Robert McAnany 2025

CREDITS

Contributors
@[Francesco Arfilli], @TeeVar

Beta Testers
@hawcad, @rob.wolbrink7456, @[Francesco Arfilli], @pedja, @TeeVar, @Seva

Helpful feedback and bug reports
@SeanCresswell, @[Francesco Arfilli], @arekkul, @[Imre Szucs], @64Pacific, @Seva, @hawcad, @rob.wolbrink7456, @pedja, @TeeVar, @jpoat-seesai

Feedback from users

OMG .....love your work buddy!

Management of standard parts is a huge use of my time and this may solve that!

Thx, another great tool for SolidEdge​ Users!

Cool tool! I have been looking for something just like this. (...) Great job, and making it open source is just extra good karma.

Another excellent utility. Appreciate your contributions to the community.

DESCRIPTION

Solid Edge Storekeeper is a utility to create, organize, and share standard parts. It is free and open source and you can find it Here. Please note the standard part templates were created with SE2024. You will need that version or newer to use them. (Update: @TeeVar, generously contributed a set of templates created with SE2019.)

Fasteners, retainers, structural shapes, and more in ANSI and ISO format are included. There are over 30k items available. There is no database; everything is done in Excel. It is fully customizable. If you upgrade Solid Edge, no change to the program or its data is required.

The program handles two types of standard parts. One consists of items like fasteners. These are defined in dimension tables and created as needed. The other consists of vendor-type items like pneumatic fittings. Each of these has its own model file. Both types are eligible for the handy automatic patterning option (see separate section below for details).

Tree Search

For items like fasteners, use Tree Search. Navigate to the desired item, select a material, then right-click and choose an action. If the part is not already in the library, the program creates it. The possible actions are:

• Add to assembly Adds the part to the assembly and activates the Place part command.
• Replace selected Replaces a selected part in the assembly.
• Replace all Replaces all occurrences of a selected part in the assembly.
• Scroll to selected Scrolls the tree to the selected part in the assembly.
• Fastener stack Opens the fastener stack dialog. See the separate section below for details.

Property Search

For vendor-type parts, use Property Search. Enter the search terms, then click . Locate the desired item on the list, then right-click and select an action. The possible actions are:

• Add to assembly, Replace selected, Replace all Same as above.
• Open Opens the selected file in Solid Edge.
• Open folder Opens the file's directory in Windows File Explorer.

Note, the program does not come with any vendor-type parts; you're on you own for that. Simply add what you need (and probably already have) to the library, in a subdirectory if you prefer.

That's pretty much all there is to know about vendor type parts. For the others, a bit more information follows.

You can set the file names according to your preference. You can specify the material or any other SE file property. File names and properties can accept formulas as input. So you can do stuff like:

Structural shapes are not quite the same as fasteners. While the cross section is standard, the length and likelihood of additional features is not. Usually the part doesn't even belong in the library. For these, you can change the Save in option from Library to Assy Dir or Other. The program prompts for a filename, and for Other, a location.

Who Needs This Program?

Me, for one. What makes it different? First, it's free and open source, and is actively maintained. It beats the pants off of scrolling through massive directories in Windows File Explorer. You're in control -- any part it creates belongs to you, and is stored where you want. It's customizable, has no database, and doesn't care if you upgrade Solid Edge.

Also, unlike Family of Parts, files are only created as needed. Each part is stand-alone, not tied back to a master file.

Unlike web-based offerings, the program is integrated with your parts library and works directly with Solid Edge. It updates the properties you specify, using the naming conventions you define. If you want adjustable parts (see the provided springs example), or any other SE-specific functionality, the program handles it like the native file that it is.

Finally, it has a secret weapon -- all of us. Contributions are welcome! Please message me on the Solid Edge Forum, or raise an Issue on GitHub, for ideas on how to get started.

Uh-oh. The Marketing guy just showed up. He wants to "Synergize our stakeholders and leverage this cross-promotion opportunity". I bet he does.

Hello there!! I'm Big Mike! Do you want to do things better and faster with less work?! Of course you do! That's why you need Solid Edge Housekeeper!

Is it free and open source?! Yes! Is it a batch utility?! YES!! Does it find annoying little errors in your project?! YES YES YES!!!! You are going to LOVE IT!!

