SolidWorks enables you to create several types of tables on drawings, such as the Bill of Materials, or BOM. Design Tables that are used in parts and assemblies can also be shown on the drawing to create a tabulated type drawing. Hole Tables enable you to chart the center locations and sizes of holes for easy access to manufacturing data. Revision Tables can work with Workgroup PDM (Product Data Management) or by themselves to help you document the revision history of a drawing. General Tables are also available for any specialized items that are not covered by the other table types.
The Bill of Materials (BOM) is one of the most frequently used types of tables that are available in SolidWorks. BOMs are intended for use with assemblies, but can also be used with individual parts for specialized applications. The information that you can expect to see on a BOM includes item number, filename, quantity used, description, and any other custom property that you would like to add to it. A typical BOM is shown in Figure 24.1.
BOMs are made in one of two ways. The default BOM is made from a special SolidWorks table, while an Excel-based BOM is driven by Excel. While Excel has advantages and disadvantages, many users appear to prefer the default BOM. Excel and SolidWorks table-based BOMs are not interchangeable, so if you plan to customize the default templates, you need to make a decision in which type of BOM you will want to develop the BOMs.
Note
BOMs can also be placed directly in the assembly and even in multi-body part files.
The BOM shown in Figure 24.1 is a default SolidWorks table-based BOM. The differences between the displays of the two types of BOM are mainly cosmetic; the bigger difference is in the functionality. The PropertyManager interface for the SolidWorks Bill of Materials is shown in Figure 24.2.
Like other types of data, the SolidWorks table-driven BOM starts from a template. The BOM in Figure 24.1 was created from the default BOM template. When a BOM is initiated, you can select the template in the Table Template panel near the top of the PropertyManager, as shown in Figure 24.2.
Table-based BOM templates are created in much the same way that other templates are created:
Specify the settings
Delete the document-specific data
Save the template
Access the template from a library location
To save the template, right-click the BOM and select Save As. In the Files of Type drop-down list, select Template (*.sldbomtbt, which stands for SolidWorks Bill of Materials Table Template). Any of the settings, additional columns, links to properties, and so on are saved to the template and reused when you create a new template from it.
Best Practice
Put the BOM template in your library area outside of the SolidWorks installation folder. Then put the path in the Tools
A table anchor locks a corner of the table to a selected point on the drawing sheet format. If no point is selected in the format, then the table is placed at a corner of the sheet. To specify a point in the format to act as the anchor, you must be editing the format. Right- click the sheet and select Edit Sheet Format). Then right-click a sketch endpoint in the format, select Set As Anchor, and specify which type of table the anchor is for. You can set different anchor locations for different types of tables. Figure 24.3 shows the selection and menus for this option.
Tip
You should save the format and drawing template with these table anchors specified so that you do not need to re-specify them for each new document. If you want to check a Sheet Format to see what anchors exist, you can expand the Sheet in the FeatureManager of the drawing.
You can use one of three BOM types in SolidWorks: Top-level only, Parts only, or indented.
As the name suggests, the Top-level only BOM only shows components on the top level. It treats subassemblies as a single entry. As a result, if the top-level assembly shown on the drawing is made up of five subassemblies and two individual parts, and you select the Top-level only option, then only seven items are shown in the BOM.
The Parts only BOM ignores subassembly structure and only displays parts in an un-indented list.
The Indented BOM shows the parts of subassemblies in an indented list under the name of the subassembly. This is the most complete list of SolidWorks documents used because it includes all parts and assemblies.
The Show Numbering option for indented assemblies is only activated after the Indented option is selected and you have placed the table. When you use this option, it causes subassembly parts to be numbered with an X.Y number system. For example, if item number 4 is a subassembly and it has three parts, those parts are numbered 4.1, 4.2, and 4.3.
The Configurations panel of the BOM PropertyManager displays slightly differently for Top-level only BOMs compared to the other types. The Top-level only BOM type enables the option to show multiple assembly configs and display the quantities for top-level components in separate columns, as shown in Figure 24.4. This figure shows that the configuration named "D" has some suppressed parts, including some parts that are now not used in the "D" configuration, and that therefore have a zero quantity. Notice the available options for dealing with zero-quantity parts.
