Substrates in Momentum

A substrate definition describes the media where a circuit exists. An example is the substrate of a multilayer circuit board which consists of layers of metal traces, insulating material, ground planes, vias that connect traces, and the air that surrounds the board. A substrate definition enables you to specify properties such as the number of layers in the substrate, the dielectric constant, and the height of each layer for your circuit.

A substrate definition is made up of substrate layers and metallization layers . Substrate layers define the dielectric media, ground planes, covers, air or other layered material. Metallization layers are the conductive layers in between the substrate layers, and they are used in conjunction with the layout layers. By mapping layout layers to metallization layers, you can position the layout layers that your circuit is drawn on within the substrate. An example of a substrate is shown below. It contains four substrate layers and two microstrips with a via.

Substrate definitions can be saved and used with other circuits. A variety of predefined substrates are included with Advanced Design System, which can be used "as is", or modified to your design specifications.
The steps for defining a substrate include:

• Defining the substrate layers
• Mapping the layout layers to metallization layers
• Specifying metallization layer conductivity
• Solving the substrate

Details on how to work with existing substrate definitions and create new ones follow.

Selecting a Predefined Substrate

Momentum includes a number of predefined substrate definitions, so it may not be necessary to create a substrate from scratch. Substrate files end with the extension .slm .
To open a predefined substrate:

1. In the layout window, select Momentum > Substrate > Open.
2. If you want to open a supplied substrate, click Yes . A list of supplied substrate files appears.
   If you want to open a substrate that has been saved as part of the project, click No. A list of substrate files that are saved as part of the project appear.
   For more information on locating substrate files, refer to To save a named file, choose Momentum > Substrate > Save. Identifying Where Substrates are Saved.
3. Select the substrate file, then click OK .

Creating/Modifying a Substrate

This section provides information about creating, modifying and editing a substrate. For information on metallization layers, refer to Defining Metallization Layers.

Defining Substrate Layers

You can define a substrate from scratch or edit an existing one. A substrate must have, at the minimum, a top plane and a bottom plane.

Note Do not use substrate components that might appear on layout component palettes. You must use the dialog box under Momentum > Substrate > Create/Modify to create or edit substrate definitions.

To define substrate layers:

1. Choose Momentum > Substrate > Create/Modify .
2. If this is a new definition, three default layers appear in the Substrate Layers Field:
   • Free_space (top plane)
   • Alumina (dielectric)
   • GND (bottom plane)
     These layers represent a basic substrate definition that includes the three types of substrate layers in Momentum.
   • Free_Space represents the top plane of the substrate. In this definition, it is defined as an open boundary .
   • Alumina represents a dielectric layer of finite thickness. These layers are also referred to as interface layers .
   • GND represents the bottom plane of the substrate. GND defines a closed boundary .

     Closed boundaries define ground planes or other closed boundaries, such as the lid or bottom of an enclosure.

     For an existing substrate definition, you may see more layers with different names, but they will all be one of these three basic types of layer, and the substrate will have a top and bottom plane. A substrate definition must have a top plane and a bottom plane, and these planes can be defined either as open boundaries or closed boundaries.

3. Select the layer of interest.
4. To create a substrate, you will edit these layers, rename them, and add to them as desired. More information on how to perform these tasks is detailed in the following sections.
5. When you are finished defining the substrate, click OK to dismiss the dialog box.

Defining an Open Boundary

An open boundary represents a layer of infinite thickness, such as air. An open boundary can be used to define other gases or infinitely-thick materials by editing the relative permeability and permittivity values of the boundary.
To define an open boundary:

1. Select the Free_Space layer or another open boundary layer.
2. Select Open from the Boundary list.
3. From the Permittivity (Er) listbox, select a format for the relative permittivity of the boundary. You can enter the components of relative permittivity as:
   • Real and imaginary
   • Real and loss tangent
   • Real and conductivity, conductivity in Siemens/meter
     The real portion of the relative permittivity, , is a dimensionless quantity and is identical to the material's relative dielectric constant, . For more information on this parameter, refer to Dielectric Permittivity.
     To represent a dielectric that dissipates the power of a high-frequency electric field, enter the dielectric loss tangent, , of the material in the Loss Tangent field. The smaller the loss tangent, the less lossy the material. For more information on this parameter, refer to Dielectric Loss Tangent.
     Enter the components of the relative permittivity in the fields below the listbox.
4. From the Permeability (MUr) listbox, select a format for the relative permeability of the boundary. You can enter the components of relative permeability as:
   • Real and imaginary
   • Real and loss tangent
     The real portion of the relative permeability, , is a dimensionless quantity and is identical to the material's relative permeability constant. For more information on this parameter refer to Dielectric Relative Permeability.
     To represent a dielectric that dissipates the power of a high-frequency magnetic field, enter the magnetic loss tangent, , of the material in the Permeability Loss Tangent field. The smaller the loss tangent, the less lossy the material. For more information on this parameter, refer to Dielectric Magnetic Loss Tangent.
     Enter the components of the relative permeability in the fields below the listbox.
5. Click Apply to accept the open boundary definition.

