VCO Simulation Problem via AWR Microwave Office - Page 1
Forum section: electronics / rf-microwave

author: MrBalthazar
author_rank: Contributor
timestamp: September 08, 2024, 02:13:16 pm
content: Hello,I want to simulate a vco design with awr but I got unexpected results in the simulation.Where do you think I'm making a mistake?I get the spectrum output below even if I don't activate the transistor.This is the circuit I want to simulate:My AWR DesignVaractor ModelResult

author: RoGeorge
author_rank: Super Contributor
timestamp: September 08, 2024, 03:08:30 pm
content: Quote from: MrBalthazar on September 08, 2024, 02:13:16 pmNever tried MW office, but -300 dBm or lower means digital noise of the floating point arithmetic used by the simulator. That spectrum doesn't have much to do with the circuit. It means that the transistor does not oscillate at all.

author: MrBalthazar
author_rank: Contributor
timestamp: September 08, 2024, 03:12:00 pm
content: So what do you suggest? ADS simulation?

author: RoGeorge
author_rank: Super Contributor
timestamp: September 08, 2024, 03:26:34 pm
content: That's another simulator I never used. My go to is SPICE based simulators, the favorite being LTspice. Free to use and no limitation.For the oscillator to start, maybe change the transistor's beta, or adjust the ratio between C3 and C4. Another method to fast-start any oscillator is to put a current source in parallel with the LC rank, and pulse one period at the beginning, to "crank-start" the oscillator.

author: LM21
author_rank: Regular Contributor
timestamp: September 09, 2024, 05:58:37 am
content: LTspice oscillators usually start to oscillate if you have max time small enough. If the circuit is capable of oscillation. Some times components values are so extreme that a colpitts circuit does not oscillate.

author: RFDx
author_rank: Regular Contributor
timestamp: September 09, 2024, 06:25:43 am
content: Works in a SPICE based simulator. Try a normal cap instead of the varicap diode first. With 0.5p...7p the tuning range is 1.05...1.2GHz. Both BFR193 and BFP420 can be used. Output power (incl. harmonics) into a 50 Ohm load is about 0dBm @ max. frequency and somewhat less @ min. frequency. The bias point of the transistor isn't quite right yet and would benefit from some adjustment.

author: G0HZU
author_rank: Super Contributor
timestamp: September 09, 2024, 04:22:01 pm
content: Quote from: MrBalthazar on September 08, 2024, 02:13:16 pmIt looks like you are using the harmonic balance simulator to analyse this oscillator. If so, you need to include the oscillation probe tool in order to allow the simulator to analyse the large signal (steady state) condition using the harmonic balance engine.Harmonic balance simulates in the frequency domain and the system needs to be in a steady state (repetitive over infinite time) in order for it to provide a valid output. I think you need to add the oscillator probe for the system to be able to analyse a VCO like this.Also, looking at the oscillator circuit, I think you could have issues if you try and use a BFR193 BJT in a real circuit. This BJT may struggle to produce adequate negative resistance up towards 1200MHz, especially when you factor in the influence of real world components and a typical PCB layout.Also, I can't see how it can fully tune across 1000-1200MHz using the published circuit values.However, my main point is that I think that you aren't using the harmonic balance simulator correctly. You need to add the oscillation probe. You can also do a phase noise analysis if you add a noise analysis to the simulation.