Editing a Layout

As in other areas of the program, most edit commands enable you to select one or more components either before or after you select the edit command. The most commonly used editing commands, Copy, Delete, Move, Rotate, and Undo are performed in a layout just as they are in any other part of the program. As in other areas of the program, you can edit text, and you can change either the attributes of existing text, or define the attributes of all subsequent text.

An electrically complete layout circuit has all components connected. This chapter provides information on editing and connecting layout circuit components.

Using Selection Filters

Selection Filters enable you to specify the types of components you want to include or exclude in sections. Any component that is turned off is not selected when you click on it individually, attempt to enclose it in a selection window, or choose the Select All command. Only the Select By Name and Deselect By Name commands ignore the selection filters.

By default, all types of components are turned on except Drawing Format.

Choose Options > Preferences > Select

Editing Shapes

There are a variety of editing operations you can perform on common layout shapes. For details on these editing operations, refer to the section of interest:

Selecting Shapes

In addition to the selection features provided by the selection filters, you can quickly select all items on a layer you specify or you can select all items in a nodal interconnect.

To select all items on a given layer:

  1. Choose Select > Select All On Layer.
  2. In the dialog box that appears, select the layer containing the items you want to select for editing. To select all items on multiple layers, click Apply after selecting each layer, then click OK. The items on the chosen layers are selected for editing.

To select all items in a nodal interconnect:

  1. Choose Select > Select Interconnect > Nodal to select the polygons, paths, rectangles, wires and traces that make a nodal interconnect. Choose Select > Select Interconnect > Nodal With Components to select shapes and component instances that are interconnected.
  2. Use the mouse to select a shape. All shapes in the same interconnect will also be selected.

Manipulating Polygons and Polylines

There are several ways to modify polygons and polylines after drawing them:

Creating a Polygon from Intersections or Polylines

To create a polygon from the union of two intersecting closed shapes:

  1. Select the two shapes.
  2. Choose Edit > Merge > Union.


To create a polygon from the intersection of two closed shapes:

  1. Select the two shapes.
  2. Choose Edit > Merge > Intersection.


To create a polygon from two intersecting closed shapes, with the intersection removed:

  1. Select the two shapes.
  2. Choose Edit > Merge > Union Minus Intersection.

Converting a Shape to a Polygon

To convert a shape to a polygon:

  1. Select the shape, where the shape can be a circle or polygon containing an arc.
  2. Choose Edit > Modify > Convert To Polygon. All curves are converted to line segments that approximate their original shape. The number of line segments used in this conversion is determined by the setting Arc/Circle Resolution (degrees) in Options > Preferences > Entry/Edit.

Joining Multiple Polylines

To join selected polylines (with coincident endpoints) into a single polyline:

  1. Select the individual polylines you want to join.
  2. Choose Edit > Modify > Join. All coincident endpoints are joined. You can verify what has been joined by clicking on the shape to select it and observing whether or not the entire shape is selected.

To verify what has been joined, click the shape to select it and observe whether or not the entire shape is selected.

Converting a Polygon into Individual Two-point Line Segments

To convert a polygon into individual, two-point line segments:

  1. Select the polygon.
  2. Choose the command Edit > Modify > Explode. All vertices are disconnected leaving individual line segments that you can edit as needed.

Converting a Polygon into a Single Polyline

To convert a polygon into a single polyline:

  1. Select the polygon.
  2. Choose Edit > Modify > Break. The starting and ending points of the polygon are broken, identified by a marker, and you can now manipulate the shape as a polyline.

Chopping a Selected Region Off of a Shape

To chop a selected region off of a polygon, rectangle, circle, or wire/trace, do the following:

  1. Select the shape.
  2. Choose Edit > Modify > Chop.
  3. Use the mouse to draw the rectangular region to be chopped over the object.

Extending the Endpoint of a Polyline

To extend the endpoint of a polyline to a designated reference line segment:

  1. Choose Edit > Modify > Extend.
  2. Click on the line that you want to extend.
  3. Click on the reference line.

Cropping a Shape

To save the specified area of a polygon, rectangle, circle, or wires/trace and delete the remainder, do the following:

  1. Select the shape.
  2. Choose Edit > Modify > Crop.
  3. Use the mouse to draw the rectangular region to be saved over the object.

