kicad-design-for-manufacture

### Module positions - created on 04/10/17 16:52:49 ###
### Printed by Pcbnew version kicad 4.0.5
## Unit = mm, Angle = deg.
## Side : top
# Ref     Val                 Package                                                  PosX       PosY       Rot  Side
C1        1u                  C_0603                                               122.5000   -90.5000   90.0000  top
C2        10n                 C_0603                                               124.6505   -86.0425  270.0000  top
C3        1u                  C_0603                                               127.3500   -98.7500   90.0000  top
C4        47u                 C_1210                                               121.0000   -81.5000   90.0000  top
C5        10u                 C_0805                                               123.8250   -82.0000   90.0000  top
D1        LED_ALT             LED_0603                                             132.2070   -80.2640  180.0000  top
L1        Ferrite_Bead_Small  R_0603                                               120.5000   -90.6310   90.0000  top
P1        CONN_01X06          Pin_Header_Straight_1x06_Pitch2.54mm_SMD_Pin1Right   114.0675   -95.4630    0.0000  top
R1        1k                  R_0603                                               124.7140   -88.9000  270.0000  top
R2        1k                  R_0603                                               128.9050   -80.2640    0.0000  top
U1        LD3985M33R          SOT-23-5                                             121.7150   -86.5670   90.0000  top
U2        4050                SO-16-N                                              122.0500  -101.8500  270.0000  top
## End

1. Manually look up the dimensions of the device itself, as described above using the Panasonic data sheet.
   
   
2. Manually enter these into Library Expert Lite and click various buttons.  This will produce a footprint inside the program, which can be viewed.
   
   
3. One any necessary adjustments are made, this can be exported as a KiCad.mod file.  In principle it can be saved in a library, but I had difficulty getting KiCad's Footprint Editor to recognise the new arrival, so I exported it to a separate directory, and imported that file into Footprint Editor.
   
   
4. There are a number of things to change and clean up, such as making SMT pads rounded rectangles.
   
   
5. Then the footprint can be saved into a library.

1. Click the "Surface Mount" button at the top.
   
   
2. From the list at the left, select "Chip" and click the "OK" button.  This results in:
   
   
   
   
   
3. Click the "Nom/Tol" radio button, enter the device dimensions, four values from the Panasonic data sheet into the "Nom" column, for rows A, D, E and L:
   
     A = 0.60 = height (Z) of the resistor, from the t column of the data sheet.
   
     D = 2.00 = length (X) of the resistor, from the L column.
   
     E = 1.25 = width (Y) of the resistor, from the W column.
   
     L = 0.40 = length (X) of the electrical contact, from the b column.
   
   Then for those rows in the "- Tol" column, enter 0.  In the "Family" pull-down list, select "Resistor".  The result, for me, appeared as:
   
   
   
   
4. Click the "OK" button.  This will generate an updated graphic display of the footprint, and seems to be necessary if we want to change some items in other tabs and sub-tabs.
   
   
5. This next step can be omitted - this is to show where we choose the density level, which is how compact the software makes our footprint. Click on the Terminal tab and then its Density Level sub-tab.  The default is Nominal (N) which is what I want.  The other options are Most and Least, and the actual values these presets control can be fine-tuned.
   
   
6. This next step can be omitted - this is to show where we could choose the height and line-thickness of the silkscreen component legend text and I think the lines on this layer which depict the outline of the component. (I later decided to set the text size and line widths with =a direct edit of the footprint file exported by Library Export Lite, rather than relying on Library Expert Lite's settings - each of which has to be manually set again for every fresh footprint which is generated.) Click on the Drafting tab and then its Legend sub-tab.  The defaults are presumably from IPC-7531:  Outline Width from 0.12 to 0.10 and  Ref. Des. Height from 1.20 to 1.00.
   
   The sub-tab Assembly has similar settings for a rectangle which will be on KiCad's F.Fab layer, for an assembly drawing which shows the outline of the resistor.
   
   The sub-tab Courtyard concerns a rectangle (or something more complex for larger, more complex-shaped components) which will be drawn on KiCad's F.CrtYd Courtyard layer, as well as an optional, default-on, cross-hair with circle ("target") at the X = 0, Y = 0 position (AKA the centroid).  I didn't change anything.  I am not sure that "Expand Courtyard to Include Legend" should be ticked, but it made no difference in this instance.
   
   The sub-tab Component has settings for a set of thin lines which will be on KiCad's Dwgs.User layer.  The lines create three rectangles in this example, one for the outline of the whole resistor and one each for each electrical terminal (contact).
   
