Contact us

Name *
Telephone *
E-mail *
Message text *

Requirements for printed circuit boards for surface mount technology

General

This page specifies general technical requirements for designing printed circuit boards with the use of electronic components designed for surface mounting. IPC-7351 and IPC-782 recommendations were used at compilation.

In addition to general requirements stated in GOST 23.751-86 this recommendations that take into consideration characteristic properties of equipment allow to avoid mistakes in the design of printed circuit boards.

The process of preparing printed circuit boards for automated mounting at ELARA JSC included several stages:

  • checking conformance to the requirements for surface mounting of components, primary imposition, checking technological effectiveness of a product, coordination of technical questions with the customer;
  • creating a technological panel (printed circuit board panel) taking into account technical characteristics of mounting equipment, the number of printed circuit boards in the order, peculiarities of production and cost of silk screen printing, etc.;
  • arranging technological zones on the panel.

If necessary the number of printed circuit boards on the panel and its appearance may be agreed with the customer – designer of the unit.

Requirements for designing printed circuit boards intended for automated mounting of surface mount components

Requirements for the base panel of the printed circuit board:

  • Panel dimensions must be from 50 x 50 mm to 460 x 440 mm. Recommended aspect ratio must not be over 1:3. Small size printed circuit boards are accepted only on multiple panels.
  • Thickness of a PCB panel sheet must be from 0,6 mm to 3 mm (0,024”...0,2”).
  • Technological zones on the panel where allocation of components is not allowed, must be in accordance with Figure 1. 

Technological zones (Figure 7) simultaneously fulfill several functions:

- they are used to fix the panel on the assembly line for automatic installation of components;
- they allow for component allocation near the edge of the PCB;
- they are used for allocating fiducial marks;
- they are used to reinforce the panel with its minimum thickness and a large number of internal cutouts.

    As a rule technological zones a located along a long side of the panel and are 5 mm wide. On the periphery of technological zones there are 3,3 mm diameter holes used to fix the panel in automatic machines. Technological zones are separated from the panel by means of scribing method or using bridges.

    In case it is impermissible to use technological zones, areas of the PCB free from components and corresponding to the characteristics of technological zones must be provided for. 

    Figure 1

    Figure 1. Zones forbidden for component allocation

    A is the side used for installing SMD components:

    - 3 mm wide forbidden zone from the upper edge of the panel (Figure 1);
    - 5 mm wide forbidden zone from the lower edge of the panel (Figure 1);

    B is a PCB side opposite to SMD components:

    - 5 mm wide forbidden zones from the upper and lower edges of the PCB (Figure 1);
    - Distortion of the PCB panel must not exceed the values shown in Figure 2.

    Figure 2

    Figure 2. The PCB side for soldering SMD components.

    • if there arises a necessity to install add-on components on the PCB prior to installing SMD component their height must not exceed the following values:

    - 6,5 mm (0,26”) on the PCB side for SMD component installation (Figure 3);
    - 10 mm* (0,4”) on the PCB side opposite to SMD components (Figure 3).

    * there must be a minor increased tolerance – 20 mm max.

    Figure 3

    Figure 3. The PCB side for soldering SMD component.

    Marks on the PCB (Fudicial Marks)

    A mark on the PCB is the centre of a coordinate system at the stage of PCB assembly. It allows for the equipment to correct current coordinates measurement inaccuracies that are accumulated in the process of automated installation of components on the PCB. There are two types of starting point marks: Global Fiducials and Local Fiducials.

    • Global Fiducials are used for the whole PCB or in case of several PCBs combined into a panel for connecting the whole panel. Minimum two Global Fiducials are required. They are usually located in diagonally opposite corners of the PCB as far from each other as possible. Global Fiducials must be present on all layers containing components.
    • Local Fiducials are used to bind a specific component (usually with a big number of leads and a small pitch between them) in order to calculate coordinates (X,Y offsets). Local starting point marks are usually located diagonally on the periphery of the area covered by this component. In case of a lack of free space it is allowed to use one Local Fiducial of a starting point, preferably in the centre of the area occupied by the component. 

    All the marks are located beyond areas where it is forbidden to locate connectors and components.

