Access Keys:
Skip to content (Access Key - 0)

Agilent Technologies

  


Getting Started with EMDS for ADS

This section is intended to help you get started with EMDS for ADS. It illustrates basic tasks and exercises using EMDS. The subsequent sections contain more in-depth reference information and examples.

Layout Basics

There are two basic ways to create a layout:

  • From a schematic (in a Schematic window)
  • Directly (in a Layout window)

The best approach to creating a layout depends on the design and the designer.

This section describes how to create a layout automatically from a finished schematic, and how to use the basic features in a Layout window to create a layout directly.

Note

When you are through working in layout, release the Layout license so that it is available to another user. To do this, choose File > Release Layout License from the Layout window.

Creating a Layout from a Complete Schematic

If all data is contained in the schematic, it is very simple to create a layout.

  1. In the Schematic window, build the schematic shown here, then choose the menu command Layout > Generate/Update Layout (the schematic is the source representation). The Generate/Update Layout dialog box appears.

    By default, the layout will begin with P1, at 0,0, with an angle of 0 degrees. There is no existing layout, so the Equivalence (the layout component that corresponds to the starting component in the schematic) is shown as not created.

    At this point, all of the elements in the schematic are highlighted, indicating that they all need to be generated.
  2. Click OK.

The Status of Layout Generation dialog box appears. It displays the number of designs processed, the number of items regenerated (created) in the layout, the number of items that are oriented differently in the layout than in the schematic, and the number of schematic components that were not placed in the layout.

The program automatically opens a Layout window and places the generated layout in it. The orientation of the layout is different from that of the schematic, because the layout is drawn from left to right across the page, beginning at the Starting Component.

Creating a Layout Directly

Launch Advanced Design System and create a project. To display a Layout window, choose Window > New Layout from the ADS main window, or choose Window > Layout from an open Schematic window.

The following tasks are performed the same way in a Layout window as they are in a Schematic window:

  • Selecting components
  • Placing and deselecting components
  • Changing views
  • Hiding component parameters
  • Coping and rotating components
  • Using named connections

Connecting Components with a Trace

As in a Schematic window, you can connect components without having them actually touch. In a Layout window, this is done by placing a trace between the component (in the same way a wire is used in the Schematic window). Either choose Component > Trace , or click the Trace button in the toolbar.

Unlike wires in a Schematic window, a trace in a Layout window may be inserted alone (click twice to end insertion).

Shapes

In Layout you can insert shapes, using either Insert commands or toolbar icons:

With each shape, you can either click and drag to place it, or define points by coordinate entry (choose the shape, then choose Insert > Coordinate Entry ).

  • path : starting point, segment end (click), and end point (double-click)
  • polygon : starting point, vertex (click), and end point (double-click) that closes the shape
  • polyline : starting point, segment end (click), and end point (double-click)
  • rectangle : two diagonal corners
  • circle : center and circumference point
  • arc : (Insert command only) center and circumference point
    Note

    The final segment of polygons and polylines can be entered by pressing the space-bar rather than double-clicking the mouse.

    Experiment by drawing different shapes to get the idea of how each is created.

Layers

In a Layout window, items are placed on a layer. The name of the current insertion layer is displayed in the toolbar and in the status bar.

Changing the Insertion Layer

There are many ways to change the insertion layer:

  • In the toolbar, retype the name of the layer and press Enter.
  • In the toolbar, click the arrow next to the layer name. Choose a name from the list of currently defined layers.
  • Choose the command Insert > Entry Layer and select a layer from the list.
  • Choose the command Options > Layers and select a layer from the list of defined layers in the Layer Editor dialog box.
  • Choose the command Insert > Change Entry Layer To , and click an object whose layer you want to make the current insertion layer.
  • Use the Layers window, that is opened when a Layout window is opened and select a name in the list of currently defined layers.

Experiment with placing shapes on different layers. Remember to click OK to accept a change in a dialog box.

Copy to a Different Layer

Experiment with copying shapes from one layer to another; use the command Edit > Advanced Copy/Paste > Copy to Layer. Note that the copied shape is placed at exactly the same coordinates as the original. Move one to see them both.

Default Layer Settings

Choose the command Options > Layers to display the Layer Editor. This is where you can edit the parameters of any defined layer, add layers, or delete existing layers.

Clicking Apply updates layer definitions but does not dismiss the dialog box.

Experiment with layer parameters. Note that you can toggle the visibility of all items on a layer. Protected means you can not select items on that layer.