When you are making changes to a model, parts are often either suppressed or deleted altogether. Some company documentation standards require that parts that are removed from a BOM remain on the bill and appear with strikethrough formatting, although this may be a relic from days gone by when it was more difficult to remove items from hand drawings.
Keep Missing Items and Zero Quantity Display have both been moved to Tools
The Zero Quantity Display settings are only used for configurations where some components are not used in some configurations. The three options that are available are
Quantity Of Dash. Substitutes a dash for the quantity value.
Quantity Of Zero. Uses a zero for the quantity value.
Blank. Quantity value is blank.
Item numbers for components listed in the BOM can start at a specific number and be given a particular interval. The Do not change item numbers option means that even when rows are reordered, item numbers stay with their original components.
The Follow Assembly Order option, which is also available through the right mouse button (RMB) menu, means that the order of the components in the BOM follows the order of the components in the Assembly FeatureManager. If the order is changed in the assembly, it also updates in the drawing.
The BOM Contents are handled by functionality available right on the BOM or through the RMB menu. Figure 24.5 shows a simple BOM with the RMB menu. For example, you can drag the row numbers to reorder BOM items, and right-click to hide them. Row numbers are only displayed after you select the BOM table.
You can add columns or rows to the BOM for additional properties or manually added parts (such as items you wouldn't model, like paint or glue). To change the property displayed in a column, double-click in the column header. In previous releases, many of the settings and options now found on the RMB menu were found in a more complex Bill of Materials Properties window. The newer arrangement is more intuitive. Most SolidWorks users know to try the RMB menu if they select something and don't get the option they are looking for in the PropertyManager.
If you are already familiar with formatting an Excel-based BOM, then you will quickly get used to formatting the SolidWorks table-based BOM. Figure 24.6 shows the table unselected on the left and selected on the right. While it's selected, you have access to a full range of appearance and organization options through the RMB menu.
To move the table, click outside the upper-left corner and drag the table to a new location. When the table is selected, a border appears around it that is not normally visible, and is not printed with the drawing. You can change the properties of a row or a column by selecting just outside of the row or column to the top or the left.
You can establish spacing and width of rows or columns by dragging the border on the left side of the column with the split cursor or by accessing the column width setting through Formatting in the RMB menu.
While it is activated, you can also expand a panel to the left and another to the top by clicking the three small arrows in the selected BOM border. Figure 24.7 shows the left panel, called the Assembly Structure panel, expanded with the cursor pointing to the three small arrows. In addition to showing the assembly structure, this panel can also show which parts are ballooned on the drawing.
Notice item 7 on the BOM. It has a different symbol and no name. This is a virtual component: a component created in context but not saved to its own document file; it exists only within the assembly.
You can dissolve an assembly in the BOM. To do this, the BOM has to show an indented list, then access Dissolve from the RMB menu on the assembly icon. Any restructuring done to the BOM can be deleted by RMB+clicking the assembly icon with red arrows and selecting Restore restructured components.
If the BOM shows several parts that are identical, and you would like to combine them, again, access the option from the RMB menu.
Item numbers in indented BOMs can be flat like 1, 2, 3, or they can be detailed like 1.1, 1.2, 1.3, 2, 2.1, 2.2 to reflect parts as members of subassemblies. This formatting option is available in the BOM Type panel in the BOM PropertyManager, under the Indented option.
To add a column, right-click near where you want to add the column, and choose Insert
One of the really beautiful aspects of custom property management in the BOM is that if you just type text in a column set up to be driven by a part property, SolidWorks automatically updates the part with the property. If the property didn't exist in the part previously, SolidWorks also creates the property. This is another very nice addition to the software.
Note
If you create a BOM with the columns and properties that you like, then you can save it to a template as described earlier in this chapter.
