Re: Not even ... (lame parameter stepping)
Panama Mike wrote: Oh, yes, now I see the problem. There was a problem introduced.
If you add the line ".param R=5K" the circuit will fail
but the line2 ".param" or ".param R=5K nix=3K" will not
cause it to fail. There be an update next week (we're on
vacation today and tomorrow) that will also accept the old
syntax.
Thanks for reporting the problem. Hi Mike, Just checked, and the bug with stepped parameters that are also explicitly defined at the end of a parameter statement is back (or never got properly squashed). Without adding the closing "nix" parameter the simulation refuses to run as before.
|
Steve, I haven't been able to figure out how to plot the Middlebrook
function in the sample Mike posted. Is there only one Plot.def file
or should it be saved as Middlebrook.def if the file name is
Middlebrook.asc? How do you use the function in a plot command
after it has been defined? Some kind of step by step or point me to
where in the help file I can find help on this would be appreciated. It's a new feature. Make sure you have the current version, 2.04. Then create/edit the file from the waveform window menu command Plot Settings=>Edit Plot Defs File. There is only one plot.defs file, the one in the same directory as the scad3.exe executable. On another note, is there a way to use a dot command to load a plot
setting file when a simulation is run. No, but this should be added, that is, the ability to load the plot settings in the file mysim.plt whenever mysim.asc or mysim.cir is run. --Mike __________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month!
|
I haven't been able to figure out how to plot the Middlebrook
function in the sample Mike posted. Is there only one Plot.def file
or should it be saved as Middlebrook.def if the file name is
Middlebrook.asc? How do you use the function in a plot command
after it has been defined? Some kind of step by step or point me to
where in the help file I can find help on this would be appreciated.
On another note, is there a way to use a dot command to load a plot
setting file when a simulation is run.
|
Re: Open Loop response for OpAmp And New User-Defined Functions for Plotting Released today.
Thanks Mike,
?
That should be quite useful. I don't get this level of service from the simulator I pay $100,000 a seat for!
?
Regards,
??????????? Steve
Panama Mike wrote:
Steve,
I've added user-defined functions to LTspice.? From a waveform window execute
Plot Settings=>Edit Plot Defs File to create and edit the file.? You might want
to enter the line
.func middlebrook(x,y) = (x*y-1)/(x+y+2)
Then you can more easily plot the exact loop gain from a closed loop system.? Below is your
circuit showing the exact loop gain and the approximated by just the voltage gain.
Version 4
SHEET 1 2168 1300
WIRE 416 64 416 80
WIRE 320 192 416 192
WIRE 416 160 416 192
WIRE 416 192 512 192
WIRE 96 160 96 144
WIRE 96 240 96 224
WIRE 96 320 96 336
WIRE 96 64 96 48
WIRE 128 192 240 192
WIRE 32 208 64 208
WIRE -80 320 -80 288
WIRE -80 208 -80 176
WIRE -80 176 64 176
WIRE 304 384 272 384
WIRE 272 384 272 288
WIRE 272 288 320 288
WIRE 384 384 464 384
WIRE 464 384
464 288
WIRE 464 288 384 288
WIRE 704 416 704 448
WIRE 592 192 656 192
WIRE 656 192 656 336
WIRE 656 384 464 384
WIRE 704 336 656 336
WIRE 656 336 656 384
WIRE 272 384 -128 384
WIRE -128 384 -128 176
WIRE 112 608 112 560
WIRE 112 688 112 672
WIRE 112 768 112 784
WIRE 112 480 112 464
WIRE 144 640 448 640
WIRE 48 656 80 656
WIRE -64 736 -64 720
WIRE -64 640 -64 624
WIRE -64 624 80 624
WIRE 288 832 256 832
WIRE 256 832 256 736
WIRE 256 736 304 736
WIRE 368 832 448 832
WIRE 448 832 448 736
WIRE 448 736 368 736
WIRE 672 800 672 832
WIRE 624 640 624 720
WIRE 624 832 448 832
WIRE 672 720 624 720
WIRE 624 720 624 832
WIRE 256 832 -112 832
WIRE -112 832 -112 624
WIRE -112 624 -64 624
WIRE 544 640 576 640
WIRE 448 640 464 640
WIRE 576 640 624 640
WIRE 1088 384 1088 352
WIRE 1088 464 1088 448
WIRE 1088 544 1088 560
WIRE 1088 272 1088 256
WIRE 1120 416 1408 416
WIRE 1024
432 1056 432
WIRE 848 512 848 496
WIRE 848 416 848 400
WIRE 848 400 896 400
WIRE 1264 608 1232 608
WIRE 1232 608 1232 512
WIRE 1232 512 1280 512
WIRE 1344 608 1376 608
WIRE 1376 608 1376 512
WIRE 1376 512 1344 512
WIRE 1456 592 1456 608
WIRE 1408 416 1408 496
WIRE 1408 608 1376 608
WIRE 1408 496 1408 608
WIRE 1232 608 800 608
WIRE 800 608 800 400
WIRE 800 400 848 400
WIRE 992 400 1024 400
WIRE 896 400 912 400
WIRE 1024 400 1056 400
WIRE -128 176 -80 176
WIRE 1456 512 1456 496
WIRE 1456 496 1408 496
FLAG 416 64 0
FLAG 96 48 0
FLAG 96 336 0
FLAG 32 208 0
FLAG -80 320 0
FLAG 704 448 0
FLAG 112 464 0
FLAG 112 784 0
FLAG 48 656 0
FLAG -64 736 0
FLAG 672 832 0
FLAG 448 640 X
FLAG 576 640 Y
FLAG 1088 256 0
FLAG 1088 560 0
FLAG 1024 432 0
FLAG 848 512 0
FLAG 1456 608 0
FLAG 896 400 X2
FLAG 1024 400 Y2
SYMBOL voltage 96 160 M180
WINDOW 0 24 104 Left 0
WINDOW
3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 25
SYMBOL voltage 96 336 M180
WINDOW 0 24 89 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V2
SYMATTR Value 25
SYMBOL current 416 80 R0
WINDOW 38 39 48 Left 0
SYMATTR SpiceModel AC
SYMATTR InstName I1
SYMATTR Value 1
SYMBOL voltage 336 192 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName V3
SYMATTR Value 0
SYMBOL voltage 496 192 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 -32 56 VBottom 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V4
SYMATTR Value 0
SYMBOL res 688 320 R0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL res -96 192 R0
SYMATTR InstName R2
SYMATTR Value 1k
SYMBOL res 400 368 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R3
SYMATTR Value 1k
SYMBOL cap 384 272 R90
WINDOW 0
0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C1
