3 Data Preparation

This section contains information about the inputs that are required for running EMIR analysis in Voltus-Fi-XL.

Voltus-Fi-XL Flow Overview

The Voltus-Fi-XL-Spectre^® Accelerated Parallel Simulator (APS)/eXtensive Partitioning Simulator (XPS) flow is a two-step flow.

Step1: Simulation is run using Spectre APS/XPS and the simulation database is generated.

Step2: The simulation output generated in the above step is provided as input to Voltus-Fi-XL, which performs the following electromigration and voltage drop (EMIR) analyses:

- Power IR/EM analysis
- Signal IR/EM analysis
- Structural analysis

Voltus-Fi-XL generates text reports of IR drop and EM violations and displays them as plots on the Virtuoso® layout. It also provides batch mode support for IR/EM analysis and report generation.

Voltus-Fi-XL supports both static and dynamic EMIR analysis.

Spectre APS/XPS EMIR Flow Overview

With MMSIM/SPECTRE12.1, SpectreAPS and Spectre XPS, Cadence delivers a new EMIR solution. This dynamic power EMIR and signal EM capability uses a new technology, and is designed to provide higher capacity and better performance compared to existing EMIR solutions. Within this flow, SpectreAPS can be used for high accuracy EMIR analyses; while Spectre XPS can be deployed for high performance and high capacity EMIR simulation.

In an EMIR flow, a circuit is evaluated together with the parasitic resistor and capacitor network, which models the IR drop or the EM effect. There are two general approaches of solving such a problem.

Direct EMIR analysis: When high accuracy is needed, a brute-force simulation of the entire system – circuit plus parasitic resistances and capacitances – can be performed to accurately calculate EMIR of any net. This approach is called the “one-step” method, where the EMIR simulation performance and capacity is subject to the limitation of the circuit simulator being used.
Iterated EMIR analysis: To conduct EMIR simulation on circuits with much larger power and signal nets, within a shorter time, there is an alternative approach that involves decoupling the nonlinear circuit simulation from the linear RC net analysis. You can iterate the linear RC net analysis by modifying the layout, however, the nonlinear circuit simulation is done only once. This approach is called the “two-step” method. The decoupling of the linear RC nets from the nonlinear circuit is not mathematically equivalent to the original design and certain inaccuracy is introduced but it provides the benefit of simulation performance and capacity.

The above two approaches are depicted in the figure below.

For high accuracy EMIR analysis of small design blocks, or designs with smaller numbers of RC nets, the direct EMIR analysis method is recommended, where SpectreAPS and Spectre XPS SPICE mode are fully supported. SpectreXPS does not support direct EMIR analysis.

To gain higher performance and higher capacity on medium to large designs, the iterated EMIR analysis method is recommended. SpectreXPS is used for these large-scale simulations as it is able to take full advantage of the FastSPICE technology. Both, Spectre APS and Spectre XPS SPICE mode support iterated EMIR analysis.

The Spectre APS/XPS EMIR flow requires a complete testbench that contains Detailed Standard Parasitic Format (DSPF) files – with parasitic and instance sections describing the circuit to be analyzed – and stimuli, device models, and so on. The presence of a +emir statement on the Spectre command line enables the EMIR analysis during circuit simulation. The details of EMIR analysis, including the type of analyses to be performed, nets to be analyzed, and the output to be generated, are specified using an EMIR configuration file.

Using either direct EMIR analysis or iterated EMIR analysis, the circuit simulation is performed first with various voltages and currents being calculated. Next, a standalone tool, emirutil, is called to post-process the simulation results and generate IR and EM reports. By default, this postprocessing step is invoked automatically.

The output of the EMIR analysis is an EMIR text report, which lists the EM and/or IR information of the specified nets. In addition, an OA database is generated to enable the visualization of the EMIR results on the Virtuoso layout using Voltus-Fi Custom Power Integrity Solution tool.

This flow is shown in the below figure.

Data Requirements for Voltus-Fi-XL

The following inputs are required for EMIR analysis in Voltus-Fi-XL:

A simulation output directory that contains the EMIR database
The qrcTechFile with EM Models for EM rules, text-based ICT file, or the emDataFile.txt file with EM rules
Layer map file – this file is required to map the layer names in the simulation result file and the technology file
This file is required only if the layer names in the two files are different.
APS/XPS-to-DFII layer map file for solid shape display and structural analysis
Net names (optional)
Information about the type of analysis to be performed (peak, avg, rms, absAvg)

xDSPF Requirements

The third-party netlist file or xDSPF is used to provide all the parasitic information of the design for performing simulation using the Spectre APS/XPS simulators. The xDSPF must include the following information:

All power ground nets extracted
Layer information with each resistor
x, y co-ordinates of the parasitic resistors, and
Decoupled RC of all signal nets

DSPF files are created using the parasitic extraction tools and their content and format is heavily dependent on the extraction tool and the extraction runset. Often simulation problems occur due to problems in the DSPF file. To ensure that the DSPF file is compatible with the simulation requirements use the Standard Parasitic Format (SPF) Checker utility before using the file in the MMSIM/SPECTRE EMIR flow.