    The following forms of starting point marks are used, A = (0,8...3,0) mm (0,03”...0,12”) (Figure 4):

    - filled/painted circle (preferable);
    - filled/painted square;
    - filled/painted turned/rotated square;
    - isolated/solitary cross.

    A recommended size “A” for a starting point mark is 1 – 1,5 mm.

    Starting point marks on the PCB (panel) must be uniform in shape and size.

    It is allowed to use Global Fiducials of a bigger size than Local Fiducials.

    For example: Global Fiducials – 1,5 mm, Local Fiducials – 1 mm.

    Applicable starting point marks are shown in Figure 4. 

    Figure 4

    Figure 4. Applicable starting point marks

    In the area around the mark it is forbidden to use conductors, components and solder mask (Figure 4). The correlation between the free zone and the mark is 3:1.

    All the marks must be shown in the conductor layer.

    Marks must be free from the solder mask and have a smooth, light reflecting metal coating (nickel, pewter, silver, etc.). The plane surface of the mark must be within 15μm.

    The distance between the marks and the edge of the PCB must not be less than 5,0 mm (0,2”) plus the width of the gap.

    It is recommended to allocate the marks at the spots as shown in Figure 5.

    Рисунок 5


    Figure 5. Example of starting point marks allocation

    Module multiplication

    In case of mounting small size printed circuit boards automatically they are combined into an integrated panel (multiplication) and are located on one workpiece (Figure 6).

    Figure 6

    Figure 6. Example of allocating several PCBs on one workpiece

    The distance between PCBs must meet the requirements of the applied PCB separation technology: milling (Figure 7), scribing (Figure 8).

    Figure 7

    Figure 7. Example of separation by milling

    The “score lines”, on the one hand, must ensure sufficient strength of the PCB panel at solder mask application, mechanical installation and component soldering, and on the other hand, provide for a guaranteed separation of finished PCBs at breaking.

    Рисунок 8

    Figure 8. Example of separation by scribing

    General guidelines on PCB construction:

    • Allocation of the PCB's “zero”:

    - the PCB's “zero” must be located in the absolute coordinate system in point (100;100).

    • Allocation of conductors and components:

    all uncased and planar lead components (SMD) must be located on one side of the PCB. If this condition is impossible to fulfill the components must be divided into “light” and “heavy” one, and located on different sides of the PCB. For example, passive components could be placed on one side, and microcircuits on the other;
    land dimensions must conform to the sizes recommended for this casing dimension type (you can clarify the information on land dimensions in the component datasheet or in IPC7351 or IPC-782);
    - clearance between components must not be less than the ones shown in Figure 9.

    Рисунок 9

    Figure 9. Minimum clearance between components

    - components must not be allocated closer than 1,25 mm (0,05”) from the edge of the workpiece, and closer than the forbidden zones indicated above;
    - sharp angles in the metallization layer must be avoided when routing conductors;
    - ground bus must be everywhere possible;
    - pay attention to the necessity of a forbidden zone around mounting holes;
    - hole diameters of components with leads must not exceed lead diameters for more than 0,25 mm (0,01”);
    - hole diameters on the drawing are indicated taking into consideration thickness of metal plating;
    - distance from the edge of an unsupported hole to the land or conductor must not be less than 0,5 mm (0,02”);
    - it is preferable to orient polar components equally;
    - it is preferable that a maximum number of components has an identical dimension-type of the casing. For example, resistors and capacitors – 0805, etc. This method of selecting components allows the mounter to achieve maximum performance;
    - rotation of a component around its axis with 1 degree increment;
    - maximum height of a component is 20 mm;
    - for components with lead pitch 0,5 mm and less it is necessary to leave space for allocating Local Fiducials;
    - conductors located under SMD components must be covered with protective mask;
    - vias under SMD components must be covered with protective mask;
    - to prevent the PCB from distorting in the process of production and mounting while heating in a furnace it is necessary to allocate testing areas on external and internal layers (for multilayer PCBs) equally along the surface of the printed circuit board and produce them in the shape of a net made of conductors;
    - the distance from the edge of an unsupported hole to a land or a conductor must not be less than o,5 mm;
    - to reduce egress of heat from lands during soldering (to eliminate cold soldering) it is necessary:

    a) to use narrow conductors directly connecting a land and a wide conductor as shown in picture 10. The width of a “narrow” conductor is selected depending on the accuracy class of the board and the current passing through it.

