Hello,

I have attached a simple test bench whose purpose is to learn how to use a current controlled current source (CCCS) in LTspice.

I1 is the controlling current source and does a dc sweep (.dc I1 0 1m 2u). I want to define F1, the CCCS, in terms of I1.

For this test, F1 should simply (follow) do the same thing as I1.

In the pull-down menu for F1, there are two fields: "Value" and "Value2". My guess is that these refer to the controlling current source and the gain, respectively. I have tried giving these fields the proper values (these values appear on the schematic), but the simulation won't run and returns errors related to an unknown controlling current or an unknown gain.

Thank you so much for your time and consideration.

David Levy

 

Hello

I know it seems silly but you can only specify a voltage source in the parameters of the CCCS.
Place a voltage source in series with the branch containing the current you wish to apply to the CCCS.
Then, specify 0 (zero) as the voltage in the voltage source. This causes LTspice to recognize the voltage source as a "current meter" as it will now monitor current. Then specify the voltage source in the params of the CCCS.

So...the parameters specified in the CCCS should look something like this:

V1 1

Where V1 is the "current meter" instance name, and 1 is the desired gain.

eT

 

Here's an example LTspice circuit using the current-controlled current-source F1.
Value V1 in the attribute editor indicates the current through V1 is being monitored, and the Value2 of 10 indicates the current is amplified by a factor of ten.
This can be seen in the simulation where the current generated by V1 in R1 (blue trace) is amplified by a factor of 10 in R2 (yellow trace).

 

Here's an example LTspice circuit using the current-controlled current-source F1.
Value V1 in the attribute editor indicates the current through V1 is being monitored, and the Value2 of 10 indicates the current is amplified by a factor of ten.
This can be seen in the simulation where the current generated by V1 in R1 (blue trace) is amplified by a factor of 10 in R2 (yellow trace).

View attachment 198251

Hello,

Um....If your gonna do that, you might as well use a VCCS.

eT

 

I have tried these suggestions. They all work.

My question has been answered clearly, thoroughly and quickly. What a great resource!

Digging through this website, I found that someone else offered yet another way, which was to use an "arbitrary behavioral current source" (bi). This worked as well.

The bi source seems to offer quite a lot of flexibility. I was able to create the square of the controlling current. In the Value field I wrote

I=i(I1)*i(I1)

The Value2 field did not require an input.

Thanks to all for your expertise and prompt help. Sharing knowledge is a blast.

David

 

.If your gonna do that, you might as well use a VCCS.

The circuit was just to demonstrate how the CCCS model worked, as the TS wanted.
It was not intended to have any practical application.

But the two circuits would not act the same.
A VCCS would give the same value for I(R2) if the value of R1 varied, whereas in the demo circuit, I(R2) would track the value of R1.

 

Hello,

I have attached a simple test bench whose purpose is to learn how to use a current controlled current source (CCCS) in LTspice.

I1 is the controlling current source and does a dc sweep (.dc I1 0 1m 2u). I want to define F1, the CCCS, in terms of I1.

For this test, F1 should simply (follow) do the same thing as I1.

In the pull-down menu for F1, there are two fields: "Value" and "Value2". My guess is that these refer to the controlling current source and the gain, respectively. I have tried giving these fields the proper values (these values appear on the schematic), but the simulation won't run and returns errors related to an unknown controlling current or an unknown gain.

Thank you so much for your time and consideration.

David Levy

Hello again,

Here is the way to use the "F" device as described in post #2.

eT

 

Thank-you!

I actually needed to learn this in order to solve a problem (it wasn't idle curiosity). Thanks for your help with that.

Below are some examples of what I learned from this website yesterday.

Notes: The voltage source that is required to be in series with the controlling current source is allowed to have a nonzero value. I actually have a circuit where I need that voltage source to be nonzero, and the sim works fine, as does this one, where the voltage source is 0.5V. Also, note that the behavioral current source doesn't need reference to such a voltage source.

Thanks again!
David

 

Thank-you!

I actually needed to learn this in order to solve a problem (it wasn't idle curiosity). Thanks for your help with that.

Below are some examples of what I learned from this website yesterday.

Notes: The voltage source that is required to be in series with the controlling current source is allowed to have a nonzero value. I actually have a circuit where I need that voltage source to be nonzero, and the sim works fine, as does this one, where the voltage source is 0.5V. Also, note that the behavioral current source doesn't need reference to such a voltage source.

Thanks again!
David

View attachment 198319

V2's value is having no effect because the current source I1 will force 1ma of current thru V2 no matter what its value.

eT

 

V2's value is having no effect because the current source I1 will force 1ma of current thru V2 no matter what its value.

eT

I agree. Actually, the sim is a DC sweep of I1, and your comment applies correctly to each value of the DC sweep.

David