Searching \ for '[EE] LTSpice grounds problem' in subject line. ()
Help us get a faster server
FAQ page: www.piclist.com/techref/microchip/ios.htm?key=spi
Search entire site for: 'LTSpice grounds problem'.

Exact match. Not showing close matches.
'[EE] LTSpice grounds problem'
2011\11\17@112359 by

Hello,
on LTSpice if I want to simulate two independent circuits, the program forces me to specify a ground for each.

However, by my tests the two grounds seem to be "invisibly" interconnected each other.

This is probably the right way to be (tm), but..

how do I simulate two different circuits which must be galvanically isolated each other, just like in real life? (and I don't want to use transformers)

Thanks!

With kind regards,
Mario
> Hello,
> on LTSpice if I want to simulate two independent circuits, the program forces me to
> specify a ground for each.
>
> However, by my tests the two grounds seem to be "invisibly" interconnected each
> other.
>
> This is probably the right way to be (tm), but..
>
> how do I simulate two different circuits which must be galvanically isolated each
> other, just like in real life? (and I don't want to use transformers)
>
> Thanks!
>
> With kind regards,
> Mario

Put a 100 Megohm resistor between them. Then LTspice thinks they are different circuits, and at that value of resistor they are to all and intents, isolated.

-- Scanned by iCritical.
I am no expert on Spice, but perhaps...

Create two circuit nodes to be the "local grounds" for each of your separate circuits.  Connect those two nodes via appropriate network (R and C in parallel?) to a "real" ground node. This will represent how they are connected in the real world, typically at least through leakage. Note that the value of R in that network could approach, or even perhaps be, infinite for a truly isolated circuit. C could be quite small, but probably won't be zero for anything close to real world.

-- Bob Ammerman
RAm Systems

{Original Message removed}
Yes, this can be a workable approach. It can sometimes result in
simulations failing to converge, though, if the leakage current
greatly alters the voltage seen in part of the circuit. The issue is
that LTSpice represents the voltage at each node as a single number so
it must have a reference point which is common to all nodes in the
design.

Beware, too, that some spice models (including some of Linear Tech's
built-in ones) connect some of their internal nodes to the GND net
without showing this connection. I have run into this problem with
some op-amps where I tried to simulate a floating circuit with an
op-amp in it. I used a large value resistor to connect the local
grounds of the two parts of the design which were isolated from each
other, but the op-amp assumed that its power supply range had GND
somewhere in-between Vcc and Vee. I would get very different values
from my simulation if I varied the relative voltage between the two
halves of my sim.

Sean

On Thu, Nov 17, 2011 at 12:22 PM, Bob Ammerman <picramroadrunner.com> wrote:
{Quote hidden}

> {Original Message removed}

More... (looser matching)
- Last day of these posts
- In 2011 , 2012 only
- Today
- New search...