Other Layout Defaults

The Options > Preferences command displays the Preferences for Layout dialog box. This dialog box has 11 tabs; clicking a tab brings the corresponding panel to the front.

Click the Grid/Snap tab.

This panel is where you set the snap grid and display grid parameters.

The display grid appears on the screen as a series of vertical and horizontal lines or dots that you can use for aligning and spacing items in the drawing area.

Adjust Grid Visibility and Color
  1. In the Display area, choose Major, Minor, or both.
  2. Choose the Type of display (Dots or Lines). You may have to zoom in to see the grid display.
  3. Click the colored rectangle next to the word Color, and choose the desired color for the grid. Click OK to dismiss the color palette.
  4. Click Apply. Experiment with different settings
    Note

    The drawing area color is the Background color under the Display tab.

Adjust Snap and Grid Spacing

The ability to display a major grid as an increment of the minor grid enables you to gauge distances and align objects better in a layout.

  1. In the Spacing area, change the Minor Grid display factors for both X and Y. The larger the number, the wider the grid spacing.
  2. Click Apply. Experiment with different settings. If a display factor makes the grid too dense to display, it is invisible unless you zoom in.
  3. Now experiment with the Major Grid.

Adjust Pin/Vertex Snap Distance

Pin/vertex snap distance represents how close the cursor must be to a pin of a component or a vertex of a shape before the cursor will snap to it.

A large value makes it easier to place an object on a snap point when you are unsure of the exact location of the snap point. A small value makes it easier to select a given snap point that has several other snap points very near it.

Place several components and several shapes in the drawing area and experiment with different settings of Pin/Vertex Snap.

Screen pix specifies sizes in terms of pixels on the screen. For example, if you choose 15, the diameter of the snap region is 15 pixels.

User Units specifies sizes in terms of the current units of the window. For example, if you are using inches and choose 0.1 user units, the diameter of the snap region is 0.1 inch.

Experiment with Snap Modes

Snap modes control where the program places objects on the page when you insert or move them; you can change snap modes when inserting or moving a component, or drawing a shape. When snap is enabled, items are pulled to the snap grid.

Experiment with different snap modes turned on or off to see how they affect the placement of items in a Layout window.

   Snap Mode  Priority
You can restrict or enhance the manner in which the cursor snaps by choosing any combination of snap modes. This table lists the snap modes, and their priorities.    Pin  1
 Vertex  2
 Midpoint
 Intersect
 Arc/Circle Center
 Edge  3
 Grid  4

Angle Snapping automatically occurs when only Pin snapping is enabled and you place a part so that the pin at the cursor connects to an existing part. The placed part rotates so that it properly aligns with the connected part.

For example, if you have a microstrip curve at 30° and place a microstrip line so that it connects to it, the microstrip line will snap to 30° so that it properly abuts the curve.

Enable Snap toggles snap mode on and off. You can also toggle snap mode from the Options menu itself, and there are snap mode buttons on the toolbar.

Except for pin snap, the pointer defines the selected point on the inserted object.

When you set all snap modes OFF, you can insert objects exactly where you release them on the page. This is sometimes called raw snap mode. Like other snap modes, the raw snap mode also applies when you move or stretch objects.

Pin When a pin on an object you insert, move, or stretch is within the snap distance of a pin on an existing object, the program inserts the object with its pin connected to the pin of the existing object. Pin snapping takes priority over all other snapping modes.

Vertex When the selected location on an object you insert, move, or stretch is within the snap distance of a vertex on an existing object, the program inserts that object with its selected location on the vertex of the existing object.
In vertex snap mode, a vertex is a control point or boundary corner on a primitive, or an intersection of construction lines.

Midpoint When the selected location on an object you insert, move, or stretch is within the snap distance of the midpoint of an existing object, the program inserts that object with its selected location on the midpoint of the existing object.

Intersect When the selected location on an object you insert, move, or stretch is within the snap distance of the intersection of the edges of two existing objects, the program inserts that object with its selected location on the intersection of the existing objects.

Arc/Circle Center When the selected location on an object you insert, move, or stretch is within the snap distance of the center of an existing arc or circle, the program inserts that object with its selected location on the midpoint of the existing arc or circle.

Edge When the selected location on an object you insert, move, or stretch is within the snap distance of the edge of an existing object, the program inserts that object with its selected location on the edge of the existing object. Once a point snaps to an edge, it is captured by that edge, and will slide along the edge unless you move the pointer out of the snap distance.

