PSPICE transformer - floating nodes and grounds

I've tried to take whatever suggestions I've found on the net, but I'm still having this problem. I get these errors when I'm trying to simulate.

Node N00256 is floating
Node VOUT1 is floating
Node N00214 is floating
Node GND is floating
Node N00227 is floating
Node N00195 is floating


The circuit is attached. What am I doing wrong?
And yes, I had a ground below R2 IN ADDITION to the primary side ground, and I was getting the same errors as well.
Anybody help? Thanks.

Ground in SPICE is node zero. The fact that you are getting GND as floating makes me think it needs a node zero. Try changing the name of you GND connection to zero.

Keith

Try changing the name of you GND connection to zero.

Click to expand...

Or use a different GND (AGND) symbol.

keith1200rs said:

Ground in SPICE is node zero. The fact that you are getting GND as floating makes me think it needs a node zero. Try changing the name of you GND connection to zero.

Keith

Click to expand...

there is no gnd0 component in the version i have. It's just gnd, and i also have earth ground and a few others.

So, what exactly should i rename it to?

"gnd0"? "0"? something else?

its unbelievable that SPICE has been around for a million years, yet it's so hard to implement an ideal transformer

Are you able to get it to generate a spice netlist that we can look at?

palikari said:

its unbelievable that SPICE has been around for a million years, yet it's so hard to implement an ideal transformer

Click to expand...

It is no use blaming the software! You need to learn how to use it. There are plenty of tutorials on the internet.

The ground node is simply a number zero "0". I don't use PSpice but I am sure there will be a ground symbol already numbered zero.

Keith

hi,there is a gnd 0 (simulation ground) in pspice,i rarely remember it but you could press 'g' key to find.Good luck.

palikari said:

its unbelievable that SPICE has modelledaround for a million years, yet it's so hard to implement an ideal transformer

Click to expand...

I think you'll find very few spice transformers that are modelled on coupling inductors, ideal or otherwise

I think you'll find very few spice transformers that are modelled on coupling inductors, ideal or otherwise

Click to expand...

Your words are mysterious. Most people will model transformers as coupled inductors in SPICE. With PSpice or LTSpice you have also the option to specify a saturable magnetical core with the K statement.

abaz said:

Are you able to get it to generate a spice netlist that we can look at?

Click to expand...

yes, here it is, thanks.


*Libraries:
* Local Libraries :
* From [PSPICE NETLIST] section of pspiceev.ini file:
.lib "nom.lib"

*Analysis directives:
.TRAN 0 1s 0 .01
.PROBE
.INC "transformer1to1-SCHEMATIC1.net"


**** INCLUDING transformer1to1-SCHEMATIC1.net ****
* source TRANSFORMER1TO1
R_R3 N00256 VOUT1 1k
K_TX1 L1_TX1 L2_TX1 .999
L1_TX1 N00755 GND 20
L2_TX1 VOUT1 N00227 .148
R_R4 GND N00227 100meg
V_V1 N00210 GND
+SIN 0 230 60 0 0 0
R_R1 N00210 N00755 10
R_R2 N00227 N00256 1k

**** RESUMING transformer1to1-schematic1-myprof.sim.cir ****
.INC "transformer1to1-SCHEMATIC1.als"



**** INCLUDING transformer1to1-SCHEMATIC1.als ****
.ALIASES
R_R3 R3(1=N00256 2=VOUT1 )
K_TX1 TX1()
L1_TX1 TX1(1=N00755 2=GND )
L2_TX1 TX1(3=VOUT1 4=N00227 )
R_R4 R4(1=GND 2=N00227 )
V_V1 V1(+=N00210 -=GND )
R_R1 R1(1=N00210 2=N00755 )
R_R2 R2(1=N00227 2=N00256 )
_ _(vout1=VOUT1)
_ _(GND=GND)
_ _(GND=GND)
.ENDALIASES

**** RESUMING transformer1to1-schematic1-myprof.sim.cir ****
.END

ERROR -- Node N00256 is floating
ERROR -- Node VOUT1 is floating
ERROR -- Node N00755 is floating
ERROR -- Node GND is floating
ERROR -- Node N00227 is floating
ERROR -- Node N00210 is floating

- - - Updated - - -

snail888 said:

hi,there is a gnd 0 (simulation ground) in pspice,i rarely remember it but you could press 'g' key to find.Good luck.

Click to expand...

i know what ur talking about, but i dont see it. Here is what I have to choose from:

The symbol you are looking for is in the PSPICE library source and has the name "0". You apparently missed to load the library.

I do have the Source library. I just checked my Source library and there is no ground at all.

Maybe the library organisation has been changed. In this case you should refer to the installed PSPICE capture examples. They should be working, because they use the right GND symbol.

FvM said:

Maybe the library organisation has been changed. In this case you should refer to the installed PSPICE capture examples. They should be working, because they use the right GND symbol.

Click to expand...

weird
ok I looked at the installed analog example, and yes it had the gnd0. SO I copied and pasted it into my schematic, and it worked!

Then, I looked at my Source library, and it's still not there. But when I clicked the gnd icon, it was in there! I had clicked it before, and it wasn't. I dont understand this. But at least I have it now.

Here is a screenshot of it now:

You can review the properties of the "0" GND symbol to see which library it's originated from. Apparently it's not the CAPSYM (or any other) library you have already opened.

yea, it shows that it's from the source.olb library...but yet is not listed in there

it doesn't even show up when I click on the gnd icon, unless I copy and paste one into the schematic from another schematic (i.e., the installed example). Then when I click the gnd icon again, it shows up! But still doesn't show up in the Source.olb library.

FYI, I am using the Orcad Demo version (Capture, not Schematic) from the electronics-lab website

Strange. The selection for "Place Ground" should look like below:

FvM said:

Your words are mysterious. Most people will model transformers as coupled inductors in SPICE. With PSpice or LTSpice you have also the option to specify a saturable magnetical core with the K statement.

Click to expand...

Sorry for the late reply and more so for possibly being mistaken...
A long, long time ago (ie. Iv'e forgotten a lot) I struggled with transformer simulation in spice and started looking around for spice transformer models. The majority of the examples I found hardly ever used coupled inductors. MOst of them used voltage dependant voltage sources, with math functions to simulate saturable cores etc, etc. I have looked through my archives and cant seem to find any of the material I gathered at the time.

As for the K statement I only had spice3 documentation and was not aware of any possible enhancements in pspice or ltspice. Here's a quote from the documentation I have

3.1.8. Coupled (Mutual) Inductors

General form:
KXXXXXXX LYYYYYYY LZZZZZZZ VALUE

Examples:
K43 LAA LBB 0.999
KXFRMR L1 L2 0.87

LYYYYYYY and LZZZZZZZ are the names of the two coupled inductors, and VALUE is the
coefficient of coupling, K, which must be greater than 0 and less than or equal to 1. Using the ’dot’
convention, place a ’dot’ on the first node of each inductor.

Click to expand...

I am by no means an expert in these matters and am happy to learn something new, but I cant help but feel that the coupling coefficient would be linear whilst saturation would be non-linear

The PSPice non-linear coupling model is described in the Refernce manual, chapter Inductor coupling and magnetic core. The part library has also models for popular ferrite cores, the number of turns and an optional scaling factor for the core cross section has to be given to define an inductor or transformer.

In LTSpice, the non-linear core parameters are speciied with the inductor (L) component, the syntax is described in the on-line help. I didn't yet try it, but it seems to give a similar functionality as the PSPice core model.