Task 5: Generating Padstacks

A padstack is a component’s interface to the board. For a single layer board, the layout will require one set of pads with holes for a Plated Through-Hole (PTH) component. For a multilayer board, a more complex arrangement of pads is required, with each pad being assigned to one or more footprint layers. Some examples of padstacks are shown below.

Figure 1: Padstack Examples

 

Note
  • It is recommended that the footprint library is kept simple, with only the minimum required number of layers defined. This allows a "one-to-many" assignment of pads for inner conductor layers.
  • Individual pads can be assigned per conductor layer, but this may increase the time required for library maintenance.

 

Generating a Plated Through-Hole (PTH) Padstack

In this task, you will create a Plated Through-Hole (PTH) padstack using the pads that were built in the last task. You will use this padstack in later tasks when building footprints.

  1. On the eCADSTAR Library Editor ribbon, click Home > Editors > Padstack. The Padstack Editor dialog is displayed.

Figure 2: Opening the Padstack Editor

  1. In the Padstack Editor dialog, click Add Padstack. "NewPadstack-1" is created.

Figure 3: Adding a Padstack

  1. In the Padstack Name column, change the name of the padstack to "DIY-c200h120m220". This name represents a 2mm circle, with a hole of 1.2mm and a mask of 2.2mm.
  2. In the Drill diameter column, change the value to "1.200". The Multiple Layer Contact column becomes non editable and the check box is set.
  3. In the Slot Length column, leave the value at "0.000".
  4. In the Plated column, select the check box.
  5. In the Build-up Via column, ensure this check box is deselected. This completes the general parameter settings for the padstack.
  6. To set the first layer's parameter settings, in the Layer column, select Top_Resist.
  7. In the Connected Pad column, select DIY-c220.

Figure 4: Configuring the Padstack Editor

Adding a Padstack Layer

  1. In the Padstack Editor dialog, select the newly-built padstack, and click Add Padstack Layer.
  2. For the new layer, select Top_Elec in the Layer column.
  3. In the Connected Pad column, select DIY-c200.
  4. In the Unconnected Pad column, select DIY-c200.
  5. In the Thermal Pad column, select DIY-tc200.
  6. In the Clearance Pad column, select DIY-c220.

Adding a Second Padstack Layer

  1. In the Padstack Editor dialog, click Add Padstack Layer to add a second layer.
  2. For the new layer, select Bottom_Resist in the Layer column.
  3. In the Connected Pad column, select DIY-c220.

Adding a Third Padstack Layer

  1. In the Padstack Editor dialog, click Add Padstack Layer to add a third layer.
  2. For the new layer, select Bottom_Elec in the Layer column.
  3. In the Connected Pad column, select DIY-c200.
  4. In the Unconnected Pad column, select DIY-c200.
  5. In the Thermal Pad column, select DIY-tc200.
  6. In the Clearance Pad column, select DIY-c220.

Adding a Fourth Padstack Layer

  1. In the Padstack Editor dialog, click Add Padstack Layer to add a fourth layer.
  2. For the new layer, select Inner in the Layer column.
  3. In the Connected Pad column, select DIY-c200.
  4. In the Unconnected Pad column, select DIY-c200.

 

Note
Leaving this cell empty will allow pad suppression to occur automatically within the PCB Editor. When a padstack has track or copper area connected, it will display the Connected Pad. When there is no track or no copper area connected, it will display the Unconnected Pad.

 

  1. In the Thermal Pad column, select DIY-tc200.
  2. In the Clearance Pad column, select DIY-c220.
  3. In the Padstack Editor dialog, click OK.
  4. In the displayed dialog, click Yes to accept changes.

 

Note
Note that the newly-created layers are not ordered correctly. Close, and then re-open the Padstack Editor dialog to display the layers in the correct order, as shown below.

 

 

Figure 5: Re-Ordering Layers

This procedure is demonstrated in the following video.

Generating a Padstack for a Surface Mount Device (SMD)

In this task, you will create a Surface Mount Device (SMD) padstack using the pads that you created in task 3. You will use these in later tasks when building footprints.

  1. On the eCADSTAR Library Editor ribbon, click Home > Editors > Padstack. The Padstack Editor dialog is displayed.
  2. Follow the instructions in the previous task in this topic, but make the following changes:
  3. Change the name of the padstack to "DIY-r207_66m227_86".
  4. Only add the layers Top_Elec, Top_Paste and Top-Resist.
  1. In the Drill Diameter column, specify a value of "0.000".

The completed padstack parameters are shown below.

Figure 6: The Completed Padstack

This procedure is demonstrated in the following video.

Next topic: Placing Padstacks and Assigning Pin Numbers