Splitting a Shape

To split a polygon, rectangle, circle, or path/trace into multiple objects:

  1. Select the shape.
  2. Choose Edit > Modify > Split.
  3. Use the mouse to draw the rectangular region to be split away from the rest of the object.

Stretching the Edge of a Shape

You can redefine a shape by stretching an edge (a segment between two vertices).

  1. Choose Edit > Move > Move Edge. You are prompted to enter the location of the line.
  2. Click once on the edge you want to stretch. A ghost image moves and changes as you move the cursor, showing how the shape will be redrawn.
  3. Click again to define the new shape.

Scaling Shapes

To scale an object or text by a percentage:

  1. Choose Edit > Scale/Oversize > Scale and the Scale dialog box appears.
  2. Enter scaling factors for both X and Y.
    Scaling factors must be positive. Scaling factors greater than 1.0 increase the size of objects, while factors less than 1.0 decrease the size of objects. To scale the objects uniformly, enter the same scaling factor for both X and Y. For text, only the X scale is used.
  3. Click OK and you are prompted to enter a reference point on the object around which to scale.
  4. Click to specify the reference point, and the object is scaled.


To scale an object relative to the design units:

  1. Select the object.
  2. To replace the original object with a scaled image, choose the command Edit > Scale/Oversize > Oversize.
    To place a copy of the selected object (using the size you specify) on the current entry layer, preserving the original object, choose the command Edit > Scale/Oversize > Copy & Oversize.
    When you select either of these commands, a dialog box appears.
  3. Enter the sizing amount. A positive number increases the size of the object; a negative number decreases the size.
  4. Enter a cutoff angle for mitering corners. Any angle of a polygon smaller than the specified cutoff angle is mitered. Default = 45°.
  5. Make any changes in the dialog box, and click OK.

If you chose Oversize in step 2 above, the object is scaled to the specified size.

If you chose Copy & Oversize in step 2 above, a copy of the selected object is drawn on the current entry layer, at the specified size.

Manipulating Vertices

Note
To select, move, or delete a vertex, the Vertices select filter must be on (see Using Selection Filters).


To add a vertex to a polygon or polyline:

  1. Choose Edit > Vertex > Add.
  2. Click on a point between two existing vertices, and move the mouse. A flexible line is drawn between the vertices and the cursor.
  3. Click again to specify the new point and the shape is redrawn.


To move a vertex:

  1. Select Edit > Move > Move, click on the vertex, and move the mouse. A flexible line is drawn from the affected vertices to the cursor.
  2. Click again to specify the new location, and the shape is redrawn.

To delete a vertex:

  1. Draw a selection window enclosing all vertices that you want to delete.
  2. On the toolbar, click the delete button. The shape is redrawn without those vertices.


To delete an arc from a polyline

  1. On the toolbar, click the delete button.
  2. Click anywhere on an arc. The arc is deleted and the former endpoints of the arc are connected with a straight line.

Converting a Vertex to an Arc

You can convert any vertex to an arc and specify the desired radius of the arc, with respect to the units of the window.

  1. Choose Edit > Point > To Arc. You are prompted enter location of the vertex, and a dialog box appears.
  2. Set the radius as desired and click Apply.
  3. Click on any vertex that you want to convert to an arc. The vertex is redrawn accordingly.

    You can continue converting vertices in this manner using a different radius each time if desired, but you must click Apply each time you change the radius.
  4. When you are through making these changes, click OK to dismiss the dialog box.

Converting a Vertex to a Mitered Edge

You can convert any vertex to a mitered edge and specify the desired length of the mitered edge, with respect to the units of the window.

  1. Choose Edit > Vertex > Miter. You are prompted enter location of the vertex, and a dialog box appears.
  2. Set the miter length as desired and click Apply.
  3. Click on any vertex that you want to convert to a mitered edge. The vertex is redrawn accordingly.

