PCB Tech - The basic process and skills of making PCB

1. Preliminary work of circuit board design

1. Use the schematic design tool to draw the schematic and generate the corresponding network table. Of course, in some special cases, such as the circuit board is relatively simple, there is already a network table, etc., it is not necessary to design the schematic diagram, and directly enter the PCB design system. In the PCB design system, you can directly use the parts and packaging. Generate a netlist.

2. Manually change the network table. Define the pads that are not on the schematic diagram such as the fixed pins of some components to the network connected to it. If there is no physical connection, it can be defined to the ground or the protective ground. Change the pin names of some devices with inconsistent pin names in the schematic diagram and PCB package library to be consistent with those in the PCB package library, especially diodes and transistors.

2. Draw the package library of non-standard devices defined by yourself

It is recommended to put all the parts drawn by yourself into a special design file for PCB library created by yourself.

Three, set up the PCB design environment and draw the printed circuit board with a hollow in the middle, etc.

1. The first step after entering the PCB system is to set up the PCB design environment, including setting the grid size and type, cursor type, layout parameters, wiring parameters and so on. Most of the parameters can use the system default values, and after these parameters are set, they are in line with personal habits and do not need to be modified in the future.

2. Planning the circuit board is mainly to determine the frame of the circuit board, including the size of the circuit board and so on. Put a proper size pad on the place where the fixing hole needs to be placed. For 3mm screws, 6.5~8mm outer diameter and 3.2~3.5mm inner diameter pads can be used. For standard boards, they can be imported from other boards or PCB izards.

Note: Before drawing the border of the circuit board, the current layer must be set to the Keep Out layer, that is, the wiring layer is prohibited.

4. After opening all the PCB library files to be used, import the netlist file and modify the part package

This step is a very important part. The netlist is the soul of PCB automatic routing, and it is also the interface between the schematic design and the impression circuit board design. Only after the netlist is loaded, can the circuit board be wired.

In the process of schematic design, ERC inspection will not involve the packaging of parts. Therefore, when designing the schematic diagram, the packaging of the parts may be forgotten. When the netlist is introduced, the packaging of the parts can be modified or supplemented according to the design situation.

Of course, you can manually generate the netlist directly in the PCB, and specify the part package.

Fifth, the location of the layout of the parts package, also known as the part layout

Protel99 can carry out automatic layout or manual layout. For automatic layout, run "Auto Place" under "Tools". You need to be patient with this command. The key to routing is layout, and most designers use manual layout. Use the mouse to select a component, hold down the left mouse button, drag the component to the destination, release the left button to fix the component. Protel99 has added some new skills in the layout. New interactive layout options include automatic selection and automatic alignment. Using the automatic selection method can quickly collect similar packaged components, and then rotate, unfold and organize them into groups, and then they can be moved to the desired position on the board. When the simple layout is completed, use automatic alignment to neatly expand or shrink a group of similar components.

Tip: During automatic selection, use Shift+X or Y and Ctrl+X or Y to expand and contract the X and Y directions of the selected component.

Note: The layout of parts should be comprehensively considered from the aspects of mechanical structure heat dissipation, electromagnetic interference, and the convenience of future wiring. First arrange the devices related to the mechanical size, and lock these devices, then the large position-occupying devices and the core components of the circuit, and then the peripheral small components.

6. Make appropriate adjustments according to the situation and then lock all devices

If the board space permits, some wiring areas similar to the experiment board can be placed on the board. For large boards, more fixing screw holes should be added in the middle. There are heavy components or larger connectors on the board and other stressed components should also be fixed screw holes. If necessary, some test pads can be placed in appropriate positions. It is best to add them in the schematic diagram. Increase the size of the via hole of the pad that is too small, and define the network of all the fixed screw hole pads to the ground or the protective ground.

After placing it, use the VIEW3D function to check the actual effect and save it.

