Tutorial 1.10: Assign Footprints to Switching Regulator and MOSFET Transistor

The footprint for Switching Regulator Controller LTC1624CS8

Check Footprint Assigned to Switching Regulator

1.        The next symbol 14 which is   U1 -    LTC1624CS8.

2.        KiCad has allocated the footprint Package_SO:SOIC-8_3.9x4.9mm_P1.27mm.

3.        Right-click on symbol 14 which is  U1 – LTC1824CS8 and select View Footprint.

4.        You should see the footprint as shown in figure 1.10A below:

Fig. 1.10A: Footprint Allocated By KiCad to U1 Switching Regulator Controller.

5.       From the SOIC-8_3.9x4.9mm_P1.27mm footprint name and measurements made 

          by the Vernier caliper or Measure distance between two points tool we 

          can conclude:

           5.1      SOIC - it is a Small Outline Integrated Circuit which is a surface- 

                        mounted integrated circuit (IC).

           5.2      8 – it has 8 pins.

           5.3      3.9x4.9mm – the IC has a horizontal body width of 3.9mm and a 

                        vertical length of 4.9mm.

          5.4      P1.27mm – the pin spacing is 1.27mm. 

          5.5     The total measured vertical length of all the pads included =  4.40mm.
             
          5.6     The total measured internal horizontal width between the pads = 3.00mm.

          5.7     Total measured external width between the pads included = 6.92mm.

6.      If we measure the pads with the Vernier caliper or Measure distance between two 

         points tool the horizontal width of a pad is 2.00mm and the vertical height of a pad

          is 0.6mm.

7.      If we get the datasheet from Linear Technology on the LTC1624 we see the LTC1624

          is a High-Efficiency SO-8 N-Channel Switching Regulator Controller as shown 

          in figure 1.10B below:

Fig. 1.10B: LTC1624: High-Efficiency Switching Regulator Controller Datasheet

8.     From the datasheet, the package description of the LTC1624 is as shown in 

        figure 1.10C below.

Fig. 1.10C: Package of LTC1624 Switching Regulator Controller.

8.     It is described as having an S8 Package 8-Lead Plastic Small Outline.

9.      In the datasheet, the body width is given as between (3.810 – 3.988)mm, compared

         with 3.9mm given in KiCad footprint.

10.    In the datasheet, the body length is given between (4.801 – 5.004)mm, compared 

         with 4.9mm given in KiCad footprint.

11.    In the datasheet, the pin spacing is given as 1.270mm typically, compared with 

         1.27mm given in the KiCad footprint.

12.    In the datasheet, the pin width is given as between (0.355 – 0.483)mm, compared 

         in the KiCad footprint, this is measured in that the pad has a width or vertical 

         height of 0.6mm. This, of course, acceptable as the pads must be wider than the 

         pin width. 

13.    In the datasheet, the pin length is given as between (0.406 – 1.270)mm, compared 

         in the KiCad footprint, this is measured in that the pad has a horizontal width 

         or length of 2.00mm. This, of course, acceptable as the pads must be longer 

         than the pin length.  

14.     In the datasheet, if three-pin spacings as given in the datasheet is taken as 

          1.27mm x 3 = 3.81mm plus the width of a pin as given as 0.483mm 

          which is 3.81mm + 0.483mm= 4.293mm. 

         That can be compared with the total vertical length of all the pads included =  

         4.40mm measured in the KiCad footprint. 

15.     In the datasheet, the total internal width between the pads is estimated as  

          a worst case shortest distance is 5.791mm - (2x1.270mm =2.54mm) = 3.251mm. 

          This should be compared with the KiCad footprint where the total internal width 

          between the pads is measured at 3.00mm.

16.     In the datasheet, the total external width between the pads is given as (5.791 - 

          6.197)mm when compared with the KiCad footprint is measured at 6.92mm.

17.     It, therefore, seems this footprint as allocated by KiCad is fine.

Download Footprint From Ultra Librarian And Check Footprint

You can watch this video on YouTube cab licking on Download Footprint From Ultra 

Librarian And Check Footprint.