    Figure 10

    Figure 10. Example of leading wide conductors to lands

    b) All the bridge connections between SMD microcircuit connectors must be located beyond soldering area.

    Figure 11

    Figure 11.

    c) SMD component lands located on large testing areas must be separated from testing areas by bridge connectors (Figure 12).

    Figure 12

    Figure 12. Example of SMD lands allocation on large testing areas

    d) around the land apply solder mask that prevents molten solder from from moving along the conductor.

    • Recommendations for making vias.

    To a large extent the quality of surface mount components mounting depends on the correct production of vias. Incorrect allocation of vias in relation to SMT components lands is a common mistake of designers.

    - allocation of vias under SMD components and on lands is unacceptable;
    - via diameter must be selected based on the PCB thickness and PCB thickness/ minimum plated hole diameter correlation recommended by the manufacturer.

    The figure below (Figure 13) demonstrates the recommended allocation of vias and lands.

    Figure 13

    Figure 13. Example of via allocation

    • Recommendations for marking a PCB.

    On a PCB there are markings of:

    - graphic and positional component designations (graphic component designations must reflect polarity and orientation of components on the PCB);
    - PCB, version designations and designation of the manufacturing company and its address (usually a code number and a PCB change number);
    - the designed location, marked by the outline for the PCB number and production date marking, the number given in the process of mounting can be either come in the form of a stick-on label or marked manually;
    - silk screen printing is used for marking graphic and positional component designations on the PCB. It is preferable to make the rest of the markings in the conductor layer. It is preferable to locate silk screen printing only those areas of the PCB that are covered by solder mask;
    - component marking elements that are located next to each other must not cross over and overlap.

    It must be taken into account that marking elements on lands free from mask and covered with final finish (POS-61, immersion gold, etc.) will not be applied.

    • Recommendations for PCB construction when using the reflow soldering technology for soldering radio elements:

    - all the passive components must be parallel to each other;
    - all the SOIC components must be perpendicular to longitudinal axes of passive components;
    - longitudinal axes of SOIC and passive components must be perpendicular to each other;
    - longitudinal axes of passive components must be perpendicular to the direction of PCB movement on the line of reflow soldering.

    Completeness of the provided design documentation

    Technical documentation provided by the customer must include:

    - a project file/s (PCAD file is indispensable to develop control software for a surface mount assembly line);
    - a completed PCB order form (if it is necessary to order PCBs);
    - an assembly drawing (in any CAD format);
    - specification indicating component descriptions, their positional designations on the PCB, nominal values and casing types.

    Incorrectly prepared project and technical documentation files complicate or sometimes make it impossible to perform assembly and mounting works.

    Requirements for electrical testing of the module

    If the customer decides to perform electrical testing of modules there appear several requirements.

    Testability requirements the customer's products:

    • a PCB must have two fiducial marks in the upward-most left and downward-most right angles of the PCB. The accuracy of fiducial marks coordinates must be up to 0,1 mm;
    • contacting of fly-probes with mounting contact lands of the Programme and methods of testing (but not terminal leads of the Programme and methods of testing) is allowed;
    • it is optimal to use test lands with 0,89 – 0,95 mm in diameter and unmasked vias with no less than 0,7 mm in diameter; minimum acceptable pitch between test lands and vias must be no less than 2,5 mm. Test lands must be covered by a material that protects from oxidation (e.g. solder), and must not be covered by lacquer, flux or some other materials;
    • the PCB must have a zone free from components and test points no less than 3 mm along its length and on both sides from the edge to fix the PCB for testing;
    • the length of electronic components terminal leads inserted into the holes from the side contacting with test pins and fly-probes must not exceed 1,6 mm in order to avoid destruction of test pins.

    Requirements for test software design

    The customer must provide the following:

    • the electric schematic diagram of the product under test in the form of the CAD file in a known format;
    • parts list of the product under test;
    • PCAD file for the PCB under test with filled nominal values of passive components;
    • the assembly drawing of the product under test.

    Download/Print 
     

    Place an order      

    If you have any questions contact us via e-mail elmodul@elara.ru or call us at
    +7 (8352) 22-17-68, 22-13-74, 22-14-95.


    page up