Description

Managed Open Parts Library (MOPLib)

Previously named Generic High Energy Physics Parts Library (GHEPlib).

This is a CAD data library with support for multiple CAD tools.

Not to be confused with Seeed Studio's Open Parts Library

Objectives

Multi-CAD tool support
Data reuse where reasonable
Quality control: revision controlled, standards compliant, production tested
Uniform look, size, and style across CAD tools
User friendly: good-looking, paper print readable, publication ready, documented
Low coupling with optimization for different use cases (design density, formatting preferences, etc.)
Wide manufacturing technology support

Related Tools

Dependencies

Supported CAD tools
- Siemens PADS VX2.3 or higher
- Siemens DxDesigner (assumed import ability from PADS)
- Altium Designer 23 or newer (tested)
- KiCAD
Python 3 (Legacy)
- For management tools
GCC
- For management tools
SQLite
Qrbot (Android, optional but recommended tool for barcoding)

Used On

Caribou v2 project
Internal (confidential) projects at contributor sites

Primary Developers

Brookhaven National Laboratory
Carleton University Particle Physics Instrumentation Group

Installation Instructions

General Tips

All CAD tools require copying the repository to an accessible location. It is recommended to choose a central location with no spaces in the path name.

For example when admin/root priviliedges are available:

"C:\lib\MOPLib"
"/opt/MOPLib"
"/usr/local/lib64/MOPLib"
"/usr/local/lib/MOPLib"
"/lib/MOPLib"
"/lib64/MOPLib"

Siemens

Setup -> Settings -> Project -> Symbol Libraries

Alternately, the .prj file can be edited directly:

LIST IndependentLibraries
VALUE "DIR [W] . (symbols)"
VALUE "DIR [R] ${SDD_HOME}\Libraries\xDX_Designer\SymbolLibrary\Globals (Globals)"
[...]
VALUE "DIR [W] C:\lib\MOPLib\Siemens\custom (MOPLib_custom)"
VALUE "DIR [R] C:\lib\MOPLib\Siemens\borders (MOPLib_borders)"
VALUE "DIR [R] C:\lib\MOPLib\Siemens\mfg_import (MOPLib_mfg_import)"
VALUE "DIR [W] C:\lib\MOPLib\Siemens\mfg_mod (MOPLib_mfg_mod)"
ENDLIST

TODO DxDatabook integration

KiCAD (version 5)

It is recommended to add the library as a global library:

Preferences -> Manage Symbol Libraries... Preferences -> Manage Footprint Libraries...

Alternately, directly edit the text files:

~.config/kicad/sym-lib-table

TODO example

~.config/kicad/fp-lib-table

TODO example

Porting Designs

This is needed anytime the library name changes or for older designs which are meant to transition to this library.

Siemens

#. Change symbol names to those that are desired from the library #. Tools -> Update Library Partitions...

Select symbol-> Right click -> Symbol-> Reposition Properties Select symbol-> Right click -> Symbol-> Reset Text Properties

May be very useful to rapidly clean up a schematic

KiCAD

#. Clever text based search and replacements can be done on the schematic and layout files

Management Instructions

Use dbeaver. See any entry as an example.

Table Descriptions

Primary keys in each table are indicated with "PK"

CAD_table
- Relates parts to the preferred CAD files. A single part can have many CAD models or data files but only a few are preferred and/or tested.
- MFG = Manufacturer
- PN = Part Number. This is the primary manufacturer part number (not distributor, not internal)
- All symbols, footprints, and simulation models are references to CAD files in the Data_table
Data_table
- path: This can be a path to a file or a section of a file.
  - If this refers to sections of a file, identifiers relevant to each CAD tool should be used.
  - Symbols recognized by the CAD tool can be used. This is useful for default libraries.
- author: The most recent editor of the data. As soon as the data or a file is modified, the author is considered to have changed. This is for liability tracing
- release_version:
  - If a default library is used, the exact release version should be indicated.
  - If a file was directly downloaded from a manufacturer, the date of the download should be indicated.
- sym_group:
  - Some parts are best represented by multiple separate symbols. This indicates that they should be grouped together.
- deployment_history: A short description of the harshest environmental deployment that the design within the file has survived. Examples include "not deployed", "functional", "functional after shock and vibration testing...", "functional after high temperature testing..."