The SPF Checker utility analyzes the DSPF file, reports problems that may cause simulation problems, and creates an EMIR conf file with recommended mapping statements.

Note:

Ensure that there is no pin on the substrate shorting in the xDSPF. Set the extractor accordingly.
Voltus-Fi-XL supports the generation of the xDSPF file using Quantus both from the GUI and in batch mode.

Simulation Requirements and Setup

For viewing IR drop and EM analysis results in Voltus-Fi-XL, the simulation database generated using Spectre APS/XPS simulators is loaded into Voltus-Fi-XL.

For EMIR analysis, ensure the following while performing simulation.

Create a complete simulation testbench with the DSPF files containing the post-layout data of the design, including fingered devices and net parasitics. Use the dspf_include statement to read the DSPF content, as shown below.
```
dspf_include "sram.spf" (Spectre syntax)
```
```
.dspf_include "sram.spf" (SPICE syntax)
```
Though include/.include statements are also supported, it is recommended to use dspf_include/.dspf_include statements, which automatically handle duplicated subcircuit definitions and port order differences.
Use the SPF Checker utility before using the file in the MMSIM/SPECTRE EMIR flow.
Define the EMIR configuration using the EMIR control file (emir.config), and include the control file with the +emir statement on the Spectre command line, as shown below.
```
% spectre +aps +emir=emir.conf input.scs (APS solver)
```
```
% spectre +xps +emir=emir.conf input.scs (XPS solver)
```
Before plotting EMIR results, ensure that the simulation result file is available in the output directory of the simulation results.

The naming convention for the simulation results file is; *.emir#_bin. For example, the result file could be named, xps.emir0_bin.This file is required for displaying IR and EM plots and generating text reports in Voltus-Fi-XL.

In the APS direct method of simulation, no intermediate database files are created. However, in the iterated method, EMIR files have the emirtap file extension. The 1^st stage EMIR circuit simulation creates the tap device voltage profiles that are stored in the pwl files, and used in the 2^nd stage. The 2^nd stage RC network solver writes all IR drop and EM current values into the binary database with the extension emir0_bin. This binary database is used by emirutil/emirreport for creating the text/HTML/CSV reports, and by Voltus-Fi-XL to visualize the results in the layout.

Direct method: design.emir0_bin, design.rpt_ir, design.rpt_em

Iterated method: design.emirtap.emir0_bin, design.emirtap.rpt_ir, design.emirtap.rpt_em

All intermediate and output files are written into the Spectre output (raw) directory.

For large designs, you can compress the intermediate (pwl, pdb) and the EMIR database files (emir0_bin) by specifying the “eisopt zipfiles=2” option in the EMIR conf file.

EMIR Control File Options Supported in Voltus-Fi-XL

The following table summarizes the EMIR control file options supported in Voltus-Fi-XL. These are specified in the configuration file using the emirutil command.
.