    You can continue converting vertices in this manner using a different miter length each time if desired, but you must click Apply each time you change the length.
  4. When you are through making these changes, click OK to dismiss the dialog box.

Moving Shapes or Text to a Different Layer

To move shapes or text to another layer:

  1. Select the object you want to move.
    Note
    Do not use the Move To Layer command to move ports to a different layer; set the Layer parameter of the port to the desired layer.
  2. Choose Edit > Move > Move To Layer. A dialog box appears with a list of currently defined layers. Select the desired layer and click OK. The selected object immediately takes on the color and other display characteristics of the selected layer.
Note
The following items can be moved to another layer using the context-sensitive menu that appears when you right-click with the pointer positioned over any of these items: Polygon, Polyline, Rectangle, Circle, Arc, Text, Arrow, Wire, Construction Line, Path, Trace.

Manipulating Dimension Lines

Dimension lines can be moved and modified.

Moving Endlines

A dimension line can be stretched using the Edit > Move > Dimension Line Endline command. This is done as follows:

  1. Choose Edit > Move > Move Dimension Line Endline.
  2. Move the cross-hairs over the dimension line end that you want to stretch and click.
    Note
    If you have trouble selecting the end of the dimension line, see if the dimension line arrowhead is visible. If it is not, zoom in and try selecting the end of the dimension line again.
  3. Move the cross-hairs to the desired position and click.

Modifying Dimension Lines

To modify the attributes of a dimension line, do the following:

  1. Double-click on the dimension line.
  2. The Dimension Line dialog box appears.
  3. Choose the parameter that you want to change from the Select Parameter list.
    The choices are:
    LineLength - The length of the dimension line.
    LineOffset - The dimension line vertical offset from the x-axis.
    Endline - The height of the end line from the dimension line.
    ArrowLength - The length of the arrow.
    ArrowWidth - The width of the arrow.
    ArrowDir - The arrow direction. The possible values are inward and outward.
    TailLength - If ArrowDir is inward, this represents the length of the arrows' tails.
    Layer - The dimension line layer.
    TextOffset - The text offset from the dimension line.
    TextHeight - The text height.
    Precision - The displayed length precision.
    TextPosition - The text position in relation to the dimension line. Available choices are above, below, left, or right.
    TextUnits - The unit to use to display distance.
  4. Edit the parameter settings
  5. Click OK to save the change and close the dialog box.

Moving an Object to the Coordinates 0,0

By default, the coordinates 0,0 are located in the center of the Layout window. You can reposition an object that you have placed or drawn elsewhere, at the origin.

  1. Choose Edit > Modify > Set Origin. You are prompted, enter origin location.
  2. Click the point of the object (for example, pin 1) that you want to position at 0,0 and the object is moved; the specified point is now located at 0,0.
Note
You can use the View All command to bring the object back into view.

Forcing an Object onto the Grid

If an object is offset from the current grid spacing, you can force it to the nearest grid point. If the selected object is an component with pins, pin 1 is forced to the nearest grid point.

  1. Select the object.
  2. Choose Edit > Modify > Force to Grid. The selected object snaps to the grid.

Editing Layout Hierarchy (Flatten)

When you are ready to generate final artwork, you can remove levels of hierarchy. This process copies all data from the referenced design to the current representation, resulting in the removal of one level of hierarchy. Repeat this process for each level of hierarchy you want to delete. When you finish, the design will be intact, but contain no references that could affect the final design.

  1. Open the top-level hierarchical design.
  2. Select an instance.
  3. Choose Edit > Component > Flatten.
    This copies all data from the component to the current representation and deletes the reference to the subdesign. Note that one level of hierarchy is removed.
  4. Repeat this procedure for each instance you want to flatten.
  5. To check that all hierarchy levels have been removed choose Tools > Hierarchy. This should produce an empty report.
  6. Save the design.
Note
If you want to remove all levels of hierarchy with one command, choose File > Generate artwork.

