Creating Linked Notes in SOLIDWORKS
SolidProfessor - Sam Sanchez | February 25, 2016 | Comment
Using SOLIDWORKS, it is not uncommon for users to want to store more information than just 3D geometry inside of CAD files.
For example, many users like to keep track of part numbers, which detail a description of the part for a bill of materials (BOM) and other relevant production information. This could include a vendor used for a purchased component.
These can be easily managed in SOLIDWORKS using file properties. In the video tutorial above, we’ll walk through how this can be done.
There are a few important things to keep in mind when storing values in the file properties of a part or assembly. This is especially true when leveraging the information elsewhere, like linking to notes in the bill of materials (BOM).
In the tutorial video above, we demonstrate these ideas using a step stool part in small, medium and large configurations.
Users can access a part or assembly’s file properties by going to the “File” dropdown menu and selecting “Properties.” The file’s property window has three tabs.
The first is the “Summary” tab, where users can add document properties like the author name, key words and comments.
The “Custom” tab is the custom properties for the file. SOLIDWORKS attempts to apply these properties globally across every configuration within the file.
The “Configuration Specific” tab allows users to override custom property values based on which configuration is selected. This tab can also be used to store separate custom properties to be maintained at the configuration level.
We’ll enter some properties in the Custom tab for this tutorial. There are some default properties listed here, which users can access by clicking the down arrow or by typing in a name for the property.
We’ll select “Description” for the first item in this window leave “Type” as “Text.” For the value, we will enter “Wooden Step Stool.”
The next item, we list as “Company Name,” leave it as Text and enter the value as “SolidProfessor.” Additional items are added under the values of “Buy” and “StoolWorks,” for additional data concerning companies bought from and vendors.
Next, we’ll add properties in the Configuration Specific tab. Here, the “Apply to:” dropdown menu, shows which configuration the changes are being applied to.
For the sake of the tutorial, we want to keep track of the parts numbers at the configuration level since each variation of our stool assembly has a unique part number. To do this, we’ll select “PartNo,” meaning part number, from the drop down for the property name. We’ll also enter the part numbers for the large, medium and small tool configurations.
In the case that we got our small tools from a different vendor than those for the medium and large assemblies, we can add a second configuration specific property here to override the StoolWorks vendor value. We can do this by typing the other vendor’s name in the Value box and click OK.
Next, we’ll leverage these custom properties. In the tutorial video above, we create a new drawing of the stool part using an isometric view on a sheet. We’ll add a BOM table here.
If users click a column, a couple of dropdown menus appear. These allow a user to link a column to a custom property.
For the tutorial, we’ll edit the column headers to show a few of the properties previously added. Both the custom properties and any configuration specific properties will be shown in the list under “Property name.”
Users can link these properties to a note by launching the “Note” tool from the “Annotations” tab within command manager and clicking a location on the sheet to place the note.
In the property manager, notice there is an icon to link to property. When clicked, a dialogue box appears, where users can choose to use custom properties from the current document, which is the drawing itself.
We haven’t added any custom properties in this tutorial, so only the default properties are available.
Alternatively, users can select “Model found here” and choose “Current drawing view” to use custom properties from the model and the view specified in the sheet properties.
We can also choose “Selected component or other drawing view,” which is the annotation attached.
For this tutorial, we’ve selected “Current drawing view.” Next, we’ll add the note, which depicts the value entered earlier.
This is parametric, so if a user goes back and changes the property, the note updates.
In the video above, we add a second view to this drawing, showing the small configuration of the stool, which was recorded as having a different vendor.
None of the values in the BOM update after inserting this assembly into the drawing. To update the BOM, users would have to create a new one.
However, we can show notes that refer to the small stool’s properties. To do this, users must launch the note tool, select the small stool to attach the note, click to place it on the sheet and select “Link to Property.” This time, we’ll select the component to which the annotation is attached and we’ll select “Vendor” under property name.
After clicking OK, we can see it shows the configuration specific property for the small configuration.
If a user does not want to show the leader, but still wants to link the notes, just click the “No Leader” icon in the property manager.
You can learn more about the new capabilities in SOLIDWORKS 2016 by signing up for a free membership.
About the Author
Sam Sanchez is an Applications Engineer with SolidProfessor and a CSWP. Sanchez is an alumni of UC San Diego, and in her free time enjoys 3D printing and hanging out with her dog Ruby. You can see more training videos on a wide range of CAD, CAM & BIM topics at www.solidprofessor.com.
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