Keyword	Option Set	Explanation	Default Value
`net`	`name=[instance1.net1instance1.net2....]`	Defines the nets for which the analysis is performed. instance defines the instance of the subcircuit containing the net. net defines the net name inside the subcircuit instance as it is defined in the `DSPF *\| NET` definition. If the DSPF file is included on the top level, the instance name is not required. Wildcarding is supported for net names but not instance names.	`none`
`net`	`analysis=[imax iavg iavgpos iavgneg iavgabs iacpeak irms vmax vavg]`	peakEM, avgEM, avgEM for i>0, avgEM for i<0, avgabsEM, rmsEM, peakIR, avgIR Note: To perform AC-Peak analysis in Voltus-Fi-XL, ensure that the `imax` and `iavg` options are specified in the control file.	`iavg, vmax`
	`pwrgate=[powernet1 powernet2...]`	Enables power gate handling. You need to specify the power supply net driving the power gate and the internal power supply net driven by the powergate. If one power supply net drives multiple power gates, then you need to specify one statement with all internal power supply nets. For example: If the internal and external net names are as follows and XTOP is the top cell name: `pair1 ->[VDD VSS] pair2 ->[VDDM VDDM1] pair3 ->[VDDM VDDM2]` Then the following settings can be specified where the second setting will not override the first: `pwrgate=[XTOP.VDD XTOP.VSS]` `pwrgate=[XTOP.VDDM XTOP.VDDM1 XTOP.VDDM2]`	`none`
	`analysis=[sigvmax sigvavg] reftype=[avg max]` `[findsrc=yes]`	`sigvmax` - max signal net IR drop. `sigvavg` - avg signal net IR drop. `avg` - reference voltage for IR drop is the average voltage of all subnodes at every time point. `max` - reference voltage for IR drop is the maximum voltage of all subnodes at every time point. `findsrc=yes` - Use voltage from subnode which is connected to vsource. The feature automatically traces through the design or source resistors.	`none`
	For versions before MMSIM/SPECTRE15.1 ISR2, the syntax is as follows: `design_res_models=[name=<cell_name> w=<width parameter name> l=<length parameter name> layer=<layer name> unit=<multiplier to get length/width * geounit in um>]` For MMSIM/SPECTRE15.1 ISR2 and later versions, the syntax is as follows: `design_res_models=[name=<cell_name> w=<width parameter name> l=<length parameter name> layer=<layer name> unit=<multiplier to get length/width in m>]`	Specifies the design resistor models for which EMIR analysis will be performed. Note: The design resistor models are specified for cells and not for the instances of the cell. For example, for the design resistor provided in the xDSPF file as: `XR1 XR1#PLUS XR1#MINUS r_user wr=1e-06 lr=5e-06` In this example, width (`wr`) and length (`lr`) are in meters. The design resistor models will be specified in the following manner: Before MMSIM/SPECTRE15.1 ISR2, `design_res_models=[name=r_user w=wr l=lr layer=mt1 unit=1e6]` MMSIM/SPECTRE15.1 ISR2 and later: `design_res_models=[name=r_user w=wr l=lr layer=mt1 unit=1]` where, `r_user` is the design resistor model name `lr` is the length parameter name specified in the xDSPF `wr` is the width parameter name specified in the xDSPF `mt1` is the layer for the EM rules. The tool will apply `mt1` layer rules from the ICT file for this resistor	`none`
		Before MMSIM/SPECTRE15.1 ISR2 `1e6` is the unit that is calculated as design resistor `W/L` in netlist `* unit/geounit`. For example: For `lr=5e-06` and `unit=1e6`, the length value of design resistor in `um` is as follows: `l=5e-061e06=5um` MMISM15.1ISR2 and later `1` is the unit that is calculated as design resistor `W/L` in netlist ` unit`. For example: For `lr=5e-06` and `unit=1`, the length value of design resistor in meters is as follows: `l=5e-06*1=5e-06m`
`solver`	`method=[auto \| direct \| iterated \| profonly \| iteronly]`	`auto` - direct for APS, iterated for XPS (default)\| `direct` - forced direct method, not available for XPS `iterated` - forced iterated approach, available for APS and XPS `profonly` - iterated flow - circuit profile generation `iteronly` - iterated flow - RC network iteration	`auto`
	`speed=[1\|2\|3\|4\|5\|6\|7\|8]`	Defines the speed/accuracy trade-off for PN and SN RC network solver. `1` - highest accuracy, lowest speed `8` - lowest accuracy, highest speed	`5`
	`inputwf=file_name`	Specifies the waveform file that contains the results from circuit simulation when `method=iteronly` is used.	`none`
	`report_tapi=on`	Specifies to generate tap current reports. When this option is specified, outputs the `rms`, `avg`, and `max` tap currents in the `.emir#_bin` simulation result file.	none
`static`	`ifile=”filename”`	Enables static EMIR analysis. The file defines the subckt instance port currents. Note: Static EMIR analysis cannot be combined with the dynamic EMIR analysis.	`none`
	`analysis=[ipwc] pwc_threshold=1e-6`	Enables pulse-wise EM current calculation for violation visualization. The `pwc_threshold` option defines the current threshold for finding the start of the pulse. Any value below `pwc_threshold` is considered as zero. The `emirutil_dump_pwc_info=1` option generates an ascii report in the <name>`.pwc0_raw` file for debugging purpose only.	`none`
	`vref`	Defines the optional voltage reference value for `vmax` and `vavg` analyses.	`none`
`emirutil`	`techfile="emDataFile"`	Specifies the EM rule file in the emdatafile, qrctechfile, or ictfile format. Layer names that are not case-sensitive are supported, allowing easier match between the DSPF and `emData` file. The EM rule file can be predefined in the configuration file using the `EMTECHFILE` environment variable or in the `.cdsinit` file as follows: `envSetVal("spectre.envOpts" "emTechFile" string <path to the file>` The rule file defined in the configuration file has a higher priority followed by the rule file specified in `.cdsinit`. Alternatively, you can use the `emdatafile="emDataFile"` option to specify the techfile in the emdata format, `qrctechfile="qrcTechFile"` to specify the Quantus tech files, and `ictfile="ictfile"` to specify the file in the ICT format. The EM rule file in emdatafile format can be predefined using the EMDATAFILE environment variable, or emRuleFile in `cdsenv`. The EM rule file defined in `cdsenv` has a higher priority.	`none`