Physical Connectivity Engine

The ADS Physical Connectivity Engine enables you to establish electrical interconnects based on polygon shaped layout artwork and performs interconnect information extraction on the fly.
Key features include:

Polygon-Based Layout Connectivity

Polygon-based layout connectivity removes the interconnect constraints of wires and traces and provides the ability to establish electrical connections with polygon based layout artwork. It also enables the use of custom tailored native interconnect configurations exhibiting electrical connectivity.

This functionality gives you the flexibility to start a design either in schematic or layout, implement custom tailored layout interconnects (beyond simple traces), perform on the fly layout interconnect information extraction, and back annotate custom tailored interconnects to the schematic.

Other benefits include more robust design crosschecks between layout and schematic; open connections, nodal and components' values mismatches, zero width wires in layout, overlaid components, layout shapes touching but belonging to different nodes, polygon/component overlapping, and non pin to pin connections. Significant improvements to design connectivity validation include polygonal shapes touching or overlapping but belonging to different nodes or not making a pin to pin connection.

The physical connectivity engine now takes care of potential connectivity problems that went unchecked previously, mainly due to the lack of arbitrary layout artwork connectivity information. For more information, refer to Creating Interconnects with Shapes.

Simplified Vertical Interconnects

As polygon shapes now exhibit electrical connectivity characteristics resembling real world conditions, vertical electrical connections are possible without requiring pre-built via components. Designers are no longer limited to the availability of pre-built via components in design kits (for MMIC designs) or component libraries (for PC board and module design) to establish vertical electrical connections. You can also define pin-less vias either in via macros or by overlapping layout artwork on a multi layered stack. The advantages of the new pin-less vias are simplified vertical connections, and the absence of the need to have via components placed in schematic as well as layout. See Creating Interconnects with Shapes for more information.

Edge/Area Pins

Another enhancement to ADS Layout connectivity is the expansion of pins beyond the point pin concept to include edge and area pins. This capability is most useful for design kit and component library developers, because it allows them to define unique edge and area pins to their layout components, however simple or complex they may be. For more information, refer to Designating Edge and Area Ports.

Nodal and Physical Interconnect Verification

The physical connectivity engine also enhances the ability to perform robust interconnect verification. Because all polygonal shapes in layout carry electrical connectivity information, you can perform a significant number of verification checks, including nodal and physical connectivity checks, at any point in the design process. For more information, refer to Checking Connectivity Information in Layout.

Nodal interconnect check enables you to check the design's nodes in schematic and layout (the definition of node is understood as a pin/port and all touching interconnects, excluding design components, whether they are active or passive.) This feature is very useful for performing schematic/layout nodal cross-probing to verify the accuracy of their designs as simple wires in schematic transform into elaborate physical interconnects. For more information, refer to Highlighting Interconnects and Cross-Probing.

Physical interconnect check provides the ability to highlight all shorted (touching) metal in multi layer hierarchical designs. This enables an easy to perform interconnect integrity check for a design's physical layout, which identifies what a given metal trace, path, polygon, or transmission line touches. For more information, refer to Highlighting Interconnects.

These capabilities can help microwave designers check the validity of their designs' physical as well as nodal connectivity without overlooking important high frequency attributes. The physical connectivity engine accomplishes this by extracting physical and nodal connectivity information upon opening a design (i.e. during design loading into layout environment) as well as while editing a design layout (i.e. on the fly extraction). Because connectivity extraction is performed in real time, large design files may take significantly longer to load into the layout environment. The amount of time required depends on hardware configuration, and upon available memory (where connectivity information is stored).

Usage Notes

  1. The Physical Connectivity Engine requires a proper definition of the shape and pin layer binding. Otherwise unwanted connections and false connectivity warning messages may be generated.
  2. When loading a large layout (i.e. reticle layout), you might observe a delay. This delay is caused by the real-time extraction of the layout connectivity information.
    For these reasons, you may need to disable the Physical Connectivity Engine. For more information and step-by-step instructions, refer to Disabling Layout Connectivity Features.

