2DTL

Home: Modeling2D (TL)

The Transmission Line Modeling method parses a single trace or a group of traces and divides them into a finite number of straight segments. For each segment the program checks for any conductive areas surrounding the traces which may serve as reference conductors.  All traces in a segment, in combination with additional reference areas, define its cross-section. The primary transmission line parameter per unit length (R’, L’, C’, G’) will be calculated by a static 2D field solver. In a following step all segments will be transformed into an equivalent circuit. The procedure even considers vias and creates related equivalent circuits as well. Finally all circuits will be connected together into one single electrical model representing the whole trace or group of traces.

The procedure implies that only TEM propagation modes can be considered and this causes a limitation. The model is only valid in a frequency range from DC to a maximum frequency. This is due to the fact that the primary transmission line parameters are static parameters and only valid when the geometric dimensions behind the 2D field calculation are significantly smaller than the shortest wavelength of the propagating wave. The method is best used in the classical SI analysis where wave propagation effects on signal lines into high-speed multi-layer boards have to be analyzed. The method assumes ideal power delivery systems and does not take into account any effects like ground bouncing.

The figure below shows the dialog box for the 2DTL solver. It consists of three separate tabs for Selection, Meshing and Modeling. In the upper left corner the number of currently Selected nets is shown. At the right hand side there is the field Length units which allows to select a certain unit. Changing the unit does not affect any dimensions.

 

Number of elements

The frame is folded by default and has to be expanded by clicking on the +-sign first. It  includes information which is generated during the meshing process (see 2DTL Meshing tab).

 

Selection tab

The Selection nets frame  includes all selected nets which should be meshed and transformed into an equivalent circuit model. The nets have to be selected in the Navigation Tree or in the Main View. In addition, the Insert model frame includes a list of those components (must be a passive two-pin device, see Passive Device Modeling) which are connected between the selected nets on the left column. The components are found automatically and the choice does only depend on the list of selected nets.

 

 

The toolbar above the Selected nets frame provides buttons to select and de-select nets:

 

Pin activating / deactivating: A net in the Selected nets list can be further expanded by clicking on its +-sign. After an expansion all Component pins, that the net is connected to,  will be displayed as can be seen in the figure below:

 

 

By default, those pins which are not connected to any component on the right side are checked and every checked pin will appear in the schematic symbol of the equivalent circuit as shown in the figure below:

 

 

If the user wants to control the visibility of a pin he just have to activate or de-activate the corresponding button. In the example below the pins IC201-36 and IC203-36 are de-activated and the pin R706-7 is activated:

 

 

After another modeling step the corresponding schematic symbol will look like in the figure below:

 

 

In order to activate or de-activate all pins of a certain net at once, the user can select the corresponding net in the Select net list, perform a right-mouse-click and choose either Include All or Exclude All.

 

Insert model for:

PCBS automatically looks for passive two-pin components which are connected between the nets listed in the Selected nets frame. The found components are stored in the Insert model frame on the right hand side of the dialog box. This feature provides a convenient way to generate reasonable equivalent circuits for a signaling path even if the path is separated in different nets. As a prerequisite of course, an appropriate electrical model has to be assigned to the component (see: Component Modelling).

The figure below shows a resistor (actually a resistor array) that separates two selected nets:

 

 

By default, the components in the Insert model frame are checked as shown in the figure below:

 

 

If a component is checked its equivalent circuit will be inserted within the equivalent circuit of the overall signal path. The generated schematic block will look like in the figure below (assumed that the corresponding pins inside the Selected nets frame were left unchecked):

 

 

If a component is de-activated by the user the corresponding pins in the Selected nets frame will be automatically activated as shown in the figure below:

 

 

 

The corresponding schematic block will look like in the figure below. There are two further pins (R706_2 and R706_7) where the user can connect a separate equivalent circuit of a resistor (see Passive First Order Modeling):

 

 

 

2DTL Meshing tab

The Meshing tab enables the user to enter all settings which are necessary to divide the selected nets into a group of straight segments. The figure below shows the meshing tab:

 

 

Search distance for coupling:

Parallel segments of different (but selected) nets are considered electromagnetically coupled if their distance is smaller than the given Search distance for coupling. The larger this parameter is the more sections will be coupled.