Database Integrity

By default, SQLite doesn't have Foreign Key constraints enabled.

They were enable with:

PRAGMA foreign_keys = ON;

No good method found to automatically ensure UUID uniqueness in the database directly via the SQLite database structure.

A (64 bit integer) UUID can be generated with the following SQL for SQlite:

select max(parts.UUID), max(CAD_data.UUID)+1 from parts, CAD_data;
select max(max(parts.UUID), max(CAD_data.UUID))+1 from parts, CAD_data;

Useful SQL Queries

select 'BOM ID', UUID from parts where (manufacturer_part_number0 = "CRF0805-FZ-R020ELF") or (manufacturer_part_number1 = "CRF0805-FZ-R020ELF") or (manufacturer_part_number2 = "CRF0805-FZ-R020ELF");

BOM ID is to be entered for reference to a spreadsheet

IP Control

License

See License File
Data can be imported from manufacturers into this library only if that data is accompanied by a waiver of ownership (stated as "free to use for any purpose including sale and open source")
Imported data without modification is kept in separate import libraries. If data is modified or customized, it should first be copied to the custom libraries. The indicated author should also change.

Directory Structure

. ├── Altium │ ├── custom │ ├── document_templates │ └── test_project ├── FreeCAD │ └── custom ├── golden_BOMs ├── KiCAD │ ├── custom : full custom by library authors │ ├── import_variant : import from any external source with modifications │ ├── mfg_import : direct import from part manufacturers (no changes) │ └── SnapEDA_import : direct import from SnapEDA (no changes) ├── LTSPice : models ├── mechanical │ └── custom : fully custom by library authors ├── mfg_supplied : source CAD data that was supplied by manufacturers (any format) ├── ngspice : models ├── part_specs ├── pin_numbering ├── PSpice : models ├── Siemens : DxDesigner │ ├── borders │ ├── custom : fully custom by library authors │ ├── golden_symbols : known good symbols from legacy projects │ ├── mfg_import : direct import from manufacturers (no changes) │ ├── mfg_mod : import from external sources with modifications │ └── test_project ├── SnapEDA_supplied : source CAD data as provided by SnapEDA └── tools

Inventory Integration

Some options:

https://alternativeto.net/software/inventree/about/ https://alternativeto.net/software/partbolt/about/ https://alternativeto.net/software/partsbox/about/ https://alternativeto.net/software/axt-parts/about/ https://alternativeto.net/software/snipe-it/about/ https://alternativeto.net/software/storedown/about/ https://alternativeto.net/software/part-db/about/ https://alternativeto.net/software/bomist/about/ https://alternativeto.net/software/partkeepr/about/

Top options are InvenTree and PartKeepr

Planned Work / TODO

BOM exporter
- implement merging of components with notes
- implement new "construction" property applicable to resistors (wirewound, thin film, thick film, etc.)
- Dual pretty and field names in column titles for quick editing
- Change to new multiplier strategy (BOM, schematic and/or layout)
- (s) on Ref designators

Conventions

General ECAD

Use dedicated "BOM Item" symbols or fiducial place holders for connection-less additional BOM items (gender adapters, screws, mechanical items, if mechanical items are stored in electrical schematics for the given project)
Use resistors and proper connectivity for placeholders of additional BOM items that can be represented as parasitics: pin inserts, wires, etc.

Pin Mapping for CAD Data Reuse / "Generic Parts"

There are multiple ways to handle generic symbols and footprints:

part + generic symbol + pin remapped footprints
- E.g. PART_NUM, BJT, SOT23_123
- In practice this is very challenging to manage
part + pin remapped symbol + footprint
- E.g. PART_NUM, BJT_123, SOT23
part + generic symbol + generic footprint + pin map file to associate pin numbers, pin names, or pin IDs between the symbol and footprint
- Different CAD tools use different values to link schematic and layout.
Part + one symbol + one footprint, 1 to 1 map
- PART_NUM, BJT_123, SOT23_123

Symbols and footprint pin mapping is dictated by the CAD tool (pin names or pin IDs are sometime used) and symbols and footprints must comply with this.