Connecting Layout Components

Regardless of how you connect components, you should turn pin snapping on before you begin (Options > Preferences > Grid/Snap > Pin). Keep in mind that while it doesn't always cause performance problems, the intersection snap mode is the slowest of all snap modes so you should use this mode only when necessary. For more information, refer to Changing Grid and Snap Settings under the section on Setting Layout Options in the Customization and Configuration documentation.



Checking Connectivity Information in Layout

In the Layout view, the Check Design command provides access to information about the characteristics of your design. To access it, select Tools > Check Design. The Check Designs dialog will appear and list any warnings found in the Description field. These warnings are based on the selected items under the Check Design Options menu. The Location field shows the x and y coordinates that refer to a specific warning message location. Selecting either the location number or description will highlight the instance on the layout. Checking the Auto Zoom box will zoom the layout in on the location of the warning.

To see the details of any of the warnings listed, select the warning and click the Details button. An information window will list exact coordinates, instances, etc.

To access the Check Design Options menu click the Options button.
The options to check for are:

Highlighting Interconnects

There are two choices for viewing the connectivity between objects on your layout:

Show Nodal Interconnect

Choosing Tools > Check Connectivity > Show Nodal Interconnect and clicking on a pin, wire, trace or polygon in your layout will highlight all objects at the current level that are connected to the same logical node. Nodal highlighting is used to highlight the interconnect metal between components.

Note that Show Nodal Interconnect , does not highlight components.

Show Physical Interconnect

Choosing Tools > Check Connectivity > Show Physical Interconnect and clicking on a pin, trace or polygon in your layout will highlight all objects that are physically connected to the object you selected, throughout the hierarchy. Physical highlighting is used to highlight all metals including those that are part of components. Physical highlighting will follow connections through vias onto another metal layer. Objects are physically connected when shapes on the same layer touch or overlap and when connections to another layer are made by a via.

Note that the red metal in the inductor is highlighted because it is connected to the green metal layer by a via at its center. Also, the highlighting extends to the dual gates of the FET at bottom right.

Cross-Probing

To see the schematic representation of a specific node in your layout, choose Schematic > Show Equivalent Node and click the pin, wire, trace or polygon that you would like to see in the schematic. When you view the schematic, the wire or pin representing the node of the object that you selected in the layout will be highlighted.

Disabling Layout Connectivity Features

Disabling layout connectivity features is only meant to be used when the layer binding cannot be properly set or when there are specific performance problems with large designs such as reticles.

To disable layout connectivity features,

  1. Choose the Tools > Preference menu option from the ADS Main window.
  2. Uncheck the Enable Physical Connectivity Engine option in the Main Preference dialog box.

If a project is open, ADS will close that project after asking to save changes. The project will be re-opened automatically.

The following functionality will be disabled in schematic:

The following functionalities will be disabled in layout:

To re-enable layout connectivity features, check the Enable Physical Connectivity Engine option in the Main Preference dialog box.

Working with Transmission Lines

For some types of design work, designing from the layout can save considerable time. This is especially true in designs with complex transmission lines. In layout, transmission lines can be created either by placing transmission line elements manually or by inserting traces and converting them to transmission lines later. Regardless of how you create them, there are a number of ways you can edit them.

Splitting a Transmission Line

You can replace one transmission line element with two identical elements.

  1. Choose Edit > Transmission Line > Split Transmission Line.
  2. On the transmission line, and click on a reference point.


Replacing a Transmission Line Element

You can replace one transmission line element with two identical elements and a tee.

  1. Select Edit > Transmission Line > Tap Transmission Line. A Tap Length dialog box appears where you specify the length of the tee element.
  2. Type a number for the tap length, and click OK.
    Either an MTEE or STEE is inserted, depending on whether an MLIN or SLIN was tapped.
  3. On the transmission line, click on a reference point where you want the tee element inserted.
Hint
The third pin of the tee will be placed on the transmission line edge closest to the cursor.