		The `layermap` file provides the mapping between the xDSPF and the layout database. It is applicable only for `qrcTechfile` and `ictfile`.
	`EMOnlyICTFile=”emOnlyICTFile”`	Specifies the process and EM models to be used for EM analysis. Note: This file can only be provided with the `qrcTechFile` flow.	`none`
	`res_pdata_sw=[on]`	When the bounding box coordinates are included in the xDSPF file and this option is set to `on`, prints the coordinates of resistor bounding box in the electromigration report. If this option is not specified in the EMIR conf file or the coordinates are not included in xDSPF, the node coordinates of resistors are printed instead of the bounding box coordinates.	`none`
	`rcIrcxFile=[./RC_your_file.ircx]`	Specifies the RC iRCX file provided by the foundry to be used for EM analysis.	`none`
	`emirIrcxFile=[./EMIR_your_file.ircx]`	Specifies the EMIR iRCX file provided by the foundry to be used for EM analysis.	`none`
	`ir_in_em=[true \| false]`	When set to `true`, reports the maximum IR drop value for each metal resistor/via in the EM current report. It adds a “Max IR” column in the EM report. This value is the higher IR drop value of the two nodes of the resistor.	`false`
	`tap_model_report=yes \| no`	When set to `yes`, the software reports the device model names for all the tap devices in the dynamic and static analysis report files – `.rpt_ir` and `.spgs`.	`none`
	`layerSetupFile=`filename	Specifies the name of the layer setup file to be used for the Voltus-Fi Quantus shape server flow. By default, the Voltus-Fi Quantus shape server flow reads the “`layer_setup`” file from the path specified in the "`_qrc_tech_dir`" file of the `qrc run dir`. Use this option to specify a file other than the default file. For example: `emirutil layerSetupFile=layer_setup_1`	`none`
	mdLayers=”md`layer1 mdlayer2 mdlayer#`”	Specifies the list of metal diffusion layers that need to be combined for EM analysis. For example, to calculate the distance between terminal vias (`Lv2v`), for thermal analysis (SHE) and so on. The default value is shown below. `emirutil mdLayers=”MD_STI MD_OD MD_STI_SRM MD_OD_SRM M0_OD M0_STI MD_STI_CPP85 MD_OD_CPP85”`	`MD_STI MD_OD MD_STI_SRM MD_OD_SRM M0_OD M0_STI MD_STI_CPP85 MD_OD_CPP85`
	`mergeMDLayers=[true \| false]`	Enables combining of metal diffusion layers that are specified using the variable, `mdLayers`, for calculating the effective Blech length. When set to `false`, no merging of metal diffusion layers is done for the Blech length calculation. `emirutil mergeMDLayers=true`	`true`
	`mt=8`	Specifies the number of CPUs used by clients for multithreading. `emirutil mt=8`	`8`
	`postTclCmdFile=[conf.tcl]`	Specifies the Tcl file that contains user-specified commands for querying specific resistor and node information and creating customized EM and IR drop analysis reports. For details about the commands that can be written in the file (`conf.tcl`), see the “Batch Mode Execution” chapter.	`none`
	`layermapfile=”mapfile”`	Specifies the layer map file that provides the mapping between the layer names in the simulation database to the layer names in the technology file.	`none`
	`layermap=[(rcxLayer=rcx_layer_name1 ictLayer=ict_layer_name1) (rcxLayer=rcx_layer_name2 ictLayer=ict_layer_name2)]`	Specifies the mapping between the layer names in the simulation database to those specified in the technology files (qrcTechFile and ICT file) for the EM analysis flow. It maps the layer names in the xDSPF file to the ICT layer names. `rcxLayer` is the layer name in the simulation database. `ictLayer` is the layer name in the ICT EM file. Example: `emirutil layermap=[(rcxLayer=M1 ictLayer=T1) (rcxLayer=M2 ictLayer=T2)]` This option is used if the `layermapfile` option is not available.	`none`
	`autorun=[true \| false]`	`true` - run `emirutil` automatically to generate a text report. `false` - manually run `emirutil`.	`true`
	`reportCurrentAmp=[true \| false]`	`true` - reports the current of the resistor in ampere (A). `false` - reports the current of the resistor in milliampere (mA).	`true`
	`report=[text \| html \| csv]`	Defines the type of report created by `emirutil`. `text` - creates a report in text format. `html` - creates the report in HTML format. `csv` - creates the report in CSV format. Note: Multiple entries are supported.	`text`
	`report_voltage=[true \| false]`	When set to `true`, IR reports display the absolute voltage value instead of the IR drop value and in the GUI, the Virtuoso layout displays the absolute voltage plots instead of the voltage drop plots. `emirutil report_voltage=true`	`false`
	`notation=[s \| e]`	Notation for the text and html reports. `e` - engineering scale number (for example, 5.02m) `s` - scientific notation (for example, 5.02e-3)	`e`
	`sort_by_net=yes\|no`	Report IR and EM results per net, or all nets. `yes` - report EMIR results per net `no` - combine EMIR results or all nets into one report.	`yes`
	`power_gate_extra_report`	When specified, adds additional information in the `rpt_pwg` file about power gates. This option is used only for power-gated designs.	`none`
	`filter_ir_ threshold=`value	Defines the IR voltage drop threshold for the node being reported. `filter_ir_threshold=0.01` reports all nodes with IR drop above `0.01V`.	`no filter`
	`filter_ir_ percent=`value	Defines the percentage of nodes being reported starting from the biggest IR drop. For example, `filter_ir_percent=5` reports the top 5 percent IR drop nodes in the report.	`no filter`