   Hint You can create a ground plane from a open boundary layer by selecting the layer and choosing Close from the Boundary list.

Defining an Interface Layer

Interface layers have finite thickness, and they can be characterized using relative permittivity and permeability values. The thickness of a layer can be an arbitrary value, with these considerations:

• Thin substrates are substrates less than one micron in thickness, and they require special meshing considerations. Substrates less than 0.1 micron should be avoided.
• Thick substrates should be less than 0.5 wavelength in thickness. The recommendation for thick substrates is based upon typical design values. For example, a 10 mil substrate with a cover height (air) of 300 mils would be acceptable for frequencies up to 20 GHz, which is 0.5 wavelength.
  To edit an interface layer:

1. Select the Alumina layer or other interface layer of interest.
2. Enter the thickness of the layer in the Thickness field and select the appropriate units in the adjacent listbox.
3. From the Permittivity (Er) listbox, select a format for the relative permittivity of the boundary. You can enter the components of relative permittivity as:
   • Real and imaginary
   • Real and loss tangent
   • Real and conductivity, conductivity in Siemens/meter
     The real portion of the relative permittivity, , is a dimensionless quantity and is identical to the material's relative dielectric constant, . For more information on this parameter, refer to Dielectric Permittivity.
     To represent a dielectric that dissipates the power of a high-frequency electric field, enter the dielectric loss tangent, , of the material in the Loss Tangent field. The smaller the loss tangent, the less lossy the material. For more information on this parameter, refer to Dielectric Loss Tangent.
     Enter the components of the relative permittivity in the fields below the listbox.
4. From the Permeability (MUr) listbox, select a format for the relative permeability of the boundary. You can enter the components of relative permeability as:
   • Real and imaginary
   • Real and loss tangent
     The real portion of the relative permeability, , is a dimensionless quantity. For more information on this parameter refer to Dielectric Relative Permeability.
     To represent a dielectric that dissipates the power of a high-frequency magnetic field, enter the magnetic loss tangent, , of the material in the Permeability Loss Tangent field. The smaller the loss tangent, the less lossy the material. For more information on this parameter, refer to Dielectric Magnetic Loss Tangent.
     Enter the relative permeability components in the fields below the listbox.
5. Click Apply to accept the layer definition.

Defining a Closed Boundary Layer

A closed boundary represents a plane, such as a ground plane. It is a layer with zero thickness. It can be defined as a perfect conductor, or you can specify bulk conductivity or sheet impedance to characterize it as a lossy conductor.
To edit a ground plane:

1. Select the ///GND/// layer of interest.
2. Select Closed from the Boundary list.
3. From the Plane listbox, select a format for the ground plane. You can specify the ground plane using these parameters:
   • Perfect conductor
   • Bulk conductivity in Siemens/meter
   • Sheet impedance in Ohms/square
     Conductivity is entered as a real number. Impedance is entered as the real and imaginary components of a complex value.
     Enter the ground plane parameters in the field below the listbox.
4. Click Apply to accept the closed boundary definition.

   Hint You can create an open boundary layer from a ground plane by selecting the ground plane and choosing Open from the Boundary list.

Renaming a Layer

To rename a layer:

1. Select a substrate in the Substrate Layers list.
2. The name appears in the Substrate Layer Name field. Edit the name as desired.
3. Click Apply .

   Note A ground plane is identified as ///GND/// and its name cannot be changed.

Deleting, Adding, and Moving Layers

To organize your substrate layers in the correct order, you can delete, add, and move layers.
To delete a substrate layer:

1. Select a substrate layer in the Substrate Layers list.
2. Click Cut. The layer definition is deleted.
   To add a substrate layer:
3. Select a substrate layer in the Substrate Layers list that has the same basic property (open boundary, closed boundary, or finite thickness) as the layer you are adding.
4. Click Add .
5. The new layer is highlighted. To rename the new layer, edit the Substrate Layer Name field.
   To move a substrate layer:
6. Select the substrate layer that you want to move from the Substrate Layers list.
7. Click Cut.
8. Select the substrate layer that you want positioned below the substrate that you are moving.
9. Click Paste.

Defining Silicon Substrate Layers

The electrical behavior of Silicon material is usually specified using the dielectric constant and a resistivity (or conductivity value).
For the dielectric constant, a value for of 11.8 (11.9 is usually used).
Resistivity ( ) values are normally specified in ohm cm, and a typical value is 10.
In Momentum, you can specify the conductivity ( ) in S/m (inverse of the resistivity).
For more information, see Dielectric Conductivity.

Calculating Conductivity from Resistivity

Conductivity is simply the inverse of resistivity. Make certain that the units of resistivity are ohms m before inverting.
Example:

1. = 10 ohm cm
2. = 10 ohm cm = 0.1 ohm m
3. = 1/rho = 10 S/m

Defining Conductivity

To define conductivity for silicon substrates:

1. Choose Momentum > Substrate > Create/Modify .
2. In the Create/Modify dialogue box, select RE, Conductivity under Permittivity (ER) .
3. Specify the substrate dielectric constant and conductivity (S/m).
4. When you are finished, click OK to dismiss the dialog box.

