# Cable equalization 101 - Simulating the design and improving stability (Part 2)

Other Parts Discussed in Post: LMH6733

In “Cable Equalization 101 - Automating your design,” we saw how a spreadsheet like Excel can be used to generate an equalization design rather painlessly, and we obtained the design in Figure 1 below. Here, we will use simulation to make sure the design is stable.

Figure 1: Excel solution found in Part 1_ one of two LMH6733 stages used as cable equalizer

Since Excel doesn’t know about the non-ideal behavior of the amplifier you have chosen, it is wise to test the results of the equalization design using simulation. Without a good simulation model for the cable, one would have to rely solely on the amplifier open loop response simulation. It turns out we have the means to investigate this stability criteria for the CFA in TINA as explained further below.

From OA-13, CFA Loop Gain Analysis, the CFA transfer function shown below in Equation 1, the stability criteria states that at the frequency where Z(s) (Transimpedance Gain) intercepts Feedback Transimpedance (Rf + RI (1+ Rf/ Rg)), the phase shift should be 135˚ or less (for 45˚ phase margin). We can investigate this intercept point in TINA to increase the confidence in the design.

Equation 1: CFA transfer function

For a cable equalizer, replace Rg in Equation 1 with the complex impedance ZG, which is the parallel combination of all boost bank elements, R1, C1, R2, C2, etc., (including RG) shown in Figure 1. We rely on the amplifier (LMH6733) TINA file to model the behavior of Z(s) over frequency and also the fixed value of RI built into the model. And of course Rf is the recommended feedback resistor for this particular CFA, which is what was used in the Excel file to produce the Figure 1 solution to begin with.

Here is how we can get these pertinent plots over frequency to show in TINA for us to conduct our stability analysis:

a)      Feedback Transconductance (1 / Transimpedance) is the current flow into the inverting input (I_Rsense) in response to output (OUT1), with the loop open. Figure 2 below includes L_Large and C_Large which open the loop in AC (where we are concerned about stability and response) but leave it closed for DC to set the operating point.

b)      Z(s) is “Amp_out / I_Rsense” (TINA can easily do the arithmetic on waveforms!)

Figure 2: TINA tricks to open the loop and to sense inverting current

So, we have everything at our disposal to investigate the point of intercept of Z(s) and feedback Transimpedance graphically using TINA. See Figure 3 below for three values of resistance R1, chosen as the bank element most likely to affect stability, in order to find the optimum value of R1.

Figure 3: Open loop gain and feedback transimpedance plot intercept for three values of R1

From Figure 3, the direct Excel solution (R1= 1ohm) would be unstable because of the 40dB/decade rate of closure of the two plots (this has to do with excess phase shift around the loop). Increasing R1 to 50ohm would be excessive and would limit the frequency response, while R1=10ohm is ideal because it places a Feedback Transimpedance pole at the intercept frequency and yield about 45˚ of phase margin.

We were able to take the Excel design one step further and verify against the device’s TINA model to anticipate real world issues with the boost in noise gain we have implemented. Bench verification and optimization of the design with the actual intended cable is the next step to complete the process.

I’ve included the TINA simulation file link for those of you who like to tinker with it and test other possibilities.

8357.LMH6733 Equalization.TSC

Hope you enjoyed this blog and found it useful. Please let me know if there any questions!

Also, if you ever do a similar stability analysis on a voltage feedback amplifier, check out my two-part article on “using Pspice to analyze amplifier loop stability – part one and part two.”

• Hello,

I just re-read this blog after writing it a while back and had the following questions which I've tried to answer below, in case the readers have similar ones:

1. Figure 3 "Forard_Gain" plot is synonymous with "Transimpedance Gain Z(s)" and it is the LMH6733 Macromodel open loop gain (output voltage / inverting input current) with units of Ohm.

2. In Figure 3, I'm running the TINA-TI AC Analysis on 3 versions of the Figure 1 schematic to find the optimum value of the 1ohm resistor (resistor in series with C1).  The reference designator for this resistor is R1 (Case 1),  R7 (Case 2), and R14 (Case 3). I could not have assigned them all as "R1" because components should have unique designators.

3. I've called "Case 2" to be the optimum choice even though in Figure 3 its "rate of closure" still looks to be around 40dB/decade! That's because, I can see that Case 2 Feedback Transimpedance changes slope right around the intercept point (~158MHz) which indicates that this plot is encountering a "zero" very close to the intercept point with Z(s) and moving towards more stability.

A closer examination of the intercept point reveals that Phase Margin is actually the angle of the LMH6733 output voltage plot at the frequency of interest. Using a cursor in TINA-TI to read the "AC Bode" tab phase information, I read the following Phase Margins for the 3 cases:

Case                         Intercept Frequency                                  Phase Margin

(MHz)                                                          (Degrees)

1                                 154                                                               19

2                                 158                                                               50

3                                  260                                                              69

This confirms that Case 2 has good Phase Margin- something I determined visually by "eye-balling" the intercept point.

4. To get the Figure 3 response when working with the TINA-TI file, run "Analysis", "AC Analysis", "AC Transfer Characteristics", and "OK".

5. To see / edit the expressions for the waveforms, in the waveform display click "Edit", "Post-processor", select Show "User Defined". Select large down-arrow to have TINA-TI display the expression in the "Line Edit" area right below the arrow. For example, you will see this as the expression for the "Forard_Gain":

"Amp_out (s) / I_Rsense [3,5] (s)".

"[3,5]" refers to the netlist node numbers of "R_sense" in this example and "(s)" represents the notation for Laplace transform (vector or phase representation).

Regards,

Hooman