Footprint for the MOSFET N-CH 30V 10.9A 8-SOIC SI4128DY-T1-GE3

Create a KiCad Footprint Library File

1.     Go to the Digi-Key website for the SI4128-T1-GE3 by clicking on

        Digi-Key Si4128DY

2.     You will see the description of the MOSFET N-CH 30V 10.9A 8-SOIC 

        SI4128DY-T1-GE3 as shown in figure 1.10D below:

Fig. 1.10D: Information On the SI4128DY-T1-GE3 as It Appears on the Digikey Website.

3.     As you can see, they suggest we download the footprint or EDA/CAD Models from 

        Ultra Librarian.

4.      First, open a library file where you store your KiCad footprints.

5.      In KiCad the footprint library files have a .pretty extension.

6.       I made a library file, which I called “KICADFootprints” where I store all my 

          KiCad footprints. 

7.      I left out the .pretty extension.

8.      I suggest you create your file with a short path like right on your C drive.

9.       I suggest you call it something like: “MyKiCadFootprints.pretty”.

10.     The KiCad footprints themselves have a .kicad_mod extension.

11.     The KiCad footprints (files with a .kicad_mod file extension) themselves are 

           grouped in the particular library (file with .pretty extension). 

Create a Path to Your KiCad Library File

1.     You have to tell KiCad where your new footprints, the footprints that you add are.

2.     To do this you must create a path to your new library file.

3.     The library file is the file with the .pretty extension.

4.    You add the path in the Footprint Libraries window.

5.     To get there open the Assign Footprints window.

6.      Now click on Preferences then Manage Footprint Libraries… .

7.      Open the Footprint Libraries window.

8.      I generally put my footprints in the Global Libraries.

9.      Click on the envelope icon at the bottom or Add existing library to table.

10.     Navigate to where your KiCad footprint library file is. 

11.     In my case, it is C:/KICADFootprints.

12.     After you have finished it should be as in figure 1.10E below:

Fig. 1.10E: KICADFootprints Library Added

Download Footprint for MOSFET N-CH 30V 10.9A 8-SOIC SI4128DY-T1-GE3

1.       Go to Ultra Librarian by clicking on Ultra Librarian

2.       Type in "SI4128" in the search box.

3.        Download the footprint for SI4128DY-T1-GE3.

4.        Extract the SI4128DY-T1-GE3.kicad_mod footprint to your KiCad 

            footprint library file. 

5.        As mentioned in my case it is KICADFootprints.

5.        In the Assign Footprints window choose your KiCad footprint library.

6.        Right-click on the SI4128-Ti_GE3 Ultra Librarian file and select View Footprint.

7.       The footprint shown below in figure 1.10F should appear:

Fig. 1.10F: Ultra Librarian Si4128-T1-GE3 Footprint

8.       You can download the Vishay Siliconix datasheet by clicking on datasheet

9.      The package information of the SI4128 is shown in figure 1.10G below:

Fig. 1.10G: Package Information of SI4128

10.      From the package information, we can see the following applies:

           10.1      It is SOIC a Small Outline Integrated Circuit which is a surface- 

                        mounted integrated circuit (IC).

           10.2      It has 8 pins.

           10.3      The IC has a horizontal body width E of 3.8 - 4.00 mm. The 

                        measured width in the Footprint Editor is 4.0mm.

           10.4      The IC has a vertical length D of 4.9 - 5.0 mm. The 

                        measured vertical length in the Footprint Editor is 4.96mm.

           10.5      The IC has a horizontal body width of 3.9mm and a 

                        vertical length of 4.9mm and can, therefore, be written as 3.9x4.9mm

           10.6      The pin spacing is given as e = 1.27mm. The measured pin spacing in

                         the Footprint Editor is 1.27mm.

          10.7       The pin spacing is 1.27mm 

11.     According to KiCad, the footprint naming conventions are shown in figure 1.10H

         should be used for naming SMD IC package footprints.

Fig. 1,10H: Kicad naming conventions for surface mount integrated circuits.

