| Author |
Message |
Allen
Guest
|
 Posted:
Thu Oct 27, 2005 12:10 pm Post subject:
how to use awd to view spectre command line simulation resul |
|
|
I've done some simulation using spectre command line with some
parameters sweeping. When I view the simulation results using AWD, I
can only find the result for the last value of the parameter that I
swept. Could anyone tell me how to find the results for other parameter
values? Maybe I didn't use "sweep" function properly? Thans.
|
|
| Back to top |
|
 |
Andrew Beckett
Guest
|
| Posted:
Sun Oct 30, 2005 9:10 pm Post subject:
Re: how to use awd to view spectre command line simulation r |
|
|
On 27 Oct 2005 01:18:08 -0700, "Allen" <oceandai@yahoo.com> wrote:
| Quote: | I've done some simulation using spectre command line with some
parameters sweeping. When I view the simulation results using AWD, I
can only find the result for the last value of the parameter that I
swept. Could anyone tell me how to find the results for other parameter
values? Maybe I didn't use "sweep" function properly? Thans.
|
I can't see why this shouldn't work. Are you using the middle-mouse->Create ROF
over the psf directory name in order to create the "Run Object File" that AWD
needs?
Note, this is not needed if you're using the newer wavescan tool.
Andrew. |
|
| Back to top |
|
|
Allen
Guest
|
| Posted:
Mon Oct 31, 2005 9:10 am Post subject:
Re: how to use awd to view spectre command line simulation r |
|
|
Yes, I've been trying both tools (AWD and Wavescan) and I was able to
get the results. However I've been using "Sweep" function, I can only
find the result for the last value, say, I sweep inductance from 1nH to
10nH, after the simulation I can only find the result for the
simulation with 10nH inductor. Could you please tell me how to get the
result for other values? Thanks.
Andrew Beckett wrote:
| Quote: | On 27 Oct 2005 01:18:08 -0700, "Allen" <oceandai@yahoo.com> wrote:
I've done some simulation using spectre command line with some
parameters sweeping. When I view the simulation results using AWD, I
can only find the result for the last value of the parameter that I
swept. Could anyone tell me how to find the results for other parameter
values? Maybe I didn't use "sweep" function properly? Thans.
I can't see why this shouldn't work. Are you using the middle-mouse->Create ROF
over the psf directory name in order to create the "Run Object File" that AWD
needs?
Note, this is not needed if you're using the newer wavescan tool.
Andrew. |
|
|
| Back to top |
|
|
Andrew Beckett
Guest
|
| Posted:
Mon Oct 31, 2005 5:10 pm Post subject:
Re: how to use awd to view spectre command line simulation r |
|
|
I can't see why this wouldn't work. Similar things work fine for me. Can you
post the netlist, or a simplified form of the netlist?
Andrew.
On 30 Oct 2005 21:26:59 -0800, "Allen" <oceandai@yahoo.com> wrote:
| Quote: | Yes, I've been trying both tools (AWD and Wavescan) and I was able to
get the results. However I've been using "Sweep" function, I can only
find the result for the last value, say, I sweep inductance from 1nH to
10nH, after the simulation I can only find the result for the
simulation with 10nH inductor. Could you please tell me how to get the
result for other values? Thanks.
Andrew Beckett wrote:
On 27 Oct 2005 01:18:08 -0700, "Allen" <oceandai@yahoo.com> wrote:
I've done some simulation using spectre command line with some
parameters sweeping. When I view the simulation results using AWD, I
can only find the result for the last value of the parameter that I
swept. Could anyone tell me how to find the results for other parameter
values? Maybe I didn't use "sweep" function properly? Thans.
I can't see why this shouldn't work. Are you using the middle-mouse->Create ROF
over the psf directory name in order to create the "Run Object File" that AWD
needs?
Note, this is not needed if you're using the newer wavescan tool.
Andrew. |
|
|
| Back to top |
|
|
Allen
Guest
|
| Posted:
Tue Nov 01, 2005 9:10 am Post subject:
Re: how to use awd to view spectre command line simulation r |
|
|
Hi Andrew,
Here is a simiplified version of my netlist. When I run the sumulation
I typed "spectre input.scs", please let me know if you have any
suggesstion. Thanks a lot.
