learnpcbdesign

Here you can learn pcb footprint creation using cadence allegro

Footprint flow

• Padstack creation using pad design.
• pins placement.
• assembly outline
• silkscreen outline
• reference designator
• Draw  place bound top area
• Draw DFA bound top area
• Draw no probe top area

Let’s start  creating footprint using cadence allegro I am taking sot23 package for reference

Image 1

Image 2

Create one folder in your system name it as pcb library like–>D:\pcb library,Now we are going to  create pad in pad designer.

Open pad designer—>

Start—>all programs—>Cadence—>Release 16.3—>PCB Editor Utilities—>Pad designer

Image 3

Now we opened pad designer

Units : we can change units shown with red circle I want to create it in mm.

Drill/slot hole : we need smd pads  for our footprint so put drill diameter as ‘0’(zero)

Next go to layers

Image 4

• Select single layer mode
• Select begin layer
• Give pad dimensions in regular Pad area

Geometry–> Rectangle

Width——->0.7 (Given in land pattern)

Height——>1      (Given in land pattern)

• Now select slodermask_top 

Width—–> 0.7 (same as pad width)

Height—–>1     (same as pad height)

• Now select pastemask_Top 

Width—–> 0.7 (same as pad width)

Height—–>1     (same as pad height)

Image 5

Now we have created pad just go to file—>save as—-> browse library folder(created beginning of this process) save with name as ‘R0_7X1.pad’.

Now we are going to create this footprint in cadence allegro

Open PCB Editor go to windows—>all programs—>Cadence—>Release 16.3—>PCB Editor

Image 6

Select PCB Design XL then press ok.

Image 7

• we have opened Allegro PCB Design XL Now go to File–>New in that
• Drawing name ‘SOT23’ then click on browse and go to PCB Libraries folder click Open
• In drawing type select ‘Package symbol’
• Click ok

Now set Pad path and psm path go to setup—>user preference—>Paths—>Library—>set path for ‘padpath’ and ‘psmpath’ click on areas shown in red circles then select ‘PCB Libraries’ folder.

Image 8

Set units of your board to MM

• Go to ‘set up—>Design parameter editor’ in that change design units to Millimeter

Now we are going to place pins as shown in SOT23 land pattern

• Go to layout—>pins ‘or’ select Add pin icon on menu bar
• On the right we can see option tab in that give your pad name i.e. r0_7x1 

Shown in circles

Image 9

Lets place pins

• Type command as x -0.95  -1.2 (you can copy paste this command)
• If you Are unable to see placed pin just press F2 button(zoom fit) on your key board.
• We have placed pin no 1
• Type command x 0.95 -1.2 (you can copy paste this command)
• We have placed pin no 2
• Type command x 0 1.2 (you can copy paste this command)
• Now we have placed total 3 pins as shown in image.

Image 10

Draw Assembly outline

• Take component dimensions from data sheet that is 3.1 x 1.8(maximum values)
• On menu bar ‘Add—>Line’
• On right side go to options select class as package geometry and sub class as assembly top then set line width to 0.2
• Now enter command as “x 1.55 0.9”
• Next enter command as “ix -3.1”—> “iy -1.8” —> “ix 3.1” —>”iy 1.8”

Drawing silkscreen outline is same as assembly but in options select class as package geometry and subclass as silkscreen top.

Place bound outline

• let us take place bound outline same as assembly outline that is 3.1 X 1.8
• on menu bar ‘shape —>filled shape’
• On right side go to options select class as package geometry and sub class as place_bound_top
• Now enter command as “x 1.55 0.9”
• Next enter command as “ix -3.1”—> “iy -1.8” —> “ix 3.1” —>”iy 1.8”

Reference Designator

• On menu bar ‘add—>Text’
• In options select class as ref des and sub class as silkscreen_top
• Click outside of footprint enter text “*”
• Now go to options select sub class as assembly_top
• Click center of footprint enter text ” *”

Now you have created sot23 footprint if you any doubts or suggestions please leave a reply

We are offering online pcb layout training. interested people can contact us at gvsatish11@gmail.com