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 96 128 R0
WINDOW 0 27 42 Left 0
WINDOW 3 25 87 Left 0
SYMATTR InstName U1
SYMBOL voltage 112 576 R180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V5
SYMATTR Value 25
SYMBOL voltage 112 784 M180
WINDOW 0 31 91 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V6
SYMATTR Value 25
SYMBOL res 656 704 R0
SYMATTR InstName R4
SYMATTR Value 100
SYMBOL res -80 624 R0
SYMATTR InstName R5
SYMATTR Value 1k
SYMBOL res 384 848 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R6
SYMATTR Value 1k
SYMBOL cap 368 752 M270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C2
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 112 576 R0
WINDOW 3 19 86 Left 0
SYMATTR
InstName U2
SYMBOL voltage 560 640 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
WINDOW 38 60 56 VTop 0
SYMATTR InstName V9
SYMATTR Value 1
SYMATTR SpiceModel AC
SYMBOL voltage 1088 368 M180
WINDOW 0 36 65 Left 0
WINDOW 3 31 25 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V10
SYMATTR Value 25
SYMBOL voltage 1088 560 M180
WINDOW 0 27 85 Left 0
WINDOW 3 26 20 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V11
SYMATTR Value 25
SYMBOL res 1440 496 R0
SYMATTR InstName R7
SYMATTR Value 100
SYMBOL res 832 400 R0
SYMATTR InstName R8
SYMATTR Value 1k
SYMBOL res 1360 624 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R9
SYMATTR Value 1k
SYMBOL cap 1344 528 M270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C3
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 1088 352 R0
WINDOW 0 19 37 Left 0
WINDOW 3
27 81 Left 0
SYMATTR InstName U3
SYMBOL voltage 1008 400 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
WINDOW 38 60 56 VTop 0
SYMATTR InstName V14
SYMATTR Value 1
SYMATTR SpiceModel AC
TEXT -90 902 Left 0 !.ac dec 30 1 1G
TEXT 224 600 Left 0 ;Gv=-V(x)/V(y)
TEXT 200 72 Left 0 ;Gi=I(V3)/I(V4)
TEXT -128 -184 Left 0 ;True loop:((I(V3)/I(V4))*(-V(x)/V(y))-1)/((I(V3)/I(V4))+(-V(x)/V(y))+2)
TEXT 848 208 Left 0 ;Approximated by Voltage Gain:? -V(x2)/V(y2)
TEXT 0 -128 Left 0 ;Or plot middlebrook(-V(x)/V(y),I(V3)/I(V4))
TEXT 0 -104 Left 0 ;After you add the line
TEXT 0 -80 Left 0 ;.func middlebrook(x,y) = (x*y-1)/(x+y+2)
TEXT 0 -56 Left 0 ;to your plot.defs file
__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!
To unsubscribe from this group, send an email to:
LTspice-unsubscribe@...
Your use of Yahoo! Groups is subject to the .
Do you Yahoo!?
- Now only $29.95 per month!
|
Re: Open Loop response for OpAmp And New User-Defined Functions for Plotting Released today.
Analog, I've added user-defined functions to LTspice. From a waveform
window execute Plot Settings=>Edit Plot Defs File to create and
edit the file. You might want to enter the line
.func middlebrook(x,y) = (x*y-1)/(x+y+2)
Then you can more easily plot the exact loop gain from a closed
loop system. Mike, this is way cool! But I couldn't get the following lines
added to Plot Defs File to work:
* For a node driven by 1 amp ac (.ac analysis only):
.func Ls(x) = im( x )/w ; equivalent series inductance
.func Rs(x) = re( x ) ; equivalent series resistance
.func Cp(x) = im(1/x)/w ; equivalent parallel capacitance
.func Rp(x) = re(1/x) ; equivalent parallel resistance
LTspice seems to reject the use of the built-in functions, "im" and
"re" in a user-defined function. Whatsup?
The new code was forgetting to strip the comments before compiling the functions. Either remove the comments or update to version 2.03y availible now. Thank you very much for the report. --Mike __________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month!
|
Re: Open Loop response for OpAmp And New User-Defined Functions for Plotting Released today.
Pat,
?
I believe it is corrrect. The original version I saw did not have the negative sign before the -V(x)/V(y) term. It depends on the polarity the injected voltage and the directions of the injected currents. LTSPice and other SPICE simulators pick the dirrection of the current through some standard conventions. So depending on how you insert the current sources there can be variations in the way the equation looks due to the simulator's interpretation of the sense (direction) of the currents.
?
I haven't actually found the derivation of the equation so I?derived it myself. It might be in a book that Middlebrook wrote. ?As?I originally saw it written,?it is of the form:
?
?? Loop Gain = (GvGi - 1)/(Gv + Gi - 2)
?
If you're interested you can search for references to Dr. Middlebrook's work. There is also some information at the ISPICE website.
?
If you're?a reasonable mathematician?you can take a perfect?amplifier with some fixed gain G, insert an output impedance Zout in series with the output of the amplifier, Insert an input impedance Zin in parallel with the input of the amplifier, and insert the voltage and current sources between the two as shown in the schematic.
?
Remembering that loop gain is G(Zin/(Zin+Zout)), you can proceed to solve the system of equations by first setting the injected voltage to zero and the injected current to one, and then setting the injected voltage to one and the injected current to zero.
?
If you do that you?should be able to?derive the equation that started this discussion.
?
It's pretty good stuff because it will solve the problem without worrying much about the impedances at the point you place the injection sources. If you get enthusiastic enough you might create a subcircuit which does the injection and calculates loop gain! It's recently helped with a few real designs for me and it seems
to??????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????
;??????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????&
nbsp;?????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????&nb
sp;??????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????