Because edge snapping has priority 3, if the cursor comes within snap distance of anything with priority 1 or 2 while sliding along an edge, it will snap the selected location to the priority 1 or 2 item.

Grid When the selected location on an object you insert, move, or stretch is within the snap distance of a grid point, the program inserts that object with its selected location on the grid point.

All other snap modes have priority over grid snap mode.

Hint

Whenever possible, keep grid snapping on. Once an object is off the grid, it is difficult to get it back on.

Use 45 or 90° angles to ensure that objects are aligned evenly, and to reduce the probability of small layout gaps due to round-off errors.

Drawing Tips

This section provides suggestions and examples when drawing layouts to be simulated using EMDS for ADS. These examples take into consideration things that are necessary during the drawing phase to ensure that requirements for EMDS for ADS are met.

Using Grid Snap Modes

Working in Layout enables you to control all geometry precisely. The variety of available snap modes can help you draw and position shapes. As an example, if you are connecting shapes, you should have the vertex snapping mode turned on. You will also want to review snap mode settings prior to adding ports to a layout.

Snap grid spacing also helps control the positioning shapes. In general, snap grid spacing should be about 1/2 of the minor grid point value. For example, if the minor grid points are 1.0, then the snap grid spacing should be 0.5. This makes it easy to know how your geometry will snap into place.

For more information on snap modes and snap grid spacing, refer to Managing Projects and Designs.

Choosing Layout Layers

The standard set of layout layers begins with the layer named default. Do not use this layer for drawing your circuit. The first valid layer for EMDS for ADS is cond. For more information on layout layers, refer to Schematic Capture and Layout.

Keeping Shapes Simple

In general, when drawing shapes, you should use a minimal number of vertices per shape, since this will make the mesh easier to compute. When drawing curved objects, consider using a relatively large value for Arc/Circle Radius (under Options > Preferences > Entry/Edit ). This will minimize the number of vertices, and facets used to represent the shape.

Merging Shapes

Merging shapes is often useful for eliminating small geometry overlaps and can also, in some cases, result in simpler mesh patterns. For example, if you draw a layout using multiple polygons and you suspect there is some overlap, merging the polygons will prevent the system from returning an overlap error. To merge the shapes, select each shape that you want to merge, then choose Edit > Merge.

Viewing Port and Object Properties

Any item selected in a layout, including ports, shapes, or other components, has associated properties. One way to view the properties is to select the object of interest, then choose Edit > Properties. This method also enables you to change object properties. If you want to change properties that have been attributed to an object for EMDS for ADS, you should change these properties either through the EMDS menu or the Momentum menu selections.

To view the properties of the entire layout, choose Options > Info.

Adding a Port to a Circuit

You can add a port to a circuit either from the Schematic window or a Layout window. The procedures below include considerations for adding ports to a circuit that will be simulated using EMDS for ADS.

Adding a Port to a Schematic

  1. Select a port using by choosing the menu item Component > Port, or the port icon from the tool bar:
  2. Position the mouse where you want the port and click. Verify the connection has been made.
  3. Select the port and choose Edit > Component > Edit Component Parameters.
  4. The parameter layer= indicates the layer that the port is applied to. When you convert your schematic to a layout, all components will be assigned to layout layers. You can assign the port to a specific layer at this time. To change the layer, select layer= from the Select Parameter list, and choose a new layer from the Parameter Entry Mode listbox. Make sure that the layer you choose will also be mapped as a strip or slot metallization layer. For more information about metallization layers, refer to Substrates.
  5. Click OK to accept the new layer specification.

When you generate a layout from the schematic, you should verify that the port is positioned correctly. For more information, refer to the procedure for adding a port to a layout and to Considerations.

Adding a Port to a Layout

To add a port:

  1. Determine where you want to position the port. A port can be applied to:
    • The pin of a component
    • The edge of a component or object (such as a rectangle or polygon), usually at the midpoint
    • The surface of an object
      Note

      Do not place a port on the corner of an object. When you add a port to an edge, make sure the appropriate snap modes are enabled. It is a good practice to enable the modes Midpoint Snap and Edge Snap (under the Options menu) to ensure accurate simulation results.

