Artwork

Any item can have an artwork representation. There are several ways to define artwork for any given item you want to represent in layout, but in general, the artwork is categorized in one of two ways:

For both types of artwork, a large number of artworks are supplied, but you can also create custom artwork of either type.

Fixed Artwork

The simplest artwork is fixed artwork and over 100 fixed artwork shapes are provided. Fixed artwork can be thought of as a layout object. These objects are saved in design files and may or may not have connection pins. This type of artwork is often used for layout items that do not change size or shape based on parameter settings. For example, an SOT23 package outline is the same for any device with that package, regardless of the device operating parameters.

AEL Artwork Macros

A more flexible approach is to use the AEL artwork creation functions to define the artwork for an item. The artwork for the built-in transmission line elements (microstrip, stripline, etc.) is defined in this fashion, and over 200 AEL artwork macros are provided. These macros include functions for creating solder pads, space artwork and no artwork.

The AEL macro is versatile because it can accept parameters that are used to determine the shape, size, layer, and connection points of the layout artwork. Every reference to an item defined with an AEL macro can be different, depending on the parameters passed to it.

Special Types of Artwork

The following special types of artwork are also available: space artwork, connection artwork, and SMT package artwork.

Space Artwork

Space artwork refers to leaving a space or gap in layout. No actual artwork is created with the space macro. Instead, it instructs the program to view items connected through an item with space artwork as connected. In the layout, a gap is created separating items connected to the item with space artwork.

Using this artwork type is common for layouts where the artwork representing a simulation item may frequently change. For example, you may have an S-parameter device model (S2P) in your design and wish to swap out the referenced S-parameter file to test different devices.

If each device has a different artwork representation, there is no one package outline to assign to this element. However, by assigning space as the artwork (SPAC), you can leave a gap, whose size is a parameter of the item, and insert a layout package outline later.

Built-in item definitions have been supplied for the most common cases of simulation items that could benefit from using SPAC as artwork. These include many lumped elements as well as the S2P element, and can be found in the Lumped Components (with artwork) and the Linear Data File Items (with artwork) palette and library groups. Any item from the library of packaged parts supplied with the program, or layout object you define, can then be used to insert into the space for layout.

Connection Artwork

Connection artwork is a special case of space artwork. However, rather than leaving a gap in layout, it simply connects items that are connected through it together (a space of 0). In other words, items with connection artwork are simulated and included in your schematic, but are ignored in layout. For example, you may have included parasitic capacitors or resistors in your network that have no artwork. By assigning connection artwork to these items, you can include them in simulation and have the layout ignore them.

It is important to use items with connection artwork, rather than items without any artwork assigned at all, to ensure that the layout can be automatically synchronized with the schematic.

Like items with space artwork, the most commonly used items with connection artwork have been pre-defined and included in the program. These are also listed in the Lumped-With Artwork and the Linear Data File Items (with artwork) palette and library groups.

SMT Package Artwork

SMT package artwork is available for over one hundred parts. These artwork macros are versatile because the dimensions of the land pattern can be varied by changing the width and length of the package. The position of the land pattern, with respect to the component package, can be varied by changing the OFFSET parameter. For details on available SMT package artwork and an example, refer to the Layout Library documentation.

Supplied Artwork

Default artwork exists for all microstrip and stripline components, as well as many other components. Artwork also exists for a large number of component libraries. This artwork is in the form of AEL artwork macros.

Default artwork also exists for a number of optional libraries. This artwork is usually in the form of fixed part outlines. For packaged part libraries, it is the component footprint or outline; for other parts it is the actual part geometry.

For other parts, there is no default artwork. To include these components in layout, you need to create special component equivalents with artwork specific to your requirements. For details refer to Custom Artwork below.

Custom Artwork

Custom artwork for a design can be created before or after the simulation model. Depending on what the artwork represents, you may want to create the artwork using an AEL function, or simply create it by drawing a fixed set of shapes. Two examples are given to demonstrate how to create artwork using either method.

Depending on the type of layout you are creating, you can create the artwork as a library of fixed artwork components, as parameterized artwork macros, or a combination of both. For some layouts, capacitors come in a set of fixed, discrete capacitance values, so it may be better to create a fixed layout for each unique capacitance value. In other layouts, the capacitors can take a range of values. If implemented as an artwork macro, the macro can accept a parameter value and adjust shape dimensions to produce the corresponding artwork. Microstrip transmission lines (MLIN) are another example of a component that is best implemented as an AEL macro, because the width and length of the line are passed into the macro (using the length unit set for the design), which controls the size of the rectangle used to represent it.