Stretching a Transmission Line

  1. Choose Edit > Transmission Line > Stretch Transmission Line.
  2. Click on a node of the transmission line, and move the pointer away from the element. A flexible dashed line appears and moves with the pointer.
  3. Click on a second reference point (where you want the element to stretch to). The element is now changed to the new length.

Squeezing a Transmission Line While Maintaining its Length

You can modify an existing transmission line to squeeze it into a smaller space, specifying several characteristics in the process, such as corner type, lead length and minimum spacing.

You can adjust any or all of the following characteristics as needed:

To squeeze a transmission line into a smaller space while maintaining its length:

  1. Choose Edit > Transmission Line > Squeeze Transmission Line Keeping Length. In the dialog box that appears, set the options as desired and click Apply.
  2. You are prompted to enter the reference location. Click the pin at one end of the transmission line and you are prompted to enter the offset location.
  3. Move the pointer toward the other end of the transmission line. When the ghost image of the transmission line represents what you want, click to draw the modified transmission line.

Editing Paths, Traces and Wires

This section covers the following topics:

Converting Traces to Paths

Unlike converting traces to transmission line elements, where the conversion is one-way, you can change paths back into traces. Use the following steps to change a trace into a path:

  1. Select the desired trace.
  2. Choose Edit > Path/Trace/Wire > Convert Trace to Path.

Converting Paths to a Traces

Unlike converting traces to transmission line elements, where the conversion is one-way, you can change traces back into paths, as follows:

  1. Select the desired path.
  2. Select Edit > Path/Trace > Convert Path to Trace.

Changing the Attributes of an Existing Path/Trace/Wire
  1. Select the desired traces/paths/wires.
  2. Choose Edit > Path/Trace/Wire > Path/Trace/Wire. The Path dialog box appears.

    Corner Type - Select Mitered, Square, or Curve.
    Width - Specify the width (in layout units).
    Mitered Corner Cutoff Ratio (%) - Set a percentage of cutoff; the larger the number the more of the corner is cut off.
    Curve Radius - Specify a curve radius.
  3. Fill in the appropriate fields, and click OK.

Stretching a Wire

You can change the shape of an existing wire by stretching an edge (a segment between two vertices).

  1. Choose Edit > Move > Move Edge.
  2. Click once on the edge you wish to stretch. A ghost image moves and changes as you move the cursor, showing how the shape will be redrawn.
  3. Click again to define the new shape.

Converting a Wire to a Trace

If the separation between components is intentional, you can convert a wire to a trace.

  1. Select the wire and choose Edit > Path/Trace/Wire > Edit Path/Trace/Wire.
  2. In the dialog box that appears, change the characteristics as desired, and click OK.
    Hint
    Because traces have width, if the wire you are converting to a trace has a bend, the shortest segment that is part of that vertex cannot be shorter than 3 × w/4, where w is the width for the trace, as specified by Path Width.

Editing Component Text

By default, when you place a component in layout, its Instance Name (a unique ID) is automatically placed with it on the silk_screen layer (The Component Name is placed on the silk_screen2 layer, which is not visible by default.) Instance Names are automatically assigned but you can change them as long as you maintain unique IDs for each instance.


To change the Instance Name for a given component, use either of the following methods:


To change component text attributes (font and size):

  1. Select the component and choose Edit > Component > Component Text Attributes.
  2. Change the attributes as desired and click OK.

Using Boolean Logical Operations

In the Layout window, you can insert onto any destination layer polygons that are the result of comparing the contents of two layers. In effect, the material you select on the source layers is copied to a destination layer according to logical rules.