  2. If you want to add a port to the surface of a polygon, you may need to disable the following or other snap modes (under the Options menu):
    • Pin snap
    • Edge snap
    • Midpoint snap
  3. Identify the name of the layer on which the component or shape is entered. If you don't know the name of the layout layer, choose Options > Layers. Select each layer, noting the color in the dialog box. When the color matches that of the one in the Layout window, note the name of the layout layer. Dismiss the dialog box.
  4. Select a port using by choosing the menu item Component > Port, or the port icon from the tool bar:
  5. The Port parameters dialog box is displayed. The parameter layer indicates the layer that the port will be applied to. The parameter defaults to the currently active drawing layer.
  6. This should be the same as the layer you noted in step 3. To change the layer, select layer= from the Select Parameter list, and choose a new layer from the Parameter Entry Mode listbox. Make sure that the layer you choose is also a strip or slot metallization layer. Do not apply ports to shapes that are on layers that are mapped to via metallization layers. For more information about metallization layers, refer to Substrates.
    Note

    If you cannot find the layer name, choose Options > Layers , then select the layer name of interest from the Layers list. Note the layer number in the Number field. In the Port dialog box, select the layer= parameter and, under Parameter Entry Mode, select Integer Value . Enter the layer number, then click Apply .

  7. Click Apply to accept the new layer specification.
  8. Position the mouse where you want to place the port and click. The port is added to the circuit.
    Note

    If you are applying a port to an edge, the port must be positioned so that the arrow is outside of the object, pointing inwards, and at a straight angle. Generally, this happens automatically when you add a port to an edge. You may need to zoom in to verify this.

  9. The Instance Name in the Port dialog box is incriminated if you want to add another port. Verify the layer= parameter, then use the mouse to add the next port.
  10. When you are finished adding ports, click OK to dismiss the dialog box.

Considerations

Keep the following points in mind when adding ports to circuits to be simulated using EMDS for ADS:

  • The components or shapes that ports are connected to must be on layout layers that are mapped to metallization layers that are defined as strips or slots. Ports cannot be directly connected to vias. For information on how to define strips and slots, refer to Defining Metallization Layers.
  • Make sure that ports on edges are positioned so that the arrow is outside of the object, pointing inwards, and at a straight angle.
  • Make sure that the port and the object you are connecting it to are on the same layout layer. For convenience, you can set the entry layer to this layer; the Entry Layer listbox is on the Layout tool bar.
  • A port must be applied to an object. If a port is applied in open space so that is not connected to an object, EMDS for ADS will automatically snap the port to the edge of the closest object. This will not be apparent from the layout, however, because the position of the port will not change.
  • If the Layout resolution is changed after adding ports that are snapped to edges, you must delete the ports and add them again. The resolution change makes it unclear to which edges the ports are snapped, causing errors in mesh calculations.
Note

Do not use the ground port component in circuits that will be simulated using EMDS for ADS ( Component > Ground or the toolbar button ).
Either add ground planes to the substrate or use the ground reference ports that are described later in this section.

Examples

This section includes a number of examples to help you understand how to use the product.

The examples provided in this section include:

Designing a Microstrip Line

This section is made up of an exercise that takes you through the process of creating a schematic, converting to a planar (Layout) format, preparing the layout for simulation, simulating, and generating analysis plots.
This exercise uses many default settings and a simple circuit (a microstrip line with step in width), and illustrates how quickly a design and analysis can be accomplished.

In this exercise, you will:

  • Draw a simple microstrip line with step in width as a schematic, then generate a corresponding layout
  • Create a simple substrate
  • Define a mesh
  • Perform a simulation
  • Examine the results

Terms such as substrates and meshes may be unfamiliar, so they are explained in the course of the exercise.

This and later exercises assume that you have an introductory working knowledge of Advanced Design System, such as understanding the concept of projects, and being familiar with Schematic and Layout windows and placing components.

Drawing the Circuit

The basic steps to making the microstrip line with step in width circuit include:

  • Creating a new project
  • Adding microstrip components to the schematic
  • Converting the schematic to a layout

The schematic and layout representations are shown here. The sections that follow describe how to create both.

Creating a New Project

You should start this exercise in a new project.

  1. From the Main window, choose Tools > Preferences. Ensure that Create Initial Schematic Window is enabled. Click OK.
  2. From the Main window, choose File > New Project. The New Project dialog box appears.
  3. In the Name field, type step1.
  4. In the Project Technology Files section, choose ADS Standard: length unit - mil
  5. Click OK.

A Schematic window appears, which is where you will enter the design.

