Symbols and Footprints

When creating a schematic in Altium, there are many different ways to place components and use their footprints for the layout. In a project for the UltraZohm the UltraZohm component library is used exclusively. If the required components are not available in the current library status they must be added. Newly added components must fulfill the following requirements:

  1. A .SchLib or .PcbLib file must contain only a single symbol or footprint. If this requirement is not fulfilled it is impossible to resolve merge conflicts when people are working on the library

  2. The footprint must follow the mapping of the mechanical layers. This is vital in order to generate high quality documentation and production output. The requirements can be found under Mapping of the mechanical layers

  3. If the manufacturer supplies a 3D model of the component it must be included to the footprint.

If the user detects a footprint that does not follow the requirements mentioned above he is strongly encouraged to update the component or to open an issue and assign it to the maintainer (i.e. creator) of the component.

Extraction of footprints and symbols

In the following, 4 different ways will be presented, how to create the appropriate schematic and footprint format for the Altium DB Library used in the UltraZohm project:

Separate files for symbol and footprint

If both the schematic as well as the footprint are available from the manufacturer for Altium in separate files and if these files only contain one symbol or footprint you can start directly by integrating these components into the library. Please be aware that you will have to adjust the mechanical layers in the footprint. See UltraZohm components library for further instructions. If the desired component is combined in a library with several other components, see the following sections.

More than one symbol or fooprint in one file

If a component is in a library file (.SchLib or .PcbLib) with several other components this component must be separated from the other components in the schematic symbol library as well as in the footprint library. Altium provides the Library Splitter Wizard for this purpose so no manual extraction is required.

  1. Open the existing schematic library in Altium

../../../_images/100_Open_schematic_lib_Altium.png

Fig. 201 Altium - Open schematic lib.

  1. Use the Altium Library Splitter Wizard Tools –> Library Splitter Wizard

../../../_images/101_Use_Lib_Splitter.png

Fig. 202 Altium - Use Library Splitter Wizard.

  1. Press Next

../../../_images/102_Lib_Splitter_1.png

Fig. 203 Altium - Next.

  1. Add the schematic and footprint lib

../../../_images/103_Lib_Splitter_2.png

Fig. 204 Altium - Add schematic and footprint lib.

  1. Select both

../../../_images/104_Lib_Splitter_4.png

Fig. 205 Altium - Select both.

  1. Press Next

../../../_images/105_Lib_Splitter_5.png

Fig. 206 Altium - Next.

  1. Select the Output Directory (Therefore, it might be suitable to create one folder for the schematic symbols and one for the footprints.)

../../../_images/106_Lib_Splitter_6.png

Fig. 207 Altium - Select Output Directory.

  1. Press Next

../../../_images/107_Lib_Splitter_7.png

Fig. 208 Altium - Next.

  1. Press Next

../../../_images/108_Lib_Splitter_8.png

Fig. 209 Altium - Next.

  1. Press Next

../../../_images/109_Lib_Splitter_9.png

Fig. 210 Altium - Next.

  1. Press Finish

../../../_images/110_Lib_Splitter_10.png

Fig. 211 Altium - Finish.

  1. All schematic symbols are separated from the others

../../../_images/111_Splitted_Schematic_11.png

Fig. 212 Altium - Schematic are separated.

  1. All footprints are separated from the others

../../../_images/112_Splitted_Footprint_12.png

Fig. 213 Altium - Footprints are separated.

Now all components are separated from each other and it is possible to proceed with the instructions of UltraZohm components library .

Components are included in an integrated library

  1. Open the integrated library in Altium and choose Extract Sources

../../../_images/120_Open_Integrated_Lib.png

Fig. 214 Altium - Extract Souces.

  1. All included schematic and footprint libs will be listed in Alitum

../../../_images/121_Open_Integrated_Lib.png

Fig. 215 Altium - All included libs are visible.

  1. If more than one schematic and one footprint lib exist in the integrated library, choose the necessary footprint library and press File -> Save as.

../../../_images/122_Save_as_footprint.png

Fig. 216 Altium - Save the footprint lib.

  1. Save also the necessary schematic library.

../../../_images/123_Save_as_schematic.png

Fig. 217 Altium - Save the schematic lib.

  1. The integrated library is separated in schematic and footprint library.

../../../_images/124_Schematic_and_footprint_lib.png

Fig. 218 Altium - Schematic and footprint lib are available.

Now it can be continued with the instuction: More than one symbol or fooprint in one file.

Components are available as an ECAD MODEL

Sometimes, there are no symbols or footprints directly from the manufacturer available. Then you can use the component search engine (https://componentsearchengine.com/logPartRequest.php), where you can access a large number of already existing components or request new models for Altium.