Defining Metallization Layers

Metallization layers enable you to:

• Define the position of layout layers in the substrate
• Specify which parts of the layer are conductive
• Define the conductivity of the layout layers
  In order to identify which areas of a layout layer are conductive, a layer can be specified as:
• Strip-The objects on the layout layer are conductive, the rest of the layer is not
  
• Slot-The inverse of a strip, the objects drawn on the slot layout layer are the opposite image of the metals, hence they are not conductive, but the rest of the layer surrounding the objects is conductive. When simulated, Momentum considers the electric field distribution (the equivalent magnetic current flow) in the slot.
  

  Note Conductivity in slot metallization is ignored and perfect metallization is assumed.

• Via-The objects on the layout layer are conductive and cut vertically through one or more substrate layers. For more information on how to draw and apply vias, refer to Applying and Drawing Vias in Layout.

Some examples of using strips and slots include:

• The patches of the Double_Patch antenna example. They are drawn on the layout layer named top_met, and are conductive. This layout layer is mapped to a metallization layer that is defined as a strip.
• The slots of the Slot_dipole antenna example. The slots are drawn on the layout layer named slot. The slots are not conductive, but the area surrounding the slots is. This layout layer is mapped to a metallization layer that is defined as a slot.

Note that a layout can have many other layers that are not part of the actual circuit, such as text or error reporting layers. For the purposes of an Momentum simulation, they are ignored. If layout layers containing parts of the circuit are not mapped to metallization layers, they are ignored as well.
The steps for defining metallization layers are:

• Mapping a layout layer to a metallization layer
• Defining the conductivity of the layer
• Setting overlap precedence

Details for performing these steps are presented in the following sections.

Applying and Drawing Vias in Layout

Momentum creates a via by extruding the object that is mapped as via through the substrate layer it is applied to. Vias are drawn as lines or closed polygons. A simple line segment via is the simplest and most practical way of drawing a via. Vias drawn as lines are often called sheet vias because, when the line is extruded through the substrate, it is treated as a horizontal metal sheet. For vias of other shapes, you draw a closed polygon. So, for example, for a cylinder via you draw a circle. When the shape is mapped to a via metallization layer in Momentum, another dimension is added to the object in order for the shape to cut through the substrate. Thus a line becomes a sheet, a circle becomes a cylinder.

Regardless of how you draw vias, avoid having them extend over the sides of the objects that they connect to. Vias must be on the edge or inside the object. Any portion of the via outside of the object boundaries will not be taken into account during the simulation. The figure below illustrates various vias connecting two strips.

Vias are treated in the following manner:

• Vias are represented as infinitely thin vertical sheets of metal. If a cylinder is drawn as a via, then it is also treated as separate sheets of metal that comprise the cylinder walls.
• Vias are assumed to be opened, not covered, with current traveling on the sheet. Vias can be drawn as covered, using a cap (cover) of the same size as the via end, which is a terminating metal strip layout layer.
• A via cannot be coincident with another via if they cut through the same substrate layer and they are on different layout layers. But two vias can be coincident on the same layout layer.
• Vias should be wholly contained within any primitives that are to be connected.
• Vias can be specified with loss but are considered to have zero thickness.

Vias through Multiple Substrate Layers

Vias can be applied to multiple layers so that they cut through one or more layers.
When drawing vias that cut through multiple substrate layers, each via must be drawn once on a single layout layer. This layout layer must then be mapped as Via to each substrate layer that the via cuts through (using the Metallization tab) to assign the via layer to all substrate layers.

Mapping a Layout Layer

Layout layers that contain any shapes or components that are part of the circuit must be mapped to metallization layers. If layout layers are not mapped to metallization layers, they will not be included in the simulation.

To map a layout layer:

1. Choose Momentum > Substrate > Create/Modify .
2. Click the Metallization Layers tab.
3. Select a layer from the Layout Layers list box. Note that the layout layer default cannot be mapped to a metallization layer, the first valid layer is cond .
4. To map the layer as a slot or strip, select from the Substrate Layers list a dashed line to position the slot or strip in between two substrate layers, then click Strip or Slot.
   If you make a mistake, click Unmap , then click the correct choice.
   • A Strip defines the objects on the layout layer as conductive, the area surrounding the objects is not.
   • A Slot is the inverse of a strip, it defines the objects on the layout layer as not conductive, but the area of this layer surrounding the objects is conductive. When simulated, Momentum considers the electric field distribution (the equivalent magnetic current flow) in the slot.

     Note Conductivity in slot metallization is ignored and perfect metallization is assumed.

5. To map the layer as a via, select the substrate layer that you want the via to cut through, then click Via.
   If you want the via to cut through more than one layer, select the next layer, then click Via again.
   • A Via defines the objects on the layout layer as conductive and they vertically cut through one or more substrate layers.
6. To define the conductivity characteristics of this layer, refer to Defining Conductivity.
7. If you have or suspect that you have overlapping layers, you need to set overlap precedence. Refer to Setting Overlap Precedence.
8. Click the Apply button.