However, within this library, linkage by a positive integer is generally preferred. The reasons for this are

This transcends 2D design limits (column+row format)
This also applies to virtual / logical pins
This is compact to store

The conventions for this are:

Pin numbering provided by manufacturer should generally be preferred
Alphanumeric pin IDs (such as for BGAs) should be converted by sorting alphanumerically and ascending
Pins missing a number on manufacturer datasheets (E.g. power pads) should be assigned am unused number

Selected strategy:

For parts with 3 pins or less (transistors, potentiometers, etc.):

generic symbols are available (pin remapping is done at the symbol level).
2 pins gives 2 unique symbols
3 pins gives 6 unique symbols and one unique footprint

123 mapping conventions:

BJT CBE E.g. C→ 1 B→ 2 E→ 3
MOSFET DGS
Potentiometer top wiper bottom
TVS diodes vcc signal gnd

For parts with more than 3 pins:

It is considered a coincidence that the pinout is identical between two given parts. This even applies to fairly standard parts such as quad opamps, comparators, etc. since the pinouts usually still vary.
If a high (>3) pin count part is found to have an identical pinout to an existing symbol and/or footprint, this CAD data can be directly reused without renaming any files and only changing properties as needed. This linkage should be indicated in the database.

A "drop in" replacement occurs when:

Manufacturer: May vary
Manufacturer PN: May vary
Symbol (includes pin numbering / connectivity): No change
Footprint: No change
Part specifications: May vary but typically must be close

A "near drop in" replacement occurs when:

Manufacturer: May vary
Manufacturer PN: May vary
Symbol (includes pin numbering / connectivity): No change
Footprint: May vary
Part specifications: May vary but typically must be close

CAD Data Reuse

Note that, due to JEDEC, IEC, ANSI, ISO and other mechanical standards, footprint pin numbering is unlikely to change and footprint reuse is much more likely than symbol reuse.
- It should not be assumed that manufacturers are standards compliant: pin numbering on footprints should always be verified before using a footprint
A symbol which is a superset of another symbol is considered a completely different symbol
- This is clearer in the schematic and prevents design errors
- This is to target DRC cleanliness
- E.g. DFN and TSSOP parts have the same pin numbering but the DFN has an additional PAD connection
A symbol with multiple sub sections (units, heterogenous parts) is considered a single symbol
- This is partly driven by CAD tool limitations: many CAD tools (Altium, KiCAD) actually have the symbols grouped within the database.
- While some CAD tools (Siemens) have piece-meal symbols that could be reused, the symbols must still be linked together with properties or other data entry and it is considered best if this is included in the symbol.
Separate footprints are allowed to accommodate different assembly methods (wave, reflow, bonding, etc.)
Separate footprints for different design densities are allowed.
- If possible, it is recommended to not make a new footprint and modify footprints on a per instance basis to meet density needs. E.g. Silk screen can be removed.
- Separate footprints (schematic based footprint modification) are recommended when the CAD tool does not allow modifying footprint instances or when parts are very frequently used (passives) and manual modifications would be tedious.

Schematic Symbol Drafting

Nominally hard metric except for pin and schematic routing grid
Primary scale: 2.5mm = ½ of preferred, print ready, scale
- Note that all dimensions are scaled from what are considered comfortable in terms of reading on a paper print, hand drawing, and hand writing Text without any assistive technologies (magnifying glass, digital zoom, etc.).
- Text heights for reference:
  - 5mm ~=16pt
  - 4mm ~10pt
  - 3mm ~= 8pt
  - 2.54mm ~=6.7pt
  - 12pt and 10pt are standard publishing font sizes.
- Preferred technical drafting paper would be 5mmx5mm course grid with a 1mm fine grid (mm paper, 2x the primary scale). This is at small handwriting scale (4mm ~=10pt), hand drawing scale (~1mm tolerance), this is a standard grid paper size, and a decade increment.
- Note that, when drawing by hand, lines have the width of the pen or pencil tip. This is assumed to be 1mm (unscaled) and sets a minimum spacing on lines and geometry for them to be legible: roughly 1mm edge to edge = 2mm center to center = 1mm scaled center to center
  - In contrast, vector graphics on computers can scale and rerender lines automatically and allow them to have practically a 0 unit width.
  - This requires a clear distinction between edge to edge and center to center dimensions.

