Spiral Inductors PDK Flow Using QUEST, UTMOST IV, SmartSpice and SPAYN

Transcription

1 Application Note Spiral Inductors PDK Flow Using QUEST, UTMOST IV, SmartSpice and SPAYN Abstract: An original parameters extraction strategy has been developed using a physical and scalable 2π equivalent on-chip spiral inductors RLC circuit model. This strategy based on optimization only, was used to model spice model parameters as a function of geometrical inductor parameters. The data used in this paper were obtained by using a 3D electromagnetic Field Solver combined with a Design of Experiment (DoE) approach to make variation of layout parameters. Finally the Validation of the model was done. 1. Introduction For passive Devices (i.e Inductors, Capacitors ) like for active Devices (i.e Mosfet..) accurate spice parameters extraction is the key for subsequent reliable design. Spice model parameters of passive devices are extracted either from measurements or simulated S- parameters. The spice parameters extraction strategy for active and passive devices is however a bit different. Indeed whereas for active devices a unique set of parameters is usually extracted taking into account geometrical variations of the active devices (i.e W, L for a Mosfet) for passive devices a set of parameters is extracted per device and each spice model parameters is expressed as a function of geometrical parameters (i.e Radius, number of turns for an Inductors). We will present in this note the complete SIMUCAD flow from 3D Inductors simulation to spice models parameters modelisation and validation using QUEST, UTMOST IV and SmartSpice. 2. 3D Inductors Simulation Inductors simulation was made by QUEST, SIMUCAD 3D electromagnetic field solver. QUEST computes a 3D structure resulting of the layout information, process and techno file inputs, and output RLGC parameters, S-Y-Zparameters, Q factor QUEST is based on a 3D field solver elaborated in collaboration with CEA-LETI, where an original formulation of the Quasi-Static Maxwell equa- Figure 1: Automatic Multi-geometry layouts generation within QUEST. tions is used. See [1] for more details. As mentioned in the introduction the aim of the PDK generation is to give to designers the possibility to change easily turns or radius of an inductor for example, so that they can tune the inductance value accordingly. To do so, the first step is thus to create and simulate inductors with different geometries. For that purpose, the LISA script language of SIMUCAD layout editor Expert was used directly within QUEST [2], to create a generic parameterized inductance GDS layout as a function of layout parameters (radius, wire space, wire width, number of coils) as shown in figure 1. Using the Design of Experiment (DoE) feature of QUEST, variations of layout geometrical parameters can be done. These layouts will be distributed on a multi-cpus machine to optimize simulation time. We have decided for this study to make variation of turns and radius of the Inductor. The turns were varied from 2 to 4 and radius from 40um to 60um. A third-level full factorial DoE was used generating 9 different inductors. Simulation results (S-parameters, Y-parameters, quality factor, Inductance, resistance ) are then directly imported in UTMOST IV for subsequent spice parameters extraction as shown in Figure 2. Page 1

2 Figure 2: QUEST simulation results including all layouts directly imported to UTMOST IV. Figure. 3: Equivalent electrical model of Inductor. 3. Spice Parameters Extraction 3.1 Fixed Model The objective is now to extract RLC parameters of a user defined electrical spice model for each layout. To do so a spice simulation has to be done and result of this simulation has to be compared to QUEST simulation results (i.e Y-parameter from spice simulation is compared to Y- parameters from QUEST). An optimizer is used in between to make variation of spice parameters until spice simulation match QUEST results. We use the optimization module of UTMOST IV to accomplish this task. The performance of this module is the result of embedded spice simulator (i.e SmartSpice for speed issue) and a collection of optimization method either local or global (for accuracy issue) [3]. For this Inductor example a frequency independent equivalent RLC spice model was chosen and shown in Figure 3. This model contains 18 parameters [4] that have to be extracted with UTMOST IV optimization module. A spice netlist describing the model is defined in UTMOST IV and initial, minimum and maximum values were set for each parameters as shown in Figure 4. Initial values of each parameter can be obtained either from empirical formula [4] [5] or by QUEST simulations. In the case of a fixed model we simply pass to the optimizer 18 parameters and ask him to find the best set of 18 parameters matching the simulated data (Y-parameters). We choose the simulated annealing optimizer algorithm since it is a global optimizer, thus assuming that there may be multiple minima and attempt to locate the global minima. See reference [3] for more details. The frequency range for the optimization was kept below the Self-Resonant-Frequency (SRF). Figure 5 shows good extraction accuracy since the RMS error is less than 3.5%. Figure 4: Spice netlist and spice parameters range definition. Page 2