To simplify creating new items with artwork, AEL functions and a library of fixed artwork are provided. The AEL functions include: functions that generate a space or gap in layout (this allows an artwork to be inserted later), macros for pad placement (for 2-, 3-, and 4-pin components), routines to create different types of PCB pads, a predefined set of commonly used components with space, connection, or pad artwork, and a way to provide a simple electrical connection between items. The fixed library contains artwork for most popular packaged parts outlines, including a large SMT library (For lists of the supplied fixed and AEL macro artwork items, choose File > Design Parameters and view the drop-down list associated with each artwork type.)

Creating a Layout Object

To create a layout object:

  1. For a layout object, open the Layout window and draw the shapes representing the object.
    Optionally, you can add connection points or pins (Adding Pins/Ports to Artwork). You do not need to add pins if the object is going to be used as artwork to be inserted into a layout gap (refer to Space Artwork).
  2. When the artwork is drawn, choose File > Design Parameters in the Layout window for layout objects, or from the Schematic window for schematic objects.
  3. Select Fixed as the Artwork Type if it is to be included in a schematic, otherwise select Not Synchronized.
  4. Type the name of the currently open design file in the Name field (without the.dsn extension).
  5. Type (or select if it already exists) the name of the library in which you want the item stored.
  6. From the Model list in the Simulation field, select Not Simulated.
  7. Check the Layout Object box and click OK.
  8. Save the design.

Adding Pins/Ports to Artwork

For any artwork item you create that will be connected electrically, you will need to add pins. Pins represent an electrical connection point to which a trace, wire, polygon or the pin of another item can be connected. When a port (point port) is placed into a layout and this layout is placed as an instance into another layout, you will see a corresponding pin at a single x,y point.

You can also place edge and area ports in a layout and these will become edge and area pins when the layout is placed as an instance into another layout. Edge and area ports must always be associated with a single (point) port. The point port defines where automatic connections will be made when using design synchronization. If you need to have multiple connection points that represent a single electrical connection to the component, it is suggested that you use multiple edge or area pins, but NPPORT will also work. For more information on edge and area ports, refer to Designating Edge and Area Ports under the section on Creating a Layout.

The NPPORT enables you to place multiple physical connection points that represent a single electrical port. Connecting to any same numbered NPPORT creates the connection. Any component may use NPPORT, and have as many as required. Each NPPORT representing a single connection shares the same port number. The only special requirement when using NPPORT is that one of the ports in the set be a preferred port. A preferred port (PORT component) is a connection point that the design synchronization facility uses to connect to. NPPORT is created using the NPPORT item; preferred ports are created using the standard port item. In a set of multiple ports sharing the same port number, there can be only one preferred port.

When creating artwork using AEL, the same concept applies. The only difference is that ports are created using the de_define_npport() and de_define_port() or de_draw_npport() and de_draw_port() AEL functions.

Creating Fixed Artwork

The artwork for this example is a fixed pattern representing the mounting pads for the chip capacitor. The only parameter for the subnetwork is C, the nominal capacitance. A resistor is added to the schematic to account for loss. An equation is used to calculate the resistance from the nominal capacitance.

The following schematic describes the simulation model.

To create the fixed artwork for the chip capacitor:

  1. Open the Layout window.
  2. Select an entry layer for your artwork (select Insert > Entry Layer).
  3. Optionally, make the grid visible (select View > Zoom In).
  4. Draw the shapes representing the capacitor pads. Be sure your dimensions and layers are appropriate for your design.
  5. Add ports to your artwork. The orientation of the ports determines how components will be connected to your artwork when design synchronization is run. Place port 1 on the left side of the left rectangle with the coordinates at node 1 set to 0,0. Port 1 looks like an arrow pointing into the artwork.
  6. Place Port 2, rotating it to point in to the right rectangle.
    When your capacitor is placed during synchronization, it will have connecting items placed to the right and left of it, at the same angle the capacitor is placed.
  7. Save your design.

Using Edge and Area Ports

  1. Ensure that you have already placed the port that the edge or area port will be associated with.
  2. Add a polyline or arc where the edge port will be located. This will typically be along the edge of some other polygon, rectangle, circle or path.
    or
    Add a polygon, rectangle, circle, or path where the area port will be located. If your artwork already has a polygon, rectangle, circle or path where you want the area port, you do not need to add another.
  3. Use the Edit > Edge/Area Port menu. Select the polyline, arc, polygon, rectangle, circle, or path and the port number it will be associated with. Click OK. Objects that are associated with a port number are highlighted with a light blue outline by default.

Selecting shapes in your layout will change the Port Number value in the dialog, depending on which port the object is associated with. Objects that are not associated with a port will display Not a port as the Port Number value. Objects that are associated with multiple ports will display Multiple as the Port Number value. In this example, the object on the left was selected and is associated with Port Number 1.

The Select Port dialog enables you to select all shapes already associated with a specific port. In this example, Port Number 2 was selected and the Apply button was clicked. This selected the highlighted shape.

Creating Artwork Using an AEL Macro

The artwork for this example is programmable artwork generated using an AEL function for creating a thin film (MMIC) capacitor. The capacitor area is calculated from the parameters passed into the network. You can create the network first, and then the AEL function, or vice versa. Once the artwork function is complete, you need to associate it with the network (Associating Artwork with an Item).

Note
Pins can be created using the following AEL functions: de_draw_port() (using simulator units), de_define_port() (using user units), and de_define_edge_area_port(). For details on these functions, refer to the AEL documentation.

The following schematic describes the simulation model.

To create an artwork function:

  1. Using any text editor, create the macro functions in an AEL file (the file must use an .ael extension). For details on the structure of an AEL function, refer to the AEL documentation.
    The following annotated example is for a thin film capacitor (TFC), tfc.ael: 
    ----------------------------------------------------------------------------
/* layout artwork generation function for MIMCAP element

This example assumes a MMIC process, with two metal layers, and a via layer.
The processing steps required are:    
1) deposit first metal and etch to layer 1    
2) deposit dielectric and etch vias to layer 4    
3) deposit second metal and etch to layer 2

Global technology parameters are provided to show how standard constants 
could be applied to all artwork functions 
*/
//load("stdart");      // make sure we have standard definitions
// define technology parameters, all in MKS 
decl lpad, lab, lpost, wpost, vu, lol, cpua; 
lab = 6e-6;           // length of air bridge
lpost = 6e-6;         // length of post/via
wpost = 10e-6;        // width of post/via
vu = 0.5e-6;          // via undersize
lpad = 4e-6;          // bottom plate pad length
lol = 2e-6;           // bottom plate overlap
cpua = 300e-6;        // capacitance per unit area
// actual artwork generation function
defun mimart(c, ar) 
{
decl c_mks, netu, wcap, lcap;
decl lbot, wvia, w, l;

netu = mks_factor(5); //get length conversion factor from mks
c_mks = c*mks_factor(4); // get capacitance in farads
lcap = sqrt(c_mks/cpua*ar)/netu; // get length in meters
wcap = lcap/ar; // get width in network units

// compute some useful values
lbot=(2.0*lol+lpad)/netu+lcap;// compute length of bottom plate
wvia = (wpost-2.0*vu)/netu;   // compute width of via
w = (2.0*lol)/netu + wcap; // compute overall width
l = (lab+lpost)/netu + lbot;// compute overall length

// draw lower plate and output contact
de_set_layer(1);                      // set the first metal layer
de_draw_rect(0.0, -w/2.0, lbot, w/2.0);
de_draw_rect(l-lpost/netu, -wpost/netu/2.0, l, wpost/netu/2.0);

// cut via hole
de_set_layer(4);                 // set via (dielectric) layer
de_draw_rect(l-(lpost-vu)/netu, -wvia/2.0, l-vu/netu, wvia/2.0);

// draw air bridge metal
de_set_layer(2);// set the second metal layer
de_draw_rect((lpad+lol)/netu, -wcap/2.0, lbot-lol/netu,wcap/2.0);
de_draw_rect(lbot-lol/netu, -wpost/netu/2.0, l, wpost/netu/2.0);

// add ports
de_draw_port(0.0, 0.0, -90.0);
de_draw_port(l, 0.0, 0.0);
}
----------------------------------------------------------------------------
  2. Save the file in your project networks directory.

To associate this artwork with your subnetwork:

  1. Open the network design and choose File > Design Parameters.
  2. From the General tab, select SYM_C as the Symbol Name (This is the symbol that will represent the schematic.)
  3. Set the Simulation Model to Subnetwork.
  4. Select AEL Macro as the Artwork Type.
  5. In the Artwork Name field, type the name of the function you just created. In this example, mimart. This is defined in the example by the line: 
    defun mimart(c, ar)
  6. From the Parameters tab, create the parameters C and AR, as defined in the artwork function. Both should be set to Netlisted. You can optionally set them as optimizable.

The following illustration shows the MMIC capacitor in layout with C=20 and AR=1.

Note that rather than writing the functions from scratch, you may find it helpful to copy AEL macro code from one or more of the following files and modify it in your own AEL file:
destdart.ael - Artwork macros available from the Design Parameters dialog box, located in $HPEESOF_DIR/de/ael
ckt_linear_art.ael - Existing artwork for circuit simulators, located in $HPEESOF_DIR/circuit/ael

If you want to move the .ael file to a directory other than the project's networks directory, refer to Creating Custom Libraries under the section on Customization Examples in the Customization and Configuration documentation.

Associating Artwork with an Item

When associating artwork with an item, choose one of the following artwork types:

Selecting the Appropriate Artwork Type

The following sections describe how the different artwork types are intended to be used.

Synchronized Artwork

When you create and save a network, a design definition is automatically created with certain defaults (which can be modified through File > Design Parameters) including Artwork Type. By default, the artwork type will be Synchronized. Synchronized artwork is the appropriate artwork type when the layout contains parameterized components or if the layout is a subnetwork that needs to be regenerated when a parameter is changed. When synchronized artwork is selected as the artwork type, the artwork that is generated is based on the default artwork defined for each component in the schematic. Additionally, when the design synchronization process is run, it checks the subnetwork references for any changes to its parameters and automatically regenerates the layout based on the changes.

Fixed Artwork

If your layout is comprised of fixed shapes, then Fixed artwork is the appropriate Artwork Type. The layout artwork can reside in the same design file as the schematic or in a different file.

To associate fixed artwork with an item:

  1. From the design of interest, choose File > Design Parameters.
  2. From the Artwork Type drop-down list, select Fixed.
  3. In the Artwork Name field, select or type the name of the design file containing the artwork. This can be supplied artwork or custom artwork. You do not need to include the full path, just the design file name, minus the .dsn extension. The file should reside either in your project's networks directory or in a directory whose files are automatically loaded by the program (based on the search path). For more information, refer to Creating Custom Libraries under the section on Customization Examples in the Customization and Configuration documentation.
  4. Change any other design definition characteristics as desired and click OK.

AEL Macro Artwork

If you want to generate artwork based on parameters that may change, then AEL Macro artwork is the appropriate Artwork Type.

To associate an AEL Macro artwork with an item:

  1. From the design of interest, choose File > Design Parameters.
  2. From the General tab, select AEL Macro as the Artwork Type.
  3. In the Artwork Name field, select or type the name of the function. Note, this is not the name of the AEL file, rather it is the name of the AEL artwork creation function (specified with the defun AEL function).
    The function must be in an AEL file that is loaded by the program. All AEL files in your project's networks directory are automatically loaded. For details on loading files from other directories (based on the search path), refer to Creating Custom Libraries under the section on Customization Examples in the Customization and Configuration documentation.
  4. From the Parameters tab, enter the list of parameters used by the macro and assign the appropriate characteristics including Value Type. Note the following guidelines when defining parameters:
    • Artwork parameters must be defined in the same order in which they are used by the macro and they must be listed before any other parameters. Their type should be Not Netlisted.
    • All parameters that define physical dimensions should be assigned Length as the Parameter Type. If you do not define a unit along with the Default Value, the specified value will be read as meters. When you place an instance of this subnetwork in a schematic, the specified default value is converted from meters to the current Length unit set for the Schematic window.
    • The Layer parameter is the Layer Number on which the artwork should be drawn, and must be an integer.
      Hint
      To quickly populate the list of parameters, click Copy Parameters From and select a component with parameters similar to those you need, then modify the list of parameters and their characteristics as desired.
  5. Optionally, select an appropriate Parameter Type. This selection determines the choices available for editing the parameters when you place your subnetwork.
    The following example shows Value Type and Parameter Type settings based on the cpad2 macro.

If the AEL Macro artwork is SMT package artwork:

  1. In the Design Parameters dialog box, set the Artwork Type to AEL Macro and select the appropriate Artwork Name (smtart_<part_name>).
  2. In the Parameters section, define the two parameters, SMTPAD and OFFSET.
    • For the SMTPAD parameter, set the Parameter Type to String and set the default value to the appropriate SMTPAD Instance Name (for example, PAD1). Select the Not netlisted option.
    • For the OFFSET parameter, set the type to Real, with a default value 0.

None

Select None as the Artwork Type if no artwork is to be generated or no artwork is to be used to synchronize the schematic with layout objects.

Overriding the Default Artwork Assignment

You can override the default artwork assignment for any given component.

To change the artwork for a given component:

  1. Select the component and choose Edit > Component > Edit Component Artwork.
  2. Choose from one of the following Artwork Types:
  1. Click Apply for this component and select another and repeat as needed.
  2. Click OK when you are finished.
 

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

Contents
Additional Resources