Is it possible to simulate microstrip components in pspice? i.e. quarter wavelenght stubs as bandpass filters... Open ended stub would be a series resonant short, grounded end would be a parallel resonant open.
Yes, but RTFM. I have a stripline part placed in my personal library by a Garmin engineer, back when I was doing GPS chip designs, but I don't know how it works.
...Jim Thompson
-- | James E.Thompson, P.E. | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona Voice:(480)460-2350 | | | E-mail Address at Website Fax:(480)460-2142 | Brass Rat | |
If you're using it as a "one port" device (i.e., the other end is terminated in a known impedance, including an open or a short), sure -- just compute the input impedance of the line as a function of s (that is, j*omega). The closed-form expression for a terminated transmission line is slightly messy (it's in any book covering transmission lines -- download
If you won't be having to sweep over a wide range of frequency, figure out the input impedance at a nominal figure and equate that to an equivalent R, L and/or C -- it'll be an OK narrowband approximation. In the case of 1/4 wave stubs for bandpass filters, synthesis sizes the lines such that they're equivalent to a given inductor or capacitor anyway; the results end up being slightly (but not significantly) difference than keeping the L and C's fixed components.
Simulating lossless transmission lines in SPICE is easy, because for transient analysis they're just a time delay whereas for AC analysis they're just a phase delay (proportional to frequency). Simulating lossy transmission lines is not at all easy, and you can find many papers that advocate different approaches. Most of the fancier simulators have lossy transmission line models built in, and it's best to use those unless you have a LOT of time on your hands.
There are several free programs out there such as Elsie and the AADE Filter Designer that will simulate ladder networks consisting of lumped elements and transmission lines for you, if you goal here is just to perform simulations and you're not sold on SPICE. I believe they use ABCD networks to perform the analysis -- programmatically, this is about the simplest way to implement it (something like designing and analyzing a bandpass filter built from microstrip lines using your own Matlab, MathCAD, etc. routines is a very common homework problem in university classes).
---Joel Kolstad
That's true for IDEAL lines. I'm pretty sure that there is a dissipative model in there as well.
...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC\'s and Discrete Systems | manus |
| Phoenix, Arizona Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |
I love to cook with wine. Sometimes I even put it in the food.
I have a vague memory of them being a problem in TRAN simulations. Something about the required (small) step size causing very slow simulations. But that might have been just for Pulse waveforms.
Robert
The basic problem was how to not miss transitions when you have transmission lines, one of the solutions was to reduce the max step size to one half of the shortest tline delay. If you had really small tlines, then this could really increase the simulation time...
Charlie
Pspice has lossy and lossless transmission lines.
BTW, a one time there was a bug, not sure if it has been fixed. Basically if you set up a lossy transmission line circuit, ac analysis, sweep length and plot signal at some F vs length, then you see a discontinuity, a sudden change in slope. Reltol needs to be set much smaller (/100?) which then fixes this. Plot is then smooth as would be expected. Reltol doesn't affect ac compute time AFAIR.
-- Malcolm Malcolm Reeves BSc CEng MIEE MIRSE, Full Circuit Ltd, Chippenham, UK (mreeves@fullcircuit.com, mreeves@fullcircuit.co.uk or mreeves@iee.org). Design Service for Analogue/Digital H/W & S/W Railway Signalling and Power electronics. More details plus freeware, Win95/98 DUN and Pspice tips, see: http://www.fullcircuit.com or http://www.fullcircuit.co.uk NEW - www.CharteredConsultant.co.uk - The Consultant A-List
The reason there are numerous lossy transmission line models out there is that some of the early ones had problems in that they were non-passive. In such cases, if you choose the right terminations (just R's, L's, and C's) you can create a non-stable system and get oscillations out of "nowhere." Later ones would include passivity at the expense of accuracy and presumably these days there are very good models available that are both stable and passive... but I'm not at all up to date on the models used in any particular simulator.
I would be wary of anyone's simulator that doesn't tell you whose lossy transmission line model they're using!
---Joel
AFAIR it is in one of the manuals - all greek to me though :-). AFAIR each end of the lossy transmission line is a volt and current source pair. These model the line impedance, voltage, current, black box style. Maths links the two ends. This does mean that the two ends are floating so you need to 0V reference each end which of course is different to a real circuit.
P.S. Sorry for emailing you Joel - I clicked the wrong button - DOH!
-- Malcolm Malcolm Reeves BSc CEng MIEE MIRSE, Full Circuit Ltd, Chippenham, UK (mreeves@fullcircuit.com, mreeves@fullcircuit.co.uk or mreeves@iee.org). Design Service for Analogue/Digital H/W & S/W Railway Signalling and Power electronics. More details plus freeware, Win95/98 DUN and Pspice tips, see: http://www.fullcircuit.com or http://www.fullcircuit.co.uk NEW - www.CharteredConsultant.co.uk - The Consultant A-List
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.