how to create VQFN package???

Hi,

1. To create bullet shape pin, First create Shape as pin (file\new\select ''shape symbol'') and save it in ur library, then while creating pad stack, on regular pad option select shape and give the library path of the shape where u saved.

2. add shape as top etch for thermal pad, then use add connection to draw trace on the thermal shape and double click to drop via one by one, then delet the trace (clines)

3. 0.254mm + actual pad size = Nominal Solder mask size and maintain solder mask to solder mask minimum 0.1mm air gap.

Yellaa Pugallum Erivannuke,

Raam >>--)-->

Hi,

i used allegro15.7..when i draw the custom shape pad(bullet) .i choose shape-->filled pad -->

and then draw the pad but how to change it bullet shape 

if i choose shape--> composed shape means it is possible to change oblong shape

Hello,

I know you already got a previous response to your post but I would like to provide you some addition feedback.

1. You could simple create a shape symbol to represent the bullet shaped pin.  Draw two shapes on Etch/Top, one rectangular and one round, the join them together using Merge Shapes command (Shape > Merge Shapes..)  This shape is then referenced in the padstack.

2. I would recommend adding 9 thermal pins to your symbol representing the 9 individual paste apertures. This padstack will contain a top pad and top solder paste defined as 1.2mm SQ per solder paste size on the spec sheet. These pins will need to be defined on the schematic symbol and most likely be connected to GND. Create a square shape on Etch/Top and Package Geometry/Soldermask_top in the symbol and add thermal vias per the spec sheet.  Don't be concerned with shape to pin DRCs at the symbol level because once you place the component in a design the shape will automatically adapt/assign to the net name tied to the thermal pads.  One final note: Check with your PCB fabricator to ensure that the thermal vias are small enough to prevent the solderpaste from reflowing down the thermal via holes during assembly.

3. Speak to your PCB fabricator about the tolerance on the solder mask and also confirm that they will not have any issues with a solder mask web of .08mm between the pins of this device.  The web should not be an issue but it never hurts to confirm and ask for their feedback.

Hope this helps,
Mike Catrambone
Plexus Technology Group