search

KiCad / kicad-symbols

Official KiCad schematic symbol libraries for Kicad 5
https://kicad.github.io/symbols
Other
700 stars 747 forks source link

Spice #418

Open arildj78 opened 6 years ago

arildj78 commented 6 years ago

I\m trying to get started with KiCad and Spice, but it I can't seem to find any parts with spice-models loaded. Right-clicking a part->opening properties->Edit Spice Model seems to be empty on all parts that I'm checking... Are there special libraries for spice or am I looking in the wrong place?

diggit commented 6 years ago

I guess it is because of model licensing being incompatible with KiCad repositories.

evanshultz commented 6 years ago

@arildj78 There is a library named pspice but it's marked as legacy. Did you check that library?

Right now, I honestly don't know. Let me take a look at this soon (hopefully with 24 hours). I haven't tried simulation yet in KiCad and at least one of the librarians should be well-versed in it. I am very familiar with circuit simulation from other tools so let me see if I can help.

evanshultz commented 6 years ago

I figured I should start with Wayne's video at https://fosdem.org/2018/schedule/event/cad_kicad_v5/, since it publicly showed this off recently. Start at around 9:30. He references a video by Tom and Orson, which I believe is at https://www.youtube.com/watch?v=A2_-hdRcf4U.

I do not, at this point, believe any parts in the library have really been intended for circuit simulation. I could be wrong.

SPICE directives placed on the schematic page work OK. I can transform a resistor or other 2-terminal symbol into a seemingly functional V or I source. And simple parts seem to work fine using the R, L, and C primitives. But I currently haven't figured out how to get a diode or other more complex primitive to work. I can load in an external library file and it is parsed correctly, but the model isn't being attached. Only after that would I tackle subcircuits.

Are you also able to work with the normal SPICE primitives like R, L, C and sources? Those seem easiest to get going.

I'll try to figure out more tomorrow. There seem to be a number of analogs to LTSpice in the way things work in general, but I need to figure out the details. I feel pretty confident creating a nicer library of SPICE parts will be a longer-term objective that won't be ready for KiCad v5.

evanshultz commented 6 years ago

Have you looked at the demo circuits at <KiCad install path>\share\kicad\demos? In this directory on Windows I find 4 simulations that work.

They are using symbols not in the official library that appear to be for SPICE primitives. I'll dig into this more soon. Perhaps it's as easy as adding more SPICE-specific symbols and then there's enough simulation bits available out-of-the-box to get started with simulation.

Once again, thanks for bringing this issue up!

arildj78 commented 6 years ago

I've started to figure this out by now but it wasn't intuitive. I was hoping to see the SPICE directives when browsing the SPICE MODEL and did not realize that changing between the different tabs also changed the behavior. Often this kind of behavior is controlled by radiobuttons and not by tab selection.

arildj78 commented 6 years ago

I just realized that part of the problem was me choosing operating point as the simulation mode. I'm now able to run a successful transient analysis on a simple resistor puzzle, but when I'm changing to operating point i get this:

Circuit: KiCad schematic
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
 Reference value :  0.00000e+000
No. of Data Rows : 1
Background thread stopped with timeout = 0
Error: no such vector 2
Error: no such vector 1
Error: no such vector 3
evanshultz commented 6 years ago

Ah. Yes. Can you attach your schematic? Let me look into it?

BTW, can you run the 3 simulations in the <KiCad install path>\share\kicad\demos\simulation as I mentioned above?

arildj78 commented 6 years ago

SpiceTest.zip image image

List of issues

arildj78 commented 6 years ago

I think I have solved the problem with D1. After rotating it 180 degrees it seems to work with both the supplied .lib file and with model data supplied from a comment in the schematics. From this I'm guessing that the symbol I chose had the pin assignment backwards.

1N4007.REV0.LIB.txt

arildj78 commented 6 years ago

BTW, can you run the 3 simulations in the \share\kicad\demos\simulation as I mentioned above?