3 Figure 5: Measured (QUEST simulations) and simulated results after an 18 global optimization strategy. 3.2 Scalable Model The aim here is not only to extract spice parameters for each inductor but to express these extracted parameters as a function of geometrical parameters of the inductor. Thus an optimization strategy has been developed according to the geometrical layouts under consideration. We remember that 2 geometrical parameters of the inductor have been varied (i.e turns and radius). The turns were varied from 2 to 4 and radius from 40um to 60um. The aim was to reduce as much as we can the spice parameters to optimize. Some of them can have the same value, some of them can have constant value since they do not have a lot of influence and finally some of them can be derived from the others. Since the inductor is symmetric RSK1, LSK1, RAC1, COX1, CSUB1, L1 and RSUB1 are respectively equal RSK2, LSK2, RAC2, COX2, CSUB3, L2 and RSUB3. We decide to set COXM=2COX1, RSUB2=RSUB1*RSUB1/2RSUB1 and CSUB2=2CSUB1. From 18 original parameters only 8 remained. We now want to identify among the 8 remaining parameters if some of them do not have a lot of influence and thus can be fixed to a constant value. We thus perform the overall extraction on 9 geometries considering 8 parameters to extract. Statistical analysis in SPAYN was done on each parameter and it reveal that some of them did not exhibit statistical distribution. This was verified using the rubber band capability of UTMOST IV. Indeed this feature allows the 8 parameters to be varied and see interactively their impact on the spice simulation as shown in Figure 6. Figure 6: Rubber band in UTMOST IV allow interactive spice simulations which is very useful to identify non-influenced parameters 3 parameters were fixed at a constant value. These are COX1 fixed to 2.66pF, CSUB1 fixed to 12.46fF and CP fixed to 28fF. Finally only 5 parameters have to be extracted. We finally automatically did parameter extraction on 9 different inductors geometries. The results (i.e spice parameters and geometrical inductor parameters) are directly loaded in SPAYN (figure 7) the statistical analysis tool of SIMUCAD in order to perform subsequent statistical model and validation. Figure 7: Parameter extraction results on 9 inductors geometries. Page 3

4 Figure 8: PCA analysis results within SPAYN. Figure 9: Spice simulation using spice parameters from the analytical model coming from the PCA analysis. 4. Model and Validation SPAYN has general purpose histogram, scatter plot (2D and 3D), correlation matrix, regression modeling, process monitor charts and statistical process control chart options which can be used to analyze the inductor spice model parameters. Among SPAYN features, we have used the principal Component Analysis (PCA) [6]. A direct result of the PCA is a system of quadratic equations relating the correlated parameters to the derived independent components or factors. In this experiment it was found that 2 independent dominant parameters explained more than 99% of the variance of all of the inductors spice parameters analyzed as shown in Figure 7. These dominant parameters were Turns and radius also shown in figure 8. As a consequence the 5 remaining spice parameters (L1, RSK1, RAC1, LSK1 and RSUB1) are expressed analytically as a function of geometrical parameters (Turns and radius). To validate this model we need to compare spice simulation using spice parameters calculated by the analytical model and spice simulation using spice parameters extracted by UTMOST IV. Figure 10: Spice simulation using extracted spice parameters. Page 4 Both can be done directly in SPAYN (figure 9 and 10). We need of course to provide to SPAYN a spice netlist and a control card (inputs, stimuli etc). The direct comparison of both simulations in SmartView allows the validation of the model on DoE points (9 different inductor geometries) and outside the DoE points. As shown in Figure 11 and 12 the results are very good. A final validation was done on an inductor with Turns=3 and Radius=50um. The idea being to compare the fixed model (optimization of 18 parameters) the scalable model (optimization of 5 parameters) and the analytical model coming from the PCA analysis in SPAYN. The results are shown in Figure 13 and are good even if we see a difference (+/- 5%) for the inductance since this is not a parameter on which the optimization was done. Figure 11: Comparison of spice simulation (Y-parameters, Q, L and Res) using spice parameters from the analytical model coming from the PCA analysis and spice simulation using extracted spice parameters with UTMOST IV for turns=2 and Radius=40,50 and 60um.

5 Figure 12: Comparison of spice simulation (Y-parameters, Q, L and Res) using spice parameters from the analytical model coming from the PCA analysis and spice simulation using extracted spice parameters with UTMOST IV for turns=2 and Radius=45 um. Figure 13: Comparison of measurements (QUEST simulation: meas1), Fixed model (18 parameters:ac3) and scalable model (5 parameters:ac2) for turns=3 and Radius=50um.5. Based on the scalable model parameters obtained from the statistical PCA analysis of SPAYN, we want to find out the inductor geometry that match a desired inductor target (i.e Q and/or L). For that purpose the quadratic equation obtained by the PCA analysis is pass to SmartSpice where the optimizer feature of SmartSpice is used. As an output inductor layout is synthesized according to the desired inductor performance. References: 6. Conclusion We have shown a complete flow dedicated to parameters extraction on passive devices. As shown in Figure 14, inputs can be either simulated data or measurement data. Advanced statistical analysis and flow integration allow designers to easily express spice model parameters as a function of geometrical parameters, helping them to close aggressive design. [1] J.Piquet, O.Cueto, F.Charlet, M.Thomas, C.Bermond A.Farcy, J. Torres, B.Fléchet Simulation and characterization of High-Frequency Performances of Advanced MIM Capacitors ESSDERC proceeding pp [2] QUEST: Inductance Optimization Using, 3D Field Solver based on DoE Approach, Simulation Standard Volume 16, Number 2, February [3] Application notes: Guide to UTMOST IV optimizers September 12th [4] W.Gao and Z. Yu, Scalable Compact Circuit Model and Synthesis for RF CMOS Spiral Inductors IEEE Trans. On Microwave theory and techniques Vol. 54, NO. 3, March [5] Y.Cao and all Frequency-Independent Equivalent-Circuit Model for On-Chip Spiral Inductors IEEE Journal of SolidState Circuit, Vol. 38, NO.3, March 2003 [6] J.Edward Jackson, A user guide to Principal Components, John Wiley &Sons, Inc., QUEST UTMOST SPAYN Inductor PDK (scaling rules) Measurements User Inductor SPICE Model Figure 14: Inductor user equivalent spice model extraction flow (PDK) Page 5