Unmapping a Layer

If you want to change the location of a layer or remove one from the substrate definition, use Unmap.
To unmap a layer:

1. Choose Momentum > Substrate > Create/Modify.
2. Click the Metallization Layers tab.
3. In the Substrate Layers list, select the substrate layer or the interface where the layout layer is mapped.
4. Click Unmap. This removes all layout layers assigned to this position.
5. To remap a layer, refer to the steps in Mapping a Layout Layer.

Via Simulation Models

There are three simulation models available for via objects in Momentum in ADS 2006A:

• 2D Distributed Model
• Lumped Model
• 3D Distributed
  Of these, both the Lumped Model and the 3D Distributed Model are new for ADS 2006A. The Lumped Model can be used to more efficiently simulate contact via's (the main purpose of which is to provide electrical or mechanical contact). The 3D Distributed Model yields a full 3D modeling of all the components of the via currents (including the horizontal via currents) and can be used to more accurately simulate the electrical behaviour of signal via's.

2D Distributed Model

• The default via model (available in prior releases).
• A distributed model for the via object is created by meshing the surface with rectangular cells
• Only the vertical component of the via current is modeled, using vertical oriented rooftop functions. Hence, the modeled current distribution of the vertical component varies both in the cross-section and in the vertical direction (2D current distribution).
• Each via object contributes two unknown currents per rectangular cell to the matrix equation
• The via resistance and skin effect are included using the sheet surface impedance formulation
• The via self and mutual inductances (vertical currents only) and capacitances are included in the simulation.
  

Lumped Model

• The via objects are extracted from the structure and replaced by a lumped model.
• All branches in the distributed via network topology are removed and replaced by a single lumped branch, connecting the center bottom and top cell of the via object.
• Each via object contributes only one extra unknown to the matrix equation, the lumped via current, which has only a vertical component with a constant amplitude.
• A lumped series R, L impedance is used as electrical model in the simulation of the via.
• The resistance R and inductance L of the via are automatically calculated from the geometry and the material parameters.
• The mutual inductances are NOT included.
• The self and mutual capacitances are NOT included.
• The via cells do NOT contribute to the matrix equation load process.
  
  The internal impedance (resistance and internal inductance) of the via follow from the application of the surface impedance concept for a uniform vertical current distribution on the via. That is, we have:
  
  For via mask layers specificed by a conductivity, the surface impedance Zs is calculated using the single-sided skin effect formula. Hence, the frequency dependent skin effects (yielding a higher resistance and a lower internal inductance as frequency increases) are included in the lumped via model. For via mask layers specified by an impedance, the frequency dependent skin effects are NOT included.

3D Distributed Model

• A distributed model for the via object is created by meshing the surface with rectangular cells.
• Both the horizontal and vertical components of the via current are modeled, using horizontal and vertical oriented rooftop functions. This yields a complete 3D current modelling of the via objects.
• Each via object contributes four unknown currents per rectangular cell to the matrix equation.
• The via resistance and skin effect are included using the surface impedance formulation.
• All the via self and mutual inductances and capacitances are included in the simulation.
  

Momentum Layer Mapping GUI

The Momentum layer mapping dialog has been enhanced to accommodate the new via models. The following changes are implemented:

• Unmapped layers need to be mapped first before the layer properties can be defined. Hence, all layer properties for an unmapped layer are made INVISIBLE.
• For Layers mapped as VIA, users can select one of the three simulation models (Lumped, 2D Distributed and 3D Distributed).
• The 2D Distributed model is the default VIA model used for all pre-2006A substrate definitions.
• For Layers mapped as STRIP, you can select one of the three already existing geometical models:
  Sheet (No Expansion)
  Thick (Expansion Up)
  Thick (Expansion Down)
• For Layers mapped as SLOT, there is only one selection option in the Model combo box "Ground Plane (Holes)"
• Embedded Info in the dialog provides additional information about the selected layer properties.
• The Thickness field is only visible for layers mapped as STRIP
• The Overlap Precedence field is only visible for layers mapped as STRIP

Unmapped Layer

Layered Mapped as STRIP

Layer Mapped as SLOT

Layout Layer Mapped as VIA

Selection of Via Model

Selection of Material

Examples of New Via Simulation Models

Two Coupled RF Board Via's

Silicon spiral inductor

Defining Conductivity

You can define a layout layer as a conductor or a resistor. If the layout layer is defined as a strip or via, you define the conductivity of the strip or via. However, if the layout layer is defined as a slot, it is not possible to define the conductivity of the metal around the slot. This is because a slot is assumed to be surrounded by a perfect conductor.