Yes I can. I tested the following projects with the simulation modes .tran, .ac and .op

pspice        C:\Program Files\KiCad\share\kicad\demos\pspice\pspice.pro
laser_driver  C:\Program Files\KiCad\share\kicad\demos\simulation\laser_driver\laser_driver.pro
rectifier     C:\Program Files\KiCad\share\kicad\demos\simulation\rectifier\rectifier.pro
sallen_key    C:\Program Files\KiCad\share\kicad\demos\simulation\sallen_key\sallen_key.pro

Here are the text output and my comments

pspice

.tran 1u 10m

Circuit: KiCad schematic
Background thread stopped with timeout = 0
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
Initial Transient Solution
(...)

The simulation works flawlessly

.ac dec 100 10 1Meg

Circuit: KiCad schematic
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
 Reference value :  1.00000e+001
No. of Data Rows : 501

The simulation works flawlessly

.op

Circuit: KiCad schematic
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
 Reference value :  0.00000e+000
No. of Data Rows : 1
Background thread stopped with timeout = 0
-Error: no such vector 3
-Error: no such vector 6
-Error: no such vector 9
-Error: no such vector 5
-Error: no such vector 8
-Error: no such vector 4
-Error: no such vector 2
-Error: no such vector 13
-Error: no such vector 7
-Error: no such vector 12
-Error: no such vector 11
-Error: no such vector 10
-Error: no such vector 1

The simulation does not give any data

laser_driver

.tran 10p 150n

Circuit: KiCad schematic
-Warning: Model issue on line 1 :
.model laser d(is=1e-22 rs=6 n=1.5 cjo=50p xti=100 iave=160m vpk=5) ...
-unrecognized parameter (iave) - ignored
-unrecognized parameter (vpk) - ignored
Reducing trtol to 1 for xspice 'A' devices
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
-Warning: vv1: no DC value, transient time 0 value used
Initial Transient Solution
(...)

The simulation works but it is apparently using a default diode instead of the laserdiode and it seems as if there is missing a DC value but I can't see the effect of this on the result.

.ac dec 100 10 1Meg

Not applicable for this circuit

.op

Circuit: KiCad schematic
-Warning: Model issue on line 1 :
.model laser d(is=1e-22 rs=6 n=1.5 cjo=50p xti=100 iave=160m vpk=5) ...
-unrecognized parameter (iave) - ignored
-unrecognized parameter (vpk) - ignored
Reducing trtol to 1 for xspice 'A' devices
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
-Warning: vv1: no DC value, transient time 0 value used
 Reference value :  0.00000e+000
No. of Data Rows : 1
Background thread stopped with timeout = 0
-Error: no such vector 1
-Error: no such vector 7
-Error: no such vector 3
-Error: no such vector 8
-Error: no such vector 6
-Error: no such vector 2
-Error: no such vector 4
-Error: no such vector 5

The simulation does not give any data

rectifier

.tran 1u 10m

Circuit: KiCad schematic
-Error on line 5 :
-dd1 net-_d1-pad2_ /rect_out 1n4148
-Unable to find definition of model 1n4148 - default assumed 
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
-Warning: vv1: no DC value, transient time 0 value used
Initial Transient Solution
(...)

The simulation works but it is apparently using a default diode instead of the 1n4148 and it seems as if there is missing a DC value but I can't see the effect of this on the result.

.ac dec 10 1 1Meg

Circuit: KiCad schematic
-Error on line 5 :
-dd1 net-_d1-pad2_ /rect_out 1n4148
-Unable to find definition of model 1n4148 - default assumed 
Background thread stopped with timeout = 0
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
-Warning: vv1: no DC value, transient time 0 value used
 Reference value :  1.00000e+000
No. of Data Rows : 61

The simulation works but it is apparently using a default diode instead of the 1n4148 and it seems as if there is missing a DC value but I can't see the effect of this on the result. To get meaningful data from the .ac simulation I had to change the V1 value from SINE(0 1.5 1k 0 0 0 0) to AC 1.5 SINE(0 1.5 1k 0 0 0 0)