Origin should generally be at the lower left of the symbol
Imperial metric conversion
- Pins are sized on on the fine imperial grid and intersecting metric geometry is resnapped.
  - In some cases, this results in the entire symbol being on an imperial grid.
  - This is much faster to draw than native metric length pins.
- Originally metric graphics (text, special symbols) unrelated to pins are kept on the metric grids.
Text
- Pin and net labels and numbers: 2mm [0.079"] tall
  - Goal is to nearly fill all available space between pins and nets.
- Symbol adjacent text: 2mm [0.079"] tall
  - All uniform
  - Should generally be at lower left of symbol. Exceptions apply to small parts.
- General writing text: 2mm [0.079"] tall
  - For printing, text should not be smaller than 4mm in height but this value matches the primary scale and users are expected to scale as needed for printing.
Pin length
- Minimum, no pin number label label: 0.5mm [0.020"]
- Minimum, with pin number label: 2.5mm [0.098"]
  - Fits 3 small handwritten digits giving a highest pin number of 999. Prefer longer default if possible for cleanliness.
- Typical: 5mm [0.197"], 5.08mm [0.200"]
- Length integer multiples of 2.5mm or 2.54mm
Lines
- Minimum length: 1mm
- Typical width for vector graphics: 1px / vector
- Typical width for raster graphics or vector graphics with line weight: 0.5mm
- Minimum parallel line spacing, center to center: 1mm = 1 fine grid point between lines
Pin labels
- Pin number labels are not mandatory but are recommended for ease of use and clarity. E.g. large ICs, multi-component devices, etc.
- Pin name labels are not mandatory if the connectivity is clear.
Triangles
- Perfectly equilateral triangles are preferred but have a base/height ratio of 2/sqrt(3)=1.1547 so they do not fit well onto a grid
- Closest preferred base/height ratios are
  - 4/3 = 1.333
  - 6/5 = 1.200
  - 8/7 = 1.142
- 1/1 triangles are not recommended
Circle and arcs
- smallest radius, arc, filled circle, or hollow circle: 0.5mm [0.020"]
- digital bubbles: 0.5mm [0.020"] radius
- testpoints: 0.5mm [0.020"] radius
Symbols should be as small as possible while maintaining clarity, readability, and general good appearance.
- Usually, the size is not limited by the geometry but by the adjacent text (Ref. Des.) Almost all symbols have at least 2 lines of text and thus have a minimum height of 2*2mm=4mm = 2 grid spaces.
- If drawing by hand, a similar approach would be used to not waste paper area or drawing time.
- Uniformity in scale across symbol types is not mandatory (e.g. same size triangle for all amplifiers regardless of feature set, e.g. all 2 pin components are the same size). It is recommended to size symbols as small as possible while fitting all the required information (subsymbols, text, pin labels, etc.) and while respecting all the other drafting rules (e.g. minimum and default text sizes).
- Scaling subsymbols (pin label text, digital bubbles) with overall symbol size is not mandatory. Readability is typically maintained at the original scale.
Symbol variants are allowed to accommodate different display formats or preferences (e.g. pin number labels or no pin number labels) but one symbol must always be designated a default.
Symbol names should
- be human readable (no reverse order)
- not contain special symbols (URL safe, for compatibility with file systems and to be easy to type)
- be written from least to most specific
- not contain abbreviations
1. Layout Footprints
Nominally metric
- Imperial is often what is given by the manufacturers or required by a standard. Use the following rules to convert:

The conversion strategy appropriate for the application should be used. Tight tolerances require smaller rounding errors. Note that the courser rounding is usually an integer multiple of the finer options.
For drill size matching between imperial and metric sizes, drills should always use strict (1um) conversion
Standard passive components footprint names should include whether they are imperial or metric to avoid confusion in duplicate names