When you need to manually enter text in a BOM, for example in General Tables or custom properties in BOMs, starting in SolidWorks 2010, you can use the tab and arrow keys to move the cursor between cells. In fact, most of the Excel-like functionality has been added back into the SolidWorks native table format.
A summary of the added Navigation functionality is as follows:
Enter. Move to next cell down
Tab. Move to next cell to the right
Arrow. Move cursor in any direction
Shift+Arrow. Increases selection size
Shift+Tab. Move cursor backward
Shift+Enter. Move cursor up
Home. Move cursor to first column
Ctrl+Home. Move to upper left of table
End. In combination with arrow keys goes to end indicated
Ctrl+End. Move cursor to bottom right of table
A summary of the added Editing functionality is as follows:
F2. Edit contents of cell
Double-click. Edit contents of cell
Alt+Enter. Add multiple rows to cell
Delete. Delete contents of cell without activating cell
Backspace. Delete contents of cell and activate cell
Ctrl+Delete. Delete one word at a time
Edit. Edit multiple rows heights simultaneously
Lock. Lock row height and column width
Copy. Copy cells from Excel to SolidWorks tables
You can insert a Design Table into a drawing by choosing Insert
Design Tables that are displayed in this way are often formatted visually to some extent. It is necessary to hide columns and rows unless you want the dimension or feature name syntax to display on the drawing as well as the values. Extra columns and rows are often added to make the Design Table readable. The image to the left in Figure 24.10 shows a Design Table that is formatted to be placed on a drawing. The image to the right shows the same Design Table with all the information visible. The first column and the first row are hidden to make the table more readable on the drawing, and the second column and second row use the $user_notes header to format the names.
Figure 24.11 shows the drawing with the table inserted. To display the table properly, you have to edit the table in the window of the parent document and adjust the border of the table to be exactly how you want it to appear on the drawing. The adjusted table is shown in Figure 24.11.
The labeled dimensions were created by simply making reference dimensions and overwriting the <DIM> value in the Dimension Text panel of the Dimension PropertyManager. If you would like to examine this data more closely, the drawing and part are included on the CD-ROM. The drawing is named Chapter 24–DT.slddrw.
This drawing uses a part Design Table, but you can also place assembly Design Tables onto the drawing. This type of drawing is often called a tabulated drawing.
If you need to place something on your drawing such as a Design Table, but it does not appear that the Design Table is going to meet your needs, you may want to simply copy the data out of the Design Table and re-create it in a static Excel spreadsheet. The Design Table that you place on the drawing updates if it is changed in the part or assembly, just like the drawing geometry, but you must manually update an Excel spreadsheet that is created from copied data. Again, you must answer the question about whether the automatic functions make up for the cost of setting them up to work for you. In many cases they do, but in other cases they require more work than they save.
Like other table types, Hole Tables can use templates. As with other templates, you should locate Hole Table templates in a library area outside of your local SolidWorks installation folder. You can then direct SolidWorks to this location by choosing Tools
Hole Tables use anchors in exactly the same way as BOMs. For more information, see the section on table anchors earlier in this chapter.
Figure 24.12 shows the PropertyManager for a Hole Table. The image on the left is the PropertyManager you get when you create the table, and the one on the right is the one you get when you edit the table. Figure 24.13 shows the resulting Hole Table on a drawing with a part that contains holes. The table incorporates holes from multiple views, using a different zero reference for each view.
To initiate the Hole Table function, you must first select a view. You can access the Hole Table function by choosing Insert
To specify the datum, either select an edge in each direction to serve as the zero mark for the X and Y directions or select a vertex or point to serve as the Origin in both directions.
To select the holes to be included in the table, activate the Holes panel selection box, and either select the hole edges directly or select the faces on which the holes are located. Once you place the table, you can add holes or change the datum information. To do this, click on the RMB menu of the Hole Table entry in the Drawing FeatureManager, and select Edit Feature. The RMB menu is shown in the middle image of Figure 24.12. If you simply select a Hole Table that has already been created, the Properties interface displays, as shown in the top-right image. You can resize columns and rows in the same way as for BOM tables.