.op

Circuit: KiCad schematic
-Error on line 5 :
-dd1 net-_d1-pad2_ /rect_out 1n4148
-Unable to find definition of model 1n4148 - default assumed 
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
-Warning: vv1: no DC value, transient time 0 value used
 Reference value :  0.00000e+000
No. of Data Rows : 1
Background thread stopped with timeout = 0
-Error: no such vector 3
-Error: no such vector 1
-Error: no such vector 2

The simulation does not give any data

sallen_key

.tran 1u 10m

Circuit: KiCad schematic
Background thread stopped with timeout = 0
Reducing trtol to 1 for xspice 'A' devices
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
-Warning: vv1: has no value, DC 0 assumed
Initial Transient Solution
(...)

The simulation works but it seems as if there is missing a DC value but I can't see the effect of this on the result. To get meaningful data from the .tran simulation I had to change V1 value from AC 1 to AC 1 SIN(0 1 1k)

.ac dec 10 1 1Meg

Circuit: KiCad schematic
Reducing trtol to 1 for xspice 'A' devices
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
-Warning: vv1: has no value, DC 0 assumed
 Reference value :  1.00000e+000
No. of Data Rows : 61

The simulation works but it seems as if there is missing a DC value but I can't see the effect of this on the result.

.op

Circuit: KiCad schematic
Background thread stopped with timeout = 0
Reducing trtol to 1 for xspice 'A' devices
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000
Warning: vv1: has no value, DC 0 assumed
 Reference value :  0.00000e+000
No. of Data Rows : 1
Background thread stopped with timeout = 0
-Error: no such vector 3
-Error: no such vector 6
-Error: no such vector 2
-Error: no such vector 1
-Error: no such vector 4
-Error: no such vector 5

The simulation does not give any data

Comment on the editing of Symbol Properties

It seems as if i can enter a SPICE source in the components Value field such as AC 1 SIN(0 3 1k). If I then press Edit Spice Model I can further change my values but when I press OK, the values are stored in a new field named Spice_Model. The symbol now has two fields showing data for the SPICE source, both the Value field and the Spice_Model but only the latter has effect on the simulation. If the Spice_Model field gets deleted, the Value field once again takes effect. This behaviour is confusing especially for unexperienced users such as myself.

evanshultz commented 6 years ago

@arildj78 Can you give me an update how this is going? Have you figured out more since the comment above? I've been able to spend some time on SPICE simulation the last couple days and I'd like to help ferret out issues and be able to provide better support for KiCad users who want to simulate.

poeschlr commented 6 years ago

We have a few users over at the forum who are also able to help out. (holger is the one who is quite active. but also @bobc Just look in the simulation category https://forum.kicad.info/c/schematic/simulation-ngspice)

evanshultz commented 6 years ago

Note that I'm using the 5.0.0 released version.

.op directive as well as Operating Point tab in simulation settings fail with Error: no such vector 1

Yep, broken for me too.

I can't get D1 to show diode like behaviour during DC sweep. Neither by providing the model via a file or adding it to a comment.

Yes, pin 1 is assumed to be the anode in a SPICE D model. You can add the property "Spice_Node_Sequence" with a value of "2 1" in the UI to address this: image

It would be nice to be able to cut-and-paste a model into the SPICE model editor. As it is now, I need to provide a separate file with the model data or understand how to include it as a comment.

This can be done, at least it can be done now. The model name must match the VALUE field of the symbol. This may have changed since you tested, but I removed all properties (leaving only the top two), kept the .model D1n4007... text, and set the symbol VALUE to D1N4007. Works now.

It took ages to understand why I couldn't reference V1 in the command ".dc v1 0 9 0.1" If the SPICE command was shown after inserting values in the settings dialog it could be educational. The solution was to reference it as VV1. If opening the simulation settings dialog with .dc uncommented in the schema, it shows the DC Source as VV1. When opening the dropdown menu the only option available is V1 - this looks like a bug.