;??????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????????&
nbsp;???????????????????????????????????????????????????????????????????????????????????????????????????
?
If you really get stuck, I can find my calculations and either scan them or type them in.
?
Steve
Pat Lawler wrote:
The posted schematic has the statement:
True loop:
((I(V3)/I(V4))*(-V(x)/V(y))-1)/((I(V3)/I(V4))+(-V(x)/V(y))+2)
The formula uses signals from two different control loops to calculate
true loop gain (i(v3) & i(v4), versus v(x) & v(y)).
Is this correct?
On Tue, 15 Jul 2003 13:20:02 -0700 (PDT), Panama Mike
wrote:
>I've added user-defined functions to LTspice.? From a waveform window execute
>Plot Settings=>Edit Plot Defs File to create and edit the file.? You might want
>to enter the line
>
>.func middlebrook(x,y) = (x*y-1)/(x+y+2)
>
>Then you can more easily plot the exact loop gain from a closed loop system.? Below is your
>circuit showing the exact loop gain and the approximated by just the voltage gain.
>
>Version
4
>SHEET 1 2168 1300
>WIRE 416 64 416 80
>WIRE 320 192 416 192
>WIRE 416 160 416 192
>WIRE 416 192 512 192
>WIRE 96 160 96 144
>WIRE 96 240 96 224
>WIRE 96 320 96 336
>WIRE 96 64 96 48
>WIRE 128 192 240 192
>WIRE 32 208 64 208
>WIRE -80 320 -80 288
>WIRE -80 208 -80 176
>WIRE -80 176 64 176
>WIRE 304 384 272 384
>WIRE 272 384 272 288
>WIRE 272 288 320 288
>WIRE 384 384 464 384
>WIRE 464 384 464 288
>WIRE 464 288 384 288
>WIRE 704 416 704 448
>WIRE 592 192 656 192
>WIRE 656 192 656 336
>WIRE 656 384 464 384
>WIRE 704 336 656 336
>WIRE 656 336 656 384
>WIRE 272 384 -128 384
>WIRE -128 384 -128 176
>WIRE 112 608 112 560
>WIRE 112 688 112 672
>WIRE 112 768 112 784
>WIRE 112 480 112 464
>WIRE 144 640 448 640
>WIRE 48 656 80 656
>WIRE -64 736 -64 720
>WIRE -64 640 -64
624
>WIRE -64 624 80 624
>WIRE 288 832 256 832
>WIRE 256 832 256 736
>WIRE 256 736 304 736
>WIRE 368 832 448 832
>WIRE 448 832 448 736
>WIRE 448 736 368 736
>WIRE 672 800 672 832
>WIRE 624 640 624 720
>WIRE 624 832 448 832
>WIRE 672 720 624 720
>WIRE 624 720 624 832
>WIRE 256 832 -112 832
>WIRE -112 832 -112 624
>WIRE -112 624 -64 624
>WIRE 544 640 576 640
>WIRE 448 640 464 640
>WIRE 576 640 624 640
>WIRE 1088 384 1088 352
>WIRE 1088 464 1088 448
>WIRE 1088 544 1088 560
>WIRE 1088 272 1088 256
>WIRE 1120 416 1408 416
>WIRE 1024 432 1056 432
>WIRE 848 512 848 496
>WIRE 848 416 848 400
>WIRE 848 400 896 400
>WIRE 1264 608 1232 608
>WIRE 1232 608 1232 512
>WIRE 1232 512 1280 512
>WIRE 1344 608 1376 608
>WIRE 1376 608 1376 512
>WIRE 1376 512 1344 512
>WIRE 1456 592 1456 608
>WIRE
1408 416 1408 496
>WIRE 1408 608 1376 608
>WIRE 1408 496 1408 608
>WIRE 1232 608 800 608
>WIRE 800 608 800 400
>WIRE 800 400 848 400
>WIRE 992 400 1024 400
>WIRE 896 400 912 400
>WIRE 1024 400 1056 400
>WIRE -128 176 -80 176
>WIRE 1456 512 1456 496
>WIRE 1456 496 1408 496
>FLAG 416 64 0
>FLAG 96 48 0
>FLAG 96 336 0
>FLAG 32 208 0
>FLAG -80 320 0
>FLAG 704 448 0
>FLAG 112 464 0
>FLAG 112 784 0
>FLAG 48 656 0
>FLAG -64 736 0
>FLAG 672 832 0
>FLAG 448 640 X
>FLAG 576 640 Y
>FLAG 1088 256 0
>FLAG 1088 560 0
>FLAG 1024 432 0
>FLAG 848 512 0
>FLAG 1456 608 0
>FLAG 896 400 X2
>FLAG 1024 400 Y2
>SYMBOL voltage 96 160 M180
>WINDOW 0 24 104 Left 0
>WINDOW 3 24 16 Left 0
>WINDOW 123 0 0 Left 0
>WINDOW 39 0 0 Left 0
>SYMATTR InstName V1
>SYMATTR Value 25
>SYMBOL
voltage 96 336 M180
>WINDOW 0 24 89 Left 0
>WINDOW 3 24 16 Left 0
>WINDOW 123 0 0 Left 0
>WINDOW 39 0 0 Left 0
>SYMATTR InstName V2
>SYMATTR Value 25
>SYMBOL current 416 80 R0
>WINDOW 38 39 48 Left 0
>SYMATTR SpiceModel AC
>SYMATTR InstName I1
>SYMATTR Value 1
>SYMBOL voltage 336 192 R90
>WINDOW 0 -32 56 VBottom 0
>WINDOW 3 32 56 VTop 0
>SYMATTR InstName V3
>SYMATTR Value 0
>SYMBOL voltage 496 192 R270
>WINDOW 0 32 56 VTop 0
>WINDOW 3 -32 56 VBottom 0
>WINDOW 123 0 0 Left 0
>WINDOW 39 0 0 Left 0
>SYMATTR InstName V4
>SYMATTR Value 0
>SYMBOL res 688 320 R0
>SYMATTR InstName R1
>SYMATTR Value 100
>SYMBOL res -96 192 R0
>SYMATTR InstName R2
