--- In LTspice@..., Panama Mike <panamatex@y...> wrote:
Norbert,
If I were placing a MOSFET e.g. W=5u L=0.5u , and the length of
the
source and drain implants might be LS=1u LD=1u. LS,LD could be
defined with a .PARAM spice directive.
In some netlisters, the parameters AD AD PD PS NRS NRD can be
calculated automatically, e.g. AD=W*LD PD=2*LD+2*W NRS=LD/W.
Can the LTSpice netlister do this?
I can set .PARAM LD=1u, and I can use it in the "Monolithic
MOSFET"
popup attribute menu, but I can't pick up the device W for the
equation {W*LD} to enter in the AD box.
Yes. There's three ways to do it.
i) If using the nmos4 symbol you get the "Monolithic
MOSFET" dialog box. For length, type in {L}. And
then place a SPICE directive on the schematic such
as .param L=10u or ".step param L list 5u 7u 8u"
ii) How down the control key and right click on the body.
Enter L={L} on one of the attributes, SpiceModel, Value,
Value2, SpiceLine or SpiceLine2. These attribute names
mean nothing. Their values are concatenated for the
netlist.
iii) Move the mouse to the value of the MOSFET and right click.
Edit it to be something like "NM L={L} W={W}"
--Mike
__________________________________
Do you Yahoo!?
The New Yahoo! Search - Faster. Easier. Bingo.
Thanks Mike, that does work - but then the parameterization
is valid only for the 1 instance.
Every instance of the MOSFET symbol would need its
own .PARAM statement, and the maths entered manually.
In the end, the only way I could achieve what I wanted
was to copy the 'nmos4' MOSFET symbol, and make it a hierarchical
block 'norbmos4'
I then created a schematic 'norbmos4' for the new symbol, instantiated
an 'nmos4' in it with {L} {W} {M} for L W M and e.g. {LDIF*W} for
AD
etc.
Now I can instantiate any number of 'norbmos4' devices, add
PARAMS 'W=10u L=0.5u M=5' to this schematic block, and one
.PARAM LDIF=1u directive.
All I can say at the moment is that this netlists,and the simulator
doesn't complain - whether it works or not for simulation I don't
know yet.
The downside is that every NMOS device on my schematic is now a
'norbmos' subcircuit containing an 'nmos4'. The upside is that the
typical parasitics should be calculated for me.
On to my second day of using LTSpice .... looks good so far!
Regards,
Norbert.
