SOLIDWORKS Design Table: Create Part Configurations from Excel

Direct answer: a SOLIDWORKS design table is an embedded Excel sheet where each row is a configuration and each column controls one parameter, such as a dimension (D1@Sketch1), a feature’s suppression state ($STATE@Fillet1), or a BOM part number ($PARTNUMBER). Insert it with Insert > Tables > Design Table, let SOLIDWORKS auto-create the columns for the dimensions you pick, add one row per variant, close Excel, and rebuild each configuration to check it.

This tutorial is for mechanical engineers at equipment makers who maintain families of similar parts: plates in several lengths, brackets with and without holes, or spacers in a range of thicknesses. Use a practice part first.

When a design table is the right tool

Configurations can be created one by one in ConfigurationManager. A design table is better when:

• you have more than a few variants and they differ in the same handful of values;
• you want the full variant list visible in one grid for review;
• part numbers and descriptions must stay consistent with the variants they describe.

It is not the right tool when variants differ in topology so much that most features are suppressed in most rows. In that case, separate parts are often easier to maintain.

Step 1: Prepare the model

1. Build the base part fully defined. A sketch that is still under defined will move unpredictably when the table drives a dimension; the under-defined sketch tutorial shows how to find the missing constraint.
2. Rename the dimensions you will drive. Double-click a dimension and give it a meaningful name, for example Length@Base and HoleDia@Holes. The design table headers use these names, so clear names make the table readable.
3. Rename the features you may suppress, for example SlotCut instead of Cut-Extrude3.

Example used in this guide: a mounting plate with length, width, thickness and an optional slot.

Step 2: Insert the design table

1. Choose Insert > Tables > Design Table.
2. In the PropertyManager, choose Source: Auto-create.
3. Under Edit Control, choose whether the model may change the table. For a controlled family, many teams pick Block model edits that would update the design table, so the table remains the single source.
4. Under Options, decide whether new parameters and configurations added in the model are added to the table automatically.
5. Click OK, then select the dimensions to include (Length, Width, Thickness) in the dialog that appears.

An Excel sheet opens inside SOLIDWORKS. Row 2 holds headers; the first column holds configuration names; the first data row is the current (Default) configuration.

Step 3: Add the variants

Add one row per configuration. Example (values invented for practice):

Configuration	Length@Base	Width@Base	Thickness@Base	$STATE@SlotCut	$PARTNUMBER	$DESCRIPTION
PL-200	200	80	6	S	PL-200	Plate 200 x 80 x 6
PL-300	300	80	6	S	PL-300	Plate 300 x 80 x 6
PL-300-SLOT	300	80	6	U	PL-300-SLOT	Plate 300 slot
PL-400	400	100	8	U	PL-400	Plate 400 x 100 x 8

Header notes:

• Dimensions: DimensionName@SketchOrFeatureName, in the part’s units.
• $STATE@FeatureName: S (suppressed) or U (unsuppressed).
• $PARTNUMBER: the part number shown in a BOM for that configuration. Use $C to use the configuration name, $D for the document name, or type a value.
• $DESCRIPTION: the configuration description.
• $PRP@Property: a configuration-specific custom property, for example $PRP@Material Code.

Click outside the sheet in the graphics area to close Excel. SOLIDWORKS reports the configurations it created.

Step 4: Check every configuration

1. In ConfigurationManager, double-click each configuration.
2. Press Ctrl+Q to force a rebuild and watch for errors.
3. Measure one controlled dimension per configuration to confirm the table drove it.
4. Check that suppressed features really are suppressed only where intended.
5. Open File > Properties > Configuration Specific to confirm the part number and description.

A failing row is usually a bad header name, a unit mismatch, or a value that makes geometry impossible (for example, a slot longer than the plate). Fix the cell, rebuild, and re-check that row.

Step 5: Use the configurations in an assembly and BOM

Insert the part into an assembly and pick the configuration in the component properties. In a BOM, each configuration appears with the part number set by $PARTNUMBER. If the BOM shows something different, the column might be reading another property, or the configuration’s BOM option might be overriding it; the BOM part numbers and configurations tutorial shows how to trace the four values behind a displayed number.

Editing the table later

• Right-click Design Table in ConfigurationManager and choose Edit Table (in place) or Edit Table in New Window.
• To add a parameter later, add a column with the exact header syntax, or edit the dimension in the model if the table is set to accept model edits.
• Keep one source. If edits happen both in the model and in the table, values drift. Decide which one is authoritative and set Edit Control to match.
• Linked Excel files: a design table can be linked to an external Excel file. This suits teams who maintain variant lists outside CAD, but the link must be updated and the file controlled like any other engineering record.

Common problems and fixes

“Unable to resolve header” – the header text does not exactly match a dimension or feature name. Copy the name from the dimension properties.

Values ignored after closing Excel – the cell was still in edit mode, or Edit Control blocks the change. Re-open the table, press Enter in the cell, and close again.

A configuration rebuilds with errors – geometry fails for that combination of values. Check sketch relations and the feature order, not only the numbers.

BOM groups different variants into one row – two rows share the same $PARTNUMBER. Give each configuration its own approved part number.

Mates break when switching configurations in an assembly – a face referenced by a mate is removed in one configuration (for example by suppressing a feature). Mate to faces or planes that exist in every configuration; see the mates troubleshooting guide.

Practice checklist

• [ ] Base part fully defined; dimensions and features renamed
• [ ] Design table inserted with Auto-create and the intended Edit Control
• [ ] One row per variant with dimension, $STATE, $PARTNUMBER and $DESCRIPTION columns
• [ ] Every configuration rebuilt and measured
• [ ] Part numbers confirmed in properties and in a test BOM
• [ ] One authoritative source for values decided and documented

From configured parts to configured equipment

Design tables handle variation inside one part. Equipment makers also face variation in which parts are used and where they go for each order. MST AI Engineer addresses that level with three modules: drawing to model, layout and connections, and mechanical assembly AI, which places approved parts from your library into a native, editable SOLIDWORKS assembly. Read more on SOLIDWORKS assembly automation for configured equipment or watch the native assembly demo.

FAQ

Do I need Excel installed to use design tables? Yes. SOLIDWORKS uses an installed Microsoft Excel to create and edit design tables.

Can a design table drive an assembly? Yes. Assembly design tables can control component configurations, suppression and assembly-level dimensions such as mate distances.

Can I delete the design table and keep the configurations? Yes. Deleting the table leaves the configurations, but they will no longer be driven from one grid.

What is the difference between a design table and a configuration table? A configuration table is an in-SOLIDWORKS grid for configuration-specific values; a design table is Excel-based and supports more parameter types and formulas.

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Managing part families across many equipment orders? Request a team trial for your design team and bring a real configured product. We will work through it with your own parts in SOLIDWORKS. Request a team trial →

FOR EQUIPMENT MANUFACTURERS AND DESIGN TEAMS

Talk to the engineering team.

Tell us what your team designs and which repetitive task you want to improve. A short, non-confidential description is enough to discuss a relevant demo. Arrange a private channel with MST before sharing company drawings or models.

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