Allen
simulator lang=spectre
global 0
parameters indu=1n
include "/home/dai/6HP/models/spectre/definitions.scs"
include "/home/dai/6HP/models/spectre/design.scs"
include "/home/dai/6HP/models/spectre/process.scs"
include "input_CMOSLNA_modified.scs_new"
R29 (net064 0) resistor r=50 m=1
R28 (net096 net074) resistor r=59.9m m=1
R27 (net0002 net072) resistor r=3.2m m=1
C29 (net0002 0) capacitor c=183f m=1
V11 (net0999 0) vsource type=pwl wave=[0 0 50p 0 51p 10m 101p 10m 102p
0]
R26 (net075 net049) resistor r=59.9m m=1
R_PCB0 (net068 net0001) resistor r=1m m=1
R25 (net0001 net051) resistor r=3.2m m=1
C28 (net0001 0) capacitor c=183f m=1
R16 (net155 net74) resistor r=3.2m m=1
R18 (net0003 net76) resistor r=3.2m m=1
R_PCB3 (0 net0003) resistor r=1m m=1
C23 (net0003 net0003) capacitor c=183f m=1
C19 (net0003 net0003) capacitor c=183f m=1
R14 (net0003 net82) resistor r=3.2m m=1
R23 (net068 net0999) resistor r=50 m=1
R17 (net133 net78) resistor r=59.9m m=1
R19 (net81 net80) resistor r=59.9m m=1
R15 (net85 net84) resistor r=59.9m m=1
R13 (net155 net88) resistor r=3.2m m=1
R5 (net147 net90) resistor r=59.9m m=1
L33 (net072 net096) inductor l=89.000p m=1
L32 (net074 net169) inductor l=indu m=1
L32 (net074 net169) inductor l=5n m=1
L31 (net051 net075) inductor l=89.000p m=1
L30 (net049 net112) inductor l=indu m=1
L27 (net78 net98) inductor l=indu m=1
L29 (net76 net81) inductor l=89.000p m=1
L28 (net80 net104) inductor l=indu m=1
L25 (net84 net104) inductor l=indu m=1
L26 (net74 net133) inductor l=89.000p m=1
L23 (net88 net147) inductor l=89.000p m=1
L24 (net82 net85) inductor l=89.000p m=1
L15 (net90 net98) inductor l=indu m=1
C26 (net096 0) capacitor c=70f m=1
C24 (net075 0) capacitor c=70f m=1
C20 (net133 0) capacitor c=70f m=1
C21 (net155 0) capacitor c=183f m=1
C22 (net81 0) capacitor c=70f m=1
C18 (net85 0) capacitor c=70f m=1
C9 (net147 0) capacitor c=70f m=1
C17 (net155 0) capacitor c=183f m=1
V0 (net0004 0) vsource dc=2.5 type=dc
R_PCB4 (net155 net0004) resistor r=1m m=1
// ---------------------------------------
indu_sweep sweep param=indu values=[1n 3n 5n 7n 9n]
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27
\
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5
maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 ckptclock=1800 \
sensfile="../psf/sens.output"
tran tran stop=15n write="spectre.ic" writefinal="spectre.fc" \
annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
saveOptions options save=allpub |
|
| Back to top |
|
|
Svenn Are Bjerkem
Guest
|
| Posted:
Wed Nov 02, 2005 1:10 pm Post subject:
Re: how to use awd to view spectre command line simulation r |
|
|
In article <1130825984.920345.247720@g44g2000cwa.googlegroups.com>,
oceandai@yahoo.com says...
| Quote: | indu_sweep sweep param=indu values=[1n 3n 5n 7n 9n]
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27
\
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5
maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 ckptclock=1800 \
sensfile="../psf/sens.output"
tran tran stop=15n write="spectre.ic" writefinal="spectre.fc" \
annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
saveOptions options save=allpub
|
What happen if you do:
indu_sweep sweep param=indu values=[1n 3n 5n 7n 9n] {
tran tran stop=15n write="spectre.ic" writefinal="spectre.fc" \
annotate=status maxiters=5
}
Use resultbrowser in awd and click with left button on the wanted signal
of *any* sweep run to bring up the calculator. press the plot or erplot
buttons and the calculator will plot your wave family.
--
Svenn |
|
| Back to top |
|
|
Allen
Guest
|
| Posted:
Sat Nov 05, 2005 9:10 am Post subject:
Re: how to use awd to view spectre command line simulation r |
|
|
Svenn Are Bjerkem wrote:
| Quote: | In article <1130825984.920345.247720@g44g2000cwa.googlegroups.com>,
oceandai@yahoo.com says...
indu_sweep sweep param=indu values=[1n 3n 5n 7n 9n]
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27
\
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5
maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 ckptclock=1800 \
sensfile="../psf/sens.output"
tran tran stop=15n write="spectre.ic" writefinal="spectre.fc" \
annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
saveOptions options save=allpub
What happen if you do:
indu_sweep sweep param=indu values=[1n 3n 5n 7n 9n] {
tran tran stop=15n write="spectre.ic" writefinal="spectre.fc" \
annotate=status maxiters=5
}
Use resultbrowser in awd and click with left button on the wanted signal
of *any* sweep run to bring up the calculator. press the plot or erplot
buttons and the calculator will plot your wave family.
--
Svenn
|
Hi Svenn,
That worked. Thanks a lot.
Allen |
|
| Back to top |
|
|
|
|
|
|
FAQ
Memberlist
Register
Profile
Log in to check your private messages
Log in