To define conductivity:

1. Choose Momentum > Substrate > Create/Modify .
2. Choose the Metallization Layers tab.
3. Select a mapped layout layer from the Layout Mapping list.
4. Select the conductor type from Type list in the Layout Layers section. Choose Sheet Conductor , Thick Conductor (up) or Thick Conductor (down).
5. Set the Thickness.
6. Select the conductivity definition from the Conductivity list:
   • Perfect conductor
   • Sigma (Re, Im)
   • Impedance (Re, Im)
     Perfect Conductor means the strip, via, or metal around the slot is a perfect conductor and is lossless. No further definition is required.
     Sigma (Re, Im, thickness) specifies bulk conductivity as a complex number. Enter bulk conductivity's real and imaginary value in the respective fields below the Conductivity list, in Siemens/meter or Siemens/centimeter. The imaginary value is important for super-conductivity applications. Enter the metal thickness in the Thickness field above the Conductivity list and select the appropriate units. These values will be used to calculate the dc and high frequency loss mechanisms when determining the equivalent surface impedance. For example, the bulk conductivity of gold is 41,000,410 Siemens per meter with any arbitrary thickness. The equivalent DC sheet impedance that will be used when conductivity and thickness are specified is:
     
     where σ r is the real part of the conductivity (S/m) and t is the thickness of the conductor (m).
     At high frequencies, the equivalent sheet impedance will be equivalent to:
     
     where δ is the skin depth given by:
     
     with f as the frequency (Hz) and µ0 the free space permeability. This high frequency loss specification corresponds to a single sheet skin-effect loss model, meaning that it assumes the current at high frequency is assumed to be concentrated on one side of the finite thickness conductor.

     Note A double sheet skin effect loss model can be activated by setting the following variable in the momentum.cfg file: MOM3D_USE_SHEETLOSSMODEL=2 The default for this variable is '1', which means a single sided skin effect loss. This configuration flag should only be used when conductors with finite thickness are simulated and are not expanded as finite thickness conductors. The double sided skin effect loss model results in identical DC losses as the single sided skin effect loss model. However, at high frequencies, the single sided skin effect loss model assumes a concentration of the current on one side of the conductor, whereas the double sided skin effect formula assumes an equal current distribution on both sides of the conductor.

     Impedance (Re, Im,) specifies conductivity in terms of sheet impedance, in Ohms/square. Enter the real and imaginary component of the value in the Real and Imaginary fields, respectively.

     Note Momentum treats such metal layer definitions as a constant, frequency independent loss model. The thickness entered in UI is ignored in this case.

7. When you are finished with the definition, click Apply .
8. Repeat these steps for the remaining mapped layout layers.
9. When you are finished, click OK to dismiss the dialog box.

Automatic 3-D Expansion for Thick Conductors

Conductors with finite thickness can be modeled in Momentum using the 3D metal expansion feature. This feature will automatically expand the mask of a conductor with finite thickness in the direction orthogonal to the layered medium, using the specified thickness of this conductor.

Automated 3D expansion is activated by selecting either the Thick Conductor (up) or Thick Conductor (down) expansion. In both cases, an extra dielectric layer is included in the internal Momentum substrate model. This is done for each metal layer that is expanded. The thickness values of the dielectric layers in between the metal layers are not changed, which will preserve the capacitance value between two conductors lying on top of each other in the substrates.

To select the automated 3-D Metal Expansion Substrate items:

1. Choose Momentum > Substrate > Create/Modify .
2. Click the Metallization Layers tab.
3. In the Substrate Layers list, select the substrate layer or the interface where the layout layer is mapped.
4. Select the Type drop-down list from the Layout Layer dialog box.
5. Choose either Thick Conductor (up) or Thick Conductor (down)
   
   Simulations with automatic expansion require more simulation time and memory, but result in more accurate simulation results. Typically, when the height/thickness aspect ratio is smaller than a factor of 5, the effect of accounting for the finite thickness of the conductors will need to be allowed for in Momentum simulations.

The following figure illustrates the internal substrate model when using an "up" and "down" expansion for a conductor. In both cases, an extra dielectric layer is inserted (indicated with [new] in the figure), which in the case of an "up" expansion has the dielectric properties of the layer above the metal layer. In the case of a "down" expansion, the new layer has the material properties of the layer below the metal layer.

Note Extra internal metallization layers are automatically added in Momentum to model the currents on all four sides of the finite thickness conductor.

Modeling Horizontal Side Currents for Thick Conductors

Horizontal side currents for thick conductors can be modeled automatically by selecting Momentum > Mesh > Setup and enabling the Horizontal side current (thick conductors) feature located under the Global tab in the Mesh Setup Controls dialog box. For more information on Mesh Setup Controls, refer to Defining Mesh Parameters for the Entire Circuit.

When selecting this feature no substrate database recalculation is required, by taking advantage of new construction technology for the Green functions. Visualization is available in post-processing by selecting Momentum > Post-Processing > Visualization, which can be used for both 3D mesh, as well as current visualization.

Thick conductor U-turn visualization with horizontal side currents

When the Horizontal side current toggle is set, the horizontal current components will be added on all conductors, which have been specified as automatically expanded. This results in a modeling of the current as illustrated on the following figure:

Note The horizontal current components are not added on regular vias or when users manually expand finite thickness conductors.

By default, the new horizontal side currents toggle is not set, for backward compatibility reasons.

