IPC Compliant Footprint Wizard

Now reading version 16.0. For the latest, read: IPC Compliant Footprint Wizard for version 22

The IPC Compliant Footprint Wizard creates IPC-compliant component footprints. Rather than working from footprint dimensions, the IPC Compliant Footprint Wizard uses dimensional information from the component itself in accordance with the standards released by the IPC.

Rather than requiring you to enter the properties of the pads and tracks that are used to define the footprint, the Wizard takes the actual component dimensions as its inputs. Based on the formulas developed for the IPC-7351 standard, the Wizard then generates the footprint using standard Altium Designer objects, such as pads and tracks.

For more information about creating component footprints, see the Creating the PCB Footprint page.

This dialog is compliant with Revision B of the IPC standard 7351 - Generic Requirements for Surface Mount Design and Land Pattern Standard. IPC-7351B was released in 2010 and supersedes IPC-7351A (which was released in 2007).

Accessing the IPC Compliant Footprint Wizard

The IPC Compliant Footprint Wizard is launched by clicking Tools » IPC Compliant Footprint Wizard from a PCB Library document.

The dialog can only be accessed if the IPC Footprint Generator extension is installed as part of your Altium Designer installation. This extension is installed by default, but if it is inadvertently uninstalled, the extension can be found on the Purchased tab of the Extensions & Updates page (DXP » Extensions and Updates). 

Hover over the icon and click  to download the extension. Altium Designer must be restarted to complete installation. 

If at any time you want to uninstall the extension, find the extension on the Installed tab of the Extensions & Updates page (DXP » Extensions and Updates) and click the  icon to uninstall. Altium Designer must be restarted to complete the uninstall process. 

Wizard Navigation

  • Click Cancel to close the IPC Compliant Footprint Wizard.
  • Click Back to navigate to the previous screen.
  • Click Next to navigate to the next screen.
  • Click Finish to close the IPC Compliant Footprint Wizard
Finish is available on any page of the Wizard after selecting the component type. If you click Finish before completing the entire Wizard, the footprint will be created using the system defaults for the component type you selected.

Selecting the Component Type

Choose the family of components for which you want to create a footprint on the Select Component Type page.

Click on the component type desired. The preview region on the right-hand side of the Wizard dynamically changes to show the currently selected component and also states the type of packages that are allowed to be generated.

The following table lists the component types and packages that are supported in the Wizard.

Table of supported component types and packages

Included Packages
BGA Ball Grid Array BGA, CGA
BQFP Bumpered Quad Flat Pack BQFP
CAPAE Electrolytic Aluminum Capacitor CAPAE
CFP Ceramic Dual Flat Pack - Trimmed and formed Gullwing Leads CFP
Chip Array Chip Array Chip Array
DFN Dual Flat No-lead DFN
CHIP Chip Components, 2-Pins Capacitor, Inductor, Resistor
CQFP Ceramic Quad Flat Pack - Trimmed and formed Gullwing Leads CQFP
DPAK Transistor Outline DPAK
LCC Leadless Chip Carrier LCC
LGA Land Grid Array LGA
MELF MELF Components, 2-Pins Diode, Resistor
MOLDED Molded Components, 2-Pins Capacitor, Inductor, Diode
PLCC Plastic Leaded Chip Carrier, Square - J Leads PLCC
PQFN Pullback Quad Flat No-Lead PQFN
PQFP Plastic Quad Flat Pack PQFP, PQFP Exposed Pad
PSON Pullback Small Outline No-Lead PSON
QFN Quad Flat No-Lead QFN, LLP
QFN-2ROW Quad Flat No-Lead, 2 Rows, Square Double Row QFN
SODFL Small Outline Diode, Flat Lead SODFL
SOIC Small Outline Integrated Package, 1.27mm Pitch - Gullwing Leads SOIC, SOIC Exposed Pad
SOJ Small Outline Package - J Leads SOJ
SON Small Outline Non-Lead SON, SON Exposed Pad
SOP, TSOP Small Outline Package - Gullwing Leads SOP, TSOP, TSSOP
SOT143/343 Small Outline Transistor SOT143, SOT343
SOT223 Small Outline Transistor SOT223
SOT23 Small Outline Transistor 3-Leads, 5-Leads, 6-Leads
SOT89 Small Outline Transistor SOT89
SOTFL Small Outline Transistor, Flat Lead 3-Leads, 5-Leads, 6-Leads
WIRE WOUND Precision Wire Wound Inductor, 2-Pins Inductor


  • Paste Masks are split into small fills for packages with a large thermal pad (sized 2.1mm x 1.6mm, or larger).
  • For packages involving gullwing leads, pads are trimmed to prevent them from otherwise extending under the package's body.
  • For small packages having a large central thermal pad, the peripheral pads are trimmed to ensure required clearance between the pads in accordance with the IPC Standard.
  • When pad trimming is applied, a warning is displayed within the dialog.

Preview Region

On the following pages for each component type, the Preview region dynamically updates to show new location, size, etc., for several settings.

In the Preview region, you can click  to toggle between 2D and 3D preview images. Click the icon then select 2D or 3D, whichever is appropriate. If the current image is 3D, click the icon to further define the preview by selecting/deselecting Show Simple 3D Bodies and Show Generic Models.

3D STEP Models

Previewing 3D STEP Models

If desired, you can see a preview of the 3D STEP model before generating the model. Click Generate STEP Model Preview on any page in the Wizard after selecting the component type to see a preview of the 3D STEP model in the Preview region.

The default setting for the files that are created when 3D STEP models are generated is Embedded STEP files. If these default settings are correct for your needs, you can click Finish to exit the IPC® Compliant Footprint Wizard and generate the 3D STEP model.

The subsequent pages of the Wizard change depending upon the component type you selected. Find your component type in the following list and click on the link to access the information regarding that component type. 

Choosing the Footprint Name and Description

The Footprint Description page is used to name and describe your new footprint. Altium Designer uses the information you input in the Wizard to suggest a name and description. Enable Use suggested values to use the Name and Description the system has entered. Enter any desired changes directly in the textboxes.

Selecting the Footprint Destination

Use the Footprint Destination page to select the location for the newly-created footprint to be stored. 

Select Existing PcbLib File if you want the footprint stored in an existing PCB Library file. You can enter the file directly in the textbox or use the  to open the Browse for existing PcbLib file to insert footprint into dialog and search for the desired file.

Select New PcbLib File if you want to store the footprint in a new PCB Library file. Enter the name of the new PCB Library file in the textbox. The system will append the new library file name with the extension .PcbLib. 

Select Current PcbLib File to store the footprint in the displayed PCB Library file.

Enable Produce 3D/STEP model to generate a 3D STEP model.

If you have a valid 'MCAD Co-Designer - SOLIDWORKS(R)' license, you can choose to save the model as file type Parasolid. Click the drop down to the right of Format then select Parasolid. The file shown in the External File text box is now a *.x_t file. This is the name and location of the file that will be saved. 

Select either Embedded (default) or External File. Select External File to save your 3D STEP model as an external file. The default file type is STEP and the file name appears in the External File text box with *.step as the file extension. If desired, click   to browse and select the folder in which to save your generated 3D STEP model.

Closing the Wizard

Click Finish to close the Wizard.

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.