<!-- -->

Silkscreen
- Polarity indicators included but may be covered after assembly
- All footprints should include a bounding box. The primary reason for this is to show which pads are grouped when a part is not installed. This also serves as a type of layout keepout.
Soldermask
- Dedicated shapes
Solder paste
- Dedicated shapes
Assembly layers
- Dedicated shapes
Drill layer
- Preferred mechanical drill size: 1.1mm
- Preferred microvia /laser drill size: 250um
Metal layers (external and internal, general rules for wide technology support)
- Min metal width, any geometry to any geometry, any net to any net, any plating thickness, any layer: 400um
- Min metal to metal spacing: same as min metal width

Device Property Conventions

Multiplier Format
- When the cad tool has native multiple instance support, use this instead
- multiplier (integer) = 1xmultiplier
- "" (empty) = 1
IS_INSTALLED flag
- "DNI" = "DNP" = "NP" = "0" = "no" = "No" = "NO" = false
- "" = "1" = "yes" = "Yes" = "YES" = true
- Previously, this was merged with the muiltiplier property. This was found to lack clarity and sometimes even be confusing.
Unique Resistance, Capacitance, Inductance, ... properties
- Many tools typically prefer a single VALUE property that is displayed. This is also more convenient for BOM export. However, this lacks clarity since the exact property being referred to may need to be assumed (e.g. diode forward vs. reverse voltages) It is also possible to resolve a part to have undesirable specifications due to the lack of specificity.
- Using a "spec-string" of text to encode the specifications for a given part was considered but native CAD tool support is desired.
Siemens
- Convention for DEVICE = "Symbol Name" without any suffixed that are used to identify a part of a heterogenous symbol
  - Formerly, DEVICE = "Symbol Name"_PN. As of 2023-03-08, the MANUFACTURER_PART_NUMBER property was added to enable the use of different symbols for the same part within the same design. This property name is also more explicit, clearer, and CAD tool independent
  - DEVICE must be unique since the tool uses this property for layout-schematic linkage
- MANUFACTURER_PART_NUMBER= "PART_NUMBER" before completion
- Property names target the Netlist PADS/DxDesigner flow. The PADS documentation indicates that the cases for the properties vary between the Netlist and Intgrated design flows. E.g. Part Number (PART_NUMBER)
- HETERO property is fully completed if applicable. Symbol grouping is not explicitly stored in the database
- PKG_TYPE="PKG_TYPE" (unlinked -- determined at PCB layout start)
  - PCB only parts do not have this property
- Only properties necessary for display in the symbol and basic packaging are added to the symbol
  - This is faster to enter and allows direct addition of other parameters at the schematic level as preferred by designers, assuming that mapping to database fields are managed correctly
  - This is typically, DEVICE, PKG_TYPE, PART_NUMBER, REFDES
  - Note: For some reason, properties can only be moved if they don't contain the default value

BOM Exporters

Specific Field Names must be used for compatibility with BOM exporters.

KiCAD

CSV formatted
Dual flat BOM and deduplicated BOM

Script last tested 2023-12-30 in KiCAD 7.0.7 release build Previous versions tested in in KiCAD 5.1.8

Requires kicad_netlist_reader.py which ships with KiCAD. This can be copied or symlinked to the script directory.

Command line (OpenSUSE Leap 15.4 tested): python3 "pathToFile/bom_csv_custom.py" "%I" " %O"_BOM.csv

Originally based on bom_csv_grouped_by_value_with_fp.py Components are sorted by ref and grouped by value and footprint

This exporter supports the following custom fields in KiCAD in addition to some normal KiCAD fields. It is recommended to add them to the KiCAD custom field settings.

