Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Lumped Element model vs. EM Simulation

fred3991

Junior Member level 3
Joined
Nov 26, 2020
Messages
29
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
536
Simulation of passive components

How much necessary to use the Lumped element model of passive devices (inductances, transmission lines, baluns) when designing MMIC devices on the CMOS SOI technology?
If you need to run an EM simulation in the end for a complete layout?

I mean, if instead of Spice model (lumped element model) directly use S parameters of EM simulation (for inductor, balun, or transmission line segment) - wouldn't it be better?


Are there fundamental differences when modeling a passive component in DC, AC, Harmonic balance, transient analysis modes - if using lumped element model and S parameters EM modeling? Which is better and more accurate ?
 
If the models are sufficiently accurate, you can use their models of course. But there are some difficulties while they are used due to discrete nature of -for instance- s-parameters. SPICE Models are more appropriate but the accuracy is argued. EM simulation results are also discrete and sometimes they might be troublesome due to natural their discrete structures.
It depends on also frequency. If you're working on low frequencies, that might be easier, you can use their SPICE models directly.
Briefly, all depends on the accuracy, frequency and availability.
 
If the models are sufficiently accurate, you can use their models of course. But there are some difficulties while they are used due to discrete nature of -for instance- s-parameters. SPICE Models are more appropriate but the accuracy is argued. EM simulation results are also discrete and sometimes they might be troublesome due to natural their discrete structures.
It depends on also frequency. If you're working on low frequencies, that might be easier, you can use their SPICE models directly.
Briefly, all depends on the accuracy, frequency and availability.
Let us assume that we have a broadband lumped element model in the frequency range 0 (DC) - 30 GHz, and we have the results of an EM simulation in Momentum Microwave or HFSS in the range 0 - 30 GHz with a step of 0.1 GHz.
For simulation in DC/AC / HB modes will there be a significant difference in results?
 
If you use circuit models, effects like coupling between models is not included. We don't know if that matters in your design.

Also, some circuit models might be more accurate than others ... I have seen PDK models that were rather simple and for example didn't include self resonance for MIM. Of course that matters more at higher frequencies.

Regarding your 30 GHz example: For using EM data with nonlinear simulation, don't forget that you need a frequency range that also includes a few harmonics! It is not enough to just simulate response at the fundamental frequency for use in nonlinear simulation!
 
If you work @ 30GHz, you have no chance but using EM simulation. Because equivalent simple SPICE models cannot reach to this level. Special models can be used but limited accuracy due to coupling effects.
The best option for you is to use 3D EM simulation for whole layout with active components' models. There is no other option for that frequency. Resistors, Capacitors, Inductors can be simulated in 3D EM simulations, the rest active components must have very accurate -preferably measurement based- models. Otherwise you are in trouble.
 
If you use circuit models, effects like coupling between models is not included. We don't know if that matters in your design.

Also, some circuit models might be more accurate than others ... I have seen PDK models that were rather simple and for example didn't include self resonance for MIM. Of course that matters more at higher frequencies.

Regarding your 30 GHz example: For using EM data with nonlinear simulation, don't forget that you need a frequency range that also includes a few harmonics! It is not enough to just simulate response at the fundamental frequency for use in nonlinear simulation!
In other words, let me ask the question again.
Let's imagine you design devices which operate at 8- 20 GHz on CMOS SOI or SiGe BiCMOS technology.

And all models of passive components in the PDK are represented as black boxes of 2 kinds - one of them, a black box, inside which Spice model of medium complexity valid for the range 0 - 30 GHz (and it's scalable for all geometries)

The other black box contains the results of EM modeling of the component (S - Parameters simulator Momentum Microwave for example for the same frequency range in 0.01 GHz steps). (and it's also scalable for all geometries)


What type of models would you prefer to use for the designing process? 1 or 2?
 
I am working as EM specialist with a PDK team (SiGe BiCMOS with fmax 450 GHz) and believe there is no simple answer.

Workflow: All this needs to be LVS-clean also, and not break the design/verification flow. We have some EM-based models, e.g. for inductors with/without center tap, where the user can provide his S2P/S3P EM data. But for other elements where the PDK has no predefined EM black-boxes, using EM-based data is really difficult to implement without breaking the flow.

Accuracy, stability, convergence: In 25 years in EM support, I have seen too many bad models created by chip designers. RFIC designers are usually not EM experts and don't know the tricks to get really accurate EM data. In addition, the solvers results might create non-passive, non-causal data in some cases (think of small inductors where return loss is near 0dB), which blow up your Spectre simulation. Converting S-params to robust Spectre models which internally fix all these issues has been a major task in RFIC EM simulation for many years.