Adding Microstrip Components to the Schematic

The steps in this section describe how to select a component. In the next section, it will be placed in the Schematic window.

Refer to the this figure to select the microstrip line component (MLIN) from the Microstrip Transmission Lines palette:

Placing the Components

The steps in this section describe how to place two microstrip lines in the Schematic window.

  1. Move the crosshairs to the Schematic window and click once to place the component. A schematic representation of the component is placed in the Schematic window.
  2. Move the cursor so that the crosshairs are directly over the right pin of the first component, and then click once to place a second component.

Cancelling Commands

If you continue to click without ending the current command, you will add another component with each click.

  1. Click the arrow button . The crosshairs disappear.
  2. You can also end a command by pressing the Esc key.

You will use the end command frequently in this and other exercises, so be sure you are familiar with it.

Editing Component Parameters

Below the schematic representation of each component are some of the editable parameters of the component. This section describes how to change the width of one of the strips. The result is a microstrip step in width transmission line.

  1. Click twice on the second component that you placed. The Libra Microstrip Line dialog box opens.
  2. In the Select Parameter field, select the W (width) parameter. When the field to the right shows the value of the width, change the value in this field to 35 mil. Click Apply.
  3. Click OK to dismiss the dialog box.
    Note

    If a parameter for a component is displayed in the Schematic window, you can also edit that parameter by clicking on the value and entering a new value.

  4. Verify that the width of component on the left is set to 25 mil, and if needed, change the value of this parameter.

Adding Ports to the Circuit

To complete the circuit, you must add ports, one at the beginning of the microstrip step in width and one at the end. In EMDS for ADS, ports identify where energy enters and exits a circuit. This section describes how to add ports.

  1. In the menu bar, click the Port button . Move the cursor over the Schematic window and note the orientation of the ghost icon of the port. The ports should be positioned as shown in the schematic below at the end of these steps.
  2. You may need to rotate the port to the necessary orientation. If so, click the Rotate button and move the cursor back into the Schematic window. Note the rotation of the port outline, and repeat until it is correct.
  3. Move the cursor over the open pin on the left side of the left component, then click.
  4. The command to insert a port remains active. To insert a second port, change the orientation appropriately, move the cursor over the open pin on the right side of the right component, then click.
  5. End the current command. Your schematic should now look like this figure. It is a microstrip line step in width. The width of the first part of the line is 25 mil, and it increases to a width of 35 mil. The overall length is 200 mil.
Note

All of the components are connected. Diamond-shaped pins indicate that pins are not connected, and you will need to select and move components to make complete connections.

Saving the Design

It is good practice to save your work periodically. This section describes how to save the schematic.

  1. Choose File > Save Design. When the Save dialog box appears, enter the name of the project, in this case, type step1.
  2. Click OK.

Generating the Layout

A powerful feature of Advanced Design System is the ability to convert a schematic to a layout automatically. Since EMDS for ADS requires a circuit be in Layout format, this gives you the option of drawing your circuits either as schematics or as layouts. Note that if you do choose to draw in a Schematic window, footprints of the components you use must also be available in Layout. Components that are available in Layout include transmission lines and lumped components with artwork.

This section describes how to covert the microstrip line step in width schematic that you just finished to a layout.

  1. In the Schematic window, choose Layout > Generate/Update Layout . The Generate/Update Layout dialog box appears. It is not necessary to edit fields.
  2. Click OK .
  3. A Status of Layout Generation message appears indicating that the conversion is complete
  4. Click OK .
  5. A Layout window appears, showing a layout representation of the schematic. This window may be hidden by the Schematic window, so you may need to move some windows to locate the Layout window.
  6. From the Layout window, choose File > Save Design . Name the layout step1 . You now have a layout and a schematic as part of your project.

Creating a Simple Substrate

A substrate is required as part of your planar circuit. The substrate describes the media where the circuit exists. An example of a substrate is the substrate of a multilayer circuit board, which consists of:

  • Layers of metal traces
  • Layers of insulating material between the traces
  • Ground planes
  • Vias that connect traces on different layers
  • The air that surrounds the circuit board

EMDS for ADS includes several predefined substrates for your use, or you can create your own. Complete details about substrates, including where substrates are saved, are in Substrates.