Sorry about that. Let's move on.

INSTALLATION

Please note there is some setup required before using the program. After completing this step, check the Setup section below for details.

To install, do one of the following

• Download the Latest Release (It will be at the top of the page)
• Clone the Project (See below to get the data and templates)

Downloading the Latest Release

To get the latest release, click the file SolidEdgeStorekeeper-VYYYY.N.zip. You may have to expand the Assets dropdown to see it. Your browser should prompt you to save it.

Choose a convenient location on your machine. Extract the zip file (right-click > Extract All). Verify the directory is not blocked or read-only (right-click > Properties). The program needs to be unblocked with write access to function properly.

Double-click Storekeeper.exe to run. The first time you do, you may get a Windows Protected Your PC message. You can click More Info followed by Run Anyway to launch the program.

Cloning

The data and templates are not in the GitHub repo. You need to download a Release to get them. To make them available in your development environment, copy the directories DefaultData* and DefaultTemplates* to the locations where your compiled Storekeeper.exe is located.

On my machine, the executable resides in two places: bin\Debug\net8.0-windows\ and bin\Release\net8.0-windows\. I have copies of those directories in both places.

SETUP

As noted earlier, some setup is required before using the program. If you run Solid Edge in a localized language please be sure to see the information at the end of this section.

Tree Search Toolbar

Most options are set on the Tree Search Options page (see next), but those most frequently-used are located on the toolbar itself.

• Collapse
  Closes all open nodes in the tree.

• Save in

  • Library The standard location for library parts.
  • Assy Dir The same location as the assembly file currently open in Solid Edge.
  • Other Anyplace else.

• Always on top
  Keeps Storekeeper on top of other windows. Click to toggle.

• Auto pattern
  Enables automatic patterning. Click to toggle. See separate section below for details.

• Favorites only
  Shows only your favorites in the tree. Click to toggle. See separate section below for details.

• Matl
  Available materials for the selected part. If an item only has one material defined, it is selected automatically. If you go to a different item in the tree and its material list contains the currently active material, the selection is retained.

• Tree search options (see next).

Tree Search Options

The program needs to know where to store the standard parts, and for fastener-like items, where to find the files defining their shape and spreadsheet containing their dimensions.

• LIBRARY DIRECTORY
  The library is where the standard parts you create are stored. The default is in Preferences\Library under the Storekeeper main directory.

  Note the directory is created the first time you run the program; it won't be there before that. As noted above, if you want to access your vendor-type standard parts, they must be in the library. You can place them in one or more subdirectories if desired.

• DATA DIRECTORY
  The spreadsheet contains the variables required for each size of each type of part. By default, it is stored in the Preferences\DataSE2024 directory.

  Change the data directory to Preferences\DataSE2019 if you want to use the alternative templates.

• TEMPLATE DIRECTORY
  The templates are SE part files that have variable-table-driven geometry to create new parts of a given type. By default they are stored in the Preferences\TemplatesSE2024 folder.

  As noted at the outset, the original templates were created in SE2024. They will only work if you're using that version or newer. An alternative set of templates, created with SE2019, was generously contributed by @TeeVar. To use them, change the template directory to Preferences\TemplatesSE2019.

  Even if you have a newer version of Solid Edge, you may still want to use the SE2019 templates. Unlike me, @TeeVar is an ISO native speaker. If you work with that standard, his naming conventions will probably be more familiar and useful to you.

  Note, the templates and the spreadsheet that drives them go together. If you change one, you have to change the other.

  You don't have to stick with your first choice, by the way. You can switch between the original and alternative templates at any time.

• MATERIAL TABLE
  The material table is usually your normal SE material table. However, for a quick test of the program, an alternative is to use StorekeeperSE2019.mtl or StorekeeperSE2024.mtl found in their respective Templates directory. Copy one or both to your Solid Edge Materials directory to make it available. On my machine, that location is C:\Program Files\Siemens\Solid Edge 2024\Preferences\Materials.

  If you decide to continue using the program, you would eventually want to utilize your own material table, updating material names in the spreadsheet and templates as needed.

• OPTIONS

  • Read the Excel file each time the program is launched
    Internally, the Excel file is parsed and saved in *.xml format. If you haven't changed the Excel file, this is an unnecessary step. Clearing this option tells the program to use the *.xml file it created previously.

