|
|
发表于 2008-5-11 22:03:45
|
显示全部楼层
Si9000 Transmission Line Field Solver
The Polar Instruments Si9000 Transmission Line Field Solver incorporates fast and accurate frequency-dependent PCB transmission line modelling. The Si9000 provides for both lossless and frequency-dependent modelling and extracts full transmission line parameters for a wide range of PCB transmission lines. The Si9000 uses advanced field solving methods to calculate PCB trace impedance for most single-ended and differential circuit designs. Based on Boundary Element analysis, the Field Solver is able to provide rapid modelling for a wide range of microstrip, stripline and coplanar structures.
Lossless calculations
The Field Solver provides for rapid calculation of single PCB trace impedance values against significant PCB parameters (e.g. trace height and thickness, dielectric constant, etc.) Given a target impedance the goal seeking functions of the Si9000 allow the user to calculate circuit parameter values to achieve the desired impedance.
For situations with structure dimensional constraints, the Field Solver allows the designer and board fabricator easily to accommodate variations in supplier material dimensions.
The Si9000 supports single or multiple dielectric builds in a comprehensive range of trace and dielectric configurations. The Si9000 provides models for structures with dielectric layers above and below traces, soldermask modelling and includes compensation for resin rich areas between traces.
Frequency-dependent calculations
Employing its Boundary Element Method field solving, the Si9000 extracts RLGC matrices and 2-Port (single-ended) or 4-Port (differential) S-Parameters and rapidly plots transmission line information for the structure under design. Graphing against frequency is provided for impedance magnitude, loss (conductor loss, dielectric loss and insertion loss), inductance, capacitance, resistance, conductance and skin depth. The Polar Si9000 runs within the Microsoft Windows environment and provides for simple transfer of table data to external programs such as spreadsheets or databases for subsequent analysis.
Extended substrate data
The Si9000 frequency-dependent calculations can be refined using extended substrate data. Users can assign substrate values by frequency band to accommodate material from manufacturers who specify parameters (e.g. Er and loss tangent) that vary by frequency.
Introduction to Controlled Impedance PCBs
The increase in processor clock speed and component switching speed on modern PCBs means that the interconnecting paths between components (i.e. PCB traces) can no longer be regarded as simple conductors.
At fast switching speeds or high frequencies (i.e. for digital edge speeds faster than 1ns or analog frequencies greater than 300MHz) PCB traces must be treated as transmission lines; i.e. for stable and predictable high speed operation the electrical characteristics of PCB traces and the dielectric of the PCB must be controlled.
One critical parameter is the characteristic impedance of the PCB trace (the ratio of voltage to current of a wave moving down the signal transmission line); this will be a function of the physical dimensions of the trace (e.g. trace width and thickness) and the dielectric constant of the PCB substrate material and dielectric thickness. The impedance of a PCB trace will be determined by its inductive and capacitive reactance, resistance and conductance. PCB impedances will typically range from 25Ω to 120Ω.
In practice a PCB transmission line typically consists of a line conductor trace, one or more reference planes and a dielectric material. The transmission line, i.e. the trace and planes, form the controlled impedance.
The PCB will frequently be multi-layer in fabrication and the controlled impedance can be constructed in several ways. However, whichever method is used the value of the impedance will be determined by its physical construction and electrical characteristics of the dielectric material:
The width and thickness of the signal trace
The height of the core or pre-preg material either side of the trace
The configuration of trace and planes
The dielectric constant of the core and pre-preg material
Impedance matching
Components themselves exhibit characteristic impedance so the impedance of the PCB traces must be chosen to match the characteristic impedance of the logic family in use.
If the impedance of the PCB traces does not match the device characteristic impedance multiple reflections will occur on the line before the device can settle. This can result in increased switching times or random errors in high-speed digital systems. The value and tolerance of impedance will be specified by the circuit design engineer and the PCB designer, however, it will often be left to the PCB manufacturer to conform to the designer's specification and verify that the finished boards meet the specification.
Calculation methods
The Si9000 incorporates field solving for single-ended and differential impedance structures. The discrete numerical analysis in the Si9000 uses Boundary Element Method to evaluate the residual field. A piecewise linear approximation is used with a weighted sub-division of the perimeter of the trace cross-section to predict the surface charge distribution on the trace. Having found the charge on a trace for a given voltage by the BEM method the capacitance is then simply calculated using the voltage and total trace trace charge (C=Q/V). This in turn allows the impedance of the structure to be calculated.