   Now select the Components tab again, with its Dimensions sub-tab, as depicted above.
   
   
7. Click the "OK" button.
   
   
8. If all is well, there will be no error message and the main display window will show the footprint, with no grid or scale (but the cursor can be used to show coordinates) and without some text items which will appear in the exported KiCad footprint:
   
   
   
   The pull-down list at the top left of this section of the window enables us to select something about the order the layers are drawn, but I don't yet understand it.  The icon to its left, with four coloured bars, opens up a side-bar where we can choose the colours of the layers and whether they are on or off.  See my cheatsheet0 image below.  The above image results from the default layer on-and-off settings and with the default colours.
   
   
9. Click the spanner icon at the right of the toolbar over the display window.  (If you get an error such as one announcing an unhandled exception regarding "Name cannot begin with the '3' character, hexadecimal value 0x33. Line 3, position 321." then this may be due to a line in a config file in the program's installation directory, which for me: C:\Program Files (x86)\PCB Libraries\Library Expert Lite 2017\FPXFormatPreferences.xml .  The program writes a keyword "3D_TOP" in the KiCad exporter information, which it later objects to.  This bug was fixed in the release of 2017-19 available after about 2017-10-25, so you should be able to avoid this by deleting the file or at least editing the keyword to "THREED_TOP" and installing the bug-fixed version.)
   
   
10. Select the "Translator" as "KiCad".  I also selected "Set as Default Format".
    
    
11. Select the output directory.  Then the dialogue box should look like this.  The Top and Bottom layer names can be altered if desired.
    
    
    
    
12. Press the "Create" button.  For me, this causes a file RESC200X125X60L40N.kicad_mod  to be written to the output directory. This can be imported into Footprint Editor.
    

1. GRID  Right click to set the X and Y dimensions, but I don't see any grid.
   
   
2. BG  Background colour.
   
   
3. HLT  Highlight colour.  The cursor, together with potentially the control key can be used to select one or more things, but I could only get it to work with pads at first, until I discovered that by right clicking in an empty area of the display window, I can select which of Pins, Shapes, Lines and Labels are available for selection.  Once an item is selected, right-click brings up a properties box.
   

(module RESC200X125X60L40N (layer F.Cu) (tedit 59EB4182)

  (descr "Resistor, Chip; 2.00 mm L X 1.25 mm W X 0.60 mm H body")

  (attr smd)

  (fp_text reference REF** (at 0 0) (layer F.Fab)

    (effects (font (size 1.2 1.2) (thickness 0.12)))

  )

  (fp_text value VAL** (at 0 0) (layer F.Fab)

    (effects (font (size 1.2 1.2) (thickness 0.12)))

  )

  (fp_text user %R (at 0 0) (layer F.SilkS)

    (effects (font (size 0.77 0.77) (thickness 0.08)))

  )

  (fp_line (start -0.6 -0.625) (end -0.6 0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start -0.6 0.625) (end -1 0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start -1 0.625) (end -1 -0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start -1 -0.625) (end -0.6 -0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start 0.6 0.625) (end 0.6 -0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start 0.6 -0.625) (end 1 -0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start 1 -0.625) (end 1 0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start 1 0.625) (end 0.6 0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start -1 0.625) (end -1 -0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start -1 -0.625) (end 1 -0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start 1 -0.625) (end 1 0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start 1 0.625) (end -1 0.625) (layer Dwgs.User) (width 0.025))

  (fp_line (start -1 0.63) (end -1 -0.63) (layer F.Fab) (width 0.12))

  (fp_line (start -1 -0.63) (end 1 -0.63) (layer F.Fab) (width 0.12))

  (fp_line (start 1 -0.63) (end 1 0.63) (layer F.Fab) (width 0.12))

  (fp_line (start 1 0.63) (end -1 0.63) (layer F.Fab) (width 0.12))

  (fp_line (start -0.365 -0.63) (end 0.365 -0.63) (layer F.SilkS) (width 0.12))

  (fp_line (start -0.365 0.63) (end 0.365 0.63) (layer F.SilkS) (width 0.12))

  (fp_line (start -1.56 0.88) (end -1.56 -0.88) (layer F.CrtYd) (width 0.05))

  (fp_line (start -1.56 -0.88) (end 1.56 -0.88) (layer F.CrtYd) (width 0.05))

  (fp_line (start 1.56 -0.88) (end 1.56 0.88) (layer F.CrtYd) (width 0.05))