12.      Taking into account the dimensions we already have and the KiCad 

           naming convention the footprint should be named as: 

           SOIC-8_3.9x4.9mm_P1.27mm

Vishay Recommended Minimum Pads

1.       According to the Vishay Siliconix datasheet the following minimum 
       
          pads are recommended for the Si4128DY N-Channel 30-V (D-S) MOSFET and 

          are shown in figure 1.10I below: 

Fig. 1.10I: Footprint for Si4128 as Recommended by Vishay.

2.       Comparing the Vishay datasheet recommendation with the Vernier caliper tool or 

          Measure distance between two points measurements

         we can measure as follows:

          2.1       Horizontal  pad width (as in KiCad footprint)

                       2.1.1      Vishay datasheet recommendation is 1.194mm.

                       2.1.2      Pad in footprint measured = 1.66mm.

                       2.1.3     This is acceptable as it means the pad in the footprint is a bit wider.

                    

          2.2       Vertical  pad height (as in KiCad footprint) 

                      2.2.1    Vishay datasheet recommendation of 0.559mm.

                      2.2.2     Vertical pad length in footprint measured = 0.55mm.

                      2.2.3     This is acceptable as they are virtually the same.


           2.3       External overall horizontal width of all pads included (as in KiCad footprint)

                       2.3.1    Vishay datasheet recommendation of 6.248mm. 

                       2.3.2    External width measured in footprint = 6.93mm. 
                     
                       2.3.3    This is acceptable as the footprint is a bit wider than the
      
                                   recommendation. Remember the footprint has longer horizontal

                                   width.

            2.4      The internal overall horizontal width between the pads 

                      (as in KiCad footprint)

                       2.4.1     Vishay datasheet recommendation of 3.861mm.

                       2.4.2     Measured in the footprint itself = 3.60mm.  

                       2.4.3    This is acceptable as it simply means that the pads in the footprint

                                     are slightly closer to each other when measured horizontally.
                       

            2.5       External overall vertical  length of all pads included (as in KiCad footprint)

                       2.5.1      Vishay datasheet recommendation of 4.369mm.

                       2.5.2      Measured overall external length = 4.37mm.

                       2.5.3      This is acceptable as it is virtually the same.


3.      We can, therefore, say the footprint we downloaded from Ultra Librarian is fine.

Assign Footprint to MOSFET Transistor

1.      Open the Assign Footprints window.

2.      In the middle window Symbol: Footprint Assignments click on 

        15   U2 -    SI4128DY-T1-GE3: 

3.     In the Filtered Footprints window on the right, double left click on 

        SI4128-T1-GE3.

4.    The final footprint assignments should look as shown in figure 1.10H shown below.

Fig. 1.10H: Final Footprint Assignments

5.      Click Apply, Save Schematic & Continue.

6.      Click OK.

Tutorial 1.9: Assign Footprints to Resistors

The Circuits

1.     Our circuit Eeschema circuit looks like shown in figure 1.9A below:

Fig. 1.9A: Eeschema Circuit

2.     The LTspice XVll simulation circuit of the Eeschema circuit is shown in figure 1.9B

         below:

Fig. 1.9B: LTspice Simulation Circuit.

Calculate The Power Consumption In The Resistors

Watch this video on Youtube Calculate Power in Resistors Using LTspice

Power Consumption in Resistor (10 R1 - 6.8k) in Eeschema

1.     The power plot or light blue trace of R1 - 6.8kohm in Eeschema (R3 in 

        LTspice circuit) is shown in figure 1.9C below:

Fig. 1.9C: Power Graph in R1

2.      The power in R1 in Eeschema starts at 0 then goes up to  23uW after 0.05ms. 

3.       The power thereafter remains at zero and then at 0.25ms goes briefly to 6uW.

4.       The average power in R1 as calculated by LTspce in R1 over a period of 1ms is 

          403.59nW.

5.       The point is the power consumption in R1- 6.8kohm in Eeschema  

          (R3 in LTspice circuit) is very low so a normal 250mW resistor should be more

          than adequate. 