>SYMATTR Value 1k
>SYMBOL res 400 368 R90
>WINDOW 0 0 56 VBottom 0
>WINDOW 3 32 56 VTop 0
>SYMATTR InstName R3
>SYMATTR Value 1k
>SYMBOL cap
384 272 R90
>WINDOW 0 0 32 VBottom 0
>WINDOW 3 32 32 VTop 0
>SYMATTR InstName C1
>SYMATTR Value 3p
>SYMBOL Opamps\\LT1001 96 128 R0
>WINDOW 0 27 42 Left 0
>WINDOW 3 25 87 Left 0
>SYMATTR InstName U1
>SYMBOL voltage 112 576 R180
>WINDOW 0 24 104 Left 0
>WINDOW 3 24 16 Left 0
>WINDOW 123 0 0 Left 0
>WINDOW 39 0 0 Left 0
>SYMATTR InstName V5
>SYMATTR Value 25
>SYMBOL voltage 112 784 M180
>WINDOW 0 31 91 Left 0
>WINDOW 3 24 16 Left 0
>WINDOW 123 0 0 Left 0
>WINDOW 39 0 0 Left 0
>SYMATTR InstName V6
>SYMATTR Value 25
>SYMBOL res 656 704 R0
>SYMATTR InstName R4
>SYMATTR Value 100
>SYMBOL res -80 624 R0
>SYMATTR InstName R5
>SYMATTR Value 1k
>SYMBOL res 384 848 M270
>WINDOW 0 32 56 VTop 0
>WINDOW 3 0 56 VBottom 0
>SYMATTR InstName R6
>SYMATTR Value 1k
>SYMBOL cap 368 752 M270
>WINDOW
0 32 32 VTop 0
>WINDOW 3 0 32 VBottom 0
>SYMATTR InstName C2
>SYMATTR Value 3p
>SYMBOL Opamps\\LT1001 112 576 R0
>WINDOW 3 19 86 Left 0
>SYMATTR InstName U2
>SYMBOL voltage 560 640 R90
>WINDOW 0 -32 56 VBottom 0
>WINDOW 3 32 56 VTop 0
>WINDOW 38 60 56 VTop 0
>SYMATTR InstName V9
>SYMATTR Value 1
>SYMATTR SpiceModel AC
>SYMBOL voltage 1088 368 M180
>WINDOW 0 36 65 Left 0
>WINDOW 3 31 25 Left 0
>WINDOW 123 0 0 Left 0
>WINDOW 39 0 0 Left 0
>SYMATTR InstName V10
>SYMATTR Value 25
>SYMBOL voltage 1088 560 M180
>WINDOW 0 27 85 Left 0
>WINDOW 3 26 20 Left 0
>WINDOW 123 0 0 Left 0
>WINDOW 39 0 0 Left 0
>SYMATTR InstName V11
>SYMATTR Value 25
>SYMBOL res 1440 496 R0
>SYMATTR InstName R7
>SYMATTR Value 100
>SYMBOL res 832 400 R0
>SYMATTR InstName R8
>SYMATTR Value 1k
>SYMBOL res 1360 624
M270
>WINDOW 0 32 56 VTop 0
>WINDOW 3 0 56 VBottom 0
>SYMATTR InstName R9
>SYMATTR Value 1k
>SYMBOL cap 1344 528 M270
>WINDOW 0 32 32 VTop 0
>WINDOW 3 0 32 VBottom 0
>SYMATTR InstName C3
>SYMATTR Value 3p
>SYMBOL Opamps\\LT1001 1088 352 R0
>WINDOW 0 19 37 Left 0
>WINDOW 3 27 81 Left 0
>SYMATTR InstName U3
>SYMBOL voltage 1008 400 R90
>WINDOW 0 -32 56 VBottom 0
>WINDOW 3 32 56 VTop 0
>WINDOW 38 60 56 VTop 0
>SYMATTR InstName V14
>SYMATTR Value 1
>SYMATTR SpiceModel AC
>TEXT -90 902 Left 0 !.ac dec 30 1 1G
>TEXT 224 600 Left 0 ;Gv=-V(x)/V(y)
>TEXT 200 72 Left 0 ;Gi=I(V3)/I(V4)
>TEXT -128 -184 Left 0 ;True loop:((I(V3)/I(V4))*(-V(x)/V(y))-1)/((I(V3)/I(V4))+(-V(x)/V(y))+2)
>TEXT 848 208 Left 0 ;Approximated by Voltage Gain:? -V(x2)/V(y2)
>TEXT 0 -128 Left 0 ;Or plot middlebrook(-V(x)/V(y),I(V3)/I(V4))
>TEXT 0 -104 Left 0
;After you add the line
>TEXT 0 -80 Left 0 ;.func middlebrook(x,y) = (x*y-1)/(x+y+2)
>TEXT 0 -56 Left 0 ;to your plot.defs file
>
>
>__________________________________
>Do you Yahoo!?
>SBC Yahoo! DSL - Now only $29.95 per month!
>
>
>
>To unsubscribe from this group, send an email to:
>LTspice-unsubscribe@...
>
>
>
>Your use of Yahoo! Groups is subject to
>
To unsubscribe from this group, send an email to:
LTspice-unsubscribe@...
Your use of Yahoo! Groups is subject to the .
Do you Yahoo!?
- Now only $29.95 per month!
|
Re: Open Loop response for OpAmp And New User-Defined Functions for Plotting Released today.
Pat, The posted schematic has the statement:
True loop:
((I(V3)/I(V4))*(-V(x)/V(y))-1)/((I(V3)/I(V4))+(-V(x)/V(y))+2)
The formula uses signals from two different control loops to calculate
true loop gain (i(v3) & i(v4), versus v(x) & v(y)).
Is this correct? Yes, the openloop voltage gain measured from the closed loop system is -V(x)/V(y). The open loop current gain measured from the closed loop system is I(V3)/I(V4). The equation combines them to get the open loop system gain. The alternate method just plots the voltage gain from a different section of the schematic where it is a close approximation for the circuit in question. --Mike __________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month!
|
Re: Open Loop response for OpAmp And New User-Defined Functions for Plotting Released today.