The steps in this section describe how to define a substrate.
For the microstrip line step in width example, a substrate with the following layers will be used:

  • A ground plane
  • A layer of insulation, such as Alumina
  • A metal layer for the microstrip
  • An air layer above the microstrip
  1. From the Layout window, chose EMDS > Substrate > Create/Modify. The Create/Modify dialog box opens, showing the Substrate Layers options and parameters.
  2. In the Substrate Layers field, select FreeSpace. Move to the Substrate Layer Name field and change it to read Air . Leave all other parameters at their default values and click Apply.
  3. Keep the default layers Alumina and ///GND/// , but highlight and Cut any other layers that may be showing. Click Apply.
    You currently see three of the four substrate layers that you need. The fourth (metal) layer can be found by clicking the Metallization Layers tab.
    The metal layer is automatically positioned between the Substrate layers of Alumina and air. The microstrip line is assumed to be on this layer.
  4. Click OK to dismiss the dialog box.
  5. To save the substrate with the project, choose EMDS > Substrate > Save As. Type step1 in the Selection field and click OK. The substrate step1.slm is saved in the project networks folder.
    Some other information about saving substrates:
    • A substrate definition is automatically saved with the design when File > Save is invoked from the Layout window
    • The command Substrate > Save As enables you to save the substrate definition in
      slm that can be saved anywhere and used with another design
    • When a design is opened, the substrate definition that was saved with the design is automatically loaded.

Setting up Mesh Parameters

A mesh is required in order to perform a simulation. The simplest method for generating a mesh is to skip the Mesh menu entirely and allow EMDS to automatically generate the mesh for your circuit; however, you can still choose to edit parameters that control how the mesh is generated.

A mesh is a grid-like pattern of tetrahedra that is applied throughout the volume of a circuit. Using the mesh, the electric fields within each tetrahedron volume is calculated, and any coupling effects in the circuit can also be calculated during the simulation. From these calculations, S-parameters are then calculated for the circuit.

Details about mesh definitions, seeding and generation can be found in Simulation Options.

The steps in this section describe how to set the frequency for mesh computations. All other options will remain at the default values.

  1. From the Layout window, choose EMDS > Simulation Options . An EMDS Simulation Options dialog box appears.

  2. Select Refine at a Specific Frequency.
  3. Set The mesh will be adapted at 4 GHz, and then click OK.

Performing the Simulation

The EMDS for ADS simulation process creates an initial mesh from the mesh seeding information and solves for E-field in the circuit. Using the E-field calculations, S-parameters are then calculated for the circuit.

There are a variety of options to select to set up a simulation. Details are in Simulation. This section describes the minimal steps for running a simulation.

  1. From the Layout window, choose EMDS > Simulation > S-parameters. The Simulation Control dialog box appears.
  2. Set the Sweep Type to Linear and confirm that the following parameters are set:
    • Start = 1 GHz
    • Stop = 4 GHz
    • Frequency Step = 1 GHz
      By choosing this sweep type, a linear simulation will be performed over the 1-4 GHz frequency range, selecting the frequency points to be simulated based on the step size.
  3. Click Add to Frequency Plan List . The dialog box should resemble Simulation Control Dialog.

The initial mesh is refined at the mesh frequency until the adaptive mesh refinement criteria are satisfied. Then a frequency sweep is performed.

Simulation Control Dialog
  1. Ensure that the field Open data display when simulation completes is enabled.
  2. Click Simulate. The simulation will be performed. The simulation progress and its completion will be indicated in the Simulation Status window.
  3. When the simulation is complete, the S-parameter simulation results are automatically displayed on both rectangular plots and Smith charts in a Data Display window. This is because the field Open data display when simulation is complete was enabled as a default in the simulation setup. Choose View > View All or click the View All button to view all of the plots, then zoom in on individual plots. An example of one S-parameter result is illustrated here.

This completes the first EMDS for ADS design exercise.

Designing a Microstrip Filter

This section is made up of an exercise that takes you through the process of designing a microstrip coupled-line filter. It is similar to the previous exercise, but uses fewer defaults and explores how to:

  • Create a more complex substrate
  • Specify port properties
  • Use a box to simulate the filter within a metal enclosure
  • Specify mesh parameters

Drawing the Circuit

This section is very similar to the drawing instructions in the previous exercise. The circuit is drawn as a schematic, then converted to a layout. If you need more information on how to perform certain steps, refer to the previous exercise.

Opening a New Project

Like the previous exercise, start the filter design in a new project.

  1. From the Main window, choose File > New Project.
  2. In the Name field, type filter.
  3. In the Project Technology Files section, choose ADS Standard: length unit - mil.
  4. Click OK in the New Project dialog box to create the new project.