  • Add any property not already in file
    As mentioned above, besides creating geometry, the program can also update file properties. Enabling this option tells the program to add any (custom) property not already in the file.

  • Disable fine thread warning
    The program is currently unable to properly set the thread size for ANSI UNF external threads. The program logs a warning if this occurs. Enabling this option suppresses that warning.

    The condition can cause issues with interference checking. Fixing it is optional. To do so, open the file and edit the Thread definition. On the Parameters Step, you'll note the size designation is followed by an asterisk (*). Click the drop down and select the one without it.

• Process templates in background
  A new part must be opened in Solid Edge to update its parameters. This setting tells the program to not display it in the user interface.

  Note, processing in background does not support Fit View. If you need usable thumbnail images, this option is probably not for you. Also, there is an issue when creating a part whose units do not match the default units of your Solid Edge installation. Processing in background appears to ignore the file's unit setting.

• Replace part: Suppress failed constraint
  When using the Replace command, some constraints may fail to get resolved. If this occurs, this option tells the program to suppress the constraint.

• Replace part: Allow failed constraint
  With the same situation as above, this option tells the program to leave the constraint in the failed state. This is my preferred setting. The pathfinder shows a red lightning bolt, alerting me that I need to fix something.

• Do not add files to the Recently Used list
  Enable this option to keep the program from adding newly-generated standard parts to the Most Recently Used list. Note this ability was added to Solid Edge in version 2020. If you are running an earlier version, it has no effect.

• Include drawing of part if present
  If a file in the templates directory has a drawing with the same name, the program can copy it to the library along with the part. Enable this option to do so.

• On top refresh time (milliseconds)
  If the Always on top option is enabled, this setting controls the maximum time between checks.

• Time out for part placement (milliseconds)
  If more time than this setting has passed for the Place Part command to complete, it is interrupted. This is needed to avoid an infinite loop in the program. Set it so you have ample time to constrain the part in the assembly.

• Check for new version at startup
  If you don't need a reminder about new versions, disable the check here.

Property Search Options

Additional settings for Property Search are accessed from that tab's toolbar. Click the Property Search Options button to display the form.

Properties to Search

This is where you enter the names of the properties that hold the values you want to match. You must also specify if the property is System or Custom. System properties are in every Solid Edge file. Custom properties are ones you define, probably in a template.

Solid Edge Template Files

These are your normal template files, not the ones used by the program to create standard parts. They are needed to populate the available properties, and to determine what language is in use.

Options

• Cache library file properties for faster search
  Reads all file properties and saves them in a separate file. This can speed up searches for large libraries. It takes some time to load the file initially; the status bar informs you of the progress.

Localized SE Installations

You may have more work to do if you're not using English in Solid Edge. In the spreadsheet Storekeeper.xls, there are some property names that probably need to be changed.

Open the file (located in the Preferences\Data directory) and look for entries like %{System.Title} and update as required.

AUTOMATIC PATTERNING

Standard parts, especially fasteners, are frequently patterned after placement. If this option is enabled and the feature to which a part has been assembled is a member of a pattern, the program attempts to pattern the part. There are currently a couple of limitations.

• It works in SE2024 and SE2025. It does not work in SE2019 or SE2021. Other versions have not been tested.

• It works with Smart Patterns and User-Defined Patterns (that's a hole with multiple hole circles in the profile). It does not work with (the default) Fast Patterns unfortunately, unless you get lucky and pick the hole that was used to create the pattern.

• It is sometimes unable to create a pattern when placing a fastener to a part located in a subasembly. In some cases, it helps to save the top-level assembly and try again.

FAVORITES

As mentioned above, in the tree search panel, you can have all available parts shown, or just your favorites.

Edit the Favorites column in the spreadsheets (Storekeeper.xls, AnsiFasteners.xls, etc.) to do so. For Storekeeper.xls, the entire node must be either True or False as shown below.

For the other spreadsheets, it is a line by line choice.

FASTENER STACK

A fastener stack is a grouping that consists of a fastener and related components, such as washers and nuts. To create one, on the Tree Search dialog, right-click a fastener and select the Fastener stack command. The following form is shown.