The posted schematic has the statement: True loop: ((I(V3)/I(V4))*(-V(x)/V(y))-1)/((I(V3)/I(V4))+(-V(x)/V(y))+2) The formula uses signals from two different control loops to calculate true loop gain (i(v3) & i(v4), versus v(x) & v(y)). Is this correct? On Tue, 15 Jul 2003 13:20:02 -0700 (PDT), Panama Mike <panamatex@...> wrote: I've added user-defined functions to LTspice. From a waveform window execute
Plot Settings=>Edit Plot Defs File to create and edit the file. You might want
to enter the line
.func middlebrook(x,y) = (x*y-1)/(x+y+2)
Then you can more easily plot the exact loop gain from a closed loop system. Below is your
circuit showing the exact loop gain and the approximated by just the voltage gain.
Version 4
SHEET 1 2168 1300
WIRE 416 64 416 80
WIRE 320 192 416 192
WIRE 416 160 416 192
WIRE 416 192 512 192
WIRE 96 160 96 144
WIRE 96 240 96 224
WIRE 96 320 96 336
WIRE 96 64 96 48
WIRE 128 192 240 192
WIRE 32 208 64 208
WIRE -80 320 -80 288
WIRE -80 208 -80 176
WIRE -80 176 64 176
WIRE 304 384 272 384
WIRE 272 384 272 288
WIRE 272 288 320 288
WIRE 384 384 464 384
WIRE 464 384 464 288
WIRE 464 288 384 288
WIRE 704 416 704 448
WIRE 592 192 656 192
WIRE 656 192 656 336
WIRE 656 384 464 384
WIRE 704 336 656 336
WIRE 656 336 656 384
WIRE 272 384 -128 384
WIRE -128 384 -128 176
WIRE 112 608 112 560
WIRE 112 688 112 672
WIRE 112 768 112 784
WIRE 112 480 112 464
WIRE 144 640 448 640
WIRE 48 656 80 656
WIRE -64 736 -64 720
WIRE -64 640 -64 624
WIRE -64 624 80 624
WIRE 288 832 256 832
WIRE 256 832 256 736
WIRE 256 736 304 736
WIRE 368 832 448 832
WIRE 448 832 448 736
WIRE 448 736 368 736
WIRE 672 800 672 832
WIRE 624 640 624 720
WIRE 624 832 448 832
WIRE 672 720 624 720
WIRE 624 720 624 832
WIRE 256 832 -112 832
WIRE -112 832 -112 624
WIRE -112 624 -64 624
WIRE 544 640 576 640
WIRE 448 640 464 640
WIRE 576 640 624 640
WIRE 1088 384 1088 352
WIRE 1088 464 1088 448
WIRE 1088 544 1088 560
WIRE 1088 272 1088 256
WIRE 1120 416 1408 416
WIRE 1024 432 1056 432
WIRE 848 512 848 496
WIRE 848 416 848 400
WIRE 848 400 896 400
WIRE 1264 608 1232 608
WIRE 1232 608 1232 512
WIRE 1232 512 1280 512
WIRE 1344 608 1376 608
WIRE 1376 608 1376 512
WIRE 1376 512 1344 512
WIRE 1456 592 1456 608
WIRE 1408 416 1408 496
WIRE 1408 608 1376 608
WIRE 1408 496 1408 608
WIRE 1232 608 800 608
WIRE 800 608 800 400
WIRE 800 400 848 400
WIRE 992 400 1024 400
WIRE 896 400 912 400
WIRE 1024 400 1056 400
WIRE -128 176 -80 176
WIRE 1456 512 1456 496
WIRE 1456 496 1408 496
FLAG 416 64 0
FLAG 96 48 0
FLAG 96 336 0
FLAG 32 208 0
FLAG -80 320 0
FLAG 704 448 0
FLAG 112 464 0
FLAG 112 784 0
FLAG 48 656 0
FLAG -64 736 0
FLAG 672 832 0
FLAG 448 640 X
FLAG 576 640 Y
FLAG 1088 256 0
FLAG 1088 560 0
FLAG 1024 432 0
FLAG 848 512 0
FLAG 1456 608 0
FLAG 896 400 X2
FLAG 1024 400 Y2
SYMBOL voltage 96 160 M180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 25
SYMBOL voltage 96 336 M180
WINDOW 0 24 89 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V2
SYMATTR Value 25
SYMBOL current 416 80 R0
WINDOW 38 39 48 Left 0
SYMATTR SpiceModel AC
SYMATTR InstName I1
SYMATTR Value 1
SYMBOL voltage 336 192 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName V3
SYMATTR Value 0
SYMBOL voltage 496 192 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 -32 56 VBottom 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V4
SYMATTR Value 0
SYMBOL res 688 320 R0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL res -96 192 R0
SYMATTR InstName R2
SYMATTR Value 1k
SYMBOL res 400 368 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R3
SYMATTR Value 1k
SYMBOL cap 384 272 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C1
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 96 128 R0
WINDOW 0 27 42 Left 0
WINDOW 3 25 87 Left 0
SYMATTR InstName U1
SYMBOL voltage 112 576 R180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V5
SYMATTR Value 25
SYMBOL voltage 112 784 M180
WINDOW 0 31 91 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V6
SYMATTR Value 25
SYMBOL res 656 704 R0
SYMATTR InstName R4
SYMATTR Value 100
SYMBOL res -80 624 R0
SYMATTR InstName R5
SYMATTR Value 1k
SYMBOL res 384 848 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R6
SYMATTR Value 1k
SYMBOL cap 368 752 M270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C2
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 112 576 R0
WINDOW 3 19 86 Left 0
SYMATTR InstName U2
SYMBOL voltage 560 640 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
WINDOW 38 60 56 VTop 0
SYMATTR InstName V9
SYMATTR Value 1
SYMATTR SpiceModel AC
SYMBOL voltage 1088 368 M180
WINDOW 0 36 65 Left 0
WINDOW 3 31 25 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V10
SYMATTR Value 25
SYMBOL voltage 1088 560 M180
WINDOW 0 27 85 Left 0
WINDOW 3 26 20 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V11
SYMATTR Value 25
SYMBOL res 1440 496 R0
SYMATTR InstName R7
SYMATTR Value 100
SYMBOL res 832 400 R0
SYMATTR InstName R8
SYMATTR Value 1k
SYMBOL res 1360 624 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R9
SYMATTR Value 1k
SYMBOL cap 1344 528 M270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C3
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 1088 352 R0
WINDOW 0 19 37 Left 0
WINDOW 3 27 81 Left 0
SYMATTR InstName U3
SYMBOL voltage 1008 400 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
WINDOW 38 60 56 VTop 0
SYMATTR InstName V14
SYMATTR Value 1
SYMATTR SpiceModel AC
TEXT -90 902 Left 0 !.ac dec 30 1 1G
TEXT 224 600 Left 0 ;Gv=-V(x)/V(y)
TEXT 200 72 Left 0 ;Gi=I(V3)/I(V4)
TEXT -128 -184 Left 0 ;True loop:((I(V3)/I(V4))*(-V(x)/V(y))-1)/((I(V3)/I(V4))+(-V(x)/V(y))+2)
TEXT 848 208 Left 0 ;Approximated by Voltage Gain: -V(x2)/V(y2)
TEXT 0 -128 Left 0 ;Or plot middlebrook(-V(x)/V(y),I(V3)/I(V4))
TEXT 0 -104 Left 0 ;After you add the line
TEXT 0 -80 Left 0 ;.func middlebrook(x,y) = (x*y-1)/(x+y+2)