Transmission Line Structures
Microstrip and Stripline Transmission Lines
Controlled impedance PCBs are usually produced using microstrip and/or stripline transmission lines in single-ended (unbalanced) or differential (balanced) configurations.
A micro strip line consists of controlled width conductive traces on a low-loss dielectric (in practice the dielectric may be constructed from a single dielectric or multiple dielectric layers) mounted on a conducting ground plane. The dielectric is usually made of glass-reinforced epoxy such as FR-4. For very high frequencies PTFE may be used. Other reinforcement/resin systems are also available.
For close spaced differences on woven glass reinforced dielectrics, refer to application note AP139 on the Polar Instruments web site, www.polarinstruments.com.
There are several configurations of PCB transmission line:
Exposed, or surface, microstrip
Coated microstrip (coating usually solder mask)
Buried, or embedded, microstrip
Centred stripline
Dual (offset) stripline
Single-ended Transmission Lines
Single-ended transmission lines are the commonest way to connect two devices (i.e. a single conductor connects the source of a device to the load of another device). The reference (ground) plane provides the return path.
Note that in the diagrams the trace is trapezoidal in profile and width, W, refers to the trace width nearest the upper surface, W1 refers to the trace width nearest the lower surface.
More:
Surface Microstrip
Embedded Microstrip
Coated Microstrip
Offset Stripline
Surface Microstrip
In the diagram below (surface, or exposed, microstrip) the signal line is exposed (to air) and referenced to a power or ground plane. In the Si9000 structures are categorised according to the arrangement of the dielectric with respect to the trace (below or above the trace). The diagram below shows the surface microstrip structure using a single dielectric layer below the signal trace (designated 1B)
Surface microstrip with single dielectric below the trace
The diagram below shows the surface microstrip structure using two dielectric layers below the trace (designated 2B).
Surface microstrip with two dielectric layers below the trace
Embedded Microstrip
Embedded, or buried, microstrip is similar to the surface version, however the signal line is embedded between two dielectrics and located a known distance from the reference plane.
Embedded microstrip with two dielectric layers, one below and one above the trace
In this structure the two dielectrics are arranged one below and one above the trace (designated 1B1A). Embedding the signal line can lower the impedance by as much as 20% compared to an equivalent surface microstrip construction.
Coated Microstrip
Coated microstrip with single dielectric below the trace
Coated microstrip is similar to the surface version, however the signal line is covered by a solder mask. This coating can lower the impedance by up to a few ohms depending on the type and thickness of the solder mask.
Coated microstrip with two dielectrics below the trace
Offset Stripline
In this configuration the signal trace is sandwiched between two planes and may or may not be equally spaced between the two planes. This construction is often referred to as Dual Stripline.
A second mirror trace will be positioned H1 from the top ground plane. These two signal layers will be routed orthogonally (crossing at right angles so as to minimise the crossing area).
Differential Transmission Lines
The differential configuration (often referred to as a balanced line) is used when better noise immunity and improved timing are required. In differential mode the signal and its logical complement are applied to the load.
The balanced line thus has two signal conductors and an associated reference plane or planes as in the equivalent single-ended (unbalanced) case. Fields generated in the balanced line will tend to cancel each other, so EMI and RFI will be lower than with the unbalanced line. External noise will be "common-moded out" as it will be equally sensed by both signal lines.
Note that in the following diagrams (except the Broadside-coupled Stripline) the traces are trapezoidal in profile and width, W, refers to the trace width nearest the upper surface, W1 refers to the trace width nearest the lower surface.
More:
Edge-coupled Surface Microstrip
Edge-coupled Coated Microstrip
Edge-coupled Embedded Microstrip
Edge-coupled Offset Stripline
Broadside-coupled Stripline
Edge-coupled Surface Microstrip
Edge-coupled surface microstrip with single dielectric below the trace
In this construction the gap between the traces, S1, defines the coupling factor and hence the differential impedance. The etch factor, plating density and undercut will make this construction simple to manufacture, but with a wider tolerance due to the extra processing required on external layers.
Edge-coupled Coated Microstrip
Edge-coupled coated microstrip with single dielectric below the trace
As in the case of the Surface Microstrip this construction is simple to fabricate, but the extra process of adding solder mask coating can cause impedance variations. The Si9000 enables the operator to specify the thickness of the coating outside, above and between the traces to allow for variations in the board fabricating process.
This construction is particularly sensitive to solder mask flooding with LPI (Liquid Photo Imagable) solder mask. This causes the dielectric constant in the edge coupling region to vary, depending on flood depth.