Use the following steps for any of the logical operations described in this section:

  1. Ensure that the source layers and the destination layer are not protected (Options > Layers).
  2. Choose the command Edit > Boolean Logical.
  3. In the dialog box that appears, use the drop-down lists to indicate the two source layers, the operation you want performed, and the destination layer. Except for DIFF, it makes no difference which source layer you identify first. See Edit > Boolean Logical > DIFF.
  4. Select whether you want the logical operation to apply to shapes that you select, or to all shapes on the two source layers.
    If you choose Selected Shapes, you must select at least one object on each of the two source layers.
    For Boolean operations across the hierarchy, when an instance is selected, all objects in it will also be selected.
  5. Select whether you want the original shapes deleted.
    In a hierarchical design, only the shapes at the top level of the design will be deleted.
    Traces are not deleted from the design but are used to generate boolean results.
  6. Click OK to perform the selected operation on the shapes.
    Hint
    To exclude a shape from a Boolean operation, select the shape, open its Properties dialog box (Edit > Properties), and add the following property.
    Name=DB_NO_BOOL, Value= 1, Value Type= Integer

Edit > Boolean Logical > DIFF

Use DIFF to create (on the destination layer) one or more polygons that are a copy of everything that you select on the first source layer minus the material you select on the second source layer that is in the same x, y location. In effect, the system copies the material that you select on the first source layer, and then subtracts from it the material that you select on the second layer.

In the following examples, the result on the destination layer appears to the right, beside the source layers. This does not happen in the program, where objects on the destination layer appear in the same x,y location as in the source layers.

Example 1

In this example, the cond layer is specified as the first source layer. The program first copies the rectangle on that layer. Then (in effect) the circles on the cond2 layer (the second source layer) are subtracted from it. The result is a polygon, as shown.

Example 2

In this example, the cond2 layer is specified first. The system first copies the circles on that layer. Then (in effect) the rectangle on the cond layer is subtracted from them. Only parts of the two circles at the top of the cond2 layer appear on the destination layer. Everything else on that layer lies within the boundaries defined by the rectangle on the cond layer.


A practical application of the DIFF option would be to create holes on a layer. This would be done as follows:

  1. Place all shapes on the Cond layer.
  2. Place all holes on the Hole layer.
  3. Choose Edit > Boolean Logical > DIFF.
  4. In the Boolean dialog box, go from left to right and make the following menu selections: Cond, DIFF, Hole, and Cond.
  5. In the Apply To section, select All Shapes.
  6. Select the Delete Original button.
  7. Click the OK button.

Edit > Boolean Logical > AND

Use AND to create (on the destination layer) one or more polygons that are a copy of only those things selected that are in the same x,y location on both source layers. The system deletes material that appears on only one source layer. In the following example, the destination layer contains only the parts of the circles on the cond2 layer that are inside the boundaries defined by the rectangle on the cond layer. The upper parts of the top circles are in a region where there is nothing on the cond layer, so they do not appear on the destination layer.

Edit > Boolean Logical > OR

Use OR to create (on the destination layer) one or more polygons that are a merged copy of everything selected on either source layer. In the following example, the destination layer includes (in a single, merged polygon) the rectangle on the cond layer and all of the circles on the cond2 layer. This includes the two circles at the top of the cond2 layer, even though parts of them are outside the boundaries defined by the rectangle on the cond layer.

Edit > Boolean Logical > XOR

Use XOR to create (on the destination layer) one or more polygons that are a merged copy of everything selected that appears in any x,y location on only one source layer. Anything that appears on both source layers is, in effect, deleted.

In the following example, the destination layer is similar to the first DIFF example, except that the polygon includes the parts of the two circles at the top of the cond2 layer that are outside the boundary defined by the rectangle on the cond layer. These are included because they appear only on the cond2 layer.

Creating Clearance

Choose Edit > Create Clearance and use the Create Clearance dialog to define clearance between ground planes and shapes on multiple mask layers.

  1. In a layout window, with shapes on different layers, choose Edit > Create Clearance
    Note
    To display shapes as outlines, select Edit from the Layers menu, then select Outline from the Shape Display drop down menu.
  2. The Select Planes dialog will prompt you to select the ground plane shapes. Hold down Ctrl to select more than one object. Click OK to continue, the Create Clearance menu will appear. If no objects were highlighted, an error dialog will be displayed.
  3. In the Create Clearance menu select the Clearance Layers using the arrow buttons, select which shapes to Apply to using the radio buttons, and enter the Clearance Value in layout units. Click OK.
  4. The resulting layout will reflect the clearance value selected.
 

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

Contents
Additional Resources