 

Minimum length for coupling:

Parallel segments must have a certain minimum length to be accepted for an electromagnetic coupling. The smaller the value is the more sections will be coupled.

 

Use legacy via model:

If traces of a selected net are on different layers they are connected by a via. In order to account for such a discontinuity,  the program adds a corresponding via model inside the sequence of the trace models (see Cross section models). Two different modeling approaches for vias are available: The legacy via model is a simple series R/L circuit representing the ohmic and inductive behavior of the vertical via tube. The advantage is its simplicity - fewer additional circuit elements have to be added. The disadvantage is that the approach is only accurate for frequencies below about 1 GHz. For a higher frequency the user is recommended to tag off the legacy via model option. In this case, a more sophisticated kind of via modeling technique will be used.  Here, the via model consists of a series of short modal models (see Modal models) which were derived by a former 3D full wave analysis and stored in an internal data base. These via models are valid up to a frequency range of about 20 GHz.

 

Consider padshapes:

From the high frequency point of view , the spot where a trace ends in a Pad forms a discontinuity. If the button is tagged off this discontinuity will be ignored. The advantage is that the overall size of the model does not grow. If the button is activated, the program internally converts the Pad in an Area (see Areas). As a consequence, the widening step from the trace onto the Pad is considered and the corresponding discontinuity effect is accounted for.

 

Consider meander interaction:

In general, all conductive segments which are parallel and within the specified Search distance will be electromagnetically coupled during the 2DTL modeling process. In case of  a meander structure, segments of the same nets often run in parallel and their mutual coupling can have an erroneous impact on the delay time of the structure. If the field Consider meander interaction is de-activated electromagnetic coupling between segments that belong to the same nets will be not considered.

 

Open ended terminals frame:

This frame is folded by default and has to be expanded by clicking on the +-sign first. It lists all open ended terminals which were found during the meshing process - the same open ended terminals are searched and displayed after a PCB Layout Check. The number of open-ended terminals is also shown inside the Number of elements frame at the top of the dialog box.  An open ended terminal is an end of a net which does not belong to a pin of a Component.  There may be good reason for such non-connected terminals, but they can also occur due to a broken net which is actually not intended by the user. Therefore, it is recommended to check this list before going ahead with the modeling process.

 

Cross sections frame:

This frame is folded by default and has to be expanded by clicking on the +-sign first. It lists the cross-sections of all segments which were produced during the meshing process:

 

 

All generated segments are numbered and the corresponding number of a specific segment appears as the first of  two numbers in the name. Segments with a similar cross-section will be combined automatically by the program in order to save calculation time for the 2D field calculation process. Which segments belong together is marked by the second number in the name. In the figure above the first four cross-section belong together, because they all have the same second number (15) in their name. The number of all cross-sections (TLSections) and the number of the remaining cross-sections (TLSections after combination) are also shown inside the  Number of elements frame at the top of the dialog box.

By double-clicking on a certain item in the list the corresponding cross-section geometry will be displayed in a separate window as shown in the figure below. As long as this separate window is not closed it allows the user to look at different cross-sections by simply selecting the corresponding items in the Cross sections list.

 

 

Start Meshing:

Starts the meshing, which means the generation of straight segments with their corresponding cross-sections.

 

Show Mesh:

If this button is activated the corresponding straight segments are highlighted in the Main View as shown in the figure below:

 

 

View mesh text:

Displays the corresponding names to each segment as shown in the figure below:

 

 

Hide layout:

Allows the user to hide the underlying layout geometry.

 

2DTL Modeling tab

Within the Modeling tab all necessary parameters to control the generation of an equivalent circuit can be entered and the modeling process itself can be started.

 

 

Ohmic losses:

Decides whether the conductivity of the conductor materials  shall be taken into account or not. If this button is activated the frequency dependent skin-effect on the transmission lines is taken into account (see Ohmic loss modeling) .