Edge-coupled Embedded Microstrip
Edge-coupled embedded microstrip with one dielectric below and one above the traces
The reduced processing of internal layers makes the Edge-coupled Embedded Microstrip construction easy to fabricate with more consistent results than the equivalent surface trace structure. During the manufacturing process resin will be forced in between the traces resulting in a resin-rich region (shown as Rer in the 1B1A1R model below) between the two traces. This region will result in a dielectric with Er different from the rest of the structure.
Edge-coupled embedded microstrip with resin-rich region between the traces
Edge-coupled Offset Stripline
Edge-coupled offset stripline with one dielectric below and one above the traces
As in the case of the single-ended Offset Stripline construction this structure can be made up as a dual construction with a mirrored edge-coupled differential pair set a distance from the upper reference plane. The lower pair is routed orthogonal to the upper to minimise layer to layer coupling and cross-talk.
The model below shows a structure with two layers below the traces and one above and includes the resin rich region between the traces
Edge-coupled offset stripline structure modelling the resin-rich region between the traces
Broadside-coupled Stripline
Broadside-coupled offset stripline with two substrate dielectrics, H1 and H2
This apparently simple construction is actually one of the most difficult to fabricate to produce consistent impedance results.
Despite having internal layers with minimal processing, the most common structure is that with both traces overlaid for maximum coupling.
Inner-layer mis-registration and slight offsets and differences in etching combine to make this more difficult to achieve consistent results, particularly if the traces are fine-line.
Broadside-coupled offset stripline with three substrate dielectrics, H1, H2 and H3
The Si9000 broadside-coupled model assumes symmetry of dielectric in the two H2 and H3 layers — the two layers will normally be fabricated from the same material, i.e. with the same dielectric constant.
Note that in the Broadside-coupled Stripline case the traces are trapezoidal in profile and width, W2 refers to the trace width nearest the surfaces, W1 refers to the trace width nearest the center.
Using the Si9000 Field Solver
Si9000 screen areas
The Si9000 is divided into the following areas:
Menu/Toolbar – containing all the Si9000 commands and structure range select buttons
Structure Bar – displaying available structures within the selected range
Structure Graphic – displaying the selected structure; select the parameter by clicking on the parameter "hot-spot"
Lossless calculation
Calculation Interface – displaying structure parameters/tolerances and calculation/goal-seeking results
Calculation Options – allowing the user to select parameter units, standard or extended inteface style and goal seeking convergence (see Field solving for board parameters)
Frequency-dependent calculation
Frequency-dependent Calculation Interface – displaying frequency-dependent and structure parameters
Frequency-dependent Result Graph And Tables – displaying frequency-dependent results in graphical and tabular form
More:
Menu/Toolbar
Structure Bar
Structure graphic
Calculation Interface
Calculation Options
Frequency-dependent Calculation Interface
Frequency-dependent Result Graph And Tables
Menu/Toolbar
The Si9000 Menu contains all the Si9000 commands, the structure range select buttons and the SB200 Copy and Paste buttons.
Use theFile menu commands to save, recall and print results and the Edit menu to copy frequency-dependent tabular data via the Windows clipboard to a spreadsheet or database for analysis.
Use the Configure menu to set structure parameter minimum and maximum values and goal seeking convergence settings used by the calculation engine.
The Help menu contains the Si9000 license status and links to controlled impedance-related pages on the Polar Instruments web site.
Clicking each of the Toolbar structure buttons selects the associated range of controlled impedance structures (single-ended, differential, coplanar, etc.) for display in the Structure Bar.
Use the Copy and Paste buttons to exchange controlled impedance information with the SB200 PCB Stackup Builder.
Structure Bar
Use the Structure Bar to select a controlled impedance structure from the list of structures displayed. The range of structures displayed is controlled by the associated button on the Toolbar
Structure graphic
The Structure Graphic reflects the chosen controlled impedance. Click the parameter "hotspot" (the parameter label, H1, Er1, etc.) to select a parameter field for editing.
Calculation Interface
Use the Calculation Interface to enter and modify the structure parameters and tolerances, calculate impedance values and goal seek for parameter values for a target impedance.
Standard Interface
Extended Interface
Use the Extended Interface to apply tolerances to a calculation. The colored text fields indicate which parameter affects the minimum and maximum impedance values; e.g. consider the green colored fields – variations in the minimum value of Er1 affect the maximum value of impedance.