TEXT 0 -56 Left 0 ;to your plot.defs file
__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!
To unsubscribe from this group, send an email to:
LTspice-unsubscribe@...
Your use of Yahoo! Groups is subject to
|
Re: Open Loop response for OpAmp And New User-Defined Functions for Plotting Released today.
Panama Mike wrote: I've added user-defined functions to LTspice. From a waveform
window execute Plot Settings=>Edit Plot Defs File to create and
edit the file. You might want to enter the line
.func middlebrook(x,y) = (x*y-1)/(x+y+2)
Then you can more easily plot the exact loop gain from a closed
loop system. Mike, this is way cool! But I couldn't get the following lines added to Plot Defs File to work: * For a node driven by 1 amp ac (.ac analysis only): .func Ls(x) = im( x )/w ; equivalent series inductance .func Rs(x) = re( x ) ; equivalent series resistance .func Cp(x) = im(1/x)/w ; equivalent parallel capacitance .func Rp(x) = re(1/x) ; equivalent parallel resistance LTspice seems to reject the use of the built-in functions, "im" and "re" in a user-defined function. Whatsup? analog (spiceman - who couldn't resist playing in the switchyard)
|
Re: export simulated waveforms in ascii format
--- In LTspice@..., mathias.borcke@i... wrote: I got it: LtSpUtil.exe is the tool I need
Sorry for bothering you BEFORE searching!
Mathias
-----Ursprüngliche Nachricht-----
Von: Borcke Mathias (MP TI PT1 PRE4)
Gesendet: Dienstag, 15. Juli 2003 11:08
An: LTspice@...
Betreff: [LTspice] export simulated waveforms in ascii format
Hello *
is there a possibility to export data into some binary or ascii format? If not, Mike, can you add this to your code anytime in the future?
eg:
Xvalue1 Yvalue1
Xvalue2 Yvalue2
....
if there are several traces:
Xvalue1 Yvalue1(trace1) Yvalue1(trace2) .....
Xvalue2 Yvalue2(trace1) Yvalue2(trace2) .....
....
Hello Mathias, all you have requested is possible with the program LTSPUTIL.EXE. It is located in the Files->Util section of this news group. This program is command line driven and you should run it in a DOS- box. It reads any binary or ASCII xxxx.raw file and converts the values of the selected nodes(nets) to an ASCII-text file organized in table format. It has many options and thus you should read the help file first. Best Regards Helmut PS: I have written this program.
|
Re: Open Loop response for OpAmp And New User-Defined Functions for Plotting Released today.
Steve,
I've added user-defined functions to LTspice. From a waveform window execute
Plot Settings=>Edit Plot Defs File to create and edit the file. You might want
to enter the line
.func middlebrook(x,y) = (x*y-1)/(x+y+2)
Then you can more easily plot the exact loop gain from a closed loop system. Below is your
circuit showing the exact loop gain and the approximated by just the voltage gain.
Version 4
SHEET 1 2168 1300
WIRE 416 64 416 80
WIRE 320 192 416 192
WIRE 416 160 416 192
WIRE 416 192 512 192
WIRE 96 160 96 144
WIRE 96 240 96 224
WIRE 96 320 96 336
WIRE 96 64 96 48
WIRE 128 192 240 192
WIRE 32 208 64 208
WIRE -80 320 -80 288
WIRE -80 208 -80 176
WIRE -80 176 64 176
WIRE 304 384 272 384
WIRE 272 384 272 288
WIRE 272 288 320 288
WIRE 384 384 464 384
WIRE 464 384 464 288
WIRE 464 288 384 288
WIRE 704 416 704 448
WIRE 592 192 656 192
WIRE 656 192 656 336
WIRE 656 384 464 384
WIRE 704 336 656 336
WIRE 656 336 656 384
WIRE 272 384 -128 384
WIRE -128 384 -128 176
WIRE 112 608 112 560
WIRE 112 688 112 672
WIRE 112 768 112 784
WIRE 112 480 112 464
WIRE 144 640 448 640
WIRE 48 656 80 656
WIRE -64 736 -64 720
WIRE -64 640 -64 624
WIRE -64 624 80 624
WIRE 288 832 256 832
WIRE 256 832 256 736
WIRE 256 736 304 736
WIRE 368 832 448 832
WIRE 448 832 448 736
WIRE 448 736 368 736
WIRE 672 800 672 832
WIRE 624 640 624 720
WIRE 624 832 448 832
WIRE 672 720 624 720
WIRE 624 720 624 832
WIRE 256 832 -112 832
WIRE -112 832 -112 624
WIRE -112 624 -64 624
WIRE 544 640 576 640
WIRE 448 640 464 640
WIRE 576 640 624 640
WIRE 1088 384 1088 352
WIRE 1088 464 1088 448
WIRE 1088 544 1088 560
WIRE 1088 272 1088 256