 

Dielectric losses:

Decides whether the loss angle of the dielectric materials shall be taken into account or not.  If this button is activated the frequency dependent dielectric loss is taken into account on basis of a broadband Debye model (see Dielectric loss modeling) .

 

Allow modal models:

The standard way of modeling transmission lines is to use a series of segments consisting of so called lumped elements, which model the primary transmission line parameters per unit length R', L', C'. The corresponding geometric length of a single segment is chosen by the program in such a way that its length will be significantly smaller than the smallest wave length given by the field Model valid up to frequency. The shorter the segments are the better the approximation of the transmission line effect is. The right choice of the segment length has an serious impact on an important transmission characteristic: the phase velocity or transmission delay. The internal rule is: a segment must have a maximum length of 1/20th. of the smallest wave length.

If the meshing provides electrically long segments (e.g. since the transmission lines on the PCB are not interrupted) it is more accurate to use modal models instead of lumped elements. Modal means the transmission line is not modeled by its primary transmission line parameters but by its secondary parameters wave impedance Z and transmission delay t. A simple modal model consists of two resistors on each side modeling the wave impedance Z. In addition, there are two controlled voltage sources on both sides: the voltage source on one side at time point "t" is controlled by a voltage which existed at time "t-t" on the other side of the transmission line.

 

 

There are two important advantages of the modal model: First, the transmission delay is an essential characteristic of the model and has not to be approximated as is the case for the lumped element model. Therefore, the modal model is more accurate than the lumped element model in any case. Second, a modal model needs only one single segment to describe the whole transmission line, no matter how long the transmission line actually is. Therefore, the modal model leads to less complex models in case of electrical long transmission lines.

The disadvantage of modal models may be an increased simulation time during a transient analysis, when even very short segments are modeled by modal models, too. This is because the maximum time step during a transient task must not exceed the transmission delay of the shortest modal model (otherwise the model's delay characteristic wouldn't be resolved.) If the button Allow modal models is activated the program looks for segments which equal or exceed the minimum wave length (specified by the field Model valid up to frequency) and models them as modal models. The remaining, electric short segments will be still modeled as lumped models.

 

Consider wire bond models:

Decides whether bonding wires should be considered or not. In general, a bond wire is modeled as a simple series R/L circuit representing its ohmic and inductive behavior.

 

Model valid up to frequency:

Defines the frequency up to which the equivalent circuit must still be valid. This value influences the internal size of the equivalent circuit (the number of lumped elements and the number of additional elements due to the modelling of ohmic and dielectric losses). Therefore, this frequency limit should always be chosen only as high as necessary.  Note: Due to the underlying static 2D method which generates the corresponding transmission line parameters for the segments, there is a general upper frequency limit that couldn't be exceeded. This general limit is given on account of the segment's cross-section dimensions which aren't allowed to exceed a certain fraction of the wave length of the correspondent maximum frequency. If the user's chosen maximum frequency can not be reached the program puts out a warning in the Message Window.

 

The  Options frame is folded by default. It includes some additional modeling parameters:

 

Accuracy (inside Options frame):

Controls the accuracy of the static 2D field calculation for the extraction of the transmission line parameters. Four values are available:

Signal type of unselected nets (inside Options frame):

If additional nets are detected within the specified search distance they must be assigned to any of the two available types:

Signal type of neighbouring areas (inside Options frame):

Defines how detected areas shall be interpreted:

Approximate signal lines as flat:

If the button is activated the height of the traces will not be taken into account during the static 2D calculation.

 

The Export model frame is folded by default. It allows the user to export the generated equivalent circuit into a SPICE compatible sub-circuit:

 

Export to file  (inside Export model frame):

Specifies the directory and the file where the sub-circuit should be written

 

Model name  (inside Export model frame):

Specifies the name of the sub-circuit

 

Simulator  (inside Export model frame):

Enables the user to select a specific SPICE format:

Export Model:

This button starts the export