At some point, someone in your shop opens a SolidWorks part and gets this:

Microsoft Excel is required for gauge tables. Please ensure Excel is installed and try again.

The popup appears when the Sheet Metal feature dialog tries to open the gauge table file via OLE automation. If Excel is not present — or if it has been uninstalled after the company moved to Google Workspace or LibreOffice — the gauge table feature silently stops working.

This is not a misconfiguration. It is by design. SolidWorks gauge tables are Excel files that SolidWorks reads via COM at runtime. No Excel, no gauge tables. The 2023 SolidWorks system requirements still list Microsoft Office as required for gauge/bend tables.

The frustrating part: the underlying data — thickness values, bend radii, K-factors — is not complex. You do not need a spreadsheet application to store a table of three numbers. What follows covers the three approaches that give you consistent, accurate bend behaviour without an Office license.

What gauge tables actually do

Before reaching for an alternative, it helps to understand exactly which workflow depends on Excel and which does not.

A gauge table (C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\Sheet Metal Gauge Tables\*.xls) does two things:

  1. Populates the Gauge dropdown in the Sheet Metal feature dialog with named sizes (e.g., “14 GA”, “16 GA”). Selecting a gauge auto-fills the Thickness field.
  2. For each gauge, optionally sets the Bend Radius, K-Factor, Bend Allowance, or Bend Deduction — so when you change gauge, all the bend parameters update together.

If you never use the Gauge dropdown and always type thickness by hand, you are already working without gauge table data. The K-factor, bend radius, and bend deduction can all be entered directly in the feature dialog without referencing any table.

The Excel dependency only triggers when you click the Browse button next to the Gauge field and select a gauge table file.

Approach 1: Bend tables in BTL format

What it is: A bend table is a plain-text file with a .btl extension. It predates the current Excel-based gauge tables, originating in SolidWorks 2000 and earlier. SolidWorks still reads them in every current version including 2025.

What it does: A BTL file maps combinations of thickness and bend radius to a K-factor (or bend allowance/bend deduction). It does NOT handle thickness selection — you still enter the thickness manually. What it provides is automatic K-factor lookup based on whatever thickness and radius you set.

File structure:

A BTL file is tab-delimited plain text. Open it in Notepad, VS Code, or any text editor:

Description: Mild Steel Bend Allowance
Units: mm
Thickness	Radius	BendAllowance
0.800	1.000	0.620
0.800	2.000	0.750
0.800	3.000	0.895
1.000	1.000	0.750
1.000	2.000	0.900
1.000	3.000	1.050
1.200	1.500	0.980
1.500	2.000	1.200
2.000	3.000	1.680
2.000	4.000	1.850

The first two lines are a description and units declaration. The body is a three-column table: thickness, bend radius, and the calculated value (which can be K-factor, bend allowance, or bend deduction depending on the header label in line 3).

SolidWorks interpolates between rows when the actual thickness/radius combination falls between two entries. If you go outside the table range, SolidWorks falls back to whatever value is manually set in the feature.

How to reference it in SolidWorks:

In the Sheet Metal feature PropertyManager, find the Bend Allowance section. The dropdown offers K-Factor, Bend Allowance, Bend Deduction, and Bend Table. Select Bend Table. Browse to your .btl file. SolidWorks embeds a reference to the file path — if you move the file later, the reference breaks.

Store your BTL files in the same network share as your design library. If SolidWorks is installed on multiple machines, put them in a shared folder referenced via a mapped drive letter that is consistent across machines.

What you lose compared to gauge tables:

No automatic thickness selection. No named gauges in a dropdown. You type 1.5 into the thickness field; the bend table handles the K-factor from there. For shops where the modeller knows their stock gauges and types them directly, this is a non-issue.

Approach 2: K-factor defaults in the material database

SolidWorks materials (stored in .sldmat files, typically in C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\sldmaterials\) carry mechanical properties. What is less documented is that the material database also stores default Sheet Metal Bend Allowance parameters for each material.

How to set them:

  1. Open the material database via the material panel in any part, or via Tools → Material.
  2. Navigate to your material (e.g., AISI 1008 under Steel → Low Alloy Steel).
  3. Go to the Custom tab in the material editor.
  4. Add a property named BENDING or set the sheet metal defaults through the Sheet Metal tab if your SolidWorks installation shows it.