In the table in Figure 24.13, the Combine Same Sizes option is used, which causes several of the cells of the table to merge. If you use the Combine Same Tags option, then the hole locations are not displayed — only the hole callout description and the quantity appear. Figure 24.14 shows this arrangement.
You can control the hole callout description used in Figure 24.14 by using the file named calloutformat.txt, which is found in the langenglish subdirectory of the SolidWorks installation directory. Again, if you customize this file, then you should keep it in a library external to the installation directory and list it in the Tools
Figure 24.15 shows the Revision Table PropertyManager interface where you can create and control the settings for the table. You can find the default settings for Revision Tables by choosing Tools
The settings are now contained in a single PropertyManager; a toolbar and a RMB menu were formerly contained in five PropertyManager pages.
The image in the upper left of Figure 24.15 is the PropertyManager interface that displays when you initially create the Revision Table. The upper-right image is the RMB menu for the Revision Table, and the bottom toolbar is the formatting toolbar that displays when you select the Revision Table.
You can initiate the Revision Table function through the menus or the Tables toolbar. However, this function simply creates the table; it does not populate it. You must set the table anchor in the format in order for the Table Anchor to work. Additional columns may be added or formatted to accept other data. Once you have created the columns or formatting, you can save the changes to a template, which is also available through the RMB menu.
You can add a revision to the table by right-clicking the table and choosing Revisions
Immediately after you have created the revision, if the option is enabled, you are prompted to place a balloon that contains the revision level to identify what has been changed. To finish placing symbols, you can press Esc. When you are finished placing the balloons, you can fill in the description of the revision by double-clicking in the Description cell where you want to add text. Figure 24.16 shows a Revision Table with balloon symbols placed on the drawing.
Revision Tables work by creating a Revision custom property in the drawing document, and by incrementing this revision each time a revision is added to the table. Additional columns linked to custom properties can be added to Revision Tables and Revision Table templates.
Cross-Reference
Gauge Tables and Bend Tables are specific to sheet metal parts and are covered in detail in Chapter 29. Weldment Cut Lists are a special type of table that closely resembles a BOM table in many ways. These are discussed in Chapter 31, which covers Weldments.
The General Table uses the filename extension *.sldtbt. You can create it without a template, as a simple block of four empty cells, or you can use a template that has a set of pre-created headers.
Proponents of solid modeling have been saying for years that 2D drawings are going to disappear. I'm not convinced. Paper drawings will continue to be useful until all old manufacturing methods are abandoned, and I don't see that happening in my lifetime. People who use modern manufacturing methods have already eliminated drawings, but it may never happen across the board.
But because some companies rely on 2D and paper drawings less, the industry is developing new ways to create 2D-type documentation inside a 3D document. The ANSI Y14.41 standard is primarily about this transition.
SolidWorks is responding to this type of requirement by adding features that enable you to document the 3D data. Placing BOMs in assembly files is one way of doing this. Placing 2D type data into 3D model documents can reduce the need for paper or even electronic 2D documentation. Figure 24.17 shows a BOM inside an assembly model document.
It is a little tricky to get the relative scale correct between the table and the model. To do this, you have to adjust the zoom state of the model until it is fairly small within the screen, then place the table. After the table is placed, the assembly and the table zoom together. Most users get around this issue by viewing the table in a separate window.
Another type of table that you can use within a 3D model document is the Title Block table. You can use Title Block tables inside parts and assemblies. You can use them in the drawing to fill in information about the part or assembly, while avoiding creating a full 2D drawing.
Rather than having tutorials for every table type, this chapter has tutorials only for the BOM, Hole Table, and Revision Table. You can transfer the skills you use with these types to the other types.
This tutorial guides you through the steps that are necessary to prepare an assembly for the drawing and BOM. Configurations and custom properties are used in this example. Remember that if a drawing view is cross-hatched and you cannot see the geometry, then you may have to press Ctrl+Q to rebuild it. Follow these steps:
Begin this tutorial with SolidWorks closed and Windows Explorer open.
