Mechanical symbols for mounting holes

To place the mechanical symbol mounting holes, select Place → Mechanical Symbols from the menu bar or select the Place Manual button on the toolbar. At the Placement dialog box (see Fig. 10.4), select Mechanical symbols from the Placement List. Click the Advanced Settings tab and make sure that the Library option is checked. Select the Placement List tab again, and check the box beside the CH10_MTG130NP icon. Move your pointer to the design area; the symbol will be attached to it. Left click to place the mounting hole. Recheck the box for each hole you want to add to the board design. Click OK to dismiss the dialog box.

Since the plated holes are footprints, they contain a place boundary like any other component, but on this footprint place boundaries were added to both the top and bottom layers. The symbol was designed that way so no components are allowed to be located near the holes and cannot contact the mounting hardware (standoffs, washers, or nuts, say).

The unplated holes are mechanical symbols. They contain place boundaries on the top and bottom (not shown in the figure) for the same reason, but they also contain route keep-out areas (Route keepout/All). The keep-out areas are needed so that traces cannot be routed under mounting hardware or across the unplated hole (and subsequently drilled away). The design rule checker (DRC) may not detect such a situation, because the Constraint Manager does not know about the mounting hardware that will be put into the hole, and there are no pads against which to maintain spacing rules.

Mechanical symbols for fiducials

Fiducials are marks or objects used for aligning the board with solderpaste stencils and pick and place machines.

Stencils are thin stainless steel plates or sheets through which solderpaste is squeegeed onto the board. The thickness of the stencil establishes the thickness (and therefore the amount) of the paste applied to the pads. The stencil manufacturer uses the pastemask file to fabricate the stencil.

Fiducial objects are placed at particular coordinates on both the board and the stencil, and optical equipment is used to align the stencil to the board during application of solderpaste.

During pick and place operations the fiducials on the board are used to precisely identify the location and orientation of the board so that the components are accurately placed into the solderpaste.

On the circuit board the fiducial is typically a copper mark produced during the etch process. Because the fiducials are relied on optically, the soldermask is usually removed at the fiducial location. Since the fiducial needs to be visible through the stencil, an exact copy of the fiducial needs to be included with the pastemask pattern. A fiducial object then requires etch, soldermask, and pastemask elements.

Note: Many of the native PCB Editor footprint symbols do not contain pastemask elements; so you need to add them to the footprints if you plan to fabricate a stencil and use pick and place processes to populate your board.

We next look at how to make a fiducial. Ideally we want the fiducial to be a symbol that is an element of the board rather than a component. So we want to construct the symbol on the classes and subclasses shown in Table 10.2. Unfortunately a pastemask subclass does not exist under the Board Geometry class. So, we will make one. Begin by opening a new mechanical drawing in PCB Editor as described in the mounting hole example.

To define a new subclass, select Setup → More → Subclasses… from the menu. At the Define Subclass dialog box shown in Fig. 10.5, select the class where you want to assign the new subclass. For this example, click the box next to Board Geometry.

At the Define Subclass dialog box (see Fig. 10.6), type PASTEMASK_TOP in the New Subclass: text box then hit the Enter key on your keyboard. The new class will be added to the list and displayed in the Options pane and the Color dialog box.

The geometry of a fiducial is typically specified by the user. In this example the fiducial will be a 40×40 mil². The first step is to place the copper square. Change the All Etch grid setting (Setup → Grids) to 10 by 10 mil. Zoom in to the center of the drawing area (0, 0). Select the Etch/Top class and subclass from the Options pane. Select the Shape Place Rect tool and draw a 40×40 mil box centered at coordinate (0, 0).

Next we draw the soldermask opening. Change the Non-Etch grid setting to 5 by 5 mil. Select the Board Geometry/Soldermask_Top class and subclass from the Options pane. Select the Shape Place Rect tool and draw a 50×50 mil box (5 mil larger than the pad on all sides) centered at coordinate (0, 0).

Finally the pastemask is defined. Repeat these procedures using the Shape Place Rect tool on the Board Geometry/Pastemask_Top class and subclass and draw a 40×40-mil box centered at coordinate (0, 0) directly over the copper pad. Save the drawing to create the .bsm file.

To place the fiducial, use the procedure described for placing a mechanical symbol. Place two or more fiducials on the outer perimeter of the board.

Generating the artwork

The artwork files describe elements of the design and include the Etch, Soldermask, SolderPaste, and Silk-Screen layers.

Most of the manufacturing data are basically present in the board design but not in a format that manufacturers use. The artwork creation process performs that function.

Before we begin the process, one more element needs to be added to the board, a photoplot outline.

Adding a photoplot outline

The board outline generated by the Design Outline dialog box serves as a guide for the designer during the design process, but maybe sometimes it does not contain manufacturing data for the manufacturer. That information may be contained in a photoplot outline.

To draw a photoplot outline, select the Manufacturing class and Photoplot_Outline subclass from the Options pane. From the toolbar, select the Add Rect tool (not the Shape Add Rect button). Draw a rectangle directly over the top of the board outline located on the Board Geometry/Design_Outline layer. A photoplot outline is shown in Fig. 10.7.

Optional artwork items

All the silk-screen elements in the design are associated with the individual components. You can add additional etch and silk-screen markings that are specific to the board. For example, you can use objects (mechanical symbols) on the top or bottom layers to add a company logo or add silk screen to display the board part number or manufacturing date, say, as shown in Fig. 10.7.

Once the board is ready to go, the next step is to generate the artwork files.

Artwork control form

The artwork files are generated using the Artwork Control Form dialog box (shown in Fig. 10.8). To display the Artwork Control Form dialog box, select Export → Gerber from the menu bar or click the Artwork button on the toolbar (if it is displayed). The Artwork Control Form contains two tabs, the Film Control tab and the General Parameters tab. The default settings may cause two warning boxes to be displayed. The procedure for clearing these warnings is given in the next section.

General parameters

The General Parameters tab is shown in Fig. 10.8. Use the tab to set the artwork format. Select the Gerber RS274X option if it is not already checked. In the Decimal places: box, enter the same value that is in the Integer places: box. This will handle the warning shown in Fig. 10.9A. Click OK to close the Artwork Control Form dialog box.

To handle the second warning in Fig. 10.9, change the Artwork Format in the Design Parameter Editor to match the Device type in the Artwork Control Form (Fig. 10.8). To do this, select Setup → Design Parameters… from the menu. At the Design Parameter Editor dialog box, select the Shapes tab then click the Edit global dynamic shape parameters… button to display the dialog box (see Fig. 10.10). Select the Void controls tab and choose Gerber RS274X from the Artwork format: list. Click OK twice to dismiss both dialog boxes.

Film control

The Film Control tab shown in Fig. 10.11 contains folders that in turn contain subclass items. To see the subclass items, click on the + symbol next to the folder you want to view. Initially the form contains folders related to the layer stack-up only. Folders for the other items (e.g., silk screen and soldermask) must be added.

A folder contains related items. For example, recall that there are several types of silk-screen items [component reference designators (REFDES), component outlines, board geometry text, etc.], which belong to different classes and subclasses. These items are collected and organized in folders, and a single silk-screen Gerber file is made from the collective data in that folder.

The first step then is to take an account of all the types of elements you want manufactured with your board. Table 10.3 shows the conductor type artwork elements that need to be generated; these are autogenerated and already exist in the Artwork Control Form. Table 10.4 lists some of the most common nonconductor elements that can be placed on the board. Solderpaste (Pastemask) class elements can also be generated if you are planning on using pick and place machines to populate your board. Three classes contain pick and place elements, as described in the section Generating Pick and Place files. They are added to the Artwork Control Form the same way the soldermask and silk-screen elements are added, which is described next.

For this design the top side of the board needs a soldermask and silk screen, while the bottom side of the board needs only the soldermask. Since there is no silk screen on the bottom, we have no bottom silk-screen folder. So from the table, we have three folders: a top-layer silk-screen folder, which includes the Board Geometry, Ref Des, and Package Geometry classes; a top-layer soldermask folder, which includes the Pin and Via classes; and a bottom-layer soldermask folder, which contains the same classes as the top-layer soldermask (only on the bottom layer).

In addition, we need a Gerber file for the board outline. Other types of Gerber files can be made, but for the time being, these are the only ones we need. We begin by adding the top-layer soldermask folder.

Adding elements to the artwork control form

When you add a folder to the control form, all classes that are visible in the design are added. So we begin by turning off all layers except for the classes and subclasses related to the top-layer soldermask. Use the Color dialog box to control the visibility of the classes. To turn off all the layers at once, click the Off button (Global Visibility:) at the top of the dialog box, then click the Apply button at the bottom.

Next, check the box for the Soldermask_Top subclasses in each of the Package Geometry, Board Geometry, Pin, and Via classes. The Package and Board Geometry classes have nothing on them in this design, but it does not hurt to add them to get in the practice of including them for future designs.

Once these elements are the only ones visible, open the Artwork Control Form. We will add a new folder for the top-layer soldermask items. To add a new folder to the Artwork Control Form, right click on any one of the existing folders and select Add from the pop-up menu (do not use the Add button at the bottom of the form). Enter a name for the folder in the New Film dialog box (see Fig. 10.12). The name does not have to match any PCB Editor class or subclass name, but it can be helpful if it does or is similar. The new folder now will be listed in the form, and it will contain the subclasses visible in the design.

Using this procedure, make a new SoldermaskBottom folder and include the similar classes as the top-layer soldermask folder (VIA, PIN, PACKAGE GEOMETRY, etc.).

Next we add a silk-screen object. As indicated in Table 10.4, many silk-screen objects can be added to the design. You can use the procedure just described to create the silk-screen films too. But there is another way to generate the silk-screen films using the Autosilk tool.

During the part placement steps, it is very possible that silk-screen objects can accidentally be removed (or be unable to be printed) on the soldermask because of openings in the mask, or they can become hidden under components or even printed on top of other silk-screen objects. Keeping the silk-screen objects under control can be a task. Fortunately PCB Editor has a tool that helps us keep track of them, Autosilk.

The Autosilk tool takes all of the individual silk-screen elements, combines them into one layer, and makes sure that they are not under components, over padstacks, or too far away from their respective components. To start the Autosilk process, select Manufacture → Silkscreen from the menu bar. At the Auto Silkscreen dialog box (shown in Fig. 10.13), you can select which elements you want added to the common silk-screen files (one for Autosilk_Top and one for Autosilk_Bottom). You can also set default values for some of the physical properties related to silk-screen objects. When the settings are complete, click the Silkscreen button. When the process is complete, the dialog box will dismiss itself and the results will be displayed in the command window. To view the new silk screen, make sure the Manufacturing/Autosilk_Top (or _Bottom) subclass is visible. It is also helpful to make the new silk screen a color different from the other ones.

If you do not notice a big difference, it could be that the new silk screen is directly on top of the original. This will happen if the Autosilk tool does not find anything wrong with the existing ones. To make sure the new silk screen is correct, turn off the original ones (all of them) and look at just the new one, which will be the sum of all the others. Otherwise, you should notice that some of the REFDES were moved away from fan-out vias and outside the place boundary shapes. Depending on how the autorouter routed your board, you may also notice that some of the component outlines are removed where vias are close to the component body. We now add the new silk screen to the artwork form.

If you previously made a silk-screen folder you can add the new autosilk data to the existing folder and remove the other, individual silk-screen elements.

To add an item to an existing folder, right click on any one of the existing items in that folder and select Add from the pop-up menu. At the Subclass Selection dialog box (see Fig. 10.14), check the boxes for the items you want to add and click the OK button. The items will be added to the folder. To delete an item from a film folder, right click on the item and select Cut from the pop-up menu.

The last item to add is the board outline item. The board geometry outline drawn at the beginning of the board design process does not contain Gerber data and is for the designer’s benefit. Gerber data for a board or design outline is contained in the photoplot outline.

Using the previous procedures, add a photoplot outline folder that contains the Manufacturing/Photoplot_Outline class and subclass. An example of the completed artwork list is shown in Fig. 10.15.

We are almost ready to generate the Gerber files. Before we do, check to make sure that the ground and power layers are marked as Negative in the Plot Mode: area of the Artwork Control Form and you have entered a value in the Undefined Line Width: box (a number between 5 and 10 is usually good). If you forget to add a default line-width value, any lines or text that have a width of 0 will be ignored (resulting in large blank areas on the silk screen). And recall from Chapter 8, Making and editing footprints, that many of the silk-screen outlines that come with the library use rectangles instead of lines, and rectangles always have a default width of zero. Also note that if you decide to plot the board outline using the shape created in Design_Outline instead of Photoplot_Outline drawing, you should add Board Geometry/Design_Outline subclass to the PhotoPlotArea folder and set the Undefined line width value to 10 for it as well.

Also, make sure that the Vector based pad behavior option is checked. This applies only to negative planes, but it affects how the unconnected pads on the plane layers will be represented in the artwork. Leaving this option checked removes unused pads from negative planes, which results in a larger (safer) clearance gap.

Next, populate the aperture list (skip this step if you’ve selected Gerber RS274X format). Click the Apertures… button (see Fig. 10.16). An Edit Aperture Wheels dialog box will be displayed with at least one entry. Click the Edit button to display the Edit Aperture Stations dialog box. If you do not see a list of entries, click the Auto button and select Without Rotation from the pop-up menu. After the aperture wheel list has been populated, click OK twice to get back to the Artwork Control Form.

To generate the Gerber files, click the Select All button in the Artwork Control Form to check all the folders (or just check the ones you want—the others will not be written or overwritten if they already exist). Then click the Create Artwork button. The command window will report the results and you can read through the photoplot log to look for any errors. Check the working directory and make sure that the files are present. In this example, eight files with the .art extension should have been generated. These are the Gerber files that will be sent to the board manufacturer.

That completes the artwork process. Now we move onto making the drill files.

Drill file format

As there are different formats for the artwork files, there are several types of drill formats. You need to know the format your board manufacturer requires and apply it to your design. To specify the drill format, select the Ncdrill Param button on the toolbar or select Export → NC Parameters… from the menu to display the NC Parameters dialog box (see Fig. 10.18). At the NC Parameters dialog box, you can enter a header if your manufacturer asks for one, but PCB Editor does not care if you enter one. Enter your board manufacturer’s specifications for the format (e.g., 2.4), zero suppression, Excellon format options, and the like. Once the values are set, click the OK button to save your settings.

The next step is to create the drill file. Select Export → NC Drill… from the menu to display the NC Drill dialog box shown in Fig. 10.19. If you have not scaled your design drawing in any way, enter a scale factor of 1.

If your board manufacturer prefers a particular tool sequence, you can select that here; otherwise, use the default setting.

Select the Auto tool select option. This option causes PCB Editor to look for a tool list. If one does not exist, it will create one automatically. It also adds drill tool header information to Excellon formatted files. If the Auto tool select option is not enabled, no tool list is created and the drill file contains only drill locations and manual stops where the computer numerical control machine operator is required to indicate the drill tool from a manually generated tool list.

If you know for sure that your board manufacturer can process drill files that contain both plated and nonplated hole information, you can leave the Separate files for plated/non-plated holes option unchecked. Otherwise, check the box to make two distinct drill files. Nonplated hole drill files have np in the filename, as described later, whereas the plated holes do not.

The last two options (repeat codes and optimized head travel) also depend on your board manufacturer’s preferences. If the manufacturer does not specify one way or the other, check them both.

In the Drilling: option box, select the Layer pair option. The By layer option is used for back-drilling and blind/buried-via drilling operations and is explained briefly later.

Click the Drill button to create the drill file(s). For this design with the settings chosen in the NC Drill dialog box, two drill files are generated, chapter10_manufacture-1-4.drl and chapter10_manufacture-1-4-np.drl. The naming convention is filename-startlayer-endlayer.drl. The np in the second file indicates that the file is for the nonplated drill holes. These *.drl files are the NC files your board manufacturer will use during the board fabrication.

If you chose the By layer option in Fig. 10.19, the same files would be generated, but additional drill files would also be generated, where a separate drill file is generated for each layer combination in the stack-up. The drill file names would then be, for a four-layer board for example, filename-bl-1-2.drl, filename-bl-2-3.drl…, filename-bl-3-4.drl, in addition to the one file named filename-1-4.drl. The bl in the file name indicates that the by layer option was checked.

Manually generating a tool list

Instead of using the default nc_tools_auto.txt file, you can specify your own tool list. To do so, you must uncheck the Auto tool select option and create a tool list file, which must have the file name nc_tools.txt. To generate a tool list, open a text editor such as Notepad and save it as nc_tools.txt. A tool list is shown in Fig. 10.20. Each line begins with the diameter of the drill hole. The P or N indicates whether the hole is plated or nonplated. The Tnn is the tool number, and the numbers following that indicate the + and − tolerance. Save the tool list file into the working directory, and PCB Editor will automatically look for it there.

Establishing an NC route tool list file

As for the NC drill process, you can automatically create the routing tool list, or you can specify it manually. Setting up an NC route tool list is similar to making the drill tool list described previously. A sample is shown in Fig. 10.21. Use a simple text editor (such as Notepad) and open a blank file. The contents have a line that includes the bit diameter (in inches if your design is using English units or millimeters for metric units) and a tool number for each cutting tool that will be used in the design, as defined by the line widths on the Ncroute_Path subclass. For this example the bit diameter is 0.100 in. (100 mil). Save the file into your working directory with the filename ncroutebits.txt and then close the file.

Cut marks

The actual cutting information is contained in the route path outline described later and not in the cut marks. But we begin with this optional step because cut marks can be used as a guide in placing the route path outline, and it will help make sense of the later steps.

We specified that the bit used to cut around the board is 100 mil in diameter, so the cut marks and the placement of the route outline will be based on that. To place cut marks on your board, select Manufacture → Cut Marks from the menu bar. At the Cut Mark Options dialog box (see Fig. 10.22), enter 100 as the Line width:, because that is the diameter of the cutting bit. Next, assuming that the edge of the bit will cut right along the board edge, the center of the cut path has to be offset by one half of the bit width (50 mil) from the board so that the bit does not cut into the board itself. Therefore enter 50 in the Offset: option. The line length is not critical, as it simply determines the visual length of the mark. A line length of twice the width is a good rule of thumb. If your board is not a simple rectangle, you should select both inside and outside corners in the Corner type box, otherwise the outside only is adequate. When you are ready to place the marks, click the Apply button. PCB Editor automatically places cut marks around the board outline on the Board Geometry/Cut_Marks class and subclass. An example is shown in Fig. 10.23.

Drawing the cut path

The next step is to place an outline along the cutting path. Begin by selecting the Ncroute_Path subclass under the Board Geometry class in the Options pane. Select the Add Line tool from the toolbar. Set the width of the cut in the Line width: box in the Options pane (100 mil). The center of the cut marks will serve as a drawing guide. Left click and release at the center of the cut mark to begin drawing the cutting path. Continue around the board, drawing the cut path through the center of the cut marks. When you return to the starting point, left click to end the last segment at the starting point and then right click and select Done from the pop-up menu.

Note: You must use the Add Line tool (not a rectangle) to draw the cut path so that you can specify the cut width. PCB Editor uses the width of the line to determine which cutting tool to use from the ncroutebits file when it generates the route file (*.rou). If you have only one cut path (and width) and only one tool in the ncroutebits file, PCB Editor will assume you mean to use that bit for that cut. But if you have multiple cuts (e.g., for edge slots) and multiple bits, then you have to specify the line width and have the correct bits listed in the bit file.

Fig. 10.23 shows a small 1 near the starting point. This is an indicator used to tell the NC machine where to start. A 2 at one of the adjacent corners defines the direction that the cut should be made (not the order the outline was drawn). The numbers are optional, but we will place them as a demonstration.

To place cutting order text objects, select the Add Text tool from the toolbar and the Ncroute_Path subclass under the Board Geometry class in the Options pane (same as for the cutting path outline). Left click near the corner you would like to have the cutting tool start (it does not have to be the corner you started the outline). Enter a 1 in the text block, right click, and select Done from the pop-up menu. That defines the starting point. Use the same procedure to place a 2 at the next corner. The second number defines the direction of the cut path. You can place starting and direction indicators on as many distinct cutting paths as there are on your board. You do not have to place a number at every corner of a closed path unless your board requires a special cutting process.