The cleaner path is through Document Properties:

  1. Open a sheet metal part template (.prtdot).
  2. Tools → Options → Document Properties → Sheet Metal.
  3. Set the K-factor, bend radius, and relief settings here as defaults for new sheet metal features.
  4. Save the template.

When a new sheet metal feature is created in a part based on this template, the K-factor and bend radius start from the template values rather than SolidWorks defaults.

Practical limitation: Material-database K-factor defaults apply per-material across all thicknesses and radii. Real material behaviour is not flat — 1 mm mild steel and 4 mm mild steel have different K-factors because the outer fibre stretch differs at different radius-to-thickness ratios. If your K-factor needs to vary by gauge (which is why gauge tables have multiple rows), a single material default is an approximation.

For shops bending one or two stock thicknesses, this approximation is acceptable. For shops bending the same material from 0.8 mm to 3 mm, the error compounds and the BTL approach with a proper table is more accurate.

The K-factor impact on flat pattern accuracy is described in detail in the DXF flat pattern dimensions post. The short version: a K-factor error of 0.05 on a part with six 90-degree bends in 1.5 mm mild steel produces a flat pattern error of roughly 0.45 mm — tolerable for plasma cutting, not for precise laser fits.

Approach 3: Part templates with pre-set values

The most overlooked approach: save part templates with the K-factor, material, and thickness pre-configured.

How it works:

  1. Create a new SolidWorks part.
  2. Add a Sheet Metal feature manually (Insert → Sheet Metal → Sheet Metal…).
  3. Set thickness, K-factor, and bend radius to the values for your most common stock (e.g., 1.5 mm, K = 0.42, radius = 1.5 mm).
  4. Apply the correct material via Tools → Material.
  5. Save as a part template: File → Save As → select Part Template (*.prtdot).

Create one template per common stock. Name them clearly: SM_1.5mm_MildSteel.prtdot, SM_3mm_Aluminium.prtdot.

When a modeller starts a new sheet metal part, they open the appropriate template and the bend parameters are already correct. No gauge table selection. No popup.

Where this breaks: if the modeller uses the wrong template, or if someone starts from a blank part (File → New → Part), the defaults revert to the SolidWorks installation defaults. This is a workflow discipline issue, not a technical one. Pairing templates with a clear naming convention keeps it under control.

Dealing with the vba71 / Excel prerequisite for related features

A separate but related issue: design tables and equation-driven tolerances use Excel via the VBA runtime (vba71.msi). If Excel is uninstalled but the VBA runtime is intact, design tables may still work. If Office is completely removed including VBA prerequisites, you will also lose:

  • Design tables in parts and assemblies
  • Gear Mate input from spreadsheet
  • Some Toolbox configuration tables

The fix is to reinstall just the VBA redistributable without reinstalling Office. The required installers are in the SolidWorks prerequisites directory:

C:\Program Files\Common Files\SOLIDWORKS Shared\SOLIDWORKS 20xx\setup\Administration\SWRequisites\

Look for vba71.msi and vba71_1033.msi. Run both. No Office reinstall required.

This does not restore gauge table functionality (that genuinely needs Excel COM), but it does restore design tables and equation-driven features that only need the VBA runtime.

  1. For bend accuracy: Create a BTL bend table for each material family your shop uses. Store it on a shared network path. Reference it in the Sheet Metal feature Bend Allowance → Bend Table. The K-factor lookup is automatic from that point.

  2. For thickness consistency: Build part templates for each common stock. The template contains the right thickness, material, K-factor (as fallback if the BTL file is unavailable), and bend radius for that stock.

  3. For team discipline: Add a shared folder reminder in your new-part checklist: “Did you use the SM template for this thickness?” This is the same discipline you need for drawing templates and title block properties.

  4. Leave gauge tables for what they are: If anyone on the team has Excel available and wants to set up proper gauge tables, they can — and the BTL approach and gauge table approach coexist. Parts that reference gauge tables work on machines with Excel; parts that use BTL bend tables work everywhere. The coexistence is clean.

The accuracy you get from a well-maintained BTL table is equivalent to a gauge table for the same data. The gap is only the named-gauge dropdown, which is a convenience, not a functional requirement. A shop that types 1.5 instead of selecting 16 GA will produce identical flat patterns once the K-factor lookup is in place.

For the downstream export step, CadShift reads the K-factor and bend allowance from whichever method the part uses — gauge table, BTL reference, or manual feature property — and applies it in the batch export. The batch DXF export guide covers what else happens between the flat pattern and the file the laser operator receives.