I forgot an opening quote. The lines should read: g1 1 2 i='if (time <= 1e-10) (1e-6 * v(1,2)) else (1e4 * v(1,2))' g2 3 2 i='if (time <= 1e-10) (1e4 * v(3,2)) else (1e-6 * v(3,2))' Regards. Hassan. On Mar 13, Hassan Ali <hassan@xxxxxxxx> wrote: > > > I toyed a little more with Kumar's idea. Here's the solution that works - > without long > simulation. > > Requirements: You need to know the common mode voltage at the driver output > for the corner > (fast, typ, slow) case of interest. Call that "V_cm". > > 1. In SigXplorer, go to Analyse -> Libraries. Choose Model Browser, filter for > ESpiceDevices, and click on any two-pin device (e.g. resistor50). > > 2. Click Add Model -> CloneSelection. Give a name to your clone e.g. "switch". > > 3. In the Model Browser now click on "switch" and then choose "Edit". A text > editor will > pop up. > > 4. Edit the model so that it reads as follows: > > ("switch" > ("PinConnections" > ("1" "2") > ("2" "1") > ) > ("ESpice" > ".subckt switch 1 2 > g1 1 2 i=if (time <= 1e-10) (1e-6 * v(1,2)) else (1e4 * v(1,2))' > g2 3 2 i=if (time <= 1e-10) (1e4 * v(3,2)) else (1e-6 * v(3,2))' > Vcm 3 0 V_cm > .ends switch > ") > ("Manufacturer" "myself") > ) > > > Remember to replace V_cm with the actual common voltage value. Save the file > when done. > > This ESpice element, all it does is to initialize the outputs to the > common-mode voltage > in the first 100ps of simulation. It does that by implementing two switches: > one to the DC > source that initializes the outputs, and another to the signal that comes > from the driver. > > With respect to the driver signal, the switch is opened (resistance=1megaohm) > in the first > 100ps and closed (resistance=0.1milliohm) after the first 100ps. It is > viceversa for the > DC source. > > 5. Close the model browser and close the Library browser by hitting OK. > > 6. Now place the "switch" ESpice device just before the DC-blocking cap - > with pin 2 > connecting to the cap. For a differential link you'll have to have two of > those devices - > one for each cap. > > 7. Simulate and see what happens. > > > Hassan. > > > On Mar 13, "Sanchez, Louis" <louis.sanchez@xxxxxxxxx> wrote: > > > > Hi Hassan.......... > > > > I should mention that the length of time it takes (number of pulses) is a > > function of the time constant formed by the Capacitance of the coupling > > caps, and the resistance of the load. You can play with the value of either > > the load resistance or the capacitance, and you should see the effect this > > has on the length of time it takes for the signals to stabalize. > > > > Lou A. Sanchez > > louis.sanchez@xxxxxxxxx > > > > -----Original Message----- > > From: Hassan Ali [mailto:hassan@xxxxxxxx] > > Sent: Wednesday, March 13, 2002 3:11 PM > > To: si-list@xxxxxxxxxxxxx > > Subject: [SI-LIST] Re: SPECCTRAQuest: DC level shift with series caps > > > > > > > > Thanks all for your suggestions. > > > > Actually, the sure way is that suggested by Lou - to run the simulation to > > death! > > Actually, in my case I had to run it for 2500 cycles! > > > > Kumar's trick is interesting. I tried it but it didn't really solve the > > problem. I still > > had to run the simulation for a long time to obtain 0V DC. I appended the > > "gsw 1 2 .." > > line (only one line) in the ESpice model of the capacitor. > > > > Thanks again all for the support. > > > > Regards. > > > > Hassan. > > > > > > On Mar 13, "C. Kumar" <kumarchi@xxxxxxxxx> wrote: > > > > > > try this. > > > > > > cdc 1 2 my_dccap > > > gsw 1 2 i='if (time <= 0) (1e3 * v(1,2)) else 0' > > > > > > Patrick_Carrier@xxxxxxxx wrote: > > > I agree with Lou. I know in Spice you can get around that anomaly by > > > specifying an initial charge condition on the cap. I don't think there is > > a > > > way to do that in Specctraquest though, so you need to just wait several > > > cycles to look at the waveform. > > > > > > --Pat > > > > > > -----Original Message----- > > > From: Sanchez, Louis [mailto:louis.sanchez@xxxxxxxxx] > > > Sent: Wednesday, March 13, 2002 10:55 AM > > > To: 'hassan@xxxxxxxx'; si-list@xxxxxxxxxxxxx > > > Subject: [SI-LIST] Re: SPECCTRAQuest: DC level shift with series caps > > > > > > > > > > > > Hello Hassan............ > > > > > > It will take several pulses before you see the expected results in an AC > > > coupled network. I believe that you are dealing with the initial condition > > > of time it takes for all storage elements (capacitors) to reach > > equilibrium. > > > I suggest that you lengthen the period of your analysis in the Preferences > > > section of SigXplorer. > > > > > > Lou A. Sanchez > > > > > > -----Original Message----- > > > From: Hassan O. Ali [mailto:hassan@xxxxxxxx] > > > Sent: Wednesday, March 13, 2002 6:49 AM > > > To: si-list@xxxxxxxxxxxxx > > > Subject: [SI-LIST] SPECCTRAQuest: DC level shift with series caps > > > > > > > > > > > > Hi All, > > > > > > I'm trying to use SigXplorer to simulate a link with a differential > > > driver and series DC-blocking caps. Contrary to expectations, > > > single-ended P and N outputs measured at the load are not centered > > > around 0V DC, instead each one is given a separate DC shift. When I > > > remove the series caps, the output is as expected - centered around 0V > > > DC. > > > > > > Does anybody know what I can do to have the correct single-ended outputs > > > with the series caps? > > > > > > Thanks. > > > > > > Hassan. > > ------------------------------------------------------------------ > To unsubscribe from si-list: > si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field > > or to administer your membership from a web page, go to: > <a href='//www.freelists.org/webpage/si-list'>//www.freelists.org/webpage/si-list</a> > > For help: > si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field > > List archives are viewable at: > <a href='//www.freelists.org/archives/si-list'>//www.freelists.org/archives/si-list</a> > or at our remote archives: > <a href='http://groups.yahoo.com/group/si-list/messages'>http://groups.yahoo.com/group/si-list/messages</a> > Old (prior to June 6, 2001) list archives are viewable at: > <a > href='http://www.qsl.net/wb6tpu'>http://www.qsl.net/wb6tpu</a> > > > > ------------------------------------------------------------------ To unsubscribe from si-list: si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field or to administer your membership from a web page, go to: //www.freelists.org/webpage/si-list For help: si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field List archives are viewable at: //www.freelists.org/archives/si-list or at our remote archives: http://groups.yahoo.com/group/si-list/messages Old (prior to June 6, 2001) list archives are viewable at: http://www.qsl.net/wb6tpu