Power Consumption in (11 R2 - 35.7k) in Eeschema

1.     The power plot or light blue trace of R2 - 35k7 ohm in Eeschema (R2 in 

        LTspice circuit) is shown in figure 1.9D below:

Fig. 1.9D: Power Graph in R2

2.      From the light blue trace, it can be seen that the power consumption in R2 starts at 0.

3.      After 0.1ms it starts to rise until at about 0.25ms it reaches about 130uW.

4.      After a slight overshoot, it settles at 130uW. 

5.      The average power in R2 as calculated by LTspce in R2 over a period of 1ms is 

          104.37uW.

5.      A normal 250mW resistor should be more than adequate. 

Power Consumption in R3 - 20K ohm in Eeschema

1.     The power plot or purple trace of R3 - 20k ohm in Eeschema (R1 in 

        LTspice circuit) is shown in figure 1.9E below:

Fig. 1.9E: Power Graph in R3

2.      From the purple trace or plot, it can be seen that the power consumption in 

          R3 starts at 0.

3.      After 0.1ms it starts to rise until at about 0.25 ms it reaches about 73 uW.

4.      After a slight overshoot, it settles at roundabout 71uW.

5.       The average power in R3 as calculated by LTspce in R3 over a period of 1ms is 

          58.477uW.

6.       A normal standard 250mW resistor should be more than adequate. 

Power Consumption in R4 - 0.033 ohm in Eeschema

1.     The power plot or light blue trace of R4 - 0.033 ohm in Eeschema (R4 in 


        LTspice circuit) is shown in figure 1.9E below:

Fig. 1.9E Power Trace Plot in Resistor R4 0.033 Ohm

2.      From the red trace or plot, it can be seen that the power consumption in R4 

          starts at approximately 0.08ms at a peak of 0.9W

3.      After 0.1ms it starts to rise until at about 0.15 ms it reaches a peak of about 1.4W.

4.      It then drops down to a peak of about 1.3W after 0.25ms.

5.      After that, it collapses completely to 0W at 0.28ms.

6.      It then wakes up at 0.29 ms raises briefly to perhaps a peak of 0.3W.

7.      After about 0.35ms it never exceeds a peak of 0.2W.

8.       We can thus say after 0.28ms or 280us a normal standard 250 mW resistor should 

          be more than adequate. 

9.      The question is what about the time period between 0.1 ms (100us) and 

         0.28ms   280us?   

10.     We can ask LTspice to expand the graph and then we get the power consumption in 

         R4 in the period of 0.1 ms (100us) and 0.28ms (280us) shown in figure 1.9F below.

Fig. 1.9F: Power Consumption in R4 during 60us - 280 us.

11.       We can ask LTspice to calculate the average power consumption which shown 

           in the square in the upper left and is estimated at 95.38mW.  

12.     Once again a normal standard 250 mW resistor should be able to handle this.

Current in R4 0.033 Ohm Resistor

1.     We may as well look at the current in R4 the 0.033 Ohm resistor.

2.     The Current plot in the R4 resistor is shown in figure 1.9G below:

Fig. 1.9G: Current in R4 0.33 Ohm Resistor

3.     We can say that the current in R4 peaks at 6.6A in the first 0.25 ms and after about 0.2

    

        ms peaks at 2.4A.

4.     Current in R4 in the time period between 80uS and 280uS is shown in figure 1.9H

        below:

Fig. 1.9H: Current in R4 between 100uS and 280uS.

5.     Over the time period of (80-280)us we can say the average current is 736.35mA and

    

        root mean square value is 1.7822A.  

6.     Current in R4 after 0.21 ms is shown in figure 1.9I below:

Fig. 1.9I: Current in R4 after 0.28ms

7.     The current for the time period between 210us to 1ms is on average 281.04mA and 

        the RMS value is 671.75mA. 

8.     The current plays an important role in our choice of copper thickness. 

KiCad Resistor Footprint Format

1.      Footprints are grouped into libraries (directories with .pretty extension) based on 

         their primary function. 