Adding Components to the Schematic

The steps in this section describe how to select microstrip filter components.

  1. In the Schematic window, click the Palette List arrow. The Palette List drops down.
  2. Scroll and select T-lines Microstrip __ from the Palette List.
  3. In the component palette, locate and click Mcfil. This selects the Libra Microstrip Coupled-Line Filter Section component.
  4. Crosshairs and a ghost icon of the component appear as you move the cursor over the Schematic window. Position the cursor and click.
  5. End the command either by clicking the Cancel Command button or by choosing Insert or the arrow button.

Editing the Component

This section describes how to edit several component parameters, such as the length and width, and also how to change the parameters that are displayed below the component.

  1. To edit the component parameters, double click the component.
  2. In the dialog box that appears, select one of the parameters listed below, and edit the value. Also, enable Display parameter on schematic so that the parameter will be displayed below the component in the Schematic window. Select another parameter, and continue to set the values for these parameters:
    • W = line width = 0.25 mm
    • S = spacing between lines = 0.044 mm
    • L = line length = 1.8 mm
    • W1 = width of the line that connects to pin 1 = 0.25 mm
    • W2 = width of the line that connects to pin 2 = 0.25 mm
  3. Click OK to accept the edits and dismiss the dialog box.

Copying and Placing another Component

This section describes how to make a copy of the filter section and add it to the schematic.

  1. Click the filter component on the schematic to select it. A black outline appears around it.
  2. From the Schematic window, choose Edit > Copy.
  3. Choose Edit > Paste. ** Move the crosshairs so that they are directly over the left connector of the first component and click.
  4. End the current command.

Adding Ports

Ports are required on a circuit. If you forget to add ports to the schematic, you can always add them later after the schematic is converted to a layout. In this exercise, ports will be added to the layout.

With EMDS for ADS, you can define additional characteristics to a port. This also will be performed later in this exercise.

Your schematic should now look like the figure here. Be sure that all components are connected correctly.

Saving the Design

It is good practice to save your work periodically.

  1. Choose File > Save Design.
  2. Enter filter as the file name.
  3. Click OK.

Generating the Layout

This section describes how to covert the microstrip coupled-line filter schematic that you just finished to a layout.

  1. From the Schematic window, choose Layout > Generate/Update Layout . The Generate/Update Layout dialog box and a Layout window appear.
  2. From the Layout window, choose Options > Preferences . Click the Layout Units __ tab and set the Resolution to 0.001 mm . Click OK .
  3. In the Generate/Update Layout dialog box, enter -1.8 in the X field and 0.294 in the Y field. This step identifies the placement of P1 on the layout. This step is usually optional, but specifying the location will be helpful later when the box is added to enclose the filter. Click OK .
  4. A window displaying the results of the conversion is displayed. Click OK .
    A layout representation of the schematic appears in the Layout window. It should resemble the figure here.
  5. From the layout window, choose File > Save Design . The layout name is filter . You now have a layout and a schematic as part of your project.

Defining a Substrate

This circuit uses a relatively simple substrate. In this exercise, the thickness of some of the layers is modified. A more important task is that ground planes are added to the top and bottom of the substrate. These ground planes form the top and bottom of the metal box in which the filter will be enclosed. The substrate will have the following layers:

  • A ground plane representing the top of the box
  • A layer of air
  • The microstrip filter traces
  • A layer of Alumina
  • A ground plane representing the bottom of the box.
  1. From the Layout window, chose EMDS > Substrate > Create/Modify.
  2. Select the top layer in the Substrate Layers field. In the Boundary list, select Closed . The top ground plane is added to the substrate.
  3. In the Substrate Layers list, select Free_Space . Change the Thickness to 2846 um. This sets the layer of air to an appropriate thickness.
  4. In the Substrate Layers list, select Alumina . Change the Thickness to 254 um.
  5. Keep the bottom ground plane, but select and Cut any other layers that may appear in the substrate.
  6. Click Apply.
    Note

    The top and bottom of the box enclosure are defined with groundplanes, the sides of the enclosure will be defined later in this exercise.

    You currently see four of the five substrate layers that you need. The metal layer for the microstrip filter can be found by clicking the Metallization Layers tab.

