PCB Blog - PCB Design Technology of PROTEL99SE

PROTEL99SE PCB design technology

1. Set up the software working environment

Software rule settings:

Enter Design  Rules and set the items in the options according to the design requirements:

1. Safety distance setting: The Clearance Constraint item of Routing in PROTEL99SE software specifies the distance that must be kept between the routing, pads, vias, etc. of different networks on the board. In the design of single panel and double panel, the preferred value is 10-12mil; The preferred value of PCB with four or more layers is 6-8mil; The maximum safe distance is generally unlimited.

2.  Wiring layer and direction setting: Routing Layers of Routing, setting the used routing layer and the routing direction of each layer (only the top layer is used for patch single panel, and only the bottom layer is used for direct plug-in single panel). Generally, the default value is used.

3. Setting of via options: Routing Via Style in PROTEL99SE software specifies the minimum, maximum and preferred values of the inner and outer diameters of vias. The through hole outer diameter of single panel and double panel shall be set between 40 mil and 60 mil; The inner diameter shall be set at 20mil - 30mil. The minimum outer diameter of PCB with four or more layers is 20 mil, and the maximum outer diameter is 40 mil; The minimum inner diameter is 10mil and the maximum inner diameter is 20mil.

4.  Line width option setting: Width Constraint of Routing in PROTEL99SE software specifies the width of wiring. The wiring width of single panel and double panel shall be set between 10-30mil. Under special circumstances, the maximum value shall not exceed 60mil and the minimum value shall not be less than 8mil; The minimum value of four or more layers of PCB shall not be less than 5mil, and other settings shall refer to the settings of double-sided boards. You can also add line width settings for some networks, such as ground wire,+5V power line, clock line,+12V power line, - 12V power line, AC power input line, power output line, etc. The preferred value of ground wire, clock wire and+5V power line is generally 60ml (the maximum value is unlimited, the minimum value is 8 mil, and the line shall be as wide as possible if it can be connected), and the preferred value of various power lines is generally 40ml (the maximum value is unlimited, the minimum value is 8mil, and the line shall be as wide as possible if it can be connected). Determine the maximum line width according to the relationship between PCB line width and current (about 500 mA current is allowed per mm line width).

5.  Copper coating connection option setting: The Polygon Connect Style item of Manufacturing in PROTEL99SE software specifies the copper coating connection method. Set the Rule Attributes to the Relief Connect mode, the Conductor Width to 25mil, the Conductors to 4, and the Angle to 90 degrees.

6. Physical aperture setting: The Hole Size Constraint item of Manufacturing in PROTEL software specifies the size of the physical aperture. The minimum value is set to 20mil, and the maximum value is unlimited (Note: physical holes generally refer to positioning holes, installation holes, etc.). Other items can generally use their default values.

PROTEL99SE PCB Software parameter setting:

Enter Design  Options and Tools  Preferences, and set the items in the options according to the design requirements:

1.  Visual grid option setting: select from Design  Options  Layer in PROTEL software: Top solver in Masks; Top overlay in Silkscreen; Keepout and Multi Layer in Other; Select all items below the System. The Visible Grid item specifies the size of the visible grid, which is set to 10mil (upper) and 100mil (lower) respectively.

2. Capture and device moving grid option setting: The Design  Options  Options item in PROTEL software specifies the size of capture and device moving grid, and the capture and device moving grid are both set to 10mil. Select Electrical Grid and set Range as 8mil, Visible Kind as Lines, and Measurement Uint as Imperial.

DRC verification settings:

1. Enter Tools  Design Rules Check and set the options according to the design requirements: Clear Constraints, Max/Min Width Constraints, Short Circuit Constraints and Un Routed Net Constraints of Report  Routing Rules are all selected; Select Max/Min Hole Size of Report  Manufacturing Rules; Select all options of Report  Options; On line  Routing Rules Clear Constraints is selected; Select Layer Pairs of On line  Manufacturing Rules; On line  Placement Rules, select ComponentClearance.

2. Add device library

This step is mainly to call out the components shown in the schematic diagram of the PCB from the corresponding library of components

3. Import Network Table

In the process of importing the network table, it must be ensured that there are no errors. It is strictly prohibited to design when there are errors in the network table import. (Attention must be paid to this operation) Determine the PCB size and the location and size of the positioning hole, and lock the related components

4. Layout of components

The principle of PCB layout is beautiful and generous, with proper density, in line with electrical characteristics, conducive to wiring, and divided into modules as far as possible. If possible, place the components in order, and try to ensure the symmetry between the main components and modules.