2.       Each footprint is a .kicad_mod file (stored within a .pretty directory).

Axial Resistors

1.      The format for axial resistors is:

          R_Axial_L[Length]_D[Diameter]_P[Pitch]_[Modifiers]_[Orientation]_[Options] 

2.       Where:

           2.1.       L - Length - Resistor body length.

           2.2.       D - Diameter - Body diameter.

           2.3.        P - Pitch - Lead spacing.

            2.4.       Modifiers - Modifiers to footprint specifications (Optional).

            2.5.       Orientation - Resistor orientation (Vertical / Horizontal) (Optional).

            2.6.        Options - Extra footprint options (Optional).

3.        Example: R_Axial_L3.6mm_D1.6mm_P5.08mm_Horizontal 

4.        This means the leads of the resistor are axial, the body length of the resistor is

            3.6 mm, the diameter of the resistor is 1.6 mm, the spacing between the leads are 

            5,08 mm and the footprint is for a horizontally mounted resistor.

Choose Resistor Footprint and Assign Resistor Footprint to Resistors

You can watch this video on YouTube by clicking on choose and assign resistor footprint.

Choose Resistors for R1, R2 and R3

1.     A good choice for resistors would be the Vishay MBA/SMA 0204 series.

2.     The datasheet can be found at Vishay

3.      Particulars of the resistors appear in figure 1.9J below:

Fig. 1.9J: Particulars of Vishay Resistors

4.      The technical specifications are shown in figure 1.9K below:

Fig. 1.9L: Technical Specification of Resistors

5.    From the above, we see that MBA/SMA 0204 has a DIN size of 0204, resistance range

       0,22 Ohm to 10 Mega Ohm and a rated dissipation of 0.4 W.

6.    The resistor dimensions are shown in figure 1.9L below:

Fig. 1.9L: Resistor Dimensions

 7.     The MBA/SMA 0204 resistors have:

         7.1     L = 3.0 mm.

         7.2     D = 1.6 mm.

         7.3     M (or P in KiCad) = 5.0 mm.

8.      Re-written in KiCad format it would be: R_Axial_L3.6mm_D1.6mm_P5.00mm.

Assign Footprints to Resistors R1, R2 and R3

1.     In the Assign Footprints window in the middle window Symbol: Footprint  

         Assignments click on 10   R1 -     6.8k :.

2.      In the left column under Footprint Libraries click on Resistor_THT.

3.      In the right column under Filtered Footprints double click on 

        Resistor_THT:R_Axial_DIN0204_L3.6mm_D1.6mm_P5.08_Horizontal 

4.      Click on View selected footprint icon.

5.      It is the icon with the vertical IC with red legs and magnifying glass in the lower 

          right corner.

6.       The footprint should be as shown in figure 1.9M below:

Fig. 1.9M: Resistor Footprint

7.       Click on the 3D Display icon.

8.     It is the icon with a square dark grey component mounted in a green PCB board  

          viewed from the side.

9.      It is shown in figure 1.9N below:

Fig. 1.9N: 3D View of Resistor

10.     Click on Apply, Save Schematic & Continue. 

11.      Repeat for all the other resistors up and until 12   R3 -      20k:. 

12.      After all the resistors have been assigned footprints it should like in the 

           Assign Footprints window as  shown figure 1.9O below:

Fig. 1.9O: Footprint Assignments to R1, R2 and R3

13.      Click Apply, Save Schematic & Continue.

14.      Click OK.

Choose Resistor and Design Resistor and Assign Footprint

You can watch this video on YouTube by clicking on design resistor footprint and 

assign resistor footprint.

Choose Resistor for Symbol 13 Resistor R4 0.033 Ohm 

1.      I found this SBL4R033J current sense resistor of 0.033 ohm on 

         the element 14 website.

2.      Particulars of the resistors appear in figure 1.9P below:

Fig. 1.9P: 0,033 Ohm Resistor on element 14 website

3.    It costs $2.15 for one.

4.    For the technical datasheet of the resistor click on SBL4R033J 

5.    The particulars of Tyco Electronic low ohmic current sense resistors are shown in 

        figure 1.9Q.

Fig. 1.9Q: Low Ohmic Current Sense Resistors

6.       The dimensions for the low ohmic resistors are shown in figure 1.9R below:

Fig. 1.9Q Dimensions of Low Ohmic Current Sense Resistors

Design Footprint For Resistor  R4 0.033 Ohm

1.     Open the Footprint Editor.

2.     Click File and select New Footprint ...

3.     Type in the name:

        THT_R_Axial_L18mm_D6.4mm_P40.00_Horizontal.