	`filter_em_threshold=`value	Defines the EM analysis threshold value for the resistors being reported. The value for `filter_em_threshold` is the J/Jlimit value. `filter_em_threshold=1` reports only those resistors that have a J/Jlimit value above 1. Note: Specifying this option is equivalent to filtering all passed resistors.	`none`
	`filter_resistance=0.001`	Specifies that the shorting via resistors with the resistance value equal to or less than 0.001 ohm (1 mohm) are to be filtered out from the EMIR and SHE analysis reports.	`none`
	`geounit=`value	Defines the scaling of all DSPF geometry parameters (`W, L, X, Y)`. It applies only to the `*\|NET` section, and not to the `instance` section.	`1um`
	`geounit_XY`	Defines the scaling of DSPF geometry parameters X and Y. It applies only to the `*\|NET` section, and not to the `instance` section. Note: If the `geounit_XY` and `geounit` options are specified together, the `geounit_XY` option takes precedence over the `geounit` option.	`1um`
	`geounit_WL`	Defines the scaling of DSPF geometry parameters W and L. It applies only to the `*\|NET` section, and not to the instance section. Note: If the `geounit_WL` and `geounit` options are specified together, the `geounit_WL` option takes precedence over the `geounit` option.	`1um`
	`enableDesignResistorPeakFactor= [true \| false]`	Specifies the addition of the factor, `1/(r)^1/2`, in the current limit calculation for the AC-Peak analysis of the design resistor. The software, by default, calculates the current limit for the AC-Peak analysis of the design resistor using the following equation: `I_{peak_ac(limit)}= I_{peak_dc(limit)}` To apply the factor, `1/(r)^1/2`, in your calculation, set this variable to `true`. The current limit will then be calculated in the following manner: `I_{peak_ac(limit)}= I_{peak_dc(limit)}/(r)^1/2`	`false`
	`enableDesignResistorScaling=[true \| false]`	Enables the scaling of the width and length values based on the `layout_scale` factor specified in the technology file before the EM rules are applied for EM analysis of design resistors. By default, the scaling of design resistors is enabled.	`true`
	`enableResShape true \| false`	When set to `true`, enables tagging of shapes on the layout based on full resistor shapes and terminal nodes. This option is enabled by default. To disable tagging of shapes, set the variable to false. `emirutil enableResShape false`	`true`
	`enableRMSHotSpotWaiving=[true \| false]`	Enables the RMS EM hot spot waiving analysis. By default, this feature is disabled. This variable is applicable only to the RMS EM hot spot waiving feature, which is a limited-access feature. To use this feature, contact your Cadence representative and explain your usage requirements.	`false`
	`extendPWLMatch=[true \| false]`	When the EM rules are specified in terms of PWL and the width of metal or the area of via does not match with any width/area of the PWL, the EM limit will not be calculated for this metal resistor/via. When set to `true`, the software interpolates the limit value for the `resistor/via` from the selected rule PWL as follows: minimum of PWL `i^th` value * (metal's width or via's area) / (PWL `i^th` width or PWL `area`).	`false`
	`enablePWLDensityInterpolation=[true \| false]`	Enables the current density calculation from the given PWL using current density and width, or current density and area linear interpolation for either the metal's width or the via's area. The calculation is only done when the metal’s width or the via’s area does not match the PWL width or area values. `emirutil enablePWLDensityInterpolation=true`	`false`
	`viaCountResistance=[true \| false]`	This option is set to `true` when third-party DSPF with missing via count ($N) is used for EM analysis.	`false`
	`process_scale=`value	Specifies the value by which the width and length values will be multiplied before the EM rules are applied.	`1.0`
	`prioritizedPwlRulesLayers=[all \| none \|` list_layers`]`	Specifies the list of layers for which area-based PWL search is performed first. When no match is found, then non-PWL rules are used. The default value of this variable is `“all”`, which means that this behavior is enabled for all layers. To enable the behavior for specific layers, you can specify a list of layers. To disable this behavior for all layers, set the value of this variable to `none`. In the GUI, you can set this variable in the Variables form. Example rules: `em_jmax_dc_avg 10 jmax_factor 90 2.384 95 2.078` - non-PWL baseline rule `em_jmax_dc_avg PWL 0.3582 0.001444 0.5694 0.003364 0.7164 0.0038 jmax_factor 90 2.384` - PWL rule When both the above rules are specified, the second rule is given priority over the first.	`all`
	`via_count=[useR \| useArea]`	Defines the method used for calculating the via count. `useR` - calculation based on via resistance `(emdatafile_via_resistance/dspf_via_resistance).` `useArea` - calculation based on via area `(dspf_via_area/emdatafile_via_area).`	`useR`
	`idirn=[true\|false]`	Prints the current direction in the EM report (Current Direction column). For metal resistors, the current direction is printed. That is, W means that the current is flowing from east to west. For via resistors, the direction from/to layer is printed.	`false`
	`recovery_factor`	Defines the recovery factor for iavg calculation with recovery factor. If specified, then `iavg=max(\|iavgpos\|,\|iavgneg\|)-recovery_factor*min(\|iavgpos\|,\|iavgneg\|)`. If not specified, then `iavg=iavgpos+iavgneg`
	`Tlife=”hours” \| “years”`	Specifies the lifetime for which the EM analysis will be performed. You can specify the value in either `years` or `hours`. For example: `emirutil Tlife=”20000hours”`	`“10 years”`