Seven, wiring rules settings

Wiring rules are to set up the various specifications of the wiring (such as the use level, the line width of each group, the spacing of the vias, the topology of the wiring and other rules, which can be exported from other boards through the Menu of Design-Rules, and then imported into this board. ) This step does not have to be set every time, it can be set once according to personal habits.

Choosing Design-Rules generally requires resetting the following points:

1. Safety distance (Clearance Constraint of Routing label)

It specifies the distance that must be maintained between the trace pad vias of different networks on the board. Generally the board can be set to 0.254mm, the empty board can be set to 0.3mm, and the denser patch board can be set to 0.2-0.22mm. The production capacity of very few printed board manufacturers is 0.1-0.15mm. You can set this value with their consent. Below 0.1mm is absolutely prohibited.

2. Routing layer and direction (Routing Layers of the Routing tab)

Here you can set the routing layer used and the main routing direction of each layer. Please note that the single panel of the patch only uses the top layer, and the in-line single panel only uses the bottom layer, but the power layer of the multilayer board is not set here (you can click the top layer or the bottom layer in the Design-Layer Stack Manager, and use Add Plane, double-click with the left mouse button to set, click on the layer and delete it with Delete), the mechanical layer is not set here (you can select the mechanical layer to be used in Design-Mechanical Layer, and choose whether it is available Depending on whether and whether they are displayed in single-layer display mode at the same time).

Mechanical layer 1 is generally used for the frame of the drawing board;

The mechanical layer 3 is generally used for mechanical structural parts such as bars on the drawing board;

Mechanical layer 4 is generally used for drawing rulers and annotations, etc. You can use the PCB Wizard to export a PCAT structure board by yourself.

3. Via shape (Routing Via Style of the Routing label)

It specifies the inner and outer diameters of the vias that are automatically generated during manual and automatic wiring, which are divided into minimum, maximum and preferred values, of which the preferred value is the most important, the same below.

4. Route width (Width Constraint of Routing tab)

It specifies the width of traces during manual and automatic routing. The preference of the entire board range is generally 0.2-0.6mm, and some network or net class line width settings are added, such as ground wire, +5 volt power line, AC power input line, power output line and power pack Wait. The network group can be defined in the Design-Netlist Manager in advance. The ground wire generally has a width of 1mm, and various power cables generally have a width of 0.5-1mm. The relationship between the line width and the current on the printed board is about 1 per millimeter of line width. For the current of ampere, please refer to the relevant information for details. When the preferred value of the wire diameter is too large so that the SMD pad cannot be routed through the automatic routing, it will automatically shrink to a section of trace between the minimum width and the width of the pad when it enters the SMD pad, where the Board is for the entire The line width constraint of the board has the lowest priority, that is, the line width constraint conditions of the network and the network group are first met when wiring.

5. Setting of copper connection shape (Polygon Connect Style of Manufacturing tab)

It is recommended that the Conductor Width of Relief Connect be used for 4 wires of 0.3-0.5mm at 45 or 90 degrees.

The rest of the items can generally use its original default values, and items such as the topology of the wiring, the spacing of the power layer and the length of the network matching the connection shape can be set as needed.

Select Tools-Preferences, and select Push Obstacle in Interactive Routing in the Options column (push other routes when encountering a route of a different network, Ignore Obstacle is to pass through, Avoid Obstacle is to block) mode and select Automatically Remove (automatically remove) Delete redundant traces). The Track and Via in the Defaults column can also be changed. Generally, there is no need to move them.

Place the FILL filling layer in the area where the wiring is not desired, such as the wiring layer under the radiator and the lying two-pin crystal oscillator, and put the FILL in the corresponding place of the Top or Bottom Solder for tinning.

Wiring rule setting is also one of the keys to the design of printed circuit boards, which requires a wealth of practical experience.