4.     Click OK.

5.     Click File and select Save.

6.     Choose in my case the KICADFootprints library.

Draw Pad1

1.    Select Add pad.

2.    Set the pad properties as in figure 1.9R below:

Fig. 1.9R: Properties of Pad1 of Resistor Footprint

3.   Click OK.

Draw Pad2

1.    Select Add pad.

2.    Set the pad properties as in figure 1.9R below:

Fig. 1.9R: Properties of Pad 2 of Resistor

3.   Click OK.

Draw The Front Fabrication Layer of The Footprint

The fabrication layers are used to display the simplified mechanical outline of

components on the PCB. The recommended line width is 0.1mm.

Draw The Top Horizontal Line of Mechanical Outline

1.     In the Footprint Editor click Add graphic line.

2.      Draw a horizontal line. 

3.      Set the properties of the line as in figure 1.9S below:

Fig. 1.9S: Fabrication Layer Top Horizontal Line

4. Click OK.

Draw The Bottom Horizontal Line of Mechanical Outline

1.     In the Footprint Editor click Add graphic line.

2.      Draw a horizontal line opposite and below the top horizontal line. 

3.      Set the properties of the line as in figure 1.9T below:

Fig. 1.9T: Fabrication Layer Bottom Horizontal Line

4. Click OK.

Draw The Left Vertical Line of Mechanical Outline

1.      In the Footprint Editor click Add graphic line.

2.      Draw a vertical line to the left and between the top and bottom horizontal lines. 

3.      Set the properties of the line as in figure 1.9U below:

Fig. 1.9U: Fabrication Layer Left Vertical Line

4.     Click OK.

Draw The Right Vertical Line of Mechanical Outline

1.      In the Footprint Editor click Add graphic line.

2.      Draw a vertical line to the left and between the pad and bottom horizontal lines. 

3.      Set the properties of the line as in figure 1.9V below:

Fig. 1.9V: Fabrication Layer Right Vertical Line

4.      Click OK.

Draw Left Horizontal Line Pad To Body (Left Terminal Outline)

1.      In the Footprint Editor click Add graphic line.

2.      Draw a vertical line to the left and between pad 1 and body vertical line. 

3.      Set the properties of the line as in figure 1.9W below:

Fig. 1.9W: Fabrication Layer Left Terminal Outline

4.     Click OK.

Draw Right Horizontal Line Pad To Body (Right Terminal Outline)

1.      In the Footprint Editor click Add graphic line.

2.      Draw a horizontal line to the right and between pad 2 and body vertical line. 

3.      Set the properties of the line as in figure 1.9X below:

Fig. 1.9X: Fabrication Layer Right Terminal Outline

4.      Click OK.

REF** Text On Fabrication Layer

1.      In the Footprint Editor click Add Text.

2.      Type " %R"  in the Text box of the Footprint Text Properties window. 

3.      In the Layer drop-down list choose F.Fab.

4.      The Footprint Text Properties should be as in figure 1.9Y below:

Fig. 1.9Y: Footprint Text Properties of REF**

5.     Click OK.

Silkscreen Layer

1.       The silkscreen is printed to the external surface of a PCB to aid in 

          the component identification and orientation. 

2.      This layer contains the component RefDes (reference designator) to 

          locate components on the board after assembly. 

3.       Silkscreen line width should nominally be 0.12 mm.

Draw Horizontal Lines

1.      In the Footprint Editor click Add graphic line.

2.      Draw the top horizontal line just above the top horizontal line in the fabrication layer. 

3.      Set the properties of the line as in figure 1.9Z below:

Fig. 1.9Z: Silkscreen Layer Top Horizontal Line

4.     Click OK. 

5.     Draw the bottom horizontal line in the same manner except set Start point Y:

        and End point Y: at 3,3.