    In this instance, the metal layer is automatically positioned between the Alumina and air layers.
    Note the following points about this layer:
    • Metal layers are identified by a dashed line.
    • The word cond identifies the layout layer that is mapped to this position. Refer to the Layout window, and you will see that the microstrip circuit was automatically applied to the layout layer named cond during the translation process.
    • The word strip defines the layer such that the microstrips are metal and what surrounds the microstrips on that layer is air or dielectric. Other choices are slot and via. These are described in the exercise in the next section.
  7. Click OK to dismiss the dialog.
  8. Choose EMDS > Substrate > Save As. Use the file name filter and click Save. The substrate file filter.slm is saved as part of the project.

Adding Ports to the Layout

In EMDS for ADS, you can define the ports in your circuit to be one of several types. Depending on the type you choose, the ports will be characterized in different ways. This can impact the result of a simulation, because the simulation can take these characteristics into account. With different port types, you can select one that best matches the intended application of your layout.

More detailed information about the various port types can be found in Ports.

Ports are defined in a two-step process. First, ports are added to a circuit when the circuit is drawn. Then, in EMDS for ADS, you specify the port type in order to tailor the port to your circuit. Note that you can add the port components at any time as you draw the circuit, but before a port type can be specified, a substrate must be defined for the circuit.

This section describes how to add ports to a layout and how to specify a port type for them.

  1. From the Layout window, click the port icon. A Port dialog box appears. If necessary, set layer = cond. The ports must be on the same layout layer as the microstrip filter. Click OK.
  2. Move the cursor over the open port on the left side of the layout and click. Move the cursor over the open port on the right side of the layout and click. End the command. The layout should resemble the figure here.
  3. From the Layout window, choose EMDS > Port Editor . This opens the Port Properties Editor dialog box.
  4. If necessary, drag the dialog box away from the Layout window so that both ports are visible. Click the connector P1.
  5. The Port Properties dialog box will change so that you can select a port type to be applied to P1.
  6. Select Internal from the Port Type drop down list and click Apply.
  7. Click the connector P2. Select Internal from the Port Type drop down list. Click OK to accept the port type and dismiss the dialog box.

The internal port type is selected because it can be applied to the interior of a circuit. While normally this placement of the ports on the filter would not be considered internal, they are in this case because the filter is enclosed within the box. More information on this and other port types is in Ports.

Finishing the Box around the Filter

Boxes and waveguide enclosures are useful because they introduce vertical boundaries to the design. Adding a box enables you to look at box resonance, which can have a significant effect on S-parameters in a small band centered around the box resonance frequency. More information about boxes, waveguides, and their uses are in 3D Extension.

Recall that when you defined the substrate, you defined ground planes as the top and bottom of the metal box that will enclose the filter. This section describes how to specify the dimensions and location of the sidewalls of the box.

  1. From the Layout window, choose EMDS > Box & Waveguide > Add Box .
  2. You will enter specific x, y coordinates for the left and right sides of the box. Choose Insert > Coordinate Entry . Type -4.5 , -4.5 in the X,Y fields of the Coordinate Entry dialog box and click Apply.
  3. Type +4.5 , +4.5 in the X,Y fields of the Coordinate Entry dialog box and click Apply . The box appears as shown below (you may need to click View All to see the box). Click Cancel to close the dialog box.

Performing the Simulation

This section describes how to set up and run the simulation. In this exercise, the adaptive sweep type is used in the simulation process. This the preferred sweep type, because it used a fast, highly accurate method of comparing simulated data points to a rational fitting model. Unlike the linear sweep type, where simulated data points are chosen in a linear fashion based on step size, adaptive sweep type data points are chosen based on where the most variance seen. Wherever S-parameters vary from the rational fitting model the most, more samples are taken.

  1. From the Layout window, choose EMDS > Simulation > S-parameters .
  2. Select the Adaptive Sweep Type and set these parameters to the following values:
    • Start = 1 GHz
    • Stop = 40 GHz
    • Sample Points Limit = 50
  3. Click Add to Frequency Plan List .
  4. Make sure that Open data display when simulation completes is enabled The S-parameters will automatically be plotted and displayed at the end of the simulation.
  5. Click Simulate . The simulation will be performed and its progress and completion will be indicated in the status window.
  6. Click EMDS > Simulation > Summary... and saved simulation details will be displayed. You can print the report if you wish.

Viewing Simulation Results

The S-parameter simulation results are automatically displayed on both rectangular plots and Smith charts in a Data Display window. An example of S12 plotted on a rectangular plot is shown here.