	`emLimitScale=`scale_factor_value \| “scale_factor_netfile”	Scales the EM limits of the parasitic resistors in the design before generating the EM reports. You can either apply the same scale factor to all the nets or specify different scale factors for different nets. To apply the same scale factor to the parasitic resistors of all the nets in the design, provide the value of the scale factor. `emirutil emLimitScale=`scale_factor_value For example, `emirutil emLimitScale=0.04` Note: This is applicable to `avg`, `avg abs`, and `rms` analyses. For the `avg` and `avg abs` analyses, the limit is directly multiplied by this factor. For rms analysis, the limit is multiplied by the root of this factor. To apply different scale factors to different nets in the design, provide the name of the file that contains information about the net names and the corresponding scale factors to be applied to these nets. `emirutil emLimitScale=”`scale_factor_netfile” For example, `emirutil emLimitScale=“scaleLimitFile”`	`none`
	`rmsMetalLineNumberPower=`number	Specifies the value of power on the metal lines for RMS EM analysis of power nets. If this option is not specified, the default value of `0` is considered, which means the software uses the `em_dc_rms_metal_line_num` value specified in the ICT file. If, however, this option is specified, it overrides the `em_dc_rms_metal_line_num` value specified in the ICT file.	`0`
	`rmsMetalLineNumberSignal=`number	Specifies the value of power on the metal lines for RMS EM analysis of signal nets. If this option is not specified, the default value of `0` is considered, which means the software uses the `em_ac_rms_metal_line_num` value specified in the ICT file. However, if this option is specified, it overrides the `em_ac_rms_metal_line_num` value specified in the ICT file.	`0`
	`print_em_report`	Defines the EM analysis report file to be generated in the Voltus-Fi-XL flow. `filename`: create report with specified filename `net`: create report for specified nets - all power nets (`all_power`), all signal nets (`all_signal`), all nets (`all_nets`), or net (`netname`). `threshold` - create report for resistors or nodes that have a threshold value of EM ratio above the specified value `type` - create report for specified analysis type; `javg, jmax, jabsavg, jacpeak, jacrms, rc, rcavg, rcrms, tc, tcavg,` or `tcrms.` `rule` - specifies the custom EM rule for which the report should be generated
	`extendedreport=true \| false`	Specifies that the following information should be included in the EM analysis report file: `Td`: time duration in micro second or total ‘On Time’ period `dutyR`: duty ratio `I_limit`: current limit	`false`
	`extendedRMSReport=true \| false`	When set to `true`, the following parameters are reported in the RMS EM report: `rmsT`: Delta temperature value `Lv2v:` Distance between terminal vias `rmsMetalLineNumRelaxFactor`: It specifies the rating factor corresponding to the number of power on metal lines In addition, the following is added in the header section of the report: `rmsMetalLineNumber:` Specifies the value of power on the metal lines for RMS EM analysis	`false`
	`reportUnmatchedRuleResistor=true \| false`	When set to `true`, specifies that while generating the EM analysis reports, the resistors that do not match any EM rule for the specified analysis in the ICT file should be reported in the `“#.rpt_unmatch”` file.	`true`
	`reportAllResistor=true \| false`	When set to `true`, reports all resistors of the specified nets in the `“#.rpt_all”` file. If both, `reportUnmatchedRuleResistor` and `reportAllResistor`, are set to `true`, the `reportAllResistor` setting gets priority.	`false`
	`consolidatedReport=true`	Specifies that consolidated EM and IR reports for multiple bin files will be generated in Voltus-Fi-XL.	`false`
	`worstResult=true`	Specifies that the worst result will be reported in the consolidated EM and IR reports. This option is enabled by default when the `consolidatedReport` parameter is set to `true`. For example, `consolidatedReport=true` `worstResult=true` To view all the results in the consolidated report, set this option to `false`.	`true`
	`layer_filter=[layer1 layer2...]`	Specifies the layers that are to be filtered out from the EMIR analysis reports. For example, `emirutil layer_filter=[cont odcont]` If you have specified this option and also set the `reportAllResistor` option to `true`, the resistor information for the specified layers will be filtered out from the reports.	`none`
	`violation_columns=[`column_names`]`	Specifies the columns to be displayed in the Violation Browser. You can specify multiple columns separated by a space from the following list of columns: `LENGTH_COLUMN` `RESISTANCE_COLUMN` `VIA_AREA__COLUMN` `NEEDED_NUM_VIA_COLUMN` `NET_COLUMN` `WIDTH_COLUMN` `MIN_WIDTH_COLUMN` `DENSITY_COLUMN` `CURRENT_LIMIT_COLUMN` `CURRENT_COLUMN` `PEAK_TIME_COLUMN` `TAP_NAME_COLUMN` For example, `emirutil violation_columns=[LENGTH_COLUMN RESISTANCE_COLUMN]`	`All columns are displayed`
	`disableLayoutScale=true`	When set to `true`, disables the layout scale factor defined in the ICT file for Voltus-Fi-XL EM analysis. The layout_scale factor is the ratio of the scaled dimensions divided by the drawn dimensions. The ICT file is defined based on the scaled dimensions. Quantus applies the layout_scale factor to the input design during extraction so that the design dimensions and the ICT file dimensions are consistent.	`false`
	`simpleSingleViaDefinition=true \| false`	The keyword, `single` is used to differentiate between a single square cut via and square via array. It is applicable to square via, with width equal to '`vc_width`/`min_width`', only. To support the `single` keyword for all via sizes, set the `simpleSingleViaDefinition` parameter to `true`.	`false`
