This application note covers some valuable layout concepts for doing printed circuit board designs using Microwave Office. It demonstrates how to use positive and negative layers to ease drawing ground flood regions. By utilizing some simple setup procedures it is possible to have all lines draw with a user-specified spacing to the ground flood automatically. This technique greatly simplifies drawing the ground flood when the initial layout for a circuit is complete. This application note also discusses various ways that Gerber files can be created in Microwave Office. One way is to merge the positive and negative layers to make one Gerber file. The other way is to keep the positive and negative layers separate if using a paint-scratch-paint processing technique.
Board Layout Simplification Techniques
This Application note demonstrates:
- the capability of Microwave Office to streamline Printed Circuit Board (PCB) designs
- how to properly set up Microwave Office to do PCB layout in an efficient manner, and the advantages of this approach
- several options for exporting the layout, focusing on different options for creating Gerber files.
In a PCB design, all of the components (active and passive) are used as discrete parts. The circuit is then assembled on a microwave substrate with metal patterns etched or machined to make transmission lines. This document assumes that the reader has a strong understanding of Microwave Office layout concepts. For more information on layout, see the Microwave Office User's Guide "Layout" chapter and the layout principles application notes available on AWR's web site (www.mwoffice.com). Additionally, the Microwave office project used to make all the figures in this application note is available.
The examples included here use a process technology that has a two-sided microwave board with thin-film resistors on both sides of the board. Chip components are only allowed on the top of the board. This may not be a practical technology, but it helps demonstrate many of the concepts discussed here. These techniques and discussions can easily be extended too multi-layer boards.
Typically, when designers are doing a PCB design, they design the entire circuit to fit into a fixed area. The last step is to draw the top ground plane so that it covers any area not populated by other components. While there is nothing wrong with this approach, drawing the top ground can be difficult if the board is complex and especially if there are curved lines or circles in the layout. This technique becomes even more difficult if the designer needs to make changes. Now instead of just moving one component in the layout, the component and the drawn ground plane all must be moved. The technique presented here eliminates all of these problems and allows the software to draw the proper spacings from transmission lines, pads, components, etc. to the ground plane.
Board Layout Setup
The Microwave Office layout tool simplifies the PCB layout through the use of positive and negative layers. The Microwave Office User Guide contains an excellent explanation of positive and negative layers. The basics of this concept are that for a named layer (e.g., Metal) you can have a normal layer, a positive layer, and a negative layer. The positive layer is specified by adding a "+" after the layer name (e.g., Metal+ is the positive for Metal) and the negative layer is specified by adding a "-" after the layer name (e.g., Metal-). These three layers represent one mas layer used for processing. When combined, the shapes on the negative (Metal-) layer are subtracted from the positive (Metal+) layer and the results are added to the normal layer (Metal).
When a layout is exported, Microwave Office can merge the normal, positive, and negative layers when creating the exported file. You can also specify to export each of these layers separately. Finally, you can use te built-in scripting environment to create one file that has all three layers' information using the Gerber format, allowing positive and negative layers. These formats are used with photopolotter machines that utilize a "paint-scratch-paint" processing technique. To visualize what a layer looks like when the normal, positive, and negative layers are merged, the drawing layers in Microwave Office for these layers need to be set up in a particular manner.
Figure 1 shows a microstrip line as a basic example of how these layers are used. The entire board surface is drawn with the positive layer, then the negative layer is drawn to cut a hole in the positive layer. This layer is drawn larger than the microstrip geometry. Finally, the normal layer is drawn to the exact dimensions of the microstrip line. The offset of the negative layer ffrom the normal layer creates the spacing to the ground plane.
The key to making this work is defining the necessary layers before designing the circuit. For the technology used in this example, layers are needed for:
- top and bottom metal
- top and bottom resistor
- package leads
- board outline
The following sections cover the steps to properly create the drawing layers, the layer mapping, and the line types for the chosen technology.
The First and probably most important step in setting up this type of layout is to define the draw layers. These layers must be set up in a particular way to make the layout look the same in Microwave Office as the artwork files look when exported. In this technology, positive and negative layers are needed for both the top and bottom metal layer. To display the layout properly, the layers must be in the proper order, i.e., which draw layer number is first. The order should be normal layer (Top Metal), negative layer (Top Metal_), and positive layer (Top Metal+). Figure 2 shows the drawing layer setup for this project. Notice that for Top Metal and Bottom Metal the order is as described above.
To finish setting up and properly displaying the drawing layers, the normal, positive, and negative layers should have the same Pattern. Finally, the normal and the positive layers should have the same line and fill color. The negative layer can have a line color, but the fill color should be the same as the background color of the Layout Editor, in this case white. it isn't obvious in Figure 2 that the negative layer has the same pattern as the other layers because the color is white, so it isn't displaying anything with a white background. you can change the color while setting the pattern and then change to the background color when done. Also, Figure 2 shows the negative layer for Top Metal with a line color and the negative layer for Bottom Metal without a line color. Drawing an outline for this layer is optional.
Drawing layers are also set up for the top resistor, bottom resistor, package, and leads layers.
Layout Process File (LPF)
After the drawing layers are set up, the next step is to define line types that utilize these layers to their full extent. This is done by editing the Layout Process File (LPF) in a text editor. Before you can do this, you must export the file from the project by choosing Options > Process Definition > Export.
The LPF contains definitions for line types, which are used to describe how to draw the layout for microstrip, stripline, and CPW models. The line types enable these models to be drawn with multiple layers in layout. For example, using different line types, a microstrip line can be drawn on one layers, two layers, or 10 layers, whatever number of layers is desired. This concept is used to create line types that use the normal layer to draw the line, and the negative layer to draw the spacing from the line to the ground plane.
Three line types are created for a 5, 10, and 20 mil spacing to the ground plane. These line types are shown in Figure 3.
Notice that the layer specified in each line type do not match any of the drawing layers specified in the previous section. When specifying entries in the LPF, the layer names are model layers, not drawing layers. The layer mapping set up in the following section maps the model layers to the already defined drawing layers. The line types are defined this way so that the 5, 10, or 20 mil spacing can be applied to the top or bottom metal layer of the board.
For each line type, the first layer is the normal layer and the second layer is the negative layer. Notice that each negative layer has a positive offset value. In the LPF file, the offsets are always set in meters, so these offset values are the meter equivalent of 5, 10, and 20 mil spacings. This offset is used to draw the negative layer with the proper spacing to effectively make a spacing from the line to the ground plane.
The drawing for the via model can also be set up in the LPF file. When using a via in a schematic, the layout is specified in the via definition section in the LPF. The entries for the via are shown in Figure 4.
Notice that the via layer names are not the same as any of the drawing layers. Again, these are model layers and are defined this way to easily expand the via drawing to a multiple layer board. There is only one via definition type allowed, so the layer mapping can change on which drawing layers each via is displayed. The via model layers are set up as follows: via, drawn as a circle of the via dimension in the model; vtMetal (via top metal), drawn as a square 10 mils larger than the geometry in the model; vtMetal- (via top metal negative), drawn as a square 20 mils larger than the geometry in the model, effectively drawing a 10 mil space to the ground plane. The vbMetal and vbMetal- layers are the same as vtMetal and vtMetal- except they are used for the bottom connection of the via. The flag setting determines the shape of the drawing. See the Microwave Office User’s Guide for more information. Remember that after changing the LPF file, you must import it into Microwave Office to apply the changes by choosing Options > Process Definition > Import.
Now that all of the drawing layers, the line types, and the via have all been set up, the final step is to assign the layer mapping. This is where the model layers for the line types, the via, and the thin film resistor (TFR) model are assigned to display on their proper drawing layers. Two layer mappings are needed, one for the top side of the board and one for the bottom side of the board. For the model layers, the program automatically makes each draw layer a model layer and then maps back to the same named drawing layer. After these "unity mapped" model layers, all the model layers used in the line type, via definitions, and the TFR need to be added as model layers and then mapped to the proper drawing layer. The model layers for the line type and via are shown in the LPF entries in Figure 3 and Figure 4. For the TFR element, the model layers are hard coded to "NiCr" and "Metal1". After these new model layers are added they are mapped to the proper drawing layer. Figure 5 shows the mapping for these model layers for the top of the board.
Notice that the layer names used in the LPF (model layers) are associated with the drawing layers previously defined. When this layer mapping is assigned to vias, transmission lines, or resistors, they are drawn on the drawing layers
assigned for the top side of the board. Figure 6 shows the layer mapping for the bottom of the board.
Note that the layer names for the line types and the TRF are now mapped to the drawing layers for the bottom of the board. The via mapping did not change in this example because there is only one type of via possible in the current technology. If this was a multi-layer board, the top and bottom via model layers could be mapped to different drawing layers to display the via at different heights in the stack.
Board Layout Examples
Line Type Settings
Moving Lines Between Layers (Layer Mapping)
Adding Cutout Regions
Adding Cutout Regions to Artwork Cells
Drawing Ground Spacings for Unassociated Drawing Objects
Exporting the Artwork