it is a bit more complicated than that because in your other sheet you have a pair of +/-5V rails labelled as VCC and VEE so even when you use `Run the Project` the IQ sheet still has no power because it's rails are called +5V and -5V so they don't connect across the sheets. If you change the +/-5V supply netlabels so that they are the same on both sheets (say VCC and VEE but you can use any names you like) then using `Run the Project` will run OK. But the IQ sheet will not run on it's own because ngspice does not find the supplies on the unused sheet. What you *cannot* then do is to add a pair of V sources with the *same* supply rail netnames (i.e. VCC and VEE ) to the IQ circuit so that it runs OK using `Run the Document` because if you then use `Run the Project`, ngspice will complain because you have connected the respective VCC and VEE sources on both sheets together in parallel which is not allowed. So, if you want to run the sheets separately, give one sheet a pair of voltage sourced supplies and associated nets labelled as VCC1 and VEE1 and do the same on the other sheet but lebelling things as VCC2 and VEE2 or some such scheme. Both sheets have the same supplies but will then run either individually or as a project. 2) The other mistake you made is very similar to what I have just described. You have two separate voltage sources, one on each sheet but they are both connected to a net labelled as `IN`. That works OK when running the individual documents but throws an error when running the project because then the two sources are shorted in parallel! So, just change the name of one of them (even if they are supposed to be the same signal, as long as both sources are set up the same you won't be aware of the difference). 3) One last point that you may not have picked up on (but which may not affect you in this sim). You can only use the text-in-the-schematic form of the Spice Analysis directive (i.e. typing `tran 2u 2u` etc. directly into a schematic and setting it to text type = spice) to run a **Document**. You cannot run a **Project** using that syntax. To run a **Project**, if you have no active spice directive typed directly in the schematic then you can use the **CTRL+R** Hotkeys or the **Green Man** button and select `Run the Project`. If you have an active spice directive typed directly in the schematic then you *must* use the **Green Man** button and select `Run the Project`. To run a **Document**, if you have no active spice directive typed directly in the schematic then you can use the **CTRL+R** Hotkeys or the **Green Man** button and select `Run the Document`. If you have an active spice directive typed directly in the schematic then you can use the **CTRL+R** Hotkeys or the **Green Man** button and select `Run the Document`. This allows you to run two different sims depending on what you enter the text and the dialogue box for the two run options. Note that you can also easily switch between different sims (and things like parameter values, expressions and function statements) by entering different statements and directives but only making a subset of them active (text type = spice). Leaving the rest inactive (text type = comment) makes them invisible to ngspice. Neat or what? :)

A small clarification: Adding a pair of supplies to generate rails netlabeled as +5V and -5V, fixes the problem and it then runs OK using Run the Document. However it is a bit more complicated than that because in your other sheet you have a pair of +/-5V rails labelled as VCC and VEE so even when you use Run the Project the IQ sheet still has no power because it's rails are called +5V and -5V so they don't connect across the sheets. If you change the +/-5V supply netlabels so that they are the same on both sheets (say VCC and VEE but you can use any names you like) then using Run the Project will run OK. But the IQ sheet will not run on it's own because ngspice does not find the supplies on the unused sheet. Should read as: However it is a bit more complicated than that because in your other sheet you have a pair of +/-5V rails labelled as VCC and VEE so even when you use Run the Project the IQ sheet still has no power because it's rails are called +5V and -5V so they don't connect across the sheets. If you change the +/-5V supply netlabels so that they are the same on both sheets (say VCC and VEE but you can use any names you like) then using `Run the Project` will run OK. But the IQ sheet will not run on it's own using `Run the Document` because ngspice does not find the supplies on the other, ignored sheet. Adding a pair of supplies to generate rails netlabelled as +5V and -5V, to the IQ sheet fixes the problem and it then runs OK using either `Run the Document` or `Run the Project`.

@andyfierman Awesome! Explained in the best way possible. Thank you so much for giving your time to explain in such details. I will follow your suggested steps and I am sure this time it will work fine :) Thank you.