	`cdf_percentage=`value	The variable holds the value which is mapped to the `cdf_percentage` keyword in the EM rules specified in the ICT file or the technology file. The value of the `cdf_percentage` should be between 0 and 100. For example, `emirutil cdf_percentage=”10.0”`	`none`
	`device_temp_file=`filename	Specifies the file that includes information about resistor names and their corresponding temperature values. The EM analysis for these resistors is performed at their corresponding temperatures. For example, `emirutil device_temp_file=resistor_temp.txt`	`none`
	`toggleNetFrequency=”(`net1, frequency1`) (`net2, frequency2`) (`net#, frequency#`)`”	Specifies the frequency of the nets so that the tool can derive the `Td` (total on-time period) for multiple clock cycles. You can specify frequencies for different nets as shown below. Wild cards are also supported. For example, `emirutil toggleNetFrequency=”(CLK*,2.3e9) (NET1,4.6e9)”`	`none`
	`toggleNetFrequencyFile=`filename	Specifies the name of the file that contains the net names and their corresponding frequency values. This file is used to specify the frequency of nets to compute the `Td` (total on-time period) for multiple clock cycles. This file contains net names separated by commas and the frequency values. For example, `emirutil toggleNetFrequencyFile=freq_file` A sample `freq_file` is shown below. VDD, 2e08 D*, 4e08 GSS, 3e08	`none`
	`multiplePeakPercentThreshold=`value	Specifies the threshold percentage for the peak current above which the `Td` (total on-time period) for a particular peak is added to the final `Td`. This variable is applicable only when the `dynamicACPeak` analysis is set to `multiPeak`. For example, `emirutil multiplePeakPercentThreshold=7`	`5`
	`deltaT=`temp_value	Specifies the maximum rise in temperature in degree Celsius, caused due to Joule heating. It must be a positive value. If the rise in temperature is not specified, Voltus-Fi-XL considers a default temperature of 5 degrees Celsius. This is an ideal condition wherein the design must be EM free. Example: `emirutil deltaT=4.0` This option can also be specified in the Variables form and in the command file by using the `set_variable` command.	5.0 degree Celsius
	`deltaTLayers=[(layer=`layer_name `deltaT=`temp_value`) (layer=`layer_name `deltaT=`temp_value`)]`	Specifies layer-specific deltaT values. For layers that do not have deltaT value specified for them, global deltaT value will be used. Example: `emirutil deltaTLayers=[(layer=rhim hi_em=1 deltaT=25) (layer=rhim hi_em=0 deltaT=5) (layer=M7 deltaT=10)]` In the above example, `hi_em=1` indicates high current carrying design resistor for which the `deltaT` value is `25` degree Celsius while `hi_em=0` indicates general design resistor for which the `deltaT` value is `5` degree Celsius. The `deltaT` value for `M7` layer is `10` degree Celsius. This option can also be specified in the Variables form and in the command file by using the `set_variable` command.	`none`
	`resistor_filter=[`resistor_names`]`	Filters the specified resistors in the plot. You can specify multiple resistors separated by a space. These resistors will not be displayed in the plot. Wildcards are supported. Example: `emirutil resistor_filter=[rx ry]` or `emirutil resistor_filter=[rx*]`	`All resistors are displayed`
	`exclusion_resistor_filter=[`resistor_names`]`	Filters all resistors in the plot except those that are specified. This option is used to view plots for specific resistors. Wildcards are supported. Example: `emirutil` exclusion_resistor_filter`=[rx ry]` or `emirutil exclusion_resistor_filter=[rx*]`	`All resistors are displayed`
	`removeBulkShorting=true \| false`	When set to `true`, this option removes bulk-shorting in the design. Bulk-shorting in the design results in an increase in the EM analysis runtime. This variable is only used as a troubleshooting option. Example: `emirutil removeBulkShorting=true`	`false`
	`emVariableValues=[(variable=configA` value=#`) (variable=configB` value=#`)]`	Specifies the EM variable values for current density limit calculation in the EMIR configuration file. Example: `emirutil emVariableValues=[(variable=configA value=20) (variable=configB value=10)]` Where the values of configA and configB are 20 and 10, respectively. The EM variable values passed through the configuration file will get priority over the value of same variable specified in the techfile.	`none`
	`enableContextAwareSrmsRelaxation=true \| false`	When set to `true`, this option enables the context-aware RMS Relaxation flow. Example: `emirutil enableContextAwareSrmsRelaxation=true` This flow is foundry-specific. For more information, contact your Cadence representative.	`false`
`time`	`window=[start1 stop1 start2 stop2 ...]`	Time window to which the EMIR analysis is applied. Multiple none-overlapping windows are supported.	`[0 tend]`
`spf`	`aliasterm="alias library_terminal name"`	Alias used when DSPF instance terminal names do not match the cell terminal name in the libraries.	`none`
`spgs`	`net=[net1 net2 …]`	Enables static power grid solver, and defines power nets to be analyzed.	`none`
	`pwrgate=[powernet1 powernet2 …]`	Defines power gates to be analyzed in static power grid solver.	`none`
	`rshort=value`	Resistors with R<rshort are shorted during static power grid analysis.	0
	`tap2sub net=<net_name> include=[<tap_name>] exclude=[<tap_name>]`	Converts tap to subnode.	`none`
	`tap2pin net=<net_name> include=[<tap_name>] exclude=[<tap_name>]`	Converts tap to pin.	`none`
	`sub2tap net=<net_name> include=[<node_name>] exclude=[<node_name>]`	Converts subnode to tap.	`none`
	`sub2pin net=<net_name> include=[<node_name>] exclude=[<node_name>]`	Converts subnode to pin.	`none`
	`pin2sub net=<net_name> include=[<pin_name>] exclude=[<pin_name>]`	Converts pin to subnode.	`none`
	`pin2tap net=<net_name> include=[<pin_name>] exclude=[<pin_name>]`	Converts pin to tap.	`none`

