• State Answer Suggested
  • Locked Locked
  • Replies 5 replies
  • Answers 1 answer
  • Subscribers 63 subscribers
  • Views 1372 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

Through-hole Components PCB Layout Design

Evgeniy Sokolov
Intellectual 630 points
Other Parts Discussed in Thread: TIDA-01480, TIDA-01510

Hello Community,

I am interested in your opinion on the use of thermal relief for the through-hole components related to the power supply circuits of the circuit. After reviewing several documents, such as this one, . I realized that thermal relief is required for through-hole components, but I am not sure how the application of thermal relief will affect the conductivity properties (inductance, resistance) for power circuits of the circuit, where this can play a huge role. Do you think it is necessary to use thermal relief on the power components of the circuit (power connector, capacitors, etc.)? If you think that you should not use it, then how to solder these components, because with manual installation (with a soldering iron), uniform heating of the board and its internal layers (power - planes, polygons) cannot be ensured and this can lead to a breakdown in contact of the soldered element.

  • 0
    Prodigy 5 points
    Hello Evgeniy

    This is a very good question. I will have a detailed reply Monday.
  • 0 in reply to Ed Walker
    Intellectual 630 points
    Hello Ed,
    I'd like to know your opinion, thank you for your help.
  • 0 in reply to Evgeniy Sokolov
    Prodigy 5 points

    Hello Evgeniy,

    My past designs had very large heatsinks, transformers, connectors.
    Thermal copper relief was only considered after initial prototype builds showed a problem.
    Wave solder design guidelines are based off experience, documented, then made the rule.
    So occasionally experience would show that some relief was needed for a solder location.

    One of the best treatments of PCB design is this seminar paper, by Robert Kollman.
    SEM1600 Topic 4: Constructing Your Power Supply – Layout Considerations

    Topics considered are:

    DC Parasitics (Resistance)
    AC Parasitics
    Grounds and Grounding
    Thermal Considerations
    Design Examples

    One of the more interesting concepts is the “Rule of Squares” to estimate trace resistance.
    It doesn’t directly address the thermal relief for thru-hole, there is insight in the Examples section.

    VI. Design Examples page 19
    There are several large components with thermal relief designed into the copper plane.
    All of these large PT holes are by an edge of a plane, or the plane is small.
    The hole being by the edge of the plane allows it to heat up properly for wave solder.

    Here are 2 other good papers on board design.

    Best Practices for Board Layout of Motor Drivers

    2.4         Thermal Via Connections page 9
    3             Vias page 11

    Solder mask is critical for controlling the heat during wave solder.
    The exposed copper around the via is similar to a hole for a device.
    The solder mask helps focus the heat at the place of solder.
    Solder mask clearance of 5-10mm  around a solder location is standard.

    PowerPAD Layout Guidelines
    2.2         Copper Areas
    2.3         Thermal Vias

                  

    There are also many examples of board design in TI's many reference designs.
     TI reference designs search
    Many of these designs have large components, and demonstrate proper design methods.

    You can also look at the EVM layouts of various IC's to find good examples. 

    I hope this helps.

  • 0 in reply to Ed Walker
    Intellectual 630 points

    Hello Ed,

    Thank you for the work you have done, it was useful for me.

    I studied all the documents that you submitted and turned to some reference designs in which I was interested in connecting individual components. (TIDA-01510 - C7 (thru-hole capacitor), TIDA-01480 (J1 (thru-hole power supply connector connector))) In these board designs, the capacitor and the power connector are connected directly to the polygons / planes of the power supply of the printed circuit board. But most manufacturers of printed circuit boards very often indicate that through-hole components, which are in the case of TI boards (capacitor C7 and power connector J1), must be connected through thermal relief and this is due to the fact that these components are soldered to the board not in a special oven (in which the board warms up completely, including the power layers), but manually with a soldering tip, which is unable to fully heat the board at the soldering point without damaging the component and creating a solid solder contact without disturbing its center integral domain and consequently as a result a large number of defective boards and damaged components. Therefore, I have the following questions:
    1. SLUP230 - Fig.28 & Fig.29 which of the figures the author indicated the correct trace option? (I made a conclusion for myself that the correct version is Fig.28, but I am afraid that it may be erroneous)
    2. Are there any problems in the production of boards at TI, when installing the through-hole components directly connected to the polygons / power planes? (capacitors, power connectors, etc.) Perhaps there are statistics on the number of defective boards? :)

  • 0 in reply to Evgeniy Sokolov
    Prodigy 5 points

    Greetings Evgeniy,

    SLUP230 should have been corrected long ago.
    Looking at the figures 28 and 29 I can see that figure 29 has much longer traces connecting the output capacitors.
    This picture is from the PPT presentation stack from the seminar. 
    Figure 28, the proper method to reduce series inductance, is on the left, Figure 29 on the right.
    Your intuition was correct.

    TI does not make PCB's anymore.
    PCB's are designed by TI's engineers with various CAD programs, then sent to out to be built.
    We use various assembly companies to produce boards for our Evaluation Modules and Reference Designs.

    Therefore we have no statistical data that can be shared.

    If a large solder connection is to be done by hand then yes, you may want to use some thermal relief for hand solder.
    Experience will help guide you in this instance.
    But for volume manufacturing these hand operations must be minimized.
    This is one reason prototype builds are important, they help fine tune the assembly and design problems.
    Rather than hand solder, experiment with ways to modify the PCB and wave solder process to accommodate the large connections. 

    On a side note:
    Here is the archive for Power Supply Design Seminars.
    Many great papers are stored here starting with the original Unitrode Seminars that were continued when TI acquired Unitrode.

    Have a great day Sir.