Tools
Convert HSpice CMOS Library Files to PSpice CMOS Library Files - Manually
Macros
Noise Figure the easy way.....
Add the following two lines in the [MACROS] section of pspice.prb. Do it in the "Common" Directory to make it valid for all of your designs.
VSRCSQ = 16.5757565E-21*V(RSRC:1,RSRC:2)/I(RSRC)
NF = 10*LOG10((V(INOISE)*V(INOISE))/VSRCSQ)
In your schematic make sure you name the source
resistance "RSRC".
Setup your AC analysis, checking the "Noise enabled" box and designating an
"Output Node".
Perform the AC analysis, then, in Probe, Add, Trace, "NF". Voila!
Noise Figure is automatically plotted in Probe.
Displaying dBm values in PSpice Probe.....
Add the following line in the [MACROS] section of pspice.prb. Do it in the "Common" Directory to make it valid for all of your designs.
dBm(N,Z) = VdB(N)*sqrt(500/Z)
Where "N" is the node name where you have placed a (regular) voltage marker and "Z" is the reference impedance (normally 50 ohms). In Probe, go to Plot/X Axis Settings/Process Options and check the Fourier box before calling this macro.
Return Loss and VSWR.....
Add the following three lines in the [MACROS] section of pspice.prb. Do it in the "Common" Directory to make it valid for all of your designs.
MAGGAMMA=M(2*V(IN_NODE)-V(SRC_NODE))
RET_LOSS=20*LOG10(MAGGAMMA)
VSWR=(1+MAGGAMMA)/(1-MAGGAMMA)
Follow the naming conventions as given in the NF section above. In addition name the node adjacent to the AC source "SRC_NODE" and the node following RSRC as "IN_NODE". VSWR and RET_LOSS can then be called in Probe after an AC analysis.