Calculation Options
Use the Calculation Options to specify the calculation units, interface style and goal seeking convergence settings.
Frequency-dependent Calculation Interface
Use the Frequency-dependent Calculation Interface to enter or modify parameter values used in frequency-dependent calculations. Use the Extended Substrate Data options to specify parameters by frequency range.
Frequency-dependent Result Graph And Tables
Use the Result Gaph and Table interface to view frequency-dependent calculation results in graphical and tabular form. Choose from the Display Series drop-down list for results for loss, impedance, inductance, resistance, capacitance, conductance and skin depth.
Setting Si9000 parameter limits
The Si9000 is designed to work with "real world" values. If the parameter values used in calculation are beyond the Si9000 limits, the Si9000 returns a value of zero. The user is able to control the range of values used by the Si9000 field solving engine during calculation.
Click the Configure menu; the Si9000 Configuration dialog is displayed.
Enter the values for minimum and maximum for each parameter and number of calculation iterations (Si9000 Field Solver Tries).
Lossless calculations
The Si9000 Field Solver allows the operator to perform rapid single calculations of PCB trace values against significant PCB parameters. The Si9000 Field Solver solves for impedance, propagation delay and inductance and capacitance per unit trace length.
Click the Si9000 Field Solver icon on the desktop to start the Si9000 Field Solver.
Click the Lossless Calculation tab
More:
Calculating single ended impedance
Calculating propagation delay, inductance and capacitance
Field solving for board parameters (goal seeking)
Using the Extended Interface
Calculating differential impedance
Calculating propagation delay, odd, even and common mode impedance
Calculating single ended impedance
Click on the structure type from the Structures Bar.
Select the dimension units (mils, inches, microns or millimetres) from the Units option group.
Enter the values for:
H1 (Height) — dielectric thickness
W1 and W2 (Width) — signal trace width (allowing for finished etch factor)
T1 (Thickness) — signal trace thickness
Er1 — dielectric constant
into the associated text boxes and press the Impedance Calculate button. The calculated impedance will appear in the Impedance (Zo) box.
Add explanatory notes on your particular construction, if necessary, in the Notes text box.
Calculating propagation delay, inductance
and capacitance
Click on the configuration from the Structures menu or from the Structures Bar.
Enter the parameter values as described above into the text boxes and press the More… button. For the Standard Interface single ended results are shown below
The Si9000 displays the results of propagation delay, inductance and capacitance in the selected units. Press Close to exit.
Field solving for board parameters (goal seeking)
The Field Solver can solve for board parameters given a nominal impedance value.
Enter the given board dimensions in their associated fields and the nominal impedance value in the Impedance field and click the Calculate button against the unknown dimension, e.g. Substrate 1 Height, Trace Width, etc.
Using the Extended Interface
Selecting the Extended Interface Style displays additional fields, Tolerance, Minimum and Maximum allowing the user to specify a range of values for each parameter and observe the effect of manufacturing process variations.
Fields which control the maximum impedance value are shown in green, fields which control the minimum impedance value are shown in orange.
In this example we specify a nominal impedance value of 80 ohms and observe the effects on the nominal impedance of a manufacturing variation of ±1mil in the substrate height.
Select the Extended Interface, enter a value of 80 ohms in the Impedance field and click the Substrate 1 Height Calculate button
The nominal Substrate 1 Height is calculated at 9.75 mil. Enter a value of 1mil in the Substrate 1 Height Tolerance field and click the Impedance Calculate button.
The Si9000 calculates the range of impedance for a 1mil variation in H1 as 76.27–83.40 ohms.
Other parameter tolerances can included as necessary. Enter a value of 0.5 in the Substrate 1 Dielectric Tolerance field and click the Impedance Calculate button. The impedance range should now show 72.71–87.91 ohms.
Calculating differential impedance
Calculating differential impedance is similar in technique to that for the single-ended models, but with the addition of trace separation or offset. For some models the dielectric constant of the separation region can be specified separately from the substrate dielectric constant bulk value.
Enter the parameter values and tolerances if required into their respective fields and Click Calculate; the Si9000 calculates the resulting impedance. Use the other Calculate buttons to goal seek for the parameter values required to return a target impedance.
Calculating propagation delay, odd, even and common mode impedance
For the Standard Interface clicking More… displays results for differential impedance include odd, even and common mode impedance.
Clicking More… on the The Extended Interface displays the range of results for the selected tolerances.