  (fp_line (start 1.56 0.88) (end -1.56 0.88) (layer F.CrtYd) (width 0.05))

  (fp_circle (center 0 0) (end 0 0.25) (layer F.CrtYd) (width 0.05))

  (fp_line (start 0.35 0) (end -0.35 0) (layer F.CrtYd) (width 0.05))

  (fp_line (start 0 -0.35) (end 0 0.35) (layer F.CrtYd) (width 0.05))

  (pad 1 smd roundrect (at -0.95 0) (size 0.81 1.36) (layers F.Cu F.Paste F.Mask)(roundrect_rratio 0.25))

  (pad 2 smd roundrect (at 0.95 0) (size 0.81 1.36) (layers F.Cu F.Paste F.Mask)(roundrect_rratio 0.25))

)

Text items in the footprint file which is ready to be imported into Footprint Editor

  (fp_text reference REF** (at 0 0) (layer F.Fab)

    (effects (font (size 1.2 1.2) (thickness 0.12)))

  )

  (fp_text value VAL** (at 0 0) (layer F.Fab)

    (effects (font (size 1.2 1.2) (thickness 0.12)))

  )

  (fp_text user %R (at 0 0) (layer F.SilkS)

    (effects (font (size 0.77 0.77) (thickness 0.08)))

  )

  (fp_text user "ABC %R XYZ %V POQ" (at 0 0) (layer F.SilkS)

    (effects (font (size 0.77 0.77) (thickness 0.08)))

  )

1. We can use %R and %V as we desire in fp_text items of type user to display the reference and value of this instance of the footprint in a PCB (this component in a PCB).
   
   
2. A particular instance of a footprint in a PCB design (a particular component) has a reference, and a single fp_text item of type reference which causes this reference text to be displayed on a particular layer.  Editing the text on that layer (as opposed to formally changing the reference in the Footprint Properties dialogue box) DOES change the reference. 
   
   So the fp_text item of type reference creates a visible and editable piece of text on exactly one layer.  That layer can be changed.  That text on that layer always appears as whatever the reference text of the footprint is, and editing that layer's text changes the reference.
   
   The KLC specifies that this fp_text item of type reference be for the F.SilkS layer.  As far as I know, in KiCad library footprints, the text given for this item is usually REF** - but this is just an arbitrary placeholder to provide something for Footprint Editor to display.   (It is also used as the reference text for the instance of a footprint which has been manually placed, but manual placement of footprints is not a normal part of the KiCad approach to PCB design.)
   
   I think this KLC specification is compatible with my approach.  For this to be the case, I would have to accept that if there was to be any text printed on the PCB via the F.SilkS layer directly as part of the instance of this footprint on the PCB (this component) then that text will be precisely the reference of this instance. 
   
   I can always hide this and add a separate text item if I want something else to appear instead, but this will not be part of the instance - it will just be some text I place manually in the PCB design on the F.SilkS layer. This should be fine.
   
   
3. Likewise, each instance of a footprint in a PCB design has a value, which is directly linked to a single fp_text item of type value which causes this value text to be displayed on a particular layer.
   
   The KLC specifies that this fp_text item of type value be for the F.Fab layer.  As far as I know, in KiCad library footprints, the text given for this item is usually the same as the footprint name - but this is just an arbitrary placeholder to provide something for Footprint Editor to display and to be the value of a newly manually placed instance of a footprint in a PCB design. 
   
   This KLC specification is NOT compatible with my approach. 
   
   I don't want the value on the F.Fab layer - I want the reference, so I create a separate fp_text item of type user for the F.Fab layer, and set its text to %R.  (Change A.)
   
   I want the value to be on the Eco1.User layer, and since this is the only layer on which the value will appear, I will change the fp_text item of type value so it is for the Eco1.User layer instead of the F.Fab layer. (Change B.) Therefore, if I edit this text on the  Eco1.User layer, it will change the value of this instance of the footprint.
   
   I also make a copy of the component outline graphics of F.Fab to Eco1.User.  (Change C.)

1. Those which adhere to the KLC rules.
   
   
2. Those which are produced by Library Expert Lite.
   
   
3. Modified versions of both kinds of files which suit my purposes and are ready to be imported into Footprint Editor, for visual review and possible further changes, before storing the results in the current library.
   

1. Implement changes 1, 2 and 3 above, as well as the new text sizes, by pasting my #blocktopaste in place of the three text items.
   
   
2. Manual edits to implement change 4: make a copy on the Eco1.User layer of all outline graphic items on the F.Fab layer.
   