Different levels of granularity of the mesh on the side metallization are possible:

• One cell in the horizontal direction: in case edge mesh is turned off and no Transmission Line Mesh specification is entered.

  Note This is the advised setting in case the conductors are specified as automatically expanded.

• Multiple mesh cells in the horizontal direction: in case edge mesh is turned off and Transmission Line Mesh specification is entered.
• Edge mesh in the horizontal direction: in case the global edge mesh toggle is turned on, an edge mesh is generated on all sides (top, bottom and both sides) of the automatically expanded conductor. This is illustrated below:
  

  Note The simulation time is greatly increased when multiple mesh segments are introduced on the side metallization.

Setting Overlap Precedence

Overlap precedence specifies which layout layer has precedence over another if two or more layout layers are assigned to the same metallization layer and objects on the metallization layer overlap. Precedence is used by the mesh maker so that objects on the layer with the greatest precedence number are meshed and any overlap with objects on layers with lesser numbers is logically subtracted from the circuit. If you do not set the precedence, and there are overlapping objects, a mesh will automatically and arbitrarily be created, with no errors reported. Resistive layers generated from schematics are automatically set to the highest precedence.

In some cases, you may be designing with an intentional overlap because of manufacturing layout guidelines. In this case, assign a precedence number to the layout layers that overlap with precedence order in reverse numerical order (largest to smallest). The system will draw the boundary at the edge of the higher numbered layer without returning an error.

Precedence affects only how the mesh is created, it does not affect or alter the layout layers in your design.

To specify overlap precedence:

1. Choose Momentum > Substrate > Create/Modify .
2. Choose the Metallization Layers tab.
3. Select one of the overlapping layout layers from the list of Substrate Layers in the Layer Mapping section.
4. Assign its order of precedence in the Overlap Precedence field. Either type a value directly into the field or use the arrow keys to select a value.
5. Click Apply.
6. Repeat these steps for the remaining overlapping layers.
7. When you are finished, click OK to dismiss the dialog box.

About Dielectric Parameters

The sections below give additional detail about the following dielectric parameters:

• Dielectric Permittivity
• Dielectric Loss Tangent
• Dielectric Conductivity
• Dielectric Relative Permeability
• Dielectric Magnetic Loss Tangent

Dielectric Permittivity

The relative permittivity of all dielectrics is assumed to be complex:

which can also be expressed as:

where is the real portion of and
is the dielectric loss tangent.

Examples of materials and their typical permittivity are shown in the following table.

Note The values listed in the table are for illustrative purposes only; use values specifically measured for the materials that you are using.

Dielectric Loss Tangent

The dielectric loss tangent associated with a material is a function of frequency. Examples of dielectric loss tangents for 10 GHz fields are shown in the following table.

Note These values are listed for illustrative purposes only. Use values specifically measured for the materials that you are using.

Dielectric Conductivity

For some materials (for example, Silicon), the substrate loss effects are better described using the combination ( , = conductivity) instead of ( , loss tangent). The complex dielectric constant is related to ( , conductivity) using the following formula:

where:
= 2 !mom-04-1-56.gif!frequency
= 8.85e-12 F/m (absolute dielectric constant free space)
Often, resistivity ( )is specified instead of conductivity. The relationship between resistivity and conductivity is

Resistivity is usually specified in !mom-04-1-60.gif!cm, conductivity is specified in S/m.

Example:
A typical value for resistivity of a Silicon material is
= 10 !mom-04-1-62.gif!cm
which corresponds to a conductivity value of
= 10 S/m.

Note When selecting the Substrate Layer s tab, under Momentum > Substrate > Create/Modify, if Permittivity (Er) is set to Re, Conductivity, GAMMA will not appear in the dataset and the Z0 values will be set to the default of 50 ohms. This occurs because the port solver was switched off to improve Momentum simulation speed. To switch the port solver back on, the configuration variable located in, HOME/hpeesof/config/momentum.cfg must be set as follows: MOM3D_USE_PORTSOLVER=2 This forces the port solver to run, and the Z0 and GAMMA entries will appear correctly in the dataset.

Dielectric Relative Permeability

The relative permeability of all dielectrics is assumed to be complex:

which can also be expressed as:

where !mom-04-1-66.gif!is the real portion of !mom-04-1-67.gif!and !mom-04-1-68.gif!is the magnetic loss tangent.

Examples of relative permeabilities are shown in Materials and Relative Permeability.

Note The values listed above are for illustrative purposes only. Use values specifically measured for the materials that you are using.

Dielectric Magnetic Loss Tangent

The magnetic loss tangent associated with a material is a function of frequency. An example of a material with a magnetic loss tangent is polyiron which, at 30 GHz, has a loss tangent of 0.0208.

Reading a Substrate Definition from a Schematic

Choose Momentum > Substrate > Update From Schematic to update a substrate under the following conditions:

• You have used a substrate component on a schematic, such as MSUB or SSUB
• You have already generated a layout from the schematic using Layout > Generate/Update Layout
• You then change the substrate definition on the schematic, and need to transfer it to the layout.

