DDi Tech Center

Creating inspection reports for SolidWorks models manually takes time and creates redundant work since the CAD models themselves are capable of being toleranced. Using a Design Table to control dimensions and tolerances allows users to create an inspection report in Excel while still controlling the dimensions for the SolidWorks model.

The first step after creating the model is linking the dimensions to a design table. Doing some up-front planning in naming sketches and dimensions will aid in making the Design Table more intelligent and easier to use outside of SolidWorks. A dimension can be named by changing the default system name shown in the Property Manager when the dimension is selected.

Features can be renamed by slowly single clicking twice on the feature or by selecting the feature in the Feature Tree and tapping F2 on the keyboard.

Keeping the names short, meaningful and having no spaces is a good idea although not a requirement.

Once the features and sketches are named inserting a Design Table is the next step. Selecting Insert > Tables > Design Table will start the command. Select Auto-Create and then select the dimensions to be controlled when prompted. Left click back in the modeling area once the dimensions appear in the Design Table. This will close Excel and return the system focus to SolidWorks.

Review the Configuration Manager tree to ensure the Design Table is in place and that the existing configuration is shown as being controlled by Excel.

If you get stuck the SolidWorks Help file can provide concise instructions on the step-by-step details for this portion or contact us in support.

So now the model is tied to Excel. The next step is to add the tolerancing for each of the controlling dimensions and then create a second sheet to serve as the inspection report. This will be done more simply by opening the Excel Design Table in a new window (right click on the Design Table and select Open in New Window).

To control a tolerance for a given dimension a new column needs to be created in the design table. The column header should have the following syntax: $tolerance@DimensionName@SketchName.

For example, a dimension named ‘Length’ on Sketch1 which had a symmetric tolerance of ±0.004″ would be controlled in a Design Table by the syntax ‘$tolerance@Length@Sketch1′. The value in the controlling cell in Excel would be ‘Symmetric;0.004′.

The value in the design table will depend on the type of tolerance desired. The syntax for the available tolerance types are:

• NONE
• BASIC
• MIN
• MAX
• BILATERAL;<max_variation>;<min_variation>
• LIMIT;<max_variation>;<min_variation>
• SYMMETRIC;<max_variation>
• FIT;<class>;<hole_fit>;<shaft_fit>;<type_fit>;<max_variation>;<min_variation>
• FIT_WITH_TOLERANCE;<class>;<hole_fit>;<shaft_fit>;<type>;<max_variