CAM Output from PADS Layout: Gerber and Excellon

1. PADS Layout: Gerber and Excellon Parameterization

Print settings must be configured before generating Gerber and Excellon files. The default settings do not produce the best results.

The main reason for parameterization is to use a higher print resolution. The default value of 1/1000″ is simply not sufficient for today’s high-density boards: if the database’s 10 nm resolution is rounded to a thousandth of an inch, it will have a noticeable effect on the final result.

Another, perhaps even more important reason has to do with the Gerber RS-274X format. While its use is recommended, the best compatibility with manufacturers’ CAM systems is achieved if the G36 and G37 commands are not used.

When selecting a resolution, the maximum resolution is not necessarily the best choice. The manufacturer likely does not use it when creating pattern transfer documents, and lowering the resolution can cause the endpoints of small arcs to merge, which may cause problems in some CAM systems.

It makes sense to set the parameters for both Gerber and Excellon in the same way. If you use full output resolution in Gerber but round off the drill coordinates, the end result will appear as if the holes are not centered within the pads.

1.1 Gerber Parameters

Printer configuration is a workstation-specific setting, so it is sufficient to set it up once on each computer.

1. Select ” File | CAM ” and create a new CAM subdirectory by clicking the ” Create ” button (or clear the ” default” directory).
2. To add a new document, select Add…. In the Document Name field of the window that opens, enter the name under which you want the document’s parameters to appear in the list (in the example, ” Layer 1“). The name will only appear in the “Define CAM Documents” list, not elsewhere, so choose a name that you’ll easily recognize later. The document itself is irrelevant in terms of print settings; it’s used to access the “Device Setup” menu. Under “Document Type,” select “ Routing/Split Plane ” and, from the layer menu that appears, select the corresponding layer (in this case, “ Component Side Layer 1 ”).
3. You can access the configuration settings through a document. Select one of the documents from the list using the Edit command, or select “Device Setup” from the Add Document window. Fill in the information in the window as shown in the image, and pay special attention to the highlighted items.

Key settings in the “Device Setup” window:

• Regenerate: Run this for each job file before Gerber output. It fills in the aperture table according to the job and enables Flash-type apertures for both oval and rectangular pads.
• Fill width: PADS Layout does not use aperture rotation; instead, square and rectangular pads whose sides are oriented at angles to the main axes are created by drawing them with the “Fill width” line width.
• Texts fill width: This value specifies the line width used for filling in TrueType fonts. Use a value that provides a sufficiently small rounding radius at the corners. A width that is too small may increase the size of the output file.
• Plotting size: The print area must be large enough. If the print area is too small, it will cause the layer in question to be centered.

Note: If the PCB dimensions exceed one meter, select a resolution of 4.2 metric, because the 3.3 metric format only supports up to 999 mm, and data beyond one meter will be truncated. In that case, you should set the NC Drill output format to the same value (4.2 metric).

Close the windows by clicking the OK button until you return to the Define CAM Documents window.

Example of Naming CAM Documents

6-layer printed circuit board (1+4+1 buildup). Format: Layer – Document Name – Document Type – Output File.

• Top – Layer 1 – Routing/Split Plane – Layer1.pho
• Inner Layer 2 – Layer 2 – Routing/Split Plane – Layer2.pho
• Inner Layer 3 – Layer 3 – Routing/Split Plane – Layer3.pho
• Inner Layer 4 – Layer 4 – Routing/Split Plane – Layer4.pho
• Inner Layer 5 – Layer 5 – Routing/Split Plane – Layer5.pho
• Bottom – Layer 6 – Routing/Split Plane – Layer6.pho
• Silkscreen Top – Silkscreen 1 – Silkscreen – Silk1.pho
• Silkscreen Bottom – Silkscreen 6 – Silkscreen – Silk6.pho
• Paste Mask Top – Paste Mask 1 – Paste Mask – Paste1.pho
• Paste Mask Bottom – Paste Mask 6 – Paste Mask – Paste6.pho
• Solder Mask Top – Solder Mask 1 – Solder Mask – Mask1.pho
• Solder Mask Bottom – Solder Mask 6 – Solder Mask – Mask6.pho
• Drill Drawing – Drill Drawing 1 – Drill Drawing – Drill1.pho
• Drill Drawing – Drill Drawing 3 – Drill Drawing – Drill3.pho
• Drill Drawing – Drill Drawing 6 – Drill Drawing – Drill6.pho
• Board Outline (Layer_18) – Board Outline – Custom – Board.pho
• Dimension (Layer_19) – Dimension Drawing – Custom – Dimension.pho
• NC Drill 1-6 – NC Drill – NCdrill.drl
• NC Drill 1-2 – NC Drill – NCdr1_2.drl
• NC Drill 2-5 – NC Drill – NCdr2_5.drl
• NC Drill 5-6 – NC Drill – NCdr5_6.drl

1.2 Excellon Parameters

1. In the Define CAM Documents box, select Add Document (or if the document is already in the list, use the Edit button) and in the Document Type field, selectNC Drill After this, the Drill button at the bottom will be activated.
2. From the “Device Setup” section, go to the Excellon settings.
3. Set the Excellon parameters as shown in the figure, paying particular attention to the highlighted sections.

In the NC Drill Setup window, you can set the parameters for two different documents. The default is Excellon parameterization. It makes sense to use the same representation as for Gerber files. However, since Excellon’s standard unit in millimeters is the micrometer, we recommend a resolution of 3.3 metric.

Note: If the PCB dimensions exceed one meter, select a resolution of Metric 4.2 (0000.00), because the Metric 3.3 (000.000) format only supports up to 999 mm, and data beyond one meter will be truncated. The Gerber output format must then be set to the same value (4.2 metric).