'Capacitance'
'Coupling'
'Dielectric'
'ESL'
'ESR'
'Footprint'
'Inductance'
'Impedance'
'Impedance Frequency'
'Manufacturer'
'Manufacturer Part Number'
'Max Current'
'Multiplier'
'Is Installed'
'Note'
'Power'
'Resistance'
'Sat Current'
'SRF'
'Tempco'
'Tolerance'
'Voltage'

Overall, the exported data includes: 'Capacitance'
'Coupling'
'Dielectric'
'ESL'
'ESR'
'Footprint'
'Inductance'
'Impedance'
'impedance_frequency'
'Manufacturer'
'Manufacturer_part_number' 'Max Current'
'Multiplier'
'Is Installed'
'Note'
'Power'
'Design Quantity'
'Usage Quantity'
'Reference Designator'
'Resistance'
'Sat Current'
'SRF'
'Symbol Description'
'Symbol Lib Name'
'Tempco'
'Tolerance'
'Value'
'Voltage'

"Part ID" MOPLib database identifier (uint64_t)
“Part_Number”
- Set Value = “PN” when this is used
- In general should never be empty unless parts are sourced at construction.
“Manufacturer”
- In general should never be empty unless parts are sourced at construction.
“BOM_Multiplier” TODO review The 'multiplier' field is a BOM quantity multiplier and not a design multiplier. Some CAD tools support this feature or some variety of it natively. For example:
- design multipliers
- "block instances"
- "arrayed components"
- RefDes array
- sub-units
- fractional units (e.g. ¼, ½ ) / ganged parts Typically, CAD tools assign unique reference designators to each subcomponent of each instance.
“Is In Layout”
1. Supported aliases: “DNL” = 0, “ ” (blank) = “1”
2. For CAD tools which do not have native layout omission.

This script converts the multiplier from text to an integer based on the following rules:

Empty ("") → 1
Integer → 1xinteger

The "Is Installed" flag supports the following values:

true
True
false
False
0
1
yes
no
TRUE
FALSE
NP → 0
DNI → 0
DNP → 0

Since the multiplier field applies to a single design component, the total number of components after deduplication is then the sum of the multipliers.

Siemens

A template to dump most of the useful design info within a design was developed. Grouping and deduplicatation during the export is based on the primary and secondary key settings. Primary keys will result in separate BOM lines and the grouping will be done based on the secondary key (2x nested loop implementation). For example, Reference designators are often a secondary key but, to force the export of parts without annotated reference designators, the CAD database ID was set to a primary key.

Verification Flows

PADS example project holds all newly developed symbols
- Visual review
- Tools→ PCB Interface... (Packaging)
- Tools → Diagnostics
  - Shows if schematic library is out of date
- PADS Databook → New hierarchical Verification Window
  - Shows if library items can't be found
Tested on the following CAD tools
- Altium 23
- PADS VX.2.10

Debugging Tips

Siemens

Symbols can "break" and exhibit strange behavior when instantiated. This may occur if the text of the symbols is directly edited.
- One observed symptom of this is that the tool may automatically (per an ambiguous / unknown rule set) change the case of characters in symbol names in schematics however, references to symbol filenames with different case characters still work
- Another observed symptom of this was the inability to delete or add specific properties, especially ones that are not present in the properties list.
- The solution to this is to copy and paste the symbol graphics to a new symbol -- PADS will generate a new file and therefore clean errors
All symbols and symbol instances in a HETERO part must have exactly the same properties, otherwise packaging fails
- The visibility of the property can vary between symbols
After Tools→ Update Libraries, pins may become corrupted and fail to package. To resolve this, the part must be full replaced: right click→ Replace Symbol→ Search for same symbol name→ Replace
PADS layout libraries are not compatible with DxDesigner
Tools → Property Definition Editor
- Anytime modifications are made, the project has to be closed and reopened for the changes to be visible
- This includes the symbol editor -- it must be closed and reopened along with the project
- Not all properties can be modified from this dialog
- The properties available depend on
  - the selected design flow
  - the object type (border, composite, etc.)
  - the tool editing the properties (E.g. symbol editor vs. regular schematic editor)
- A workaround to get properties available anywhere is to manually add them to the properties file.
- An example of this is the @DATETIME property commonly used for borders. While it is an official property for a netlist flow project, for an unknown reason, it was not available in the symbol editor until it was manually added as a user defined property.
  - Note that is is unclear if a custom property was necessary or PROPERTY_NAME="@DATETIME" would also work
  - @DATETIME function worked correctly with @DATETIME="" and @DATETIME="@DATETIME". @DATETIME="@DATETIME" is more practical for seeing and placing the property.
PADS locally caches symbols within the project and a forced update of the libraries doesn't seem to always work.
One odd issue that was observed was that nets connected to two separate symbol pins would automatically be renamed to the same net. Any net renames one net would automatically rename the other. The nets had separate IDs and the problem was isolated to the new schematic symbol which was developed. Initially, it was believed that the pin names and ID numbers were unacceptable but extensive testing (working around symbol caching issues) showed that this was not the case. Verification showed that the symbol was of the same version (schema) as newer symbols that were developed from scratch (non-copy, V54). The only solution to this was to fully delete the problematic pin pair and add them from scratch.
PADS standard library location: "C:\MentorGraphics\PADSVX.2.10\SDD_HOME\Libraries\xDX_Designer\StarterLibrary\StarterLibrary.dbc"
PADS BOM Exporter Formatting files have a .ipl extension and the templates are available at "C:\MentorGraphics\PADSVX.2.10\SDD_HOME\standard\templates\dxdesigner\netlist" After modifying one during export, a copy is made in the project folder.

