[ LM5088 ] New Macro Wizard Problem

Hi Britt,

Thank you so much for detail explanation!
Let me try out!!
I will come back to you, if I have further question!

Thanks,
Ken

161220-LM5088 TINA-TI Transient Reference Design_16-12-20.TSC

Hi Britt,

I'm still working with my customer for this issue, then need your support now. Attached is our tsc file for AC analysis with LM5088.
Can you please take a look into this?

Also, we have a couple of questions.

<Q1: Total Inductance, Fsw and Output Voltage>:

Quote: "The output cap, inductor, load, FB resistors, and compensation network are then added. The inductor and Vout should match the values in the params statement for the model as these will be passed to the model, not the actual inductor value."

How can I see the total inductance of this circuit?
In your example, you have 8.2uH in params and L={L} in actual inductor. This means, no external value is needed. Correct?

Also, how is Fsw determined? Is that derived from PRAMETERS?

Wrt Vout, do you mean VOUT in params and resistor divided need to be matched?





<Q2: Injection  Circuit>:

Quote: "You can now build your schematic around the model. You MUST use the Injection circuit with the large capacitor and inductor (Linj, Cinj, and V2 AC source from the picture)."

Do you have any of guideline, idea and/or tips to set the value of injection circuit?

<Q3: External Component>:

Your example does not have Cin, while there is a Cout.
Does this mean no Cin required for AC analysis?

Also, is it necessary to have Rs?

<Q4: Voltage Generator>:

It seems that your voltage generator and my one look slightly different.

Thank you for your support in advance.
Regards,
Ken

Kenichiro-san,

I have updated the .TSC file. It is attached below.

Here are the answers to your questions:

1.) The value being passed to the model is the L value of the inductor. You were passing 0 which is incorrect. It should be 6.8u since that is the value of your inductor. Please note that you have to specify BOTH values in the circuit. PSpice could use only one parameter. TINA-TI cannot. It must have both the inductor and the L value and both must be the same to get the proper simulation value. FSW is the switching frequency in Hz. I do not think that the circuit is operating at 250HZ, so I set it to 250KHz. Vout is the voltage output that is being set. This must also agree with the FB resistors that are chosen to get the proper simulation. In this case, I left it at 5V (I am assuming that is the Vout value for the circuit).

2.) You should not use the transient circuit to build the AC circuit. You did not add the injection circuit that makes the AC simulation possible. I have added it to the .TSC file below. It has an AC source, large inductor and large capacitor. This injection circuit "breaks the loop" from the frequency sweep for the Bode Plot.

3.) Cin is not usually important for the loop stability unless the input voltage is not stable. Since this is a simulation with a DC source, the source is stable and Cin is not going to effect the simulation. I have removed it from the simulation.

4.) You do not use an AC source for VIN for an AC simulation. I have changed this to a DC source for the AC simulation. For a transient simulation, I would use the source that you had originally.

I hope this information helps. I will double check the TINA-TI performance with the PSpice simulation. The magnitude looks correct, however, the phase waveform did not agree.

LM5088_AC.TSC