Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
Oct 21st, 2020, 6:23pm
 Pages: 1
 SPICE Non Linear Capacitor Modeling (Read 354 times)
 HA New Member Offline Posts: 4 SPICE Non Linear Capacitor Modeling Jan 21st, 2017, 5:06pm   I am trying to define a verilog A element which has a user defined Voltage-charge relationship of the type V=a*Q+b*Q^2 (a and b are user defined constant). The element closest to this is capacitor (V=Q/C) which is straightforward to implement in VA by assigning current using ddt. Can anybody help which is the best way to implement this system. I am not sure VA handles Q. THanks!! Back to top IP Logged
 Ken Kundert Global Moderator Offline Posts: 2294 Silicon Valley Re: SPICE Non Linear Capacitor Modeling Reply #1 - Jan 24th, 2017, 6:42am   See Modeling Varactors.-Ken Back to top IP Logged
 HA New Member Offline Posts: 4 Re: SPICE Non Linear Capacitor Modeling Reply #2 - Jan 24th, 2017, 11:08am   Thanks a lot Ken!!I had actually seen this link before and this is the reason I am here (it was written to post any questions here).I should have made my question more clear. I am trying to model an element in which we cannot represent charge as an explicit function of voltage. For e.g., V=a*Q+b*Q^2+c*Q^4If i take its derivative, C=dQ/dV----> C=f(Q). Since i cannot express Q explicitly, i cannot write I<+ddt(Q).Would really appreciate your comment on this. Back to top IP Logged
 Ken Kundert Global Moderator Offline Posts: 2294 Silicon Valley Re: SPICE Non Linear Capacitor Modeling Reply #3 - Jan 24th, 2017, 1:35pm   Oh, that is interesting. I think you model it as follows: Code:```real q; analog begin q = idt(I(cap)); V(cap) <+ f(q); end ```-Ken Back to top IP Logged
 HA New Member Offline Posts: 4 Re: SPICE Non Linear Capacitor Modeling Reply #4 - Jan 25th, 2017, 10:06am   This works like a gem. Thanks for sharing this.  :)I have one more question. If i connect this element in a ckt, say in series with normal capacitor (C1)...then KCL requires that dQ/dt of both the elements should be same.     C1      C2 (self defined VA based cap)----||------||------ If my transient signal has no dc level then Q as well as dQ/dt are same on both the capacitors. However, for a signal with an offset or with a dc level, only dQ/dt is same not the absolute charge Q since SPICE forces the middle potential to ground though gdcpath, thereby Q from C*V are different.What should be the real picture. If someone do measurements on this ckt, will he sees the same? I checked with the simulation that if capacitors are leaky, the node potential equilibrate depending on the leakage resistance of the two capacitors.Thanks Back to top IP Logged
 Pages: 1