BJT Error In ADS. Can not resolve it.

When I try to run this schematic it gives me the error that BJT1 is an instance of an undefined model BJTM1. And it gives error for every BJT that is in the circuit. How to solve this issue? Kind Regards

Using these devices from the Devices-BJT Palette you also need to place the BJT_Model component to define the device model parameters. You will need to place at least two, one for the NPN devices and one for the PNP devices maybe more if the devices are different. Each would need to have a unique ID like BJTM1, BJTM2 etc. and be reference by the Model parameter on each BJT symbol.

You will need to do similar changes to add the Diode_Model for the Diodes too.

Thanks for replying...can you please explain me step by step what i need to do....i didnt get it what you said....

---------- Post added at 13:27 ---------- Previous post was at 13:20 ----------

RealAEL i get I have to place "BJT_Model:Bipolar Transistor Model" in my schematic right? but it does not show any arrow for PNP, NPN and also how may I know which one is emitter leg? Do i NEED to place one model for each BJT or just a single model for all the BJTs please clarify....thanks

---------- Post added at 13:50 ---------- Previous post was at 13:27 ----------

RealAEL i added a seperate model for PNP, a seperate for NPN and a seperate for a DIODE. this is my schematic. However when I click on simulate it gives me some warnings (pics attaches) and the desired output is not coming. This is a noise circuit it should be producing noise at its output however its giving me something like this when i plot it on dbm......please let me know if my parameters are right on the plotting axis or not and what else is wrong here in the circuit. here are the attachments

You have red dots in the schematic showing that there are disconnected wires. For example all the DC sources have one end disconnected where there should be a ground connection. Also wires need to end on symbol pins and not just touch the body of the symbol to connect. For example look at +INPUT Port (Num=3), the wire to ground is not connected. In fact that wire and ground make no sense and should be removed. The diode on the far left is a model symbol (with no pins). This should be linked to a real diode symbol in the same way as the BJTs.

hi thankyou very much for pointing out these mistakes...I have rectified them and there is no warning....yet i am not able to see noise at the output. I have attached the changed schematic and the output which is not showing any noise...i hope u understand....thanks.......

Firstly, you are doing a linear s-parameter simulation so the oscillator circuit on the left will never work. In that configuration it is only possible to use Transient (Time Domain) Simulation.

Secondly the SP_NWA is for measuring 2 port s-parameters. Port 1 of the NWA should be connected to the input of the circuit and port 2 to the output. So remove the oscillator, connect the schematic input to port 1 of the NWA and the schematic output to port 2 of the NWA.

Finally for realistic simulation results you would need to include actual values for the transistor/diode parameters instead of using just the default values. You will need to research the actual devices you intend to use to determine realistic values.

So what do you suggest? should i shift to Pspice? i just want a simulation of the circuit....and it is becoming quite difficult in ADS....

When I try to run this schematic it gives me the error that BJT1 is an instance of an undefined model BJTM1. And it gives error for every BJT that is in the circuit. How to solve this issue?

Click to expand...

Either include a model library containing BJTM1 or refer to any of the BJT models shipped with ADS.

I wouldn't jump to any other simulator just yet. Where you are is close to the measurement you have selected, the Network Analyser. It really depends on what you are expecting to see. You need to select the type of simulator that will give you the style of results you are wanting to see. All simulator types are different.

There is one thing that is certan for ALL simulators. They all need accurate models for the active devices to get accurate simulation results. That applies to ADS, PSpice, HSpice, Spectre/SpectreRF or any other simulator that can use nonlinear Spice like models. Just leaving the default values for the model definition will not get any useful results.

So on to the simulation options.

1. Linear S-Parameter simulations. This is what you have set up in the schematic at the moment. The NWA will give you s-parameter, small signal style simulation data. That NWA though is a 2-port instrument so will give you S11, S12, S21 or S22 data. Port 1 is an output source that is connected to the input of the circuit under test and Port 2 is the load that connects to the output of the circuit under test. Just like any Vector Network Analyser you will have in a lab. This you can use to measure (mostly) the small signal performance of the amplifier in your schematic design. A VNA has to put out a finite power signal so strictly you can never measure true linear s-parameters but as long as this power is low enough then it is close. It will not measure the performance of the oscillator.

2. Harmonic Balance non-linear simulations. This can be used to measure large signal performance of your amplifier. This would include data such as Pout vs Freq, Pout vs Pin and therefore IP3 or gain compression. You could also see the Output Power spectrum like using a Spectrum Analyser on the circuit. Most of this applies to the amplifier only. It is possible to use Harmonica Balance to simulate the steady state performance of the oscillator like Frequency of oscillation and Pout but this would require some adjustment to the oscillator circuit to enable this steady state oscilation to be created. Harminic Balance can also be used to simulate Large Signal s-parameter like measurements if required.

3. Transient non-linear simulations. Time domain simulation that can be done in ADS or PSpice and other Spice based simulators. This would give you measurements of time domain data like Vout vs Time and any other measurement that can be derived from this voltage data. This could include converting the time domain voltage data to voltage spctrum data using FFT methods if required. Again transient simulation can be used to simulate the oscillator but again some specifiic technique will need to be employed to trigger the oscillations to start, this will not usually happen by itself, and also the simulation would need to be run for sufficient time to get past the start-up transient until the oscillation was running at steady state to get useful data.

So the question remains what are you expecting to see? What type of measurements do you need to simulate? The answer to that question should indicate what simulation technique you need to use.

ADS can do all three of these type of measurement. PSpice can only do #3. Again ALL simulators will require more accurate device models to get accurate simulation data.

What I would do would be first to split the circuit in two, the amplifier and the oscillator. I would use Linear s-parameter simulations on the amplifier on its own to get started. I would then use Harmonic Balance to continue the analysis further. I would then use Harmonic Balance again on the oscillator to study the steady state performance of the oscillator. I would not use Transient analysis (like PSpice) for Steady State simulation as it typically takes too long. It would be useful if start-up transient analysis is required though.

Then once the two parts were known to be working separately then it would be time to join the two together are probably use Harmonic Balance simulation to simulate the entire circuit.