To enter these components into the database, proceed as follows:

  1. Download the Model from the homepage - Part 1

../../../_images/130_Download_Model.png

Fig. 219 Altium - Download - Part 1.

  1. Download the Model from the homepage - Part 2

../../../_images/131_Download_Model.png

Fig. 220 Altium - Download - Part 2.

  1. Save the model Ok

../../../_images/132_Download_Model.png

Fig. 221 Altium - Save.

  1. Extract the zip-file

../../../_images/133_Extrahieren.png

Fig. 222 Altium - Extract.

5. Open Altium and a schematic file before the Altium Loader will be opened by selecting File –> Symbols Footprints 3D Models (If this tab does not exist, the necessary plug in is missing. Therefore read and install the Altium Library Loader https://www.samacsys.com/altium-designer-library-instructions/)

../../../_images/134_Open_ECAD.png

Fig. 223 Altium - Open Altium Loader.

  1. Open the ECAD model

../../../_images/135_Open_ECAD_MODEL.png

Fig. 224 Altium - Open ECAD Model.

  1. Navigate to the unzipped epw-file and select it

../../../_images/136_Open_ECAD_MODEL.png

Fig. 225 Altium - Select epw- file.

  1. After a short load time the following message appears. Press OK.

../../../_images/137_Altium_Library_Loader.png

Fig. 226 Altium - Altium Library Loader.

  1. The component is included in the SamacSys schematic and footprint lib (default generated)

../../../_images/138_SamacSys.png

Fig. 227 Altium - SamacSys.

At this point, the SamacSys lib can be reused or the respective symbols with the corresponding footprint can be stored in a temporary lib. Afterwards you have to continue with the instructions: More than one symbol or fooprint in one file

Mapping of the mechanical layers

When creating a component several layers types can be defined. Besides the standard layers like Top and Bottom copper overlay etc. mechanical layers can be defined. These layers carry information for the generated documentation output. In order to be able to reuse a certain output job to generate the documentation and production output the mechanical layers must follow a uniform mapping. The mapping is distinguished in two different categories:

  1. Component Layer Pairs: These layers exist symetrically on top and bottom

  2. Other mechanical layers: These layers only exist once

Table 94 shows the mapping of the component layer pairs to the functions. Even if Altium can handle the numbering of the layers automatically when assigning component layer pairs in the UltraZohm library only components that follow this layer mapping are accepted. The mapping of the additional mechanical layers from Table 95 must be considered especially in the PCB design when putting certain meta information in the layout.

Table 94 Mapping of the mechanical layer pairs

Layer

Function

M3

3D Body Top

M4

3D Body Bottom

M5

Assembly Drawing Top: Component outline

M6

Assembly Drawing Bottom: Component outline

M7

Courtyard Top

M8

Courtyard Bottom

M9

Designator Top

M10

Designator Bottom

M11

Component Center Top

M12

Component Center Bottom

M13

Value Top

M14

Value Bottom

M15

Hard Gold Plating (e.g. edge connectors) Top. Use the predefined layer pair here.

M16

Hard Gold Plating (e.g. edge connectors) Bottom. Use the predefined layer pair here.

M17

Soft Gold (ENIG) Top. No predefined layer pair. Just create two additional mechanical layers.

M18

Soft Gold (ENIG) Bottom. No predefined layer pair. Just create two additional mechanical layers.

M19

Dimensions Top

M20

Dimensions Bottom

Table 95 Mapping of the other mechanical layers

Layer

Function

M1

Board Shape

M2

Board Dimensions

M31

Route Tool Path

M32

Fab Notes

M33

Assembly Notes

M34

Board

M35

V-Cut

Unfortunately, the footprints that can be optained from the manufacturer usually do not follow the mapping from the table above. Fig. 228 shows a typical mechanical layer stackup when a component is freshly downloaded from the manufacturer homepage.

Typical layer stack in AD before editing

Fig. 228 Typical layer stack in AD before editing

In order to adapt those componennts to the required mapping the following steps are necessary:

  1. Create all required mechanical layer pairs. You do not need to create all layer pairs defined in Table 94

    • Right-click in the layer area

    • Select Add component layer pair and fill out the dialog with the mapping from Table 94

    Dialog to add a component layer pair

    Fig. 229 Dialog to add a component layer pair

  2. Move the objects from the previous layer to the new layer. Example: Moving the 3D body from layer M1 to M3

    Hide all layers except M1

    Dialog to add a component layer pair

    Fig. 230 Dialog to add a component layer pair

    Select everything on M1 (Ctrl-A) and move selected objects to M3 in the propertiers panel.

    Dialog to add a component layer pair

    Fig. 231 Dialog to add a component layer pair

    Delete M1

    Dialog to add a component layer pair

    Fig. 232 Dialog to add a component layer pair

  3. Repeat step 1 and 2 for all objects that are on the wrong layer