In earlier releases, Voltus-Fi-XL 12.1 ISR 10 and before, the geounit* option was specified as follows: geounit* = 1e6 – when values in DSPF were in meter geounit* = 1 – when values in DSPF were in um From 12.1 ISR 11 release onwards, the behavior of the geounit* option is modified as follows to synchronize it with emirutil: geounit* = 1 – when values in DSPF are in meter geounit* = 1e-6 – when values in DSPF are in um

Every net statement only supports one name and one analysis definition. If different analyses are required, use multiple net statements.

The following example performs the EMIR analysis on the X1 instance. EM and IR analyses are performed on net VDD and VSS to measure vmax and iavg. EM analysis is performed on all other nets to calculate the irms value. The Current Density limits for the EM report are read from file ./em_dir/qrcTechFile.txt. In this release, only one instance is allowed for EMIR analysis per Spectre run.

Example EMIR control file (emir.config)

net name=[X0.VDD X0.VSS] analysis=[vmax vavg] 
net name=[X0.*] analysis=[iavg imax] emirutil techfile = qrcTechfile 
layermapfile = contactmapfile

emirutil deltaT=10.0

emirutil dbu=200

emirutil dynamicACPeak=false

emirutil applyRThreshold=0.05

emirutil rmsMultiplierPin=1.0

emirutil rmsMultiplierSignal=1.0

emirutil useEncryptedWidth=true

net design_res_models = [name=resTwoTerm   l=lr   w=wr   layer=mt2 unit=1e6]

solver method=[iterated]

Multiple net names must be specified in different lines in the control file to avoid any errors. This is shown in the above example.

Output of EMIR Analysis

As output, Voltus-Fi-XL produces the following:

Power-rail and signal IR drop and EM analysis result plots displayed on the Virtuoso layout
Power-rail and signal IR drop and EM analysis result reports
Structural analysis results displayed on the Virtuoso layout
Power-grid views

Return to top

Voltus-Fi Custom Power Integrity Solution XL User GuideProduct Version IC23.1, August 2023

3

Data Preparation