Ever wish you had a good way to control what appeared under the Part Number column in your Bill of Materials? Do you have a secondary or internal part number which should appear in the BOM instead of (or in addition to) what SOLIDWORKS decides to put in the BOM? Here is information that should help you understand where these properties are generated.
Traditional Method of Controlling the Part Number
To use a value other than the filename for a part number in a BOM, the preferred technique would be to change a setting in the part’s configuration properties.
This first illustration shows how to access the properties of a configuration (click the ConfigurationManager tab, right click the configuration name, and select Properties from the menu). The Bill of Materials Options pane (shown in the next image) contains a drop down list that will allow changing the default setting of Document Name to Configuration Name or User Specified Name.
If Configuration Name is selected, then the name of the configuration is exactly what will appear under the Part Number column in your BOM. If User Specified Name is selected, a box appears that allows for typing in any text, within reason. It’s usually best to stick with alphanumeric characters, dashes and underscores.
A quick and easy way to see what will be shown as the part number in your BOM is to look in the ConfigurationManager. Look at the inset in the following image and you will see a value in brackets. That value is the text which was typed in after selecting User Specified Text.
If Document Name had been selected (which, as was mentioned previously, is the default setting) you would see the name of the part document in between those brackets.
If Configuration Name were selected, there would be nothing in between the brackets and, in fact, the brackets would disappear as well.
After all, it would be a bit silly to show the configuration name after the configuration name, wouldn’t it? If there is no value in brackets after the configuration name, then the configuration name is what’s being used as your part number.
User Defined Custom Properties as Part Numbers
Adding custom properties is how a custom column can be added to a BOM (There are plenty of reasons to use custom properties. For now, we will stick to the topic at hand).
Clicking Properties in the File menu and selecting the Custom tab will take you to a window similar to that shown in the following image.
Click in the first row under Property Name and either pick a predefined value from the list or type in something of your own.
As you can see in the image above, 3 sample property names have already been added. It’s worth talking about some of these so you know what you’re getting into if you use them.
- PartNo – This property is found in the drop down menu when entering a property name, but has no special functionality whatsoever.
- Number – Like PartNo, this property name is also found in the drop down list, but unlike PartNo, it has special functionality. If using Workgroup PDM, “Number” is one of the properties that automatically gets added to a document when checking that document into the Workgroup vault. Best to leave this one alone unless you have some special reason to use it.
- SW-Part Number – (not shown) this property is specific to weldments and is also present in the drop down list, which is the only reason it’s mentioned. Without going into a lot of extra detail, let’s just say you should not use this property unless you are involved with creating weldments in SOLIDWORKS and, even then, only in specific situations outside the scope of this blog.
- Part Number – There is absolutely nothing keeping anyone from entering a property name such as “Part Number”, “PartNumber” (no space), or some other spelling variant. However, it will probably cause confusion and won’t override SOLIDWORKS’ internal part number anyway, so why bother? Let’s look at an example to help illustrate what could happen.
The previous image shows the process of selecting a custom property named Part Number for the column heading. This is done by clicking on the letter “C” at the top of the column, clicking the Column Property command shown in the inset, and then selecting the desired property from the Property Name drop down list.
As you can see, having a second custom property named Part Number in no way affects what SOLIDWORKS will use for it’s own part number anyway (see column B in the above image), so it doesn’t really make sense to create a custom property with that same name.
If your company requires a second internal part number, or if you wish to use your own custom part number based on a custom property instead of using the traditional (and recommended) method of controlling the part number (as described earlier), use a property name that will easily differentiate it from SOLIDWORKS’ default part number label.
For example, use a property name such as InternalPartNo, CustomPartNo, or something similar. That will help keep confusion to a minimum