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 footprint 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

Fig. 292 Altium - Open schematic lib.

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

Fig. 293 Altium - Use Library Splitter Wizard.

3. Press Next

Fig. 294 Altium - Next.

4. Add the schematic and footprint lib

Fig. 295 Altium - Add schematic and footprint lib.

5. Select both

Fig. 296 Altium - Select both.

6. Press Next

Fig. 297 Altium - Next.

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

Fig. 298 Altium - Select Output Directory.

8. Press Next

Fig. 299 Altium - Next.

9. Press Next

Fig. 300 Altium - Next.

10. Press Next

Fig. 301 Altium - Next.

11. Press Finish

Fig. 302 Altium - Finish.

12. All schematic symbols are separated from the others

Fig. 303 Altium - Schematic are separated.

13. All footprints are separated from the others

Fig. 304 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

Fig. 305 Altium - Extract Sources.

2. All included schematic and footprint libs will be listed in Altium

Fig. 306 Altium - All included libs are visible.

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

Fig. 307 Altium - Save the footprint lib.

4. Save also the necessary schematic library.

Fig. 308 Altium - Save the schematic lib.

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

Fig. 309 Altium - Schematic and footprint lib are available.

Now it can be continued with the instruction: More than one symbol or footprint 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

Fig. 310 Altium - Download - Part 1.

2. Download the Model from the homepage - Part 2

Fig. 311 Altium - Download - Part 2.

3. Save the model Ok

Fig. 312 Altium - Save.

4. Extract the zip-file

Fig. 313 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/)

Fig. 314 Altium - Open Altium Loader.

6. Open the ECAD model

Fig. 315 Altium - Open ECAD Model.

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

Fig. 316 Altium - Select epw- file.

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

Fig. 317 Altium - Altium Library Loader.

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

Fig. 318 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 footprint 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 symmetrically on top and bottom

2. Other mechanical layers: These layers only exist once

Table 116 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 117 must be considered especially in the PCB design when putting certain meta information in the layout.

Table 116 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 117 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 obtained from the manufacturer usually do not follow the mapping from the table above. Fig. 319 shows a typical mechanical layer stackup when a component is freshly downloaded from the manufacturer homepage.

Fig. 319 Typical layer stack in AD before editing

In order to adapt those components to the required layer mapping there are two ways of editing your new library part:

1. Loading the stackup template file from the UltraZohm Altium Library

2. Editing the layers manually

Loading Stackup Template File

Clone the UltraZohm Altium Library Repository to your local drive (https://bitbucket.org/ultrazohm/altium_libraries/).

1. Create a new PCB Library in Altium altium-designer

   

2. Import the predefined mechanical layer stackup file that is located in the Altium Library Repository under ..\altium_libraries\templates\mechanical_layers_Pcblib

   

   

3. After successful loading of the mechanical layer stackup template file your layer set should look like following

   

Editing Layers Manually

If you prefer to editing the layers manually, then the following steps are necessary:

1. Create all required mechanical layer pairs. You do not need to create all layer pairs defined in Table 116

   • Right-click in the layer area

   • Select Add component layer pair and fill out the dialog with the mapping from Table 116

   

   Fig. 320 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

   

   Fig. 321 Dialog to add a component layer pair

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

   

   Fig. 322 Dialog to add a component layer pair

   Delete M1

   

   Fig. 323 Dialog to add a component layer pair

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