In order to retrieve the new substrate information, you must use Momentum > Substrate > Update From Schematic . Using Layout > Generate/Update Layout will not transfer the new substrate information to the layout.

To update a substrate definition from a schematic:

1. Choose Momentum > Substrate > Update From Schematic . The substrate on the correct schematic is read and the new information is entered in the Momentum substrate definition.

Saving a Substrate

A substrate definition can be saved to a file. This enables you to store the definition outside of the current project, making it easier to use the substrate definition in other designs. To save a substrate:

1. Choose Momentum > Substrate > Save As .
2. Type a name for the file and click OK . Substrate files end with the extension .slm .
   To save a named file, choose Momentum > Substrate > Save. Identifying Where Substrates are Saved
   Substrates are saved in one of two locations:

• In the directory containing supplied substrates, which is $HPEESOF_DIR/momentum/lib . You should not use this location for substrates that you have created or modified.
• The substrate information is saved in a file called <substrate_name> .slm under /networks in the current project directory.

Precomputing the Substrate

In order to perform a simulation and to calculate a mesh, Green's functions characterizing the behavior of the substrate must be computed:

• If you intend to precompute a mesh before you simulate, you must precompute the substrate first. For more information on precomputing a mesh, refer to Precomputing a Mesh.
• If the Green's functions are not computed before you start a simulation, they will be calculated and then the simulation will run.

If you are using a substrate that is supplied with Advanced Design System, you do not need to precompute the substrate functions. If you have edited the substrate or created a new one, you must precompute the substrate function.

When the computations (Green's functions) are complete, the data is stored in a database, and it will be used in the simulation of any design that uses this substrate. If the substrate has been precomputed before and there has been no changes to the substrate, it will not be recomputed unless the frequency range has been extended. The frequency range can be set when using the Momentum mode, but not in Momentum RF mode. In RF mode, the frequency range (start-stop) is not requested. Since the RF mode uses the quasi-static Green's functions, they are calculated at quasi-static frequencies automatically chosen by the program. Substrate functions calculated in Momentum mode are reusable in RF mode if they are calculated from DC to some upper frequency.

For more information about the precomputation process, refer to Theory of Operation.

To precompute the substrate function:

1. Choose Momentum > Substrate > Precompute .
2. To specify the frequency range of the computations, enter starting frequency in the Minimum field and select the frequency units. Enter the stopping frequency in the Maximum field and select the frequency units. (Not available in RF mode.)
   Be sure that the frequency range includes all frequencies that you want to simulate.
3. Click OK to start the computations.
   Once the computations are completed, you do not need to perform this step again unless the substrate is edited.

Note Be aware that the greater the number of layout layers in the substrate, the more time required to perform the calculation.

Viewing Substrate Computation Status

After the substrate calculations are started, any messages regarding the calculations will appear in the Momentum Status window. Messages usually refer to any errors found, and indicate when the calculations are complete.

If you close the status window and want to reopen it, from the Layout menu bar choose Window > Restore Status.

Stopping Substrate Computations

To stop the substrate calculations:

1. From the Momentum Status window, choose Simulation/Synthesis > Stop Simulation.

The computations will stop and no information will be saved.

Viewing the Substrate Summary

If the simulation is successful, you can view substrate, mesh, and solution statistics. Some of the information returned includes time to solve, the resources required, and cell information. To view the summary, choose Momentum > Substrate > Summary .

Reusing Substrate Calculations

Substrate definitions and substrate computations can be reused for other designs, if the substrate database is accessible. If you are unsure about access to the database, consult your system administrator.

Before a calculation begins, several folders are searched to determine if a solution has already been generated. The folders searched, in order, are:

• The project substrates folder
• The home substrates directory or the site substrates directory (made available by your system administrator)
• The folder containing the Momentum supplied substrates ( $HPEESOF_DIR/momentum/lib/substrates )

If the Substrate Calculator finds the same substrate definition, regardless of the name, it uses the one it finds instead of recomputing the same information.

Deleting a Substrate

This command erases the substrate file (.slm) that you select. If the substrate has been precomputed, the calculations remain in the database.

To delete a file:

1. Choose Momentum > Substrate > Delete .
2. Select the name of the file that you want to delete.
3. Click OK.

Substrate Definition Summary

Every change to a substrate definition requires a complete re-computation. The system checks for duplicate definitions, regardless of the name and uses previously computed data if it exists.

The entire substrate definition includes:

• Vias, in the same manner that they are part of the fabrication process.
• Air bridges, including their height and their associated vias.
• Holes in ground planes, if they are part of a slot signal path (slot or coplanar), or if they are relief holes for vias passing through a ground plane are also part of the media.
• Dielectric layer properties (Er, MUr, and loss).
• Ground plane losses and cover properties (conductivity or impedance).
• Thick Conductors up or down.

Not included as part of the substrate definition:

• Metal loss of strip and via layers

The numerical computation process, used by the substrate calculator, can take as little as one minute for stripline circuits. It can take several minutes for microstrip or even a few hours for an arbitrary multi-layered substrate with several vias.