The document on the Drill Listing tab is intended for printing on paper and is not currently used very often. The values displayed in the window fields when the “Drill Listing” tab is selected have no effect on the format of the Excel drill file.

Format String table settings:

• Drill File Start → String: M48@nMETRIC,TZ@n%. In Excellon, ” METRIC ” usually refers to micrometers (although 10 µm would also be possible). ” TZ ” means using trailing zeros (in Gerber, it is specified which zeros are not used).
• Tool Section Start → String: It is recommended to change the definition line to the following format: ` T@tC@d`, so that PADS Layout will place the tool size at this location.
• Speed/Feed: You can set the blade feed and rotation values in this field, but since manufacturers certainly have their own practices—which depend on the materials—it’s probably not worth paying attention to them.

Some CAM systems may interpret the tool size in thousandths of an inch if the number does not include a decimal point. You can add one after the letters ” d.”

Note: The ” Metric 4.2 (0000.00) ” format is used when the PCB dimensions exceed one meter, because the ” Metric 3.3 (000.000) ” format only supports up to 999 mm, and data beyond one meter will be truncated.

2. Transferring Parameters from One Machine to Another

Parameters can be transferred by copying them from one machine to another, as long as the software version is the same. The Gerber parameters for PADS 9 and VX are located in the file camdevices.dat. The Excellon parameter file has the same name as before (drill.dat). The default directory for parameter files is C:\MentorGraphics\PADS\SDD_HOME\Settings.

Attention! Do not copy files from one version to another, as the file format may change from one version to another, and the files are not originally intended to be copied. Therefore, the software does not perform syntax checking on the files.

Parameters can be transferred to the new version of PADS VX using the PADS Settings Migration program, which is installed along with PADS VX versions.

3. Other Important Printing-Related Matters

3.1 Positioning

When using Gerber files, corner and alignment marks are not needed at all, provided that the files are positioned correctly and a single Gerber file is included that contains the board outline positioned in the same way as the other documents.

Alignment is set via the ” Options” button in the” Add” or “Edit Document” window. The default setting for the ” Justification ” option in the “Plot Options” dialog box is ” Centered.” This means that the document is centered in the print area based on its minimum and maximum coordinates. However, PCB layers are different, and if alignment is calculated on a layer-by-layer basis, different layers will be aligned differently.

As a result, in printed circuit board manufacturing, the layers must first be aligned on top of each other, which creates extra work. The most difficult part is aligning the outline of the circuit board with the holes, because these documents do not share any common coordinates.

You can completely avoid alignment issues by printing each document with the “Justification” option set to ” Offset“:

• The offset value is selected so that the data to be printed remains entirely within the positive coordinate region.
• It is best to use 0.0 for the X and Y offsets and adjust the PCB origin accordingly in your design, for example, -100, -100. This is usually sufficient, even if there are layer labels placed below the PCB.
• During printing, PADS Layout checks to ensure that all data remains within positive coordinates, taking the line width into account. It’s a good idea to make sure the preview image looks like the one in the PDF guide.
• If PADS Layout indicates during printing that it is centering a document, you should check what is causing the centering. If you need to adjust the offset value, do so for each document individually.

3.2 Printing the PCB Outline

If all the lines defining the outline of the circuit board are selected in a single document, the manufacturer can easily use that information to create a routing program. No other alignment or corner markers are needed, as long as the board outline is positioned exactly the same way as in other Gerber and Excellon documents.

3.3 Generating an Aperture Table

For each job, it is recommended to select the parameters in the component-side wiring diagram document, select ” Device Setup,” and run the “Regenerate” command, as shown in section 1.1 (step 3) above.

3.4 Printing Holes Without Metal Filling

In the current version of PADS Layout, both unplated and plated holes are selected by default. This is a safe choice in the sense that there is no risk of “forgetting” the unplated holes.

When using the method described above, in which the tool size is specified in Excelon in conjunction with the tool selection command, it would be best to export the metal-filled and non-metal-filled holes to their own files and name the files so that their intended use is clearly evident from the name.

Information about hole metallization is indeed included in the report file(s) (e.g., NCdrill.rep) and in the Drill Drawing document, but if the data has to be cross-checked against different documents during the manufacturing phase, the risk of confusion increases.

However, if you export all the holes to the same Excel file, make sure that ” Non-Plated Pins ” is selected. In this case, the manufacturer must check the plating of the holes in the report (NCdrill.rep) or the drilling instructions document. It’s also a good idea to check your PCB supplier’s recommendation on this matter.

3.5 Printing the “Drill Drawing” Document

It is recommended to include machining instructions, slots, fillets, tolerances, etc., in the drilling instruction layer. Oval holes in components are generated using the “Drilled Slot” commands. Previous versions only printed the endpoints of the slot for an oval hole, making the “Drill Drawing” document absolutely essential. We recommend printing the “Drill Drawing” document even with the current version.

3.6 List of Files and Their Purposes

PCB manufacturers receive Gerber files from various PCB design software programs, in which files are named differently; therefore, the file name for the same item varies. The manufacturer’s setup process is expedited if a list of the files’ intended uses is provided along with the files, in addition to the file name being displayed graphically within the document itself.

Tip: It is a good idea to group printouts intended for the PCB manufacturer consecutively in the document list and include a common prefix in the filename (see the “Output File” filenames in the naming example). This makes it easy to select all consecutive lines during printing. With this naming convention, you can also use the template definition in the CAM350 software’s import function to automatically generate the layer definition.