Configuration and Use

To select the stack style, click the Configuration button. There are eight versions that employ nuts, and four each for thru and blind tapped holes. Note, you only choose the fastener. The related components are automatically selected based on the fastener diameter and thread.

Once the desired configuration is selected, choose the units and enter the appropriate parameters. Click Add to Assy to start the process.

The program first searches the library for a fastener length that meets the criteria. If none is found, an error is diplayed.

If a fastener is found, the program then opens separate temporary subassemblies for the top and bottom parts of the stack, and populates them with the components required for the chosen stack style.

Next, it adds each updated subassembly, in turn, to the main assembly. The subassembly is dispersed into the main assembly and the Place part command is activated.

The program waits for the Place part command to finish before proceeding. Confusingly, the command does not automatically finish when the parts have been fully constrained. You have to right-click the mouse to finish. If you notice nothing happening for a while, the program could be waiting for your input.

After the components are placed, they are converted to an Assembly group. Finally, the group is patterned if applicable, assuming that option is enabled.

Getting Parameters

The parameters Minimum thread engagement and Minimum extension are design decisions and left up to you. Clamped thickness and Thread depth are parameters of the model. Adding an easy way to get those is on the roadmap, but not currently implemented.

Today, for Clamped thickness, the quickest way may be to use the Solid Edge Measure command. It is on the Inspect Tab > 3D Measure Group.

To get Thread depth on blind holes, one way is to change selection priority from Part to Face with CTRL+SpaceBar, then select the threaded hole. On the shortcut menu, select Edit Definition and check the setting on the Options page of the Hole dialog that appears.

Changing the Related Components

In Storekeeper's Preferences directory, there are three files for each of the supplied datasets, FlatWasher.json,LockWasher.json, and Nut.json. You can edit those in Notepad to point to the desired node in the *.xml tree.

Doing it like that is not user friendly in the least. And wait until you see the tree traversal syntax. It might be easier to go with the defaults, then use Replace selected to fix things up after the fact.

Some care was taken in the creation of the templates to avoid breaking constraints when replacing parts. Hopefully it won't create extra work if you decide to give it a try.

PRE-POPULATING THE LIBRARY

Note, this feature is temporarily disabled. It does not yet support multiple materials per category.

You can add items to the library ahead of time. Enable the Pre-populate checkbox to get started.

Note, for items with multiple materials available, the material must be selected before starting this process. Click on an applicable item and select the desired material when prompted.

To select an item, enable its checkbox. Enabling the checkbox of a category header will select all items (including subcategories) below it. You can select a category, then de-select any items you don't want included.

Once satisfied with the selection, click Add to library to start the process. After you do, the Close button text changes to Stop. Click that to stop processing. It may take a few seconds to register. It doesn't hurt to click it twice.

To avoid confusion, the Add to assembly shortcut is disabled in this mode. Uncheck Pre-populate to get it back.

One handy feature missing in the TreeView control is Multiselect. That means you cannot select a range with click followed by SHIFT-click. It may be possible to add code to implement it, but it's not available now.

CREATING NEW TEMPLATES

You are of course free to create new templates any way you see fit. However, if you plan to contribute your awesome work to the project, there are a couple of things to keep in mind.

Many standard parts have a primary axis. For consistency, consider orienting it along the Y Axis as shown. For parts with a secondary axis like the pipe elbow, consider the Z Axis.

Another thing to think about is the effect of replacing one standard part with another. It would be nice not to break assembly relationships. For fasteners, I started with the socket head capscrew. When it was time to create the next one, I did a Save As on that initial part and modified it as needed. Since the head and body now have the exact same faces, Replace Part works as expected.

Variable names are something else to consider. To minimize confusion in creating and maintaining the companion spreadsheets, see if you can reuse names that have been previously established. You can check the supplied templates or spreadsheets to see what may apply to your parts.

As mentioned above, drawings of standard parts is a supported option. If you need that, simply create a drawing with the same name as the template. If the program finds such a drawing, and the option is enabled, it copies it to the library, renames it and updates the links. Enable the option Include drawing of part if present on the Tree Search Options page.

CUSTOMIZATION

The following is for those who want to customize the program. You may want to do that eventually, but you can safely skip this section if you're just getting started.

