Create a Footprint using IPC Compliant Footprint Wizard – Part 1

In this article we will explain how to create a SOIC(8) footprint for Texas Instruments NE555D precision timer using IPC Compliant Footprint Wizard. This method is ideal for drawing footprints according to IPC-7351 Compliant Footprint standards. Also, it allows to generate all three board density levels footprints.

1. Before we start we should open a datasheet for NE555 and find a package drawing page. It is on the page 27. TI Package name is D (R-PDSO-8) and it is according to JEDEC standard MS-012 variation AA. See image below for the details.

2. First of all, we need to create a new PCB library or open an existing one. If a PCB library was not opened, the option Tools will not appeared in the main menu. If one or more PCB Libraries are already opened, make sure that one of them is active by clicking on it in the Projects Window (usually on the left side of Altium Window). When you set it properly, Option Tools will appear in the top main menu. See image below for the details.

3. Choose Tools -> IPC Compliant Footprint Wizard. See image below for the details.

4. IPC(R) Compliant Footprint Wizard Window appears. Click on Next button in the lower right corner of the window. See image below for the details.

5. Next step is to select component Case/Package family or type. In our case, it is SOIC (Small Outline Integrated Package, 1.27mm Pitch; Type of leads are Gullwing).

6. Click on the Next button in the lower right corner of the window. See image below for the details.

7. In this window you need to fill out the values (dimensions) from the datasheet. In our case it is:

Overall Dimensions

Width Range (H) Minimum is 5.8 mm
Width Range (H) Maximum is 6.2 mm
Maximum Height (A) is 1.75 mm
Minimum Standoff Height (A1) is 0.1 mm
Body Width Range (E) Minimum is 3.8 mm
Body Width Range (E) Maximum is 4 mm
Body Length Range (D) Minimum is 4.8 mm
Body Length Range (D) Maximum is 5 mm

Pin Information

Number of pins are 8
Lead Width Range (B) Minimum is 0.31 mm
Lead Width Range (B) Minimum  is 0.51 mm
Lead Length Range (L) Minimum is 0.4 mm
Lead Length Range (L) Maximum is 1.27 mm

As you can see all SOIC packages have a pitch (e) of 1.27 mm or 50 mil and wizard won’t allow you to change this value.

8. Here you can also generate 3D STEP Model by checking the box (Generate STEP Model Preview) in the lower left corner of the SOIC Package Dimensions window. If you want to see prewiev of a 3D model over your footprint click on the 3D button in the lower left corner of the black right part of the window where a footprint image is shown.

9. Click on the Next button in the lower right corner of the window.

10. In this window SOIC Package Thermal Pad Dimensions, make sure that the checkbox Add Thermal Pad is unchecked because TI SOIC(8) package doesn’t have a thermal pad.

11. Click on the Next button in the lower right corner of the window. See image below for the details.

12. SOIC Package Heel Spacing Window appears. As we want to create a footprint according to IPC standard, check the box (Use calculated values) because Altium already calculates this value. In our case S Minimum is 3.26 mm and S Maximum is 4.55 mm. The minimum heel spacing is calculated by subtracting twice the maximum pin length range from the minimum body width range. The maximum heel spacing is calculated by adding the tolerance on the inner distance between the heels of the opposing rows of leads to the minimum heel spacing.

13. Click on the button Next.

14. SOIC Solder Fillets Window appears and we can set Board density Level. Check the box Use default values.

Solder Fillet refers to the shape of the solder joint between the component lead and the PCB pad. Adequate fillet is required to ensure both the strength and reliability of the solder joins. A solder joint is usually described by 3 fillets: toe, heel and side fillet. Values for those three solder fillets have been defined by IPC-7351 Standard, based on reliability testing and industry empirical knowledge. According to IPC there are three board density levels:

a) Level A – Low density (suggests higher minimal values for Toe, Heel and Side Fillets)
for SOIC package minimal values are:
Toe Fillet (JT Min) = 0.55 mm
Heel Fillet (JH Min) = 0.45 mm
Side Fillet (JS Min) = 0.05 mm

b) Level B – Medium density (suggests medium minimal values for Toe, Heel and Side Fillets)

for SOIC package minimal values are:
Toe Fillet (JT Min) = 0.35 mm
Heel Fillet (JH Min) = 0.35 mm
Side Fillet (JS Min) = 0.03 mm

c) Level C – High density (suggests lower minimal values for Toe, Heel and Side Fillets)

for SOIC package minimal values are:
Toe Fillet (JT Min) = 0.15 mm
Heel Fillet (JH Min) = 0.25 mm
Side Fillet (JS Min) = 0.01 mm

15. In our example we will generate a footprint according to Level A – Low Board density Level. Choose Level A in the drop down menu.

16. Press Finish button in the lower right corner of the window. See image below for the details.

Generated footprint will appear on the window like on the image below.

Share this:

Tutorials in the category: Altium Designer

  • 4 Ways to create a footprint in Altium Designer
  • Altium Schematic component – Create a new component, draw schematic symbol
  • CircuitStudio vs Altium Designer
  • Create a custom Altium schematic template
  • Create a Footprint using IPC Compliant Footprint Wizard – Part 1
  • Create a Footprint using IPC Compliant Footprint Wizard – Part 2
  • Create a new FPGA Project
  • Create a new Integrated Library, add Schematic and PCB library
  • Create a new PCB Project, add Schematic and PCB document
  • Free Download, Install and License Altium Designer 18, 17, 16, 15, 14, 13 and 10
  • How to compile an Integrated Library .LibPkg and generate .IntLib
  • How to Import 3D STEP model into footprint
  • Import and position 3D STEP into footprint if model is not designed according to IPC standard?
  • Replace, update and remove schematic sheet document template