LTspice transmission line problem with RC load

[eti26000]

Hello everyone,

In LTspice, when I use a RC load with a transmission line, I got an error of floating node. I don't use a gnd symbol under the capacitor on purpose because I would like to take into account the path back to the gnd at the circuit entrance on the left. I don't understand why I got this error because the simulation runs fine if I use only a resistor as load. Can someone explain me ?

 

[FvM]

Other than with real transmission line, both ports are not connected in model. You need to define the potential of both ports somehow. If the transmission line is asymmetrical, e.g. coax cable, ground connecton of secondary port would model a real transmission line best. A single transmission line model implements infinite common mode impedance which doesn't exist in the real world. A second transmission line is needed to model finite common mode impedance and common mode wave propagation, if you actually want.

 

[eti26000]

Thank you for responding
When you say two lines, you mean something like this ?

 

[D.A.(Tony)Stewart]

No. If you want a differential load then you need a differential or two single ended drivers sharing a common center ground

 

[eti26000]

My goal is to simulate a single-ended line, but with a "realistic" ground instead of "ideal" ground. A first approximation I make is to say that ground path has the same characteristic than the line itself. That's why I would like to have only one "ideal" ground net at the left side and no ground net at the right side.
The problem I encounter is that LTspice doesn't really allow to do that, I don't know why and it's kind of frustrating.
However, the only solution for this problem seems to be this :

The guy in the video uses big resistances (100Meg) just to make LTspice quiet while trying to simule a kind of "realistic" ground path.

 

[FvM]

The question involves different aspects
1. Understanding the properties of SPICE tline model
It's an ideal component with partly counter-intuitive behaviour. It has infinite common mode impedance and thus isolates ports from each other. Loading the component with common mode current has effects that will be never observed with a real transmission line.
A usefull approach is to consider it as building block for transmission line circuits. If your circuit involves common mode waves, they have to be modelled separately.
2. Floating SPICE nodes
Floating nodes cause simulation failure in some cases. Adding high ohmic resistors is a possible fix, you can also use the global gshunt option, see Ltspice help or a SPICE text book for details. In this case, the problem is brought up by tline infinite common mode impedance, but it isn't specifically related to transmission lines.
3. Which circuit problem do you want to model?
In the given circuit, transmission line port 2 has no common mode load, therefore different grounding of the port has no effect as long as you are measuring port 2 differential voltage instead of port 2 nodes against ground.

See below test with variable load between port 2+ and ground. => The setup models in no way a "realistic" ground.

4. SPICE can only simulate lumped circuits and some ideal distributed components
Consider that the behaviour of an asymmetrical transmission line, e.g. coax cable, depends on circuit geometry. Presume T1 represents 10 m of RG58 coax cable. Is it coiled up or layed straight on the ground, with which distance? Common mode impedance respectively "realistic" ground impedance seen by port 2 will be different in each case. Finally common mode impedance is coupled to free space, part of the wave will radiated.

A simulation model of 10 m straight coax cable with common mode impedance could look like below. Notice that common mode wave propagation speed is higher due to air dielectricum.

 

[eti26000]

Hello, thank you again for the response. I admit I am a bit lost with all of that.
What I would like to simulate is a single-ended track on a PCB. I extracted values of inductance and capacitance per length unit using Altium.
More precisely, the signal trought the PCB track is a square pulse and I want to see the response of the signal at the load (RC load).
Ideally, I would also like to see the effect of non-ideal ground of the signal, to take into account ground return path that exists on the PCB.

I think I understood the concept of common and differential mode when using a differential transmission line. But, since I use single-ended track, there is only one signal mode, right ?

 

[D.A.(Tony)Stewart]

Use a differential complementary step source with the -ve being the low impedance of your imperfect ground. Then compare the difference with a large R across any two points.