Organization

Earlier I referred to "a spreadsheet." In reality there are multiple spreadsheets. One, Storekeeper.xls, is the place where the overall layout of the data is handled. The others are companion files that hold detailed information about a given category of parts. These have names like AnsiFasteners.xls, IsoStructural.xls, etc.

While the use of Excel is handy, it's not all roses. Representing an arbitrary-depth heirarchical tree is awkward, for one thing. Here is how Storekeeper.xls is organized.

You'll see that the tree structure is represented by indenting. The top node is Solid_Edge_Storekeeper and in this example its first child node is Ansi_Fasteners_Steel. The first two child nodes under that are BHCS and FHCS.

In addition to child nodes under any given node, you'll notice other entries. Those are some program attributes being set, and various properties being assigned. More about properties in a bit.

In the image, the BHCS and FHCS nodes each have an entry, Nodes (plural). That is one of those program attributes just mentioned. It is the mechanism that tells the program to consult a companion spreadsheet tab for further information. Here is a small portion of the companion data for Dowel Pins.

The rows represent different sizes, the columns represent values for a given size. The first row holds the name for each value, the second holds its type. The first column lets you identify your favorite parts as discussed above.

The types Variable and LeafNodeVariable refer to entries in the template's variable table. One other type not shown in the image is ParameterString. That denotes a value that is needed in the template, but does not reside in the variable table. For those, there must be separate code to handle it. Currently only ThreadDescription is supported. See AnsiFasteners.xls for an example.

Properties and Spreadsheet Variables

Now, let's look at the other entries in Storekeeper.xls, starting at the top.

Top Level of the Tree

Here at the top level of the tree, we are defining spreadsheet variables for property names and the corresponding name in the Solid Edge file. The location of the definition in the tree defines its scope. Since these statements are at the top of the tree, they apply everywhere.

The syntax is horrible; that's how Xml likes it. While Xml is a very flexible data-representation format, it is quite rigid in this regard.

Next Level Down

In this image, we are looking at a tree node one level below the top. You'll see we are setting values for the part number, hardware status and material.

The name of the spreadsheet variable has rules. XyzProperty looks for XyzFormula to know how to proceed. The prefix, Xyz in this case, can be anything you want (except for some reserved names shown below). The suffix, Property and Formula, are the only valid choices.

Reserved Spreadsheet Variables

• TemplateProperty
• TemplateFormula
• FilenameProperty
• FilenameFormula
• MaterialProperty
• MaterialFormula
• Node
• Nodes
• TooltipFormula

So, for example to update the part number in the file, the program will use the information in PartNumberFormula to update the property defined in PartNumberProperty. In this example that tells the program to make this assignment.

%{System.Document Number} = "NA"

Material Formula

The MaterialFormula spreadsheet variable is slightly different than the others. Its value can be a comma-delimited list. For example,

STEEL,STAINLESS,STAINLESS\, PASSIVATED,BRASS

If the material name itself contains a comma, preceed it with a backslash as shown. A comma-delimited list requires special handling. This is currently the only variable that supports it.

One last thing about the MaterialFormula. It can occur in multiple places in the tree. The bottom-most definition is the one that is used. That allows you to set a default definition, say for all fasteners, then redefine it lower in the tree for any item with different options.

One More Level Down

Here we are setting up the processing of button head capscrews. You can see we need to specify what template to use and how to name the file. We must also provide the companion spreadsheet name and the tab in that file where the information is stored.

As mentioned previously, formulas can contain entries such as %{Name} and %{MaterialFormula}. Variables are populating the part file, not reading from it. That means you cannot reference a file property like %{Custom.Engineer} in a formula. Variables can only come from Storekeeper.xls or a companion spreadsheet.

In this example, we are also updating the description property. That isn't necessary for the program to function. It just illustrates how to update Solid Edge file properties. Any property in the file can be updated in this way.

One more thing about this example. Note there is a tooltip being specified. If you want one, it needs to be on the first line after a Node definition. There is a fix coming for that restriction, but it's not in there now.

OPEN SOURCE PACKAGES

This project uses these awesome open source packages.

• Excel reader ExcelDataReader
• File and folder dialogs CommonFileDialogs
• Icons Icons8
• JSON Converter Newtonsoft.Json
• Structured storage editor OpenMCDF