Draw Vertical Lines

1.      In the Footprint Editor click Add graphic line.

2.      Draw the left vertical line between the horizontal lines on the left. 

3.      Set the properties of the line as in figure 1.9AA below:

Fig. 1.9AA: Left Vertical Line in Silkscreen Layer

4.      Click OK.


5.      Draw the right vertical line on the right, between the horizontal lines.

6.     The only difference is that Start point X: and End point X: is at 9,1.

Draw The Horizontal Lines Pad To Body

1.      In the Footprint Editor click Add graphic line.

2.      Draw the left horizontal line to the right and between pad 2 and the vertical line

         of the body. 

3.      Set the properties of the line as in figure 1.9BB below:

Fig. 1,9BB: Silkscreen Left Horizontal Line Pad To Body

4.     Click OK.

5.      Draw the right horizontal line on the right, between the vertical body line and pad 2.

6.     The only difference is that Start point X: is at 9,1 and End point X: is at 18,5.

REF** Text On Silkscreen Layer

1.      In the Footprint Editor click Add Text.

2.      Type " REF**"  in the Text box of the Footprint Text Properties window. 

3.      In the Layer drop-down list choose F.SilkS.

4.      The Footprint Text Properties should be as in figure 1.9CC below:      

Fig. 1.9CC: Silkscreen Layer REF**

5.      Click OK.

Courtyard Layer


1.    The component courtyard is defined as the smallest rectangular area that

       provides a minimum electrical and mechanical clearance around the combined

       component body and land pattern boundaries. 
      
2.    It is allowed to create a contoured courtyard area using a polygon instead of a

       simple rectangle. (IPC-7351C).

3.    Courtyard uses line width 0.05mm.

4.     All courtyard line elements are placed on grid of 0.01mm.

5.      Unless otherwise specified, clearance is 0.25mm.

6.      Connectors, Canned capacitors and crystals should have a clearance of 0.5mm.

7.      BGA devices should have a clearance of 1.0mm.

8.      Kicad example of courtyard layer is shown in figure 1.9CCA below:

Fig. 1.9CCA: Kicad example of courtyard layer

9.      See Kicad Courtyard Layer Requirements.

Draw Horizontal Lines of Courtyard Layer

1.      In the Footprint Editor click Add graphic line.

2.      Draw the top horizontal line just above the top horizontal line in the fabrication layer. 

3.      As far as the total width of the courtyard is concerned, take: the pitch width along an

         axis  +  the radius of the pad.

4.     This gives us 20mm + 2.5mm/2 = 21.25mm.

5.     To this, we must add 0.25mm courtyard clearance = 21.25mm + 0.25mm = 21.50mm.

6.      However, let's make it 22mm.

7.      As far as the height is concerned we already have the top horizontal silkscreen

         line at 3.3mm.

8.     If we add 0.25mm for courtyard clearance then we have 3.3mm + 0.25mm 

        = 3.55mm.

9.      So let us make that then at 3.6mm.

10.    Set the properties of the line as in figure 1.9DD below:

Fig. 1.9DD: Horizontal Line of Courtyard

11.     Click OK.

5.       Now draw the bottom horizontal line on the courtyard layer.

5.      The only difference set Start point Y: and End point Y: at 3,5mm.

Draw Vertical Lines of Courtyard Layer

1.      In the Footprint Editor click Add graphic line.

2.      Draw the left vertical line between the horizontal lines on the left. 


3.      Set the properties of the line as in figure 1.9EE below:

Fig. 1.9EE: Vertical Line of Courtyard

4.     Click OK.

5.     Draw the right vertical line between the horizontal lines on the right.

6.     The only difference set Start point X: and End point X: to 22.

7.     Finally, the footprint for symbol 13, resistor R4 of 0.033 Ohm is as shown in

        figure 1.9FF:

Fig. 1.9FF: Footprint for 0.033 Ohm Resistor

8.     Assign footprint to 13. R4 0,033 ohm as is shown in figure 1.9GG below:

Fig. 1.9GG: Footprint Assigned To 13 R4 0.033 Ohm Resistor

Let me know if you notice any mistakes.

 
Previous: Tutorial 1.8: Create Footprint for Inductor 


Next: Tutorial 1.10: Assign Footprints to Switching Regulator and MOSFET Transistor