If you have not already done so, create a folder for a library that is not in your SolidWorks installation folder. Call it
D:Libraryor something similar. Make a folder inside this folder called Drawing Templates. Copy the files from the CD-ROM namedinch B.drwdot and inch B (no views).drwdotto this new folder.Launch SolidWorks and choose Tools
OptionsFile LocationsDocument Template. Click the Add button and add the new library path to the list. Shut down SolidWorks and restart it.Open the assembly Chapter 24 –
BOM Assy.sldasmfrom the CD-ROM.Click the Make Drawing From Part/Assembly button, make a new drawing of the assembly from the drawing template in the folder created in Steps 2 and 3.
Delete the isometric view, and in its place make a new drawing view using the named model view "exploded." If prompted to use true dimensions in an isometric view, click Accept.
Edit the sheet format. Right-click the sketch point at the location indicated in Figure 24.18. In the popup menu that appears, select Set as Anchor and then select Bill of Materials.
Exit Edit Sheet Format mode by selecting Edit Sheet from the RMB menu.
Select the new view and show it in the exploded state (right-click, Properties, Show in Exploded State). Then choose Insert
Click inside the exploded view, but not on any part geometry, and then select the Autoballoon tool from the Annotations toolbar. Toggle through the available options to see whether any of the possible autoballoon configurations meets your needs. If not, use the standard Balloon tool to select the part and place the balloon. This gives you more control over the attachment points and placement of the balloons.
Change the balloon for the short pin to be a circular split-line balloon (do this by clicking the balloon and then switching the style in the PropertyManager). Notice that the quantity appears in the bottom of the balloon. The drawing view and the BOM should now look like Figure 24.20.
Add a second leader to the balloon for the short pin by Ctrl-dragging the attachment point for the first leader from one pin to the other.
Notice that several of the parts use a default description of "description." Edit each of these parts by right-clicking the part's row in the BOM table and selecting Open <filename> from the menu. Change the Description custom property in each part. Keep in mind that this may be handled differently for configured parts.
The Bracket part is listed twice using the configuration name because of the way the configurations are set up for the parts. To list the bracket only once using the filename, open the bracket, RMB+click one of the configuration names in the ConfigurationManager, and select Properties. In the Bill of Materials Options panel, select Document Name from the drop-down list. Do this for the other configuration, as well.
Notice also that the Description field holds the configuration-specific custom property for Description, which is used in the BOM.
Toggle back to the drawing (pressing Ctrl+Tab), select anywhere on the BOM table, and then select Table Properties from the PropertyManager. Expand the Part Configuration Grouping panel, and select the Display all configurations of the same part as one item option. This changes how the bracket displays, as well as the pins.
Now add a column to the BOM that calls on an existing custom property that is already in all the parts. Place the cursor over the last column on the right and RMB+click it. Choose Insert
In the first drop-down selection box, select the Weight custom property. Click the green check mark icon to accept the changes. If the popup menu disappears and you need to get it back, double-click the column header, and it will reappear.
You can save the BOM with the additional column as a BOM template by right-clicking anywhere in the BOM and selecting Save As. You can then set the type to a BOM template and the directory to the library location for BOM templates.
If you would like to compare your results against mine, the finished drawing is called Chapter 24 – BOM Tutorial Finished.slddrw.
This tutorial guides you through creating and using setting changes that are common in SolidWorks Hole Tables. Follow these steps:
Create a new drawing from the inch B (no views).drwdot template. If you have not done the BOM tutorial, then move the drawing template named
inchB.drwdotfrom the Chapter 24 materials on the CD-ROM to your library location for drawing templates. Then create the drawing from the template.Click the Model View button on the Drawings toolbar, and browse to the part named Chapter 24 –
Hole Table Part.sldprt.Place a Front view and project a Left view and an isometric view. Then press Esc to quit the command. Finally, delete the four pre-defined views.
