Pad

also see:
Test points
Via

General

A pad in TARGET 3001! is the solderable footprint of a component. A pad is a part of a package, thus an drawing element belonging to the layout.

You can reach this mode in PCB only...
by key [1] (the numeric character 'one' above the alphabetic characters of your keyboard) or
by "Place Pad" in menu "Elements" or
by the tool under the icon

Leave this mode...
by [ESC] or M12

How to place a pad

Place a free pad by pressing M1 or [Return] at the desired position. Press [o] (options) for pad settings. The ultimate pad used for a package please place by [Return] or [Esc].

Important note: Set the grid to a reasonable value and jump from grid to grid by the use of the "arrow" keys on your keyboard. Place a pad by the key [1] to a desired grid controled point. In Place Pads mode, it is always possible to edit the number and the form of the pins by pressing M11 or [o]:

These free pads are normally used only for the definition of new packages to be saved to the libraries. Subsequential pad numbers are automatically incremented by pressing [1] or M1.

The Pad Options dialog

When you have imported a component to the schematic double click on a pad for editing it. The following dialog opens:

Position: Shows absolute coordinates
Pin number: Shows the number of the pin, the pad is related to.
Pad Name: If the naming of the pins within the package is alphanumerical, (e. g. A1 - A32, B1 - B32, etc.), here you can drop those names. The pad name must be identical to the one of the corresponding pin of the symbol. The pin number must be identical (e. g. pin name of package A1= pin number 1, A32=32, B1=33, B32=65, etc.).
Pad height and width: Shows the dimension of the pad.
Form: Shows the outline form of the pad. The following variations are selectable:

• Round (for round and elliptical solder pads (height<width))
  
• Octagonal (also oblong height<width possible)
  
• Rectangular
  
• Oval (for oblong solder pads with round endings)
  

Layer: Defines the layer where the solder pad should appear. For an smd-pad, simply a copper layer number must be entered. For a solder pad with drillhole, layer 100 (special layer) should be used, which means that the drillhole appears on all copper layers. You can define also padstacks. The according layers therefore are layers 101...254.
Rotation: Shows the orientation of the pin. The cross is the reference point.
Pad aura: The solder pad is also drawn in the corresponding deletion layer. The outline of the solder pad in the deletion layer is drawn bigger with the value given for the aura. This is of importance for generating ground planes.
Drill hole: Sets the diameter of the central drillhole. The drillhole diameter value for smd-pads is 0 (zero). Color: Define color of a pad independently of predefined color. Is color white (R=255, G=255, B=255) chosen, the predefined standard-color is used. If you wish color white although, you need minimal offset from the above mentioned RGB characters (just one point fits).
Drillhole: You will not find a simple element that represents a simple drillhole as a mounting hole in TARGET. Place a via and set its pad size dimensions smaller than the drillhole size. Also, you should delete its signal.

Solderstop/Solderpaste: You can cover one, some or all pads/vias with solderstop or solderpaste. Either you use dialog "Special" in Gerber output PCBout to cover all pads/vias or define prior to Gerber data production individual coverings with the pad-properties. Highlight one or more pads/vias and press [e] for edit. Now the dialog change pads opens. The following picture appears:

Tick the box "Solderstop" to cover pads /vias with solderstop or to free them from solderstop or just to fix solderstop to the drillhole. Green in the layout means: here is no solderstop! So this area is solderable. If you don't tick the box or leave setting "Standard" nothing happens right now. That means the decision whether solderstop is used or not is made later in the Gerber output.

Solderpaste is to be used when you use SMD components and wish to cover their pads with solder without flooding the complete board with solder. Define now individual solderpaste coverings for one or more pads if desired or leave the "Standard"- setting when the box is ticked or leave the box unticked. The decision to provide solderpaste to all or none is made later in the Gerber output.

Rectangular pad having rounded corners

When using lead free solder agens it's possible that little solder balls emerge at the tips of rectangular Pads. They may rip off and stroll alog in your layout and lead to unwanted effects in other locations. To avoid this it is recommended to round the sharp corners of rectangular pads. From TARGET 3001! V15 doubleclick a desired rectangular pad and set the rounding of the corner radius as percentage of its own (shortest) dimension. The following image shows corners of a rectangular Pad rounded by 50% (each 25% to the left and to the right).

Image: Rectangular pad with rounded corners

From version TARGET 3001! V15 by default rectangular pads have a corner rounding by 20%. You may deviate from this value at your own choice.

Non rectangular pad form

Please also see the article Polygonal pads for to draw free shaped pads (V16 feature).

Image: A power inductor having non rectangular soldering areas

In this example the recommended land patterns don't have a rectangular form. You need to draw two rectangular areas on layer 14, Area top. Copy them to layer 18, Solder mask top and 19 Solder paste top. This effects to have them within the solder paste stencil and to keep them free from solderstop varnish. Remember that all in green is free from solderstop. Now place a filled circle on layer 15 Deletion top. In order to make the areas connectible, place each a pad to them at any convenient spot.

Image: An example how it would look like in TARGET 3001!. At numbers 1 and 2 there is a regular pad behind.

Special: Two pads leading one Signal

How to construct a connection within a component package, which has only one pin in the schematic, but two pads in the layout? e.g. a clamp which is soldered on two pads but referring to only one logical pin in the schematic. In the package both pads are short-circuited...

In general, there are two situations which need fixing two pads in the layout to only one pin in the schematic:

1) The pads carry the same signal but both need to be connected. This can be needed, if GND needs to be connected several times to a processor but in schematic view only one connection shall be showed.

2) The pads in a package are short-circuited that way that the connection can carry power so that it can be used as a bridge.

Ref. 1): You can exactly overlap several connections in the schematic when creating a symbol. If you later connect a green signal line to it, all pins are touched simultaneously. For not getting all pin numbers displayed, please set the second and all further pin numbers invisible.

Ref. 2): For versions TARGET 3001! V10 and younger it is allowed to assign the same number to several pads when creating a package in the layout view. TARGET that way recognizes, that those pads are connected and assigns, when importing them, the same signal to them.

The drawing of such a package is not a problem. Nevertheless the layout of TARGET draws an air wire for two (clamp-internal) connected pads which are recognized as normal connection and processed by the router promptly as track. In fact one would prefer saving this space for other tracks. The "Zero-Ohm-Resistor" -problem is similar. In TARGET the component is constructed having an internal bridge. We are not very happy with this state...

Pad having a stretched (even rectangular) breakthrough

Sometimes data sheets show pads having rectangular breakthroughs (rectangular drillings). The only way to create that in TARGET is to place a rectangle on layer "extra milling" over the drillhole. Please also see article: "Oblong hole". Nevertheless you should consider to take a round hole though, big enough to recept the rectangular pin. This might cause less trouble.

.