Design Synchronization

Because schematic and layout information is contained in the same design file, we refer to the schematic representation and the layout representation of a design, and ADS can maintain equivalent representations of any design. You can make changes to one representation and then synchronize the other representation with it, ensuring they are equivalent. The representation you issue the synchronization command (Generate/Update) from is referred to as the source representation, and the representation that will be automatically modified to match the source representation is the target representation.

The Layout menu (in the Schematic window) contains a variety of commands that enable you to generate a layout from the schematic and to troubleshoot and modify your approach with respect to components that didn't generate in the expected manner. An equivalent set of commands can be found on the Schematic menu (in the Layout window) for generating a schematic from a layout, because the synchronization process is bidirectional.

The Synchronization Process

When you synchronize two representations, the program examines each component in the source representation and modifies or creates an equivalent component in the target representation. The synchronization process can be fully automatic or incremental. If artwork exists for all schematic components, a layout of all connected components can be generated in one step. However, if any components do not have artwork associated with them (these will be represented by a generic artwork placeholder), or the layout has components that do not connect by abutment (typical in RF designs), the layout can be created incrementally. This is done by interactively placing components one at a time or a group at a time, then connecting them using traces. In addition, there is a dual placement mode that allows interconnected components to be automatically placed in the other representation during insertion mode.

Although this process is bidirectional, the first part of this chapter describes the process from the perspective of generating a layout from a schematic. Details related to using this process in the other direction are covered under the section, Generating a Schematic (Layout-driven Design).

In general, your layout generation will be far more successful if you perform a prescribed series of checks prior to generating the layout:

Synchronization Modes

The synchronization can be complete or incremental and can be done to and from a schematic and layout.

Generate Update Place Component
Place all activated components, including those with no artwork, connected to the starting component. Update a previously generated design by placing components that have been modified. Place items that have no counterparts in the other representation.
Components with fixed location status are not moved. Components with fixed location status are not moved. Use the "Current Rep only" component placement mode.
Components that are not placed in the other representation are highlighted.   "Wire guides" show connectivity in the other representation.
Any component can serve as the starting point for which the location, orientation can be specified.   Use the "Options > Variables"; command to override the default resolution path for variable- and substrate- references.

Working with Hierarchical Designs

When working with hierarchical designs, the best approach is to start with the subnetwork that represents the lowest level in the hierarchical design and go through the checklist just mentioned, then generate the layout for that particular subnetwork. Once you are satisfied with the results, move up to the next level in the hierarchy and repeat the process. When you are finished with all the subnetworks, repeat the process for the top-level design.

When generating artwork for a subnetwork that has one or more parameters that refer to variables or instances defined in a higher level design, you must identify the top design in the hierarchy and possibly the path from the top design back down through the hierarchy (via Instance Name) to that subnetwork. The path from the top design needs to be deep enough to resolve any ambiguity between VARs, substrates, or parameters on parametric subnetworks.


To specify the location of the actual variable values, choose Options > Variables.
Top Design in Hierarchy - Type the name (or use the browser) of the top-level design in the hierarchy the subnetwork is part of.
Representation - Select Layout only when working with layout-only designs
Component Path (Instance Names) to Variable Values - Use the following guidelines to determine the appropriate path:

Identifying Components Without Artwork

Before you generate the layout, you should check for any components without pre-defined artwork and either create it or associate an existing artwork with the component.

To identify components without artwork:

  1. From the Schematic window, choose Layout > Show Components With No Artwork. All components that have no artwork associated with them are highlighted and a confirmation dialog box appears asking if you want to choose artwork for the highlighted items.
  2. Click Yes and a dialog box appears displaying the Instance Name of one of the components without artwork and offering a choice of artwork types.
    Hint
    To go back later and change the artwork association for a given component, select the component and choose Edit > Component > Edit Component Artwork.
  3. Select the desired Artwork Type and Name and click Apply to make the artwork association.
    Choose Default to display in the dialog box, the default artwork specified in the create_item() definition for the component.
    Choose Fixed to specify and use another design file to represent the artwork for the component.
    Choose Null Artwork to create a component with just pins and no artwork.
    Hint
    If you do not want a lumped component to occupy layout space, use the Null Artwork type. If you want a lumped component to have pads, choose a component from the Lumped With Artwork component palette.
  4. Repeat this process until all artwork associations are made.

Using TEE Junctions in a Schematic

When multiple transmission lines form a tee junction, one of the TEE components is required.

If three layout components are joined without the use of a tee component, as in the incorrect diagram, they will be connected with wires in the generated schematic, and the length of these wires are based on the setting in the Preferences dialog accessed through the Generate/Update dialog box. The use of tee components is not only important for layout, but is also important for proper simulation of interconnected transmission lines.