There is not an anchor in this template for a Hole Table. If you would like to create one, this would be a good time to do so. Follow the steps in the BOM tutorial for specifying the anchor point.
Click the Hole Table button in the Tables toolbar. Figure 24.22 shows a section of the Hole Table PropertyManager with the selections that you need to make for this Hole Table.
Once you have completed the selections, click the Next View button at the bottom of the PropertyManager, and make similar selections in the Left view. The holes for both views are added to a single Hole Table.
The table is created using the default settings established in Tools
OptionsDocument PropertiesTables, but you can change them here for this specific table. Click anywhere in the table, and then select Table Properties at the bottom of the PropertyManager. Changing from numerical to alphabetical assigns a letter to each hole type and a number to each instance of the type. Make this change and update the table. Figure 24.23 shows the table before and after the changes.Change the number of decimal places used in the Hole Table from two places to three. You can do this in the PropertyManager.
Deselect the Hide Hole Centers option in the Visibility panel.
Select the Combine same sizes option in the PropertyManager. This demonstrates a much cleaner table and would be a good thing to have in the tutorial.
Save the drawing.
In this tutorial, you create a basic Revision Table and make a template. Follow these steps:
Using a drawing that you completed in one of the previous tutorials, make sure that a Revision Table Anchor has been placed in the upper-right corner of the Sheet Format. You must edit the Sheet Format to do this by RMB+clicking the point that you want to use for the anchor. Remember to select Edit Sheet from the RMB menu to exit Edit Sheet Format mode.
Note
Ideally, the anchors for all table types should be set in templates and formats, but it is set up here to give you some practice creating the anchors.
Click the Revision Table button on the Tables toolbar. Select the Attach to Anchor option in the PropertyManager. Click the green check mark icon to accept the table. Figure 24.24 shows the initial stub of the Revision Table.
Tip
Drawing templates can be saved with the Revision Table stub if it also has a format. The Revision Table is not saved with the format because it has to go on the drawing sheet.
To initiate a new revision level in the Revision Table, RMB+click the table and choose Revisions
Add Revision.Depending on the default settings in Tools
OptionsDocument PropertiesDrafting StandardTablesRevision, the first revision will be either A or 1. If you are using PDMWorks Workgroup, then you may have other options.Depending on your options settings, you may immediately be prompted to place a balloon that contains the new revision level. You can place balloons with or without leaders. The balloons are meant to indicate areas of the drawing that are affected by the revision. Press Esc when you are finished placing the balloons.
Note
Be careful when using balloons on assembly drawings or other drawings that already have balloons on them for other purposes. It may be a good idea to use a distinctively shaped balloon for Revision Tables.
To add text to the Description field, simply click in the field and start typing. The text automatically wraps to fit the box.
Practice by adding a couple of revisions, balloons, and descriptions.
After you have added a couple of revisions, check the custom properties by choosing File
PropertiesCustom. Notice that a revision property has been added, and the latest revision is represented by the value of the custom property.
Note
The number of revisions kept in the Revision Table is no longer an option as it was in previous releases, but in its place you can now control how Revision Tables interact with multiple sheets. For more information, see Appendix B.
You can add columns in the same way that they were added to the BOM. You can merge and unmerge cells, and link properties to cells. With the cursor over the last column (Approved), RMB+click and choose Insert
Save the template by right-clicking anywhere in the Revision Table and choosing Save As
Rev Table Templates. Then save it to the appropriate location outside the SolidWorks installation directory.
SolidWorks enables you to work with both tables that are highly specialized for particular uses, and General Tables, which are available for any type of tabulated data. The most frequently used types are BOMs, Hole Tables, and Revision Tables. Design Tables that drive part and assembly configurations can also be placed on a 2D drawing, but in these cases, some formatting is usually necessary to make the Design Table presentable and the information on it easy to read.
Other types of tables, such as Gauge Tables and Bend Tables, and Weldment Cut Lists are specialized for sheet metal and weldment parts, respectively, and are discussed in chapters that cover those topics.