The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design >> RF Design >> vco design
https://designers-guide.org/forum/YaBB.pl?num=1111127922

Message started by s.venkatareddy on Mar 17^th, 2005, 10:38pm

Title: vco design
Post by s.venkatareddy on Mar 17^th, 2005, 10:38pm

i am doing project on pll. in designing of vco circuit i am facing problem. i used differential ring oscillator for vco.in that i used four stages.it not oscillating automatically by itself but if i provide an initial condition of 10u micro volts by using capacitor its oscillating.
can any body help me in oscillating without initial condition.

Title: Re: vco design
Post by Eugene on Mar 17^th, 2005, 10:49pm

In the real world, there is always enough noise to start the oscillator. However, most simulators model noise only in the frequency domain; they do not have time domain noise unless you insert it with a random number generator. Consequently, there is usually no noise source to start oscillations in a model. You can start the oscillations either with initial conditions or with a fictitious stimulus, such as a single short sharp current impulse on any node with a finite impedance to ground.

Title: Re: vco design
Post by venkata reddy on Mar 18^th, 2005, 4:22am

thanku u for ur answer.
but how to put that initial condition in layout.i think u will reply .help me in drawing vco gain(vcontrol vs frequency) in spectre.

Title: Re: vco design
Post by Eugene on Mar 18^th, 2005, 8:19am

It sounds like you are trying to simulate the same schematic you want to lay out and do not want to clutter your layout schematic with an ic or fictitious source. First, although I do not have much experience at back end of the design, I am about 60% sure you can still insert initial conditions without cluttering the schematic. If you chose the fictitious source alternative, you should be able to kick off the oscillation by stimulating an external node, a node in the test bench. If you kick the system anywhere hard enough, you are bound to start the oscillation. No need to worry about a 10MegaAmp kick for example, since it's only a simulation you will not damage anything.

Title: Re: vco design
Post by venki_vlsi on Mar 20^th, 2005, 6:15am

hi thanks for ur answer.

can u plz tell how to draw vco gain in cadence using spectre.(vcntl vs frequency).we r using cadence gui interface.we can operate with mouse.tell me how to do it in gui.

Title: Re: vco design
Post by Eugene on Mar 20^th, 2005, 8:41am

I know of no way within the Cadence tool set to simply draw the tuning curve (control versus frequency curve) with a mouse. However, I have successfully used two other very reasonable methods for specifying the VCO tuning within the Cadence environment.

1. Use Matlab, Mathematica, or Excel to fit a well behaved analytic function to the data and enter the function using a behavioral source. The behavioral source could be implemented using one or more primitive non-linear controlled sources or with a behavioral language such as VerilogA or SpectreHDL. OK, this method started with tools outside the Cadence environment but I suspect everyone has at least a spreadsheet tool.

2. Implement a look up table feature within a VerilogA module or with SpectreHDL. SpectreHDL has a LUT feature that VerilogA does not.

Title: Re: vco design
Post by Andrew Beckett on Mar 20^th, 2005, 11:06pm

Actually Verilog-A does have a lookup table. $table_model has existed for some time now (I believe it was introduced in IC50 MSR1 - and so it is in IC5033 and IC5141 and MMSIM60).

Andrew.

Title: Re: vco design
Post by Eugene on Mar 21^st, 2005, 8:38am

Cool. Thanks for the tip Andrew. Does VerilogA now also let you pass strings as parameters, so we can parameterize the name of the data file for the look up table?

Title: Re: vco design
Post by James on Mar 31^st, 2005, 11:53pm

venki_vlsi

Quote:

can u plz tell how to draw vco gain in cadence using spectre.(vcntl vs frequency).we r using cadence gui interface.we can operate with mouse.tell me how to do it in gui.

I use the following method in Cadence:

1. Do parametric analysis (Tools->Parametric analysis...), to set vcntl as the sweep parameter and change it from V1 to V2

2. Start the simulation (Choose Transient analysis in the Analog Environment Window)

3. Use caculator to choose the output of the VCO, then use Clip (Special Function) to choose appropriate time range and Frequency Function to see the curve of Vcntr Vs. Frequency.

Is it a correct way? ::)