Substrate Examples

Use the following examples to help you set up your own circuits:

• Substrate for Radiating Antennas
• 377 Ohm Terminations and Radiation Patterns
• Substrate for Designs with Air Bridges

Substrate for Radiating Antennas

To define a substrate for an antenna that radiates into air, you can set up the following substrate definition:

Both layers are defined as open boundaries with the characteristics of air (for permittivity and permeability, Real = 1, Loss Tangent = 0). The antenna design is positioned on the metallization layer in between the two layers of air.

377 Ohm Terminations and Radiation Patterns

It is possible to define the top and bottom layers of a design with 377 ohm terminations, then calculate radiation patterns for these structures after simulation. For such applications, note the following considerations:

• The actual value of the termination may be between 376 and 378 ohms.
• When replacing top or bottom ground layer with a 377 ohm termination, a thick layer of air in between the circuit and the 377 ohm termination is required in order to get agreement (both for S-parameter results and radiation patterns) with the simulation results with infinite top or bottom layer. An air layer of 10-20 substrate thicknesses is generally thick enough.
• There is a test on the impedance value prior to calculating the radiation patterns. The impedance value must be in the interval (377 - 10) to (377 + 10) ohm.

Substrate for Designs with Air Bridges

In order to designing a substrate definition for a design that contains an air bridge, you need to first identify components of the air bridge and their placement on layout layers. Refer to the illustration that follows.

A basic air bridge between two components consists of the follow items:

• A via that connects the bridge to the first component
• The bridge itself
• A second via to complete the path to the second component
• The layer of air underneath the bridge

The layout must be drawn on at least three independent layers:

• The vias must be on at least one layer
• The bridge must be on a different layer
• The components must be on yet another layer

No two items that comprise the air bridge (except for the vias) can be on the same layer. For this illustration, the components that are connected by the air bridge are on the same layer.

The substrate definition would consist of the following items:

• An open boundary of air
• An interface layer of air at a finite thickness. This represents the layer of air under the bridge.
• An interface layer of dielectric material

You map the layout layers to the substrate as follows:

• The bridge is mapped to the metallization layer that is in between the "Free_Space" substrate layer and the "air" substrate layer.
• The vias are mapped to cut through the finite "air" substrate layer.
• The components are mapped to the metallization layer in between the air substrate layer and the dielectric layer "GaAs" layer.

It is not required for the components that the bridge connects to be on the same layout layer or mapped to the same metallization layer. Nor do the vias need to be on the same layout layer. Just be sure that the substrate definition has the correct number of substrate layers and that the components, vias, and bridge are mapped to the appropriate metallization layers.

Drawing Air Bridges in Layout

If you are simulating an air bridge, you will have to create a layout and a substrate definition that will support the geometry. This means adding an air layer (height equal to the air bridge) which the vias will cut through. For example, you would have some geometry (like a spiral) on a dielectric layer. Then a via would rise vertically cutting through the air layer, where it would connect to a metal bridge. Then another via would connect from the bridge, down to the previous layer, and onto another path.

Ports and Air Bridges in Coplanar Designs

When you draw coplanar waveguide as slots on a ground plane, it is treated, by default, as a four-port device composed of two, coupled slot lines. To make sure that it will be simulated as coplanar waveguide, be sure to apply the Coplanar port type to the ports on the circuit. This port type combines the two ports on the same reference plane, and the two ports are treated as one. For instructions on how to apply the Coplanar port type, refer to Defining a Coplanar Port.

If you do not use the Coplanar port type, a moding problem can result when a coplanar waveguide transmission line also propagates a slot mode. If Coplanar ports are used, the slot modes are short-circuited at the port interfaces. However, if the slot modes are excited somewhere in the circuit, they can cause resonances at certain frequencies. This will appear as non-physical results because the external boundary conditions are critical to the electrical behavior in such cases. By adding air bridges (straps) near the discontinuities the voltage level of the two grounds can be equalized to eliminate the slot mode. An example of air bridges can be found on the coplanar waveguide bend example, CPW_bend_prj .

Silicon Substrate

The following is an example of a silicon substrate used in a Momentum simulation (this example is taken from examples > Momentum > Microwave > SPIRAL_prj ):

Free space

      ---------------  strip2

Layer3 (Eps=3.9)    | via

      --------------- spiral (strip)

Layer2 (Eps=3.9)

Layer1 (Eps=11.9 ; cond=12.5 S/m)

GND

Silicon Substrate with 3D Expansion

The following is an example of a silicon substrate used with automatic expansion of a thick conductor:

Free space

     -----------------Strip thick conductor up (thickness 4 mil conductivity
Sigma Re: 5e+6 S/m)

Alumina  (Eps=9.6 ; Thickness=25 mil)

GND

With the Thick conductor up selected, the substrate used for the simulation will become:
Free space
-----------------Strip
air | via (substrate layer thickness 4 mil ; Eps =1 )
-----------------Strip
Alumina (Eps=9.6 ; Thickness=25 mil)

GND

For more information on automatic 3-D expansion for thick conductors, refer to Automatic 3-D Expansion for Thick Conductors.