   
3. Edit the rectangular pad lines as mentioned above to make them specify rounded rectangles.
   

PCB Library             Exported    I transform     Full set of KiCad          Used by: 
Expert layer            footprint   to make my      layers and what I          D = Me for PCB design  
                        file KiCad  library         use them for               M = Me for manual assembly
                        layer       footprint                                  P = PCB manufacture and test company
                                                                               A = Automated SMT assembly company    
                                                   x = not editable in 
                                                   Footprint editor    

                                              TS Footprints in library use this for
                                                 through hole / surface mount  

TOP Top                 F.Cu           -->    TS     F.Cu      Top & bottom copper     D    P  A
BOT Bottom              B.Cu           -->    T      B.Cu      tracks and pads.        D    P  A

                                               S     F.Adhes   Stick large SMT                 A
                                                     B.Adhes   components to PCB 
                                                              before reflow. 

PMT Paste Mask Top      F.Paste        -->     S     F.Paste   Solder paste stencil.           A
PMB Paste Mask Bottom   B.Paste                      B.Paste

LT  Legend Top          F.SilkS --------->    TS     F.SilkS                           D M  P  A  
LB  Legend Bottom       B.SilkS   \   /              B.SilkS                                                    
                                   \[2]  
SMT Solder Mask Top     F.Mask     |/  -->    TS     F.Mask    Top & bottom solder     D    P  
SMB Solder Mask Bottom  B.Mask     |   -->    T      B.Mask    mask.                   D    P                                                    
                                  /|  
OTL Body Outline }      Dwgs.User/ |   -->    TS  !x Dwgs.User Component and terminal  D       A?
TRM Terminals    }               | |                           outlines - fine lines. 
                                 ^ | 
                                 | v               x Cmts.User
                                 | |                                 
                                 | |   [3 & 4]--> !x Eco1.User Component outlines,     D M  
                                 | |  /       TS               in thicker lines with
                                 | | /                         Values text, to aid
                                 | |/                          hand assembly of SMT &
                                 | |                           TH parts on prototypes.  
                                 |/|             
                                 | |               x Eco2.User Routing AKA milling     D    P  A 
                                 | |                           lines and text.
                                 | |              
                                 | |               x Edge.Cuts                         D    P  A
                                 ^ | 
                                 | v               x Margin
                                 | |              
CY Courtyard (top)      F.CrtYd -|------->    TS     F.CrtYd   Courtyard of SMT &      D
                                 | |                           TH components to help 
                                 | |                           place them so the 
                                 ^ |                           areas they require do
                                 | |                           not overlap.
                                 |  \                        
CY Courtyard (bottom)   B.CrtYd  /  [1]              B.CrtYd
                                /     \           
OTL Body Outline  }     F.Fab --------------> TS     F.Fab     Component outlines,     D M     A
    Ref** + Val** }                                           in thicker lines with
                                                              RefDes text.  
                                                                                                            
                                                     B.Fab

   Key:   Grey = not used.   Bold red = Used especially by humans for planning.
 
          !x = Both Dwgs.User and Eco1.User layers are used in footprints in the footprint
               library, though this is probably not how KiCad was intended to be used, since
               Footprint Editor does not allow us to edit anything on those layers. 

          I am not using the adhesive layers, but I have shown T.Adhes as being used to show how
          someone else might use them.  I plan only SMT components on the front side.  Even if 
          an SMT or TH component was to be mounted on the back side, in the footprint library 
          it would be defined on the front side.  

          Note that in transforming a component to the back side, Pcbnew cannot be expected 
          to (and with a 2017-10-19 nightly and does not) do proper reflection of the Eco1.User
          layer, since this is envisaged as an overall documentation layer, not related to one 
          side or the other.  The plan of using Eco1.User for hand assembly of prototypes with 
          components on the back side is probably OK, since the designer will be doing this and 
          will understand that the contents of this layer are not reflected or otherwise 
          transformed for such components.  

          The lines created by PCB Library Expert on Dwgs.User for the outline of the component
          and its terminals ARE correctly reflected when Pcbnew switches the footprint to the 
          back.  However, there is no front and back version of this layer.  So with a PCB with 
          components on both sides, this layer will show these outlines of all components and
          their terminals in the one layer.            

(fp_text reference DJ1 (at -4.4852 3.3936) (layer F.SilkS)
  (effects (font (size 1 1) (thickness 0.15)) (justify left bottom))

(justify mirror)