Saving and recalling results
Impedance calculation results for a board type or vendor, for example, may be saved to disk and recalled for future reference.
From the File menu choose the Save As… command. Choose a name and destination and press Save.
The program will only save calculated results.
To recall a set of results choose Open… from the File menu and choose the desired results file and press Open.
Printing results
Choose Print from the File menu to print a hard copy of the Si9000 Field Solver screen.
Frequency-dependent calculations
The Si9000 incorporates fast and accurate frequency-dependent PCB transmission line modelling, and extracts full transmission line parameters across its range of controlled inmpedance structures.
The Si9000 uses Boundary Element Method field solving to extract SPICE RLGC matrices and 2-Port S-Parameters for single-ended models or 4-Port S-Parameters for differential structures and provides high speed plotting of transmission line information for the structure under design.
The designer can choose graphing against frequency for impedance magnitude, loss (conductor loss, dielectric loss and insertion loss), inductance, capacitance, resistance, conductance and skin depth.
Click the Frequency Dependent Calculation tab; the Frequency-dependent interface is displayed.
Enter the frequency-dependent calculation parameters, loss tangent, minimum and maximum frequency, frequency steps, etc. and click Calculate.
Click the Graph tab and select the data series from the Display Series dropdown. The Si9000 displays results over the specified frequency range.
The graph below (All Losses) charts conduction loss, dielectric loss and insertion loss from 100MHz to 10GHz for a surface microstrip structure with the specified parameters.
To change the structure parameters, switch to lossless mode and modify values as required.
Select other data series and change parameters as required; the graph below shows the variation in impedance magnitude between 100Mhz and 1GHz
The graph below show the variation in skin depth between 100MHz and 10 GHz.
Using extended substrate tables
The Si9000 frequency-dependent calculations can be refined using extended substrate data. Users can assign substrate values by frequency band to accommodate material from manufacturers who specify parameters that vary by frequency. Manufacturers may specify, for example, differing values of Er across a range of frequencies, Er = 4.2 for frequencies up to 100MHz, Er = 4.15 from 100MHz up to 1GHz, Er = 4.1 from 1GHz to 10Ghz, etc.
More:
Choosing a dielectric layer frequency profile
Adding and modifying extended substrate data tables
Choosing a dielectric layer frequency profile
To choose a dielectric layer frequency profile, click the Edit button in the Extended Substrate Data screen area; the Extended Substrate Data dialog is displayed. Users may specify a frequency profile table for each dielectric layer.
Single dielectric layer
Multiple dielectric layers
Click the dropdown listbox arrow to display the list of available tables. For each dielectric layer choose a layer profile. Click Close.
To use the layer profile in frequency-dependent calculations ensure the Use Extended Substrate Data checkbox is ticked.
Adding and modifying extended substrate data tables
The Si9000 allows users to add or modify tables describing the frequency-dependent behavior of substrate material. In the table below Er decreases with frequency.
Adding a table
Click the Add Table button and choose a descriptive table name and click Add Table; the new table is added to the Extended Substrate Data Library.
Adding data to the table
Click the Add Entry button to add dielectric constant and loss tangent values for the lowest band of frequencies and click the Add Entry button. Repeat for each frequency band.
Each band is added to the table in ascending order of frequency. In this example the dielectric constant, Er decreases with frequency, but Loss Tangent, TanD remains constant.
Editing and deleting table data
To delete an entry in the table click into the data row and click the Delete Entry button. To change the data values in a table entry click into the table row and click Edit Entry; modify the values as required and click Edit Entry.
To use the new table, select the table from the dropdown list in the Set Extended Substrate Data Tables section of the dialog.
Viewing the Si9000 data tables
The Si9000 makes a comprehensive range of data for the selected structure available in a convenient tabular form.
Once calculation is complete, in single-ended mode click on the associated tab to view the Single-Ended, SPICE RLGC or 2-Port S-Parameter data.
Single-ended mode data
For differential models the Si9000 provides data for Odd and Even Mode, SPICE RLGC, and 4 Port S-Parameters.
Differential mode data
Copying Field Solver data to external programs
Selecting this command from the Edit menu takes the current results from the Field Solver and locates them on the Windows clipboard.
The result tables may then be pasted to a suitable location in a spreadsheet or database. For a spreadsheet the values are inserted beginning at the active cell location. The number of cells required depends upon the structure chosen. Ensure no important data are overwritten in the process. |
|
IP卡
狗仔卡
提升卡
置顶卡
沉默卡
喧嚣卡
变色卡
显身卡