It simulates with .dc V1 0 9 0.1 now, but the UI still shows VV1 so it seems there is work to be done: image

The simulation settings dialog box should remember the last settings used. As it is now, I need to figure out the correct string and enter it in a text box on the schema.

Did you figure this out? I don't see any effect of the .plot, .print, or .probe SPICE directives.

It would be nice if the Power library included a SPICE powersource that was preconfigured. It took me a while to figure out that the different powersymbols e.g. +9V or Vcc wasn't ment to be used as a SPICE powersource.

I will handle this in a forthcoming update to the library. See https://github.com/KiCad/kicad-symbols/issues/805

evanshultz commented 6 years ago

Regarding the VV1 thing, that was apparently cached. If I close KiCad and try again everything seems OK, so I believe that issue has been fixed.

evanshultz commented 6 years ago

I attached an updated version of you simulation to this comment. SpiceTest.zip

And now for the included simulation file, where I have comments:

laser_driver

.tran

The laser diode is using the SPICE diode model with specific parameters. It should be fine. Some parameters given do not apply in ngspice and so are ignored. This should be fine.

As the source doesn't have a DC value assigned (not needed for a pulse source during the transient analysis but needed when finding the operating point), it starts at zero. This is also fine.

rectifier

Adding the real model is as simple as putting the following as text on the schematic page:

.model 1N4148  D(Is=5.84n N=1.94 Rs=.7017 Ikf=44.17m Xti=3 Eg=1.11 Cjo=.95p
+M=.55 Vj=.75 Fc=.5 Isr=11.07n Nr=2.088 Bv=100 Ibv=100u Tt=11.07n)

I'm a bit concerned what Unable to find definition of model 1n4148 - default assumed means with regards to the actual model used, though...

.ac

Yep, there is no AC voltage for an AC analysis. Here, any value works (not just the 1.5V you used) and will be 0dB.

sallen_key

.tran

Yes, you will need a time-domain AC source to see anything useful.

Symbol properties

I can reproduce this. It is odd so I created https://bugs.launchpad.net/kicad/+bug/1786116.

ghost commented 6 years ago

I just had the same pin-reversed situation with 1N4001 diode from the spice lib. This made through to board. De-soldering them all now.

poeschlr commented 6 years ago

There is no 1N4001 symbol in the spice lib. I can only see one in the diode library. The one in the diode library has the kathode as pin 1. This agrees with how the oficial footprints are setup so i really do not quite understand how your board could have come out wrong. Did you perhaps modify the diode symbol to fit the spice model? Or did you get the symbol in question from a different source then the official library?

Edit: We can only guarantee correct pairings of footprints and symbols that are both in the official lib.

Edit2: There is however a generic diode symbol in the pspice library that has the pin numbering the other way around. So i would guess you used that one?

bobc commented 6 years ago

Unfortunately, (ng)spice uses the opposite convention to KiCad libraries for diodes, and it is not feasible to make them the same.

Therefore devices in spice.lib should not be used for "real" components, only simulation. "Real" components can be used for simulation if the pin order is specified in the symbol property dialog.

Not sure if there is a way to neatly separate the two, for now user education is the only possibility.

poeschlr commented 6 years ago

I will fill out the description field of these symbols with a clear warning that they are not intended to be used in conjunction with footprints. Maybe we should use the same pin number as with other symbols and pre fill the pin remapping for spice.

The kicad pin numbers are not arability chosen. We use the scheme suggested by IPC. I would guess it was never envisioned that simulation and PCB design collide that is why spice did not use the same numbering scheme as suggested by industry standards.

ghost commented 6 years ago

It seems I used the generic spice diode changing it's value to 1N4001. It was some months ago. Clearly I didn't realise that the pin numbering is different. Some time usually goes by before I layout the board and by that time a diode is a diode. Thanks for the replies. It's another day of learning.

nhatkhai commented 6 years ago

I think, if there is a field for pspice pin order map it may be handy for real component where it's spice model pin order is not the same as 1 2 3 ... ?

evanshultz commented 6 years ago

@nhatkhai Yes, there is. See comments above for details.