Electronic Design - PCB design skills: PADS Layout to Gerber

After the PCB design is completed, the next step is the production of the board. The production of the PCB board needs to use the Gerber file, so you will encounter the problem of converting the PCB file to the Gerber file. Different PCB design software transfers to Gerber in different ways.

*.pcb suffix files can generally be opened directly by double-clicking the file, or you can open PADS2005 and then click the toolbar File-Open (Ctrl+O) to open; while *.asc suffix files must be imported by clicking the toolbar File-Import.

1) Press Alt-S-O in turn or select Set Origin in the Setup menu to set the origin to the lower left corner of the graph (you can align the output Gerber file layer and layer)

Press Alt-S-O in turn or select Set Origin in the Setup menu to set the origin to the lower left corner of the graph

2) Click File-Tools-Pour Manager on the toolbar to bring up the copper pour menu shown in the figure below and select Hatch. For Hatch Mode, select Hatch All. Press Start to pour copper, and press Setup to open Perferences (Ctrl+Alt+G) to the system Make some proper settings for the parameters

Click File-Tools-Pour Manager on the toolbar to bring up the copper pour menu as shown below and select Hatch. For Hatch Mode, select Hatch All. Press Start to pour copper.

3) Change the unit Global-Design Units; change the minimum display line width Global-Drawing (in the graphical interface can be set by R+space+value)

Change the unit Global-Design Units; change the minimum display line width Global-Drawing

4) Change the filling grid of the copper skin to Global-Design Units, and the filling direction Drafting-Direction; the value of Copper in the Hatch Grid is the distance from the center to the center of the line filled in the large copper foil.

5) Don't rush to convert GERBER after the copper pour is completed; because some special elements may be placed on different layers due to the habit of the designer; if you do not check layer by layer first, some special elements may be missed. Press Ctrl+Alt+C to open the color setting window, and analyze the file by color setting; remove the check of the circuit layer, set the displayed layer, and tick the corresponding option; tick Visible on, which means that all visible layers are open. Set the elements used in the displayed layer to different colors.

6) Click Apply or OK to return to the graphical interface, determine which layer belongs to by color or press Ctrl+Q after clicking, and determine whether it is an element that needs to be output (you can judge by opening the line), and then open the color setting window after the analysis is completed, Uncheck Visible on and open the circuit layer one by one, check the lines and make some appropriate adjustments to the characters, focusing on whether the elements designed as Lines must be output and whether the Text is made of copper or silk screen

7) After the analysis file is completed, click the menu Setup-Pad Stacks to call up the pad stack setting window, and change the Pad Stack Type to Via. If it is not a blind hole or a buried hole plate, the hole attribute should be Through, not Parti. Otherwise, holes with Parti attributes will not be exported when exporting drilling.

8) If it is a blind hole or buried hole plate, you must click the menu Setup-Drill Partis to call up the drilling pair setting window, and see if the drilling layer is set according to the hole attribute, if not, you must add or add it accordingly. Adjustment.

9) Characters mainly check whether there are pads, fonts are too small or too large, characters are reversed, etc. If there are such phenomena, you can first move, enlarge or reduce, mirror or rotate the characters in PADS, and character line width Waiting for operation

10) So far the file has been analyzed and optimized and adjusted accordingly. Then you can press Alt+F, C to open the CAM output window.

So far, the file has been analyzed and optimized and adjusted accordingly. Then you can press Alt+F, C to open the CAM output window.

11) Click Add to add the layer to be exported, and enter the file name in the pop-up window Document Name

12) Click Layer in the Customize Document column to select the output graphic element.

Click Layer in the Customize Document column to select the output graphic element.

13) Because the Gerber file output by PADS can be aligned with all layers, you don’t need to check Board for all layers like Pads200, and don’t check Vias when solder mask is via hole cap oil. The hole pattern is based on the number of drilled layer pairs. Multiple hole maps can be output; after selecting layers and elements, you can press Preview to preview, and if they are correct, press OK to save;

14) When switching to solder mask, you need to click Option in the Customize Document column, and set the solder mask magnification value in the pop-up Plot Options- window (this is the total value of bilateral magnification, not the unilateral value like Protel).

15) When turning the hole diagram, you also need to click Option in the Customize Document column, select Drill Symbols in the pop-up Plot Options-window, and set a value different from that of the Board in the Chart Line and Line columns of the Drill Drawing Option window. It helps to quickly delete the hole map when processing the file, leaving only the Board, especially when the shape is more complicated and there are many slots), the Location column sets the coordinate value to separate the hole map from the graphics and does not overlap. When the Sizes column All generated Symbols must be deleted.

When turning the hole diagram, you also need to click Option in the Customize Document column, and select Drill Symbols in the pop-up Plot Options- window

16) After finishing the Gerber transfer, you need to drill holes. The transfer method of through holes is different from blind and buried holes. To transfer through holes, just click Add, enter the file name in the pop-up window Document Name, and under Document Select NC Drill in the list and click OK to save

17) After the Gerber and drilling are set up, select a layer with more PCB components (usually the Top layer), click Device SetupPhoto, delete the original D code in the D-Code column of the Plotter Setup window and press Regenerate Regenerate, press OK to save and propose.

18) This operation can make most of the pads in the PCB file still be pads after output, and will not become linear pads

19) Back to the Dsfine CAM Documents window, drag and select all the PCB files that need to be output with the mouse, and press Run to output. The default output path is \CAM\default in the installation directory, or you can press CAM Create to change it.