8. Automatic wiring and manual adjustment

1. Click the menu command Auto Route/Setup to set the automatic wiring function

Select all items except Add Testpoints, especially the Lock All Pre-Route option, and the Routing Grid option is 1mil. Before the automatic wiring starts, PROTEL will give you a recommended value. You can ignore it or change to its recommended value. The smaller the value, the easier the board will be 100% distributed, but the more difficult the wiring and the more time it takes.

2. Click the menu command Auto Route/All to start automatic routing

If it cannot be completely routed, it can be completed manually or UNDO once (do not use the undo all wiring function, it will delete all pre-wiring and free pads, vias), adjust the layout or wiring rules, and then re-wiring. Do a DRC after completion, and correct any mistakes. During the layout and wiring process, if errors are found in the schematic diagram, the schematic diagram and the network table should be updated in time, the network table should be manually changed (same as the first step), and the network table should be reinstalled before deployment.

3. Make preliminary manual adjustments to the wiring

The ground wires, power wires, power output wires, etc. that need to be thickened are thickened, and some wires that are wound too much are rerouted to eliminate some unnecessary vias. Use the VIEW3D function again to see the actual effect. In the manual adjustment, you can select Tools-Density Map to view the wiring density. Red is the densest, yellow is the second, and green is looser. After reading, you can press the End key on the keyboard to refresh the screen. The red part should generally be adjusted loosely until it becomes yellow or green.

9. Switch to single layer display mode (click the menu command Tools/Preferences, select Single Layer Mode in the Display column of the dialog box)

Pull the wires of each wiring layer neatly and beautifully. You should always do DRC during manual adjustment, because sometimes some wires will be disconnected and you may walk several wires from where it is disconnected. When you are almost done, you can print out each wiring layer separately for easy reference when changing wires., In the meantime, also often use 3D display and density map function to check.

Finally, cancel the single-layer display mode and save.

10. If the device needs to be re-annotated, click the menu command Tools/Re-Annotate and select the direction, and then press the OK button.

Go back to the schematic diagram and select Tools-Back Annotate and select the newly generated *.WAS file, and then press the OK button. Some labels in the schematic diagram should be dragged and dropped again for aesthetics. After all adjustments are completed and the DRC is passed, drag and drop all the characters on the silk screen layer to a suitable position.

Note that the characters should not be placed under the components or on the via pads. The characters that are too large can be reduced appropriately, and some coordinates (Place-Coordinate) and dimensions ((Place-Dimension) can be placed on the DrillDrawing layer as needed.

Finally, put information such as the name of the printing plate, design version number, company name, the first processing date of the file, the name of the printing plate file, and the processing number of the file (please refer to the figure shown in the fifth step). And you can use third-party programs to add graphics and Chinese annotations, such as BMP2PCB.EXE and FONT.EXE in the special PCB Chinese character input package for ROTEL99 and PROTEL99SE of Hongshi Company.

11. Fill teardrops on all vias and pads

Filling teardrops can increase their fastness, but it will make the lines on the board more ugly. Press the S and A keys of the keyboard in sequence (select all), then select Tools-Teardrops, select the first three in the General column, and select Add and Track mode. If you don’t need to convert the final file to PROTEL DOS format file If you want, you can also use other modes, and then press the OK button. After completion, press the keyboard X and A keys in sequence (all unselected). It must be added for patch and single panel.

12. Place the copper clad area

Temporarily change the safety distance in the design rule to 0.5-1mm and clear the error mark. Select Place-Polygon Plane to place the copper pour of the ground wire network on each wiring layer (try to use an octagon instead of an arc to wrap the pad. In the end, if you want to convert to a DOS format file, you must choose an octagon). The following figure is an example of setting copper pour on the top layer:

After the setting is completed, press OK again to draw the border of the copper-clad area. You can leave the last side unpainted, just press the right button of the mouse to start the copper-cladding. It defaults that your starting point and ending point are always connected by a straight line. When the circuit frequency is higher, the optional Grid Size is larger than the Track Width, and the grid lines are covered.