Requirements: The entire PCB layout should be grand and properly spaced, and not too tight or loose in some places. The silk screen frame shall be minimized and the modules shall be highlighted. The Chinese or English signs of modules shall be placed at symmetrical and parallel positions as far as possible, and can reflect the name and aesthetic feeling of modules.

After the layout is completed, the PCB layout should be checked. Generally, the following aspects should be checked:

(1) The size of the printed board shall be consistent with the size of the processing drawing, with positioning marks and reference points;

(2) Components shall ensure no conflict in two-dimensional and three-dimensional space;

(3) The layout of components shall be dense and orderly;

(4) Components that need to be replaced frequently shall be easily replaced;

(5) A proper distance shall be kept between the thermal element and the heating element. Where heat dissipation is required, a radiator shall be installed to ensure smooth air flow;

(6) Adjustable components shall be easy to adjust;

(7) The signal flow shall be smooth and the interconnection shall be shortest;

(8) Ensure the minimum number of vias as far as possible;

(9) It is prohibited to use Ctrl+X or Ctrl+Y to flip the device;

(10) The inner diameter of holes on a PCB cannot exceed 9 types;

(11) Components that affect the appearance, such as TO-220 packaged three terminal voltage regulator and electrolytic capacitor of the chip, shall be welded on the reverse side as far as possible; Potentiometers, middle circumference and adjustable capacitors that do not need to be adjusted shall be welded on the reverse side as much as possible, and shall not be welded through PCB, and shall be specifically stated in the product specification; Other components that especially affect the overall appearance, such as large electrolytic capacitors and relays, shall be welded on the reverse side.

PCB wiring

It is generally recommended to use the method of automatic routing+manual adjustment. Automatic routing requires routing in the order of ground wire - power line - clock line - others. Set the routing priority in the routing rules. 0 is the lowest level, 100 is the highest level, and there are 101 cases in total. In the more complex circuit boards, considering the requirements of electrical characteristics, interference and other factors, we all use manual wiring. It is prohibited to place vias on the pins of components, and the already laid wires should be locked before automatic wiring. Both aesthetic and electrical characteristics shall be taken into account when routing. If routing has a special impact on the appearance, try to go on the reverse side. In principle, do not route on the front side of the product name, model and logo (except for special circumstances), and do not route on the front side between the silk screen box and the Keepout box (except for special circumstances).

Placement of silk screen and Chinese characters

(1) Placement of product name, model and public logo

(2) Placement of component engineering number silk screen

(3) Placement of Chinese characters marked by modules

(4) Placement of test hook and test hole identification

(5) Requirements for font placement

Large area paving

Enter Place  Polygon Plane, set Connect to Net as Connect to GND in the Net Options option, select Pour Over Same and Remove Dead top, set the Grid size to 18mil in the Plane setting option, set the Track width to 20mil, and select the corresponding layer in the layer; In Hatching style, select Vertical Hatch; Others use default values.

Before large-area paving, the safety clearance value should also be set to 25mil. After large-area paving, the safety clearance value should be restored. Place FILL filling layer in the area where wiring is not desired (such as radiator and horizontal bipod crystal oscillator, HC49S crystal oscillator, front of multi turn potentiometer, TO220 packaged three end voltage regulator, etc.), and place FILL at the corresponding position of the Top Solder or Bottom Solder layer where tin is required if other network lines pass through from here.

Teardrops can increase their fastness but make the lines on the board look ugly. For patches and single panels, they must be added. Other teardrops can be selected according to the actual situation.

Repeat DRC check

Enter Tools  Design Rules Check, and set the items in the options according to the design requirements. Refer to the previous settings. After the DRC check, correct the errors found in the check. No errors are allowed after the DRC check.

PROTEL99SE PCB Main matters

The operation of the whole process needs to be careful, especially the PCB wiring must be guaranteed to be error free

In order to prevent technical disclosure, the package and name of components shall be completely deleted during plate making or archiving. A board making instruction must also be attached. For example, thickness: when making general PCB, the thickness is 1.6mm, 2mm for large PCB, and 0.8-1mm for RF PCB; Material and color, etc