Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

How do I measure power consumed in a subcircuit in TSpice?

Status
Not open for further replies.

saritac

Newbie level 3
Joined
Apr 26, 2004
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
35
TSpice help

Hi,
I have started using TSpice recently. How do I measure power consumed in a subcircuit and not the complete circuit, when I use a single voltage source.
please help

Thanks
 

goodboy_pl

Full Member level 5
Joined
Mar 12, 2002
Messages
253
Helped
16
Reputation
32
Reaction score
15
Trophy points
1,298
Activity points
3,119
Re: TSpice help

I Think this solution is general for all spice simulators:
u can define VCC/GND pins for each subckt and use current probe in each subckt to measure the supply current and use a simple function in waveform editor to see the power level.
in this way your ckt is ready for other simulation like dependency to supply/GND noise in each sub block and finding sensitive blocks.

BEST!
 

saritac

Newbie level 3
Joined
Apr 26, 2004
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
35
Re: TSpice help

Hi,
thanks a lot for replying back.

My problem is the part of the circuit for which I want power is not connected to Vdd directly. It is fed through output of another block which may have a Vdd. But I don't want the power drawn from that block in my result.

any suggestions please

Thanks again
 

vardan

Member level 1
Joined
Feb 4, 2003
Messages
34
Helped
2
Reputation
4
Reaction score
0
Trophy points
1,286
Activity points
261
Re: TSpice help

Hi!
For general case insert a zero voltage-source in your subcircuit's input. Then measure power. Other variants are possible too.
See example below.

* Power measurement
.model cmosn NMOS VTO= .7 KP=25U LAMBDA=.01 GAMMA=.5 PHI=.5
.model cmosp PMOS VTO=-.7 KP=10U LAMBDA=.01 GAMMA=.5 PHI=.5
M1n in Vdd gout Gnd cmosn L=.5u W=20u
M1p in Gnd gout Vdd cmosp L=.5u W=20u
Rload out 0 1Mega
Vdd Vdd 0 3
Vzero gout out 0
Vin in GND PULSE (0 3 0 1n 1n 98n 200n)
.tran .1n 250n
.print P1<W>='i(Rload)*v(gout)' P2<J>='(i(Vzero)*v(out))'
.print P3<W>='(-is(M1n)-is(M1p))*v(gout)' ; inward current is positive!
.power Vzero ; You can see report at the end of *.out file
.end

Vardan
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top