WIRE 1120 416 1408 416
WIRE 1024 432 1056 432
WIRE 848 512 848 496
WIRE 848 416 848 400
WIRE 848 400 896 400
WIRE 1264 608 1232 608
WIRE 1232 608 1232 512
WIRE 1232 512 1280 512
WIRE 1344 608 1376 608
WIRE 1376 608 1376 512
WIRE 1376 512 1344 512
WIRE 1456 592 1456 608
WIRE 1408 416 1408 496
WIRE 1408 608 1376 608
WIRE 1408 496 1408 608
WIRE 1232 608 800 608
WIRE 800 608 800 400
WIRE 800 400 848 400
WIRE 992 400 1024 400
WIRE 896 400 912 400
WIRE 1024 400 1056 400
WIRE -128 176 -80 176
WIRE 1456 512 1456 496
WIRE 1456 496 1408 496
FLAG 416 64 0
FLAG 96 48 0
FLAG 96 336 0
FLAG 32 208 0
FLAG -80 320 0
FLAG 704 448 0
FLAG 112 464 0
FLAG 112 784 0
FLAG 48 656 0
FLAG -64 736 0
FLAG 672 832 0
FLAG 448 640 X
FLAG 576 640 Y
FLAG 1088 256 0
FLAG 1088 560 0
FLAG 1024 432 0
FLAG 848 512 0
FLAG 1456 608 0
FLAG 896 400 X2
FLAG 1024 400 Y2
SYMBOL voltage 96 160 M180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 25
SYMBOL voltage 96 336 M180
WINDOW 0 24 89 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V2
SYMATTR Value 25
SYMBOL current 416 80 R0
WINDOW 38 39 48 Left 0
SYMATTR SpiceModel AC
SYMATTR InstName I1
SYMATTR Value 1
SYMBOL voltage 336 192 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName V3
SYMATTR Value 0
SYMBOL voltage 496 192 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 -32 56 VBottom 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V4
SYMATTR Value 0
SYMBOL res 688 320 R0
SYMATTR InstName R1
SYMATTR Value 100
SYMBOL res -96 192 R0
SYMATTR InstName R2
SYMATTR Value 1k
SYMBOL res 400 368 R90
WINDOW 0 0 56 VBottom 0
WINDOW 3 32 56 VTop 0
SYMATTR InstName R3
SYMATTR Value 1k
SYMBOL cap 384 272 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName C1
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 96 128 R0
WINDOW 0 27 42 Left 0
WINDOW 3 25 87 Left 0
SYMATTR InstName U1
SYMBOL voltage 112 576 R180
WINDOW 0 24 104 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V5
SYMATTR Value 25
SYMBOL voltage 112 784 M180
WINDOW 0 31 91 Left 0
WINDOW 3 24 16 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V6
SYMATTR Value 25
SYMBOL res 656 704 R0
SYMATTR InstName R4
SYMATTR Value 100
SYMBOL res -80 624 R0
SYMATTR InstName R5
SYMATTR Value 1k
SYMBOL res 384 848 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R6
SYMATTR Value 1k
SYMBOL cap 368 752 M270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C2
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 112 576 R0
WINDOW 3 19 86 Left 0
SYMATTR InstName U2
SYMBOL voltage 560 640 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
WINDOW 38 60 56 VTop 0
SYMATTR InstName V9
SYMATTR Value 1
SYMATTR SpiceModel AC
SYMBOL voltage 1088 368 M180
WINDOW 0 36 65 Left 0
WINDOW 3 31 25 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V10
SYMATTR Value 25
SYMBOL voltage 1088 560 M180
WINDOW 0 27 85 Left 0
WINDOW 3 26 20 Left 0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V11
SYMATTR Value 25
SYMBOL res 1440 496 R0
SYMATTR InstName R7
SYMATTR Value 100
SYMBOL res 832 400 R0
SYMATTR InstName R8
SYMATTR Value 1k
SYMBOL res 1360 624 M270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R9
SYMATTR Value 1k
SYMBOL cap 1344 528 M270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C3
SYMATTR Value 3p
SYMBOL Opamps\\LT1001 1088 352 R0
WINDOW 0 19 37 Left 0
WINDOW 3 27 81 Left 0
SYMATTR InstName U3
SYMBOL voltage 1008 400 R90
WINDOW 0 -32 56 VBottom 0
WINDOW 3 32 56 VTop 0
WINDOW 38 60 56 VTop 0
SYMATTR InstName V14
SYMATTR Value 1
SYMATTR SpiceModel AC
TEXT -90 902 Left 0 !.ac dec 30 1 1G
TEXT 224 600 Left 0 ;Gv=-V(x)/V(y)
TEXT 200 72 Left 0 ;Gi=I(V3)/I(V4)
TEXT -128 -184 Left 0 ;True loop:((I(V3)/I(V4))*(-V(x)/V(y))-1)/((I(V3)/I(V4))+(-V(x)/V(y))+2)
TEXT 848 208 Left 0 ;Approximated by Voltage Gain: -V(x2)/V(y2)
TEXT 0 -128 Left 0 ;Or plot middlebrook(-V(x)/V(y),I(V3)/I(V4))
TEXT 0 -104 Left 0 ;After you add the line
TEXT 0 -80 Left 0 ;.func middlebrook(x,y) = (x*y-1)/(x+y+2)
TEXT 0 -56 Left 0 ;to your plot.defs file
__________________________________
Do you Yahoo!?