You mentioned resistors, that is one case where I strongly recommend EM users in "my" PDKs to use lumped models from the PDK instead of trying to EM-simulate them. They want to EM to get parasitics (frequency range > 200 GHz) but you would need very deep understanding of the technology cross section to get the stackup details right in that location. EM stackups in PDK provide metal stackup but exclude stackup information in the resistor region, so users would be onm their own.

Another issue: How would you handle tolerances/corner simulation when switching to EM-only models for all components? It would not be enough to EM-simulate the nominal layout with nominal material properties.

I think the present workflow of using PDK models with a few selected EM blocks of critical routing is appropriate at 30 GHz, and avoids a lot of trouble that you might have with EM data.
 
I am working as EM specialist with a PDK team (SiGe BiCMOS with fmax 450 GHz) and believe there is no simple answer.

Workflow: All this needs to be LVS-clean also, and not break the design/verification flow. We have some EM-based models, e.g. for inductors with/without center tap, where the user can provide his S2P/S3P EM data. But for other elements where the PDK has no predefined EM black-boxes, using EM-based data is really difficult to implement without breaking the flow.

Accuracy, stability, convergence: In 25 years in EM support, I have seen too many bad models created by chip designers. RFIC designers are usually not EM experts and don't know the tricks to get really accurate EM data. In addition, the solvers results might create non-passive, non-causal data in some cases (think of small inductors where return loss is near 0dB), which blow up your Spectre simulation. Converting S-params to robust Spectre models which internally fix all these issues has been a major task in RFIC EM simulation for many years.

You mentioned resistors, that is one case where I strongly recommend EM users in "my" PDKs to use lumped models from the PDK instead of trying to EM-simulate them. They want to EM to get parasitics (frequency range > 200 GHz) but you would need very deep understanding of the technology cross section to get the stackup details right in that location. EM stackups in PDK provide metal stackup but exclude stackup information in the resistor region, so users would be onm their own.

Another issue: How would you handle tolerances/corner simulation when switching to EM-only models for all components? It would not be enough to EM-simulate the nominal layout with nominal material properties.

I think the present workflow of using PDK models with a few selected EM blocks of critical routing is appropriate at 30 GHz, and avoids a lot of trouble that you might have with EM data.
I see your point.

About the lumped simulation - nowadays I came across a set of carpet pad files for EM simulation, which includes files for nominal, and corner cases (That is, several carpet pad files are presented in the PDK).

I just see from my colleagues at the university that the lumped model element from the PDK is only used at the very beginning of the design, when creating the first draft of the circuit.
Later this component (inductance coil, or balun) is replaced by a black box S-parameters file obtained with EM modeling. And in the further design almost to the end there is work with this file of S-parameters. No one goes back to using the lumped element model from PDK again in the design process.

That's why it was interesting to me. If you had the ability to do EM modeling at the same speed as the lumped-element modeling - would that be a useful thing?
 
this component (inductance coil, or balun) is replaced by a black box S-parameters file obtained with EM modeling.
Yes, inductors and transformers are THE typical use case for RFIC EM. It is very difficult to create accurate scalable models for these devices, so EM often is the only solution.

And in the further design almost to the end there is work with this file of S-parameters.

It really depends on the workflow if using black-box data breaks the flow. In a 20 transistor design, everything is possible. In a complex chip design, having EM data is worth nothing if it breaks LVS.


No one goes back to using the lumped element model from PDK again in the design process.

As I mentioned above, using "raw" S-parameters from EM might cause all sorts of issues in transient simulation, depending on port calibration and the device under test, so "my" EM customers like Rohde & Schwarz or Infineon preferred lumped models created from EM data ("broad band spice model extraction").

Prior to having lumped model extraction (guaranteed to be stable), even the smallest amount of numerical precison error could blow up transient analysis. That was years of pain supporting EM for RFIC workflows, especially with circuits where some ports are closely spaced without resistance in between that can "absorb" numerical precision errors.

That's why it was interesting to me. If you had the ability to do EM modeling at the same speed as the lumped-element modeling - would that be a useful thing?

I'm working full time in EM for more than 25 years, so of course I see many use cases for fast EM. All the "distributed element" stuff is certainly an EM candidate. But I also see the limits of EM in the hands of chip designers, due to tool limitations or stackup model limitations or user skills.
 
Last edited:

LaTeX Commands Quick-Menu:

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top