Place the copper pours of the remaining wiring layers accordingly, observe a large area where there is no copper pour on a certain layer, place a via on the other layer where there is copper pour, double-click any point in the copper pour area and select a copper pour, Click OK directly, and then click Yes to update the copper pour. Several copper-clad layers are repeated several times until each copper-clad layer is full. Change the safety clearance in the design rule back to the original value.

14. Do DRC one more time at the end

Select Clearance Constraints Max/Min Width Constraints Short Circuit Constraints and Un-Routed Nets Constraints, press the Run DRC button, and correct any errors. Save it after everything is correct.

14. For manufacturers that support PROTEL99SE format (PCB4.0) processing, you can export this file as a *.PCB file while viewing the document catalog; for manufacturers that support PROTEL99 format (PCB3.0) processing, you can export the file Save as PCB 3.0 binary file and do DRC. Exit without saving after passing. In the case of viewing the document catalog, export this file as a *.PCB file. At present, a large number of manufacturers can only make boards drawn by PROTEL AUTOTRAX under DOS, so the following steps are indispensable for generating a DOS version PCB file:

1. Change the content of all mechanical layers to mechanical layer 1, export the netlist as a *.NET file when viewing the document directory, and export the PCB to PROTEL PCB 2.8 ASCII FILE format when viewing this PCB file *.PCB file.

2. Open the PCB file with PROTEL FOR WINDOWS PCB 2.8, select Save As in the File menu, and select Autotrax format to save as a file that can be opened under DOS.

3. Use PROTEL AUTOTRAX under DOS to open this file. Individual strings may need to be dragged and dropped or resized. All two-pin SMD components placed up and down may have the X-Y size swap of the pads, adjust them one by one. The large four-column SMD IC will also have all the pads X-Y swapped. Only half of the automatic adjustment can be done manually. Please save it at any time. Human errors are prone to occur in this process. The PROTEL DOS version has no UNDO function. If you clothed the copper and chose to use arcs to wrap the pads, then all the networks are basically connected. It is very tiring to delete and modify these arcs one by one by hand, so I recommend that you must Use an octagon to wrap the pad. After all these are completed, use the previously exported network table as the Separation Setup in DRC Route. The values should be smaller than those in the WINDOWS version. If there is any error, correct it until all the DRC is passed.

You can also directly generate GERBER and drilling files and submit them to the manufacturer to select File-CAM Manager and press Next> to display six options. Bom is the list of components, DRC is the design rule inspection report, Gerber is the gerber file, and NC Drill is the drill. Hole file, Pick Place is automatic pick and place file, Test Points is test point report. After selecting Gerber, follow the prompts to proceed step by step. Some of the parameters related to the production process capability need to be provided by the printed board manufacturer. Until you press Finish. Click the right mouse button on the generated Gerber Output 1, select Insert NC Drill to add the drilling file, and then click the right mouse button to select Generate CAM Files to generate the real output file. The gerber file can be exported and opened with CAM350 for verification. Note that the power plane is a negative output.

15. Send email or copy to the processing factory

Indicate the board material and thickness (when making general boards, the thickness is 1.6mm, extra-large boards can be 2mm, radio frequency microstrip boards, etc. are generally around 0.8-1mm, and the dielectric constant and other indicators of the board should be given), quantity, Special attention should be paid when processing. Call the manufacturer within two hours after the email is sent to confirm whether it has been received.

16. Generate a BOM file and export it and edit it into a format that meets the company's internal regulations.

Seventeen, the frame screw hole connector and other parts related to the machining of the chassis (that is, the other irrelevant parts are selected and then deleted)

Export as a DWG format file of AutoCAD R14 in metric size to the mechanical designer.

Twenty-one. Organize and print various documents.

Such as component list, component assembly drawing (and print scale should be noted), installation and wiring instructions, etc.