Altium

This Altium error was encountered:

Database error{width="9.58cm" height="4.18cm"}

(Image from https://altiumlibrary.com/GetStarted/Troubleshooting )

Instructions here were necessary to install a database driver that Altium recognizes:

https://www.altium.com/documentation/altium-designer/using-database-libraries-with-32-64-bit-altium-design-software-same-computer

http://www.microsoft.com/en-us/download/details.aspx?displaylang=en&id=13255

As administrator in cmd.exe:

AccessDatabaseEngine_X64.exe /passive

Release Info

Release Commands :

tree -a -D --du -h ./confidential > confidential_tree.txt

UUID 132

PROJECT RELEASE ID 1 DATE 2023-12-22T20:55:17+00:00 Git COMMIT 29dc0e139c4fa1718c18f1990c7dd2c5887772bf

General purpose release.
No verification done specifically for release.

UUID 137

PROJECT RELEASE ID 2 DATE 2024-01-01T10:37:24+00:00 Git COMMIT null

General purpose release.
No verification done specifically for release.

TODO

Table generators
- database to Altium database with dblink file
- database to DxDatabook database
Cleanup functions
- CAD entry deduplicator with reference updates
Import functions
- Digikey BOM
- Mouser BOM
- General BOM
Document C:\MentorGraphics\PADSVX.2.10\SDD_HOME\standard\netlist.prp

Name		Name	Last commit message	Last commit date
Latest commit History 43 Commits
.custom_git_logs		.custom_git_logs
.dbeaver		.dbeaver
Altium		Altium
FreeCAD/custom		FreeCAD/custom
KiCAD		KiCAD
LTSpice		LTSpice
Siemens		Siemens
SnapEDA_supplied		SnapEDA_supplied
images		images
mfg_supplied		mfg_supplied
part_specs		part_specs
pin_numbering		pin_numbering
releases		releases
tools		tools
.gitignore		.gitignore
.project		.project
LICENSE		LICENSE
README.md		README.md
confidential.zip		confidential.zip
confidential_tree.txt		confidential_tree.txt
database.db		database.db
documentation.md		documentation.md
mergers_acquisitions.md		mergers_acquisitions.md
pending_additions_deduplication.md		pending_additions_deduplication.md

License

maxp2/MOPLib

Folders and files

Latest commit

History

Repository files navigation

Description

Objectives

Related Tools

Dependencies

Used On

Primary Developers

Installation Instructions

General Tips

Siemens

KiCAD (version 5)

Porting Designs

Siemens

KiCAD

Management Instructions

Table Descriptions

Database Integrity

Useful SQL Queries

IP Control

License

Directory Structure

Inventory Integration

Planned Work / TODO

Conventions

General ECAD

Pin Mapping for CAD Data Reuse / "Generic Parts"

CAD Data Reuse

Schematic Symbol Drafting

Layout Footprints

Device Property Conventions

BOM Exporters

KiCAD

Siemens

Verification Flows

Debugging Tips

Siemens

Altium

Release Info

UUID 132

UUID 137

TODO

About

Topics

Resources

License

Stars

Watchers

Forks

Releases

Packages 0

Languages

Packages