Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.
i used to simulat switched c filters in spice, i used to put at the input 2 sources each with different frequancy and do transient simulation and then take the fft of the time domain output
Apply at input during one clock period 1V and them comput the FFT of the impulse response, that should be equal to the frequency response. The frequency resolution depends on the number of simulated clock cycles.
but if i want to compute the noise
i must use .noise in the hspice
i hear that there is a method of using
a source and the inductor to take the place of the cap,but i don not konw that
who can tell me ???
thanks a lot
For sc-circuit on conventional spice there are some methods.
1. Check AC for each switch state. Most have onyl two. So you can check output noise (not input refered output noise!). Stability and so on.
2. For a transfer function run transient with a gaussian random source at the input and doing a FFT.
3. For linearity use 2 tone and choose a common dominator frequency for the two tones a_n_d the clock. Run a transient 3 times the common dominator period. Make a FFT with rectangular window over the last two periods. So you could observe spectral leakage from the inital transients.
AC and noise direct is only possible with spectreRF
thanks alot
but if in the first phase
the capacitor is charged or discharged
,need i replace the capacitor with
a voltage source and then do the second phase's
ac abalysis???but in the ac i can not kwon how mang voltage it is .
how can i do ????
For conventional spice you do an AC for both phases. Simply measure the output noise. The AC transfer form the input could be zero because of the switching state.
This method only record two noise densities over time. It does not take into account noise capturing in the caps and transfering this to the output. I had problems in the past with spectreRF doing a similar analysis. SpectreRF is combining the noise contributions from all noise source over a period of a harmonic response. So what spectreRF requires is a nonzero transfer function from each noise source to the noise analysis output. But in sc circuit the transfer is by storage. So a noise voltage captured in the first phase which does not transfer to the output at the same time is negleated.
I have read a paper from Gabor Themes some years ago whci describe some of the difficulities analysing sc noise. The practical way seems to me the following:
1. Use a simulator which could extract noise voltage density between two nodes.
2. Use a voltage controlled voltage source if 1. fails.
3. Analyse the noise voltage density over each cap in your sc circuit.
4. Calculate by hand the time discrete transfer function of each cap voltage to the output. You have two, each phase!
5. Fomulate the transfer function in the z-domain
6. Combine the voltage noise densities at the caps with the z-transfer functions.
Via that way you should have the accurate output voltage noise density.
the best way to simulate SC circuits is to use spectre from c@dence
it is found is c@dence custom IC , and ver 5 is working under linux
spectre uses an algorithm which superimposes the ac analysis over the transient analysis
which means that u can simulate switched C easily with spectre, and i guess they are the only people which use this algorithm, and this is the secret for there simulator being the top in mixed signal design
i have an application note having all details and how to simulate switched c using cadence, so if anyone interested , i can upload
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.