SBC Yahoo! DSL - Now only $29.95 per month!
|
Re: Malfunction of restoring plot settings
Mathias, a) Storing/restoring of plot settings works for the x-axis but for the
y-axis it does not restore (open Plot settings file) these settings. It's supposed to always work for the vertical axis(except as you note for log scales), but it might not work for the horizontal axis because the simulation range might have changed. b) when using log scale for the y-axis the and you type in e.g:
Top 1.0V
Tick 100mV
Bottom 0.1V
check the logarithmic button and click "OK" then some 0.1fV are taken as
bottom value
left-clicking the axis another time and removing the "f" in front of the
Volt allows you to have the desired scaling The .1fV comes from the fact that there's zero or negative data in your expression and when changing to/from log an autoscale needed to be performed to set some internal data. However, I now changed the UI so that both limits and log vs. linear can be input by the user at the same time. c) when having a log-scale on the y-axis: save plot settings;
when opening this plot settings file a syntax error is reported Thank you very much for the bug report. Fixed in version 2.03w available from the web now along with the modification mentioned in (b) --Mike __________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month!
|
Malfunction of restoring plot settings
a) Storing/restoring of plot settings works for the x-axis but for the
y-axis it does not restore (open Plot settings file) these settings.
b) when using log scale for the y-axis the and you type in e.g:
Top 1.0V
Tick 100mV
Bottom 0.1V
check the logarithmic button and click "OK" then some 0.1fV are taken as
bottom value
left-clicking the axis another time and removing the "f" in front of the
"V"olt allows you to have the desired scaling
c) when having a log-scale on the y-axis: save plot settings;
when opening this plot settings file a syntax error is reported
Regards and Thanks in advance
Mathias
|
Re: auto scale after simulation / "Autoranging" checkbutton / plot se ttings file
Normally LTspice autoranges whenever you add or remove traces. You can toggle this on or off with the waveform window menu command Plot Settings=>Autoranging. If you want exactly the same plot settings between simulations, you have to use Plot Settings=>Save Plot Settings/Plot Settings=>Open Plot Settings File. --Mike --- mathias.borcke@... wrote: This auto scale sometimes bothers me if I want to compare a simulation with
one with slightly different parameters or component values.
--> Is it possible to add a checkbutton to make this selectable?
Is it possible to store/restore the y-plot range information in the Plot
Settings file (for the x-axis it works, but for the y-axis it does not
restore these settings)
Btw. the "Autoranging" checkbutton (right mouseclick in the plot area) ;
-what does it exactly do?
Thanks
Mathias
-----Ursprngliche Nachricht-----
Von: Panama Mike [mailto:panamatex@...]
Gesendet: Freitag, 11. Juli 2003 17:04
An: LTspice@...
Betreff: Re: [LTspice] Weird behaviour for ylog scale
An auto scale is performed after every simulation.
It has nothing to do with the log display. You can
save and load your plot settings by making the
waveform window the active window and using the
menu commands Plot Settings=>Save Plot Settings/
Open Plot Settings File
--Mike
--- warning@... wrote:
Hello - first time in this forum,
a small misbehaviour I have found in using the logscale for e.g. a dc
sweep of a diode:
Everytime we have made a new simulation we must adjust the lower
bound of the yaxis in log scale. It goes to the default 1e-25, also
if I gave 1e-12 before.
Thanks for the great program
Dietmar
__________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month!
|
Re: export simulated waveforms in ascii format
I got
it: LtSpUtil.exe is the tool I need
?
Sorry
for bothering you?BEFORE searching!
?
Mathias
toggle quoted message
Show quoted text
Hello *
is there a
possibility to export data into some binary or ascii format?
If not, Mike,
can you add this to your code anytime in the
future?
eg:
Xvalue1?????
Yvalue1
Xvalue2????? Yvalue2
....
if
there are several traces:
Xvalue1?????
Yvalue1(trace1)????? Yvalue1(trace2)
.....
Xvalue2?????
Yvalue2(trace1)????? Yvalue2(trace2)
.....
....
Regards
Mathias
To
unsubscribe from this group, send an email
to:
LTspice-unsubscribe@...
Your use of
Yahoo! Groups is subject to the .
|
auto scale after simulation / "Autoranging" checkbutton / plot se ttings file
This
auto scale sometimes bothers me if I want to compare a simulation with one with
slightly different parameters or component values.
-->
Is it possible to add a checkbutton to make this selectable?
?
Is it
possible to store/restore the y-plot range information in the Plot Settings file
(for the x-axis it works, but for the y-axis it does not restore these
settings)
?
Btw.
the "Autoranging" checkbutton (right mouseclick in the plot area) ; -what does
it exactly do?
?
Thanks
Mathias
toggle quoted message
Show quoted text
An auto scale is
performed after every simulation.
It has nothing to do with the log
display.? You can
save and load your plot settings by making
the
waveform window the active window and using the
menu commands Plot
Settings=>Save Plot Settings/
Open Plot Settings
File
--Mike
--- warning@... wrote:
> Hello - first
time in this forum,
>
> a small misbehaviour I have found in
using the logscale for e.g. a dc
> sweep of a diode:
> Everytime
we have made a new simulation we must adjust the lower
> bound of the
yaxis in log scale. It goes to the default 1e-25, also
> if I gave
1e-12 before.
>
> Thanks for the great program
>
Dietmar
|
export simulated waveforms in ascii format
Hello *
is there a possibility to export data into some binary or ascii format?
If not, Mike, can you add this to your code anytime in the future?
eg:
Xvalue1 Yvalue1
Xvalue2 Yvalue2
....
if there are several traces:
Xvalue1 Yvalue1(trace1) Yvalue1(trace2) .....
Xvalue2 Yvalue2(trace1) Yvalue2(trace2) .....
....
Regards
Mathias
|
Meet that special one outside your race
A nice dating site for singles from different races to gather, love
is in the air!
|
Attention: many new models now available in the files area ...
... with more uploads coming soon.
|
Re: Weird behaviour for ylog scale
An auto scale is performed after every simulation. It has nothing to do with the log display. You can save and load your plot settings by making the waveform window the active window and using the menu commands Plot Settings=>Save Plot Settings/ Open Plot Settings File --Mike --- warning@... wrote: Hello - first time in this forum,
a small misbehaviour I have found in using the logscale for e.g. a dc
sweep of a diode:
Everytime we have made a new simulation we must adjust the lower
bound of the yaxis in log scale. It goes to the default 1e-25, also
if I gave 1e-12 before.
Thanks for the great program
Dietmar
------------------------
Dr.-Ing. Dietmar Warning
DAnalyse GmbH
Schkopauer Ring 5
12681 Berlin
Germany
Tel.: 030 93498 230
Fax.: 030 93498 231
email: warning at danalyse dot de
URL:
__________________________________ Do you Yahoo!? SBC Yahoo! DSL - Now only $29.95 per month!
|
Mike Engelhardt