Using Steps and Tapers in a Schematic

You must use step or taper components to introduce changes in transmission line widths. A common error in microstrip and stripline layout is to put two different width transmission lines together without a transition component, as shown in the illustration that follows.

To account for the discontinuity, you must insert either a taper or step component between the two components.

There are a number of other discontinuities that can be included in simulation such as gaps and end effects. For a list of components relevant to your design, refer to the Introduction to Circuit Components documentation.

Checking Schematic Component Orientation

The correct orientation of all schematic components is required to successfully generate a layout. Notice the difference in the resulting layout when the orientation of Taper2 (lower illustration) is incorrect.

Pin 1 is always identified by a small tick mark, but you can see all pin numbers by turning on Pin Numbers through Options > Preferences > Pin/Tee.

Establishing Preferences

There are a number of miscellaneous settings you can control for the generation of a layout:

To adjust these options for the design you are about to generate or update:

  1. From the Schematic window, choose Layout > Generate/Update Layout > Preferences (The remaining fields in this dialog box are described in the section, Generating a Layout).
  2. Change any or all options as desired and click OK.

Generating a Layout

After performing the preliminary checks, and taking the recommended action based on the results, you are ready to generate a layout. The transmission line shown next is used to illustrate the process.


To automatically generate a layout from a schematic:

  1. Open a Layout window, and from the Schematic window choose Layout > Generate/Update Layout.
    In this example, the Starting Component field shows P1 (port 1). This can be changed by clicking a different item in the Schematic window. The Equivalent Component field is empty, indicating that the equivalent has not yet been created (in the layout). In addition, all of the components in the schematic are highlighted, indicating that they all need to be generated.
    Hint
    If choosing Generate/Update Layout causes an item to be highlighted, the highlighting indicates that the item needs to be generated, regenerated, or repositioned.
  2. Click OK and the layout is generated, as shown in the initial illustration.
    The details of the Generate/Update dialog box are as follows:

For all artwork supplied in ADS, the angle of each pin is preset to generate a reasonable topology. However, it may be necessary to flip and rotate components to get a better layout; this will have no effect on your schematic.

Placing Unplaced Components

Unplaced components are items that do not have counterparts in the other representation. When a component without artwork, such as a series capacitor, is encountered during the synchronization process, the synchronizer places a generic artwork box in its place. Once you create/assign artwork to these components, you can initiate the synchronization process again or you can individually place these remaining components one at a time, interactively, in the other representation:

The Place Components From Schem To Layout command enables you to interactively place items from one representation to the other. It is important to note that placing items in this fashion is different from placing items from a library or palette; if an item is placed from a library or palette, no association is made with its equivalent item until design synchronization is run again.

To locate unplaced items:
Choose Layout > Show Unplaced Components. The unplaced components are highlighted.

To place an unplaced component:

  1. Choose Layout > Place Components From Schem To Layout and click any of the highlighted components you want to place.
  2. Move the pointer to the Layout window. A ghost image of the item, as well as wire guides identifying the connectivity point(s), tracks with the pointer. Position the item and click.

In the illustration that follows, one of dotted lines represents the wire guides that track with the artwork and the pointer.

Using the Design Differences Dialog

The Design Differences dialog box enables you to better manage components between ADS Schematic and Layout. Using the Design Differences dialog box, you can select a design and quickly identify differences between the schematic and layout in your design. Upon identifying these differences, the dialog includes an action-oriented list which enables you to manage:

To access the Design Differences dialog box from a Schematic window,

Choose Layout > Place Components From Schem to Layout or choose Layout > Design Differences. The Design Differences dialog box appears.

To access the Design Differences dialog box from a Layout window,

Choose Schematic > Place Components From Layout to Schem or choose Schematic > Design Differences. The Design Differences dialog box appears.

Components not in layout
Components that are in your schematic, but not in your layout, are identified in the Design Difference, Components not in layout expandable list. Clicking a component in this list will highlight the component and enable you to quickly identify the component in the schematic. Once selected, the component is in placement mode which enables you to move the cursor over the layout and place the component by clicking your mouse in the desired location on your layout.

If you right click your mouse, a popup menu appears with the following options:

Components not in schematic
Components that are in your layout, but not in your schematic, are identified in the Design Difference, Components not in schematic expandable list. Clicking a component in this list will highlight the component and enable you to quickly identify the component in the layout. Once selected, the component is in placement mode which enables you to move the cursor over the schematic and place the component by clicking your mouse in the desired location on your schematic.

If you right click your mouse, a popup menu appears with the following options:

Parameter Differences
Clicking this option will highlight the component in both the layout and schematic and enable you to quickly identify the component in question and correct the parameter differences.

If you right click your mouse, a popup menu appears with the following options:

Nodal Mismatch
Clicking this option will highlight the unconnected components in both schematic and layout enabling you to quickly identify the components in question and correct the mismatch.

If you right click your mouse, a popup menu appears with the following option:

Note
Due to system limitations, layout components that refer to items on schematic could possibly be out-of-sync with respect to the schematic and not be in the Design Difference list (includes components referencing MSUBs, SMT_Art and variables).

Auto Zoom

Auto Update

Fixing and Freeing Component Positions

All items in the Schematic and Layout windows have either a fixed or free status associated with their position. If an item's position is fixed (in the target representation), then it cannot be repositioned automatically by the program during the design synchronization process. If an item's position is free, then the program may reposition that item. Understanding the basic behaviors involved will help you in manually creating designs, as well as generating one representation from another:

The following commands (found on the Layout and Schematic menus) can help you identify and change the fixed versus free status of a component, relative to the window from which you issue the command:

Component Highlighting

After choosing Layout > Generate/Update Schematic, all components that will be generated or regenerated during the design synchronization process will be highlighted. Components that meet one or more of the following conditions will be highlighted at this point:

If a component, or component sub-design (if hierarchical), contains a variable or expression in a parameter, or if the component contains SMT artwork, the component will always be regenerated during design synchronization. Therefore, these components will always be highlighted.

Dual Representation Mode

When working from either schematic or layout, it is sometimes desirable to have items placed in both representations simultaneously. This is accomplished using the dual placement or synchronization modes found in Options > Preferences > Placement.

Generating a Schematic (Layout-driven Design)

Generating a schematic from a layout involves steps similar to those used in generating a layout from a schematic. When you modify the layout, its modified parameter values can be back-annotated to the schematic in a similar fashion.

Layout items can be picked from a palette or library list and placed and interconnected in the Layout window. If a library of layout components has been created and associated with schematic and simulator items, they can be added to existing palettes or new custom palettes. For detailed information, refer to Creating Elements.

To generate a schematic from layout:

  1. Open a Layout window.
  2. Create your layout design in the Layout window (by placing items from the library and palette) and interconnecting them by abutting their pins or connecting them with traces, as shown in the following example.
    Note
    Before you can place an item (such as SLIN) in the Layout window that references a substrate item, you must place that substrate item in the Schematic window.
  3. From the Layout window choose Schematic > Generate/Update Schematic. The dialog box appears, and all items in your layout are highlighted, indicating that they need to be generated, updated, or moved in the other representation.
  4. Accept the default Starting Component (C1 in this example) or click a different item in your layout (the item you want the program to use as the starting point for generating your schematic).
  5. Click Preferences and specify the horizontal and vertical spacing that you want between the items in your schematic, then click OK.
  6. Specify the location and angle of the equivalent item in the Schematic window, and click OK. The equivalent schematic appears in the Schematic window.
    Note
    When creating Momentum layout components for use with the Schematic > Generate/Update Schematic command, you need to deselect the Add reference pin checkbox in the Create Layout Component dialog. For more information, refer to the section on Layout Components for Momentum in the Momentum documentation.

RF PCB Design Considerations

Many RF PCB applications require an interactive approach to layout. Typically, a schematic is created and simulated before layout begins. The Design Environment supports creating layout at any time, before during or after a schematic is created. A large 90,000 part library is supplied; many parts are available with their packaged-part outlines and mounting footprints.

The layout tool contains a number of features specially designed to support PCB layout. These include:

Creating the Board, System Setup

You will need to draw or import a board outline for the PCB you are designing. A number of layers have been pre-defined for PCB board layout. The silk-screen layers are defined to place text and other silk-screen information. The pcb1-9 layers are designators for trace routing using traces or the PCB transmission line components. Other layers can be used or defined as needed. There are no limits to the number of layers that can be defined, though the multi-layer PCB transmission line components have a limit of nine conductor layers.

Interactive Layout, Manual Layout

Components can be placed in layout at any point in the design. As in the schematic, parts can be placed in the layout by selecting them from a palette or library and positioning them on the board. Most of the standard SMT parts and other packaged parts are selected from library lists.

Parts can be moved to the bottom side of the board, or placed on the bottom by mirroring them. When creating a schematic for a PCB design, make sure every part has a layout equivalent. For ideal components, such a CAP, RES, etc., use the Lumped-With Artwork version of these components to account for them in layout.

Parts can also be placed directly from the schematic. The advantage is that the schematic and layout can then be kept synchronized. It is important to note that if you place items in the schematic with the library or palette lists, and then place equivalents in the layout in the same manner, the two will not be synchronized. To keep the layout and schematic synchronized, you must either use the Generate/Update feature to automatically create one representation from the other, or use interactive placement to incrementally create one representation from the other.

Automatic Design Synchronization

A layout can be automatically created from an interconnected schematic using the design synchronization feature (Generate/Update). This command will take each component in the schematic and place it in the layout so that the interconnected pins abut. While this works very well for microwave designs that have every transmission line discontinuity accounted for in the schematic, it does not usually produce acceptable results for PCB layouts that have extensive interconnections using traces. It will, however, give you an initial placement of components that can then be moved into a correct position.

Interactive Placement

Placing parts interactively from the schematic to the layout, or vice-versa, is usually the most practical method of creating a PCB layout. The Place Components From Schem To Layout (or Layout to Schem) command is used to select a part in one representation and place it in the other.

The command prompts you to pick a component in the source representation and place it in the target. If initiated from the Schematic window, you are prompted to click a schematic component and then move the cursor into the Layout window. A ghosted image of the part can then be seen moving with the cursor. You can use the arrow buttons on the palette to rotate the part before placing it. Clicking the left mouse button places the part, with the same parameter values used in the schematic.

Wire guides are displayed that indicate where each component should be connected. These lines can be re-displayed by using the Schematic > Show Connected Components command, which will draw a connection (rat's nest) depicting the interconnection of each unconnected pin using the source representation as the reference. Use Clear Highlighted Components to remove these lines.

The Schematic > Place Components From Schem To Layout (or Layout to Schem) command highlights all the components in the reference representation not yet placed in the target. Use the Clear Highlighted Components command to remove highlighting.

Fixing Part Placement and Back Annotation

When parts are placed in the layout, they are placed as free components. That is, if design synchronization is run, the part will be repositioned to abut at least one of its pins with an interconnected component. While this is the preferable method of synchronizing microwave designs, it is usually not the desirable method for PCB components.

If the parts were placed with the Place Components From Schem To Layout (or Layout to Schem) command, they will be placed as fixed components. That is, they will not be repositioned when design synchronization is run. However, if they were placed in some other manner, they will be placed as free components and will need to be set to fixed. To check the status of the placed components in layout, choose Schematic > Show Fixed Components. This will highlight each fixed component. For non-highlighted components, select these and use the Schematic > Fix Component Position to fix these components' positions.

Once the components are placed, you can use the design synchronization feature of the program to maintain parameter changes in one representation with the other. Thus, if you change the value of a capacitor in layout, you can back-annotate this change by running design synchronization from the Layout window. Each component that is not yet placed or that has a changed value will be highlighted. Clicking OK or Apply in the dialog box will update the highlighted parts in the target representation.

Trace Routing

You can use traces (or wires) to parts when you do not want to connect them merely by abutment.

Layout Versus Schematic Nodal Mismatches

You can compare the layout and schematic any time during the design process using Tools > Check Design and selecting the Nodal mismatches (layout vs. schematic) option. This will generate a report that compares the connectivity of the target representation against the source. Missing components, or pins connected differently in one representation from the other are reported.

Note
This option works on designs where the layout is composed of layout items that have schematic equivalents. It does not work on arbitrary geometry, nor does it do any device extraction. For complex layouts that are mis-connected in more than one area, running the command from both representations can help better pin-point the source of the mismatch. Using this command in conjunction with Layout > Show Unplaced Components, Show Equivalent Component, Show Connected Components commands can usually solve most discrepancy problems.

Trace Simulation

For many high-frequency PCB designs, transmission line effects become significant and need to be accounted for in simulation. In Layout, you can explicitly convert traces to transmission line components for simulation, or globally simulate traces as transmission lines without explicitly converting them. For more information, refer to Working with Traces under the section on Creating a Layout.

Meander Trace Simulation

MEANDER components are simulated using the MLIN electrical model. In order to account for the effect of bends, use Traces (which can be broken down to lines, bends, and tees), or MLIN, MBEND, MTEE directly.

Generating a Report

To generate a Bill of Materials (BOM) or Parts List with pick and place information, choose File > Reports. These reports are created using the de_bom and de_parts AEL functions and can be customized. For more information, refer to Pick and Place Report under the section on Setting Layout Options in the Customization and Configuration documentation.

Exporting the PCB layout

Most PCB layouts are manufactured via Gerber output. Gerber is supported via the optional MTOOLS Gerber translator. The design environment interfaces with the Gerber translator via mask files. A mask file can contain one or more layers. All design exporting is done through File > Export in the Layout window. For general information, refer to Importing and Exporting Layouts. For detailed information, refer to the Importing and Exporting Designs documentation.

Part and Library Creation

Though a large library of PCB discrete components is available, you may not find the components and their layout footprints you are looking for. But you can define new items in a number of ways. For details refer to Creating Elements. Note, that a large number of layout objects are also available. For non-electrical items, these can be placed directly in the layout without concern for the schematic. For electrical items, you can create a new item that uses a pre-defined layout object for layout, or you can use an ideal component such as a CAP or S2P with a gap artwork equivalent. The gap can be specified to allow the layout object to then be inserted.

 

Privacy Statement  | Terms of Use  | Legal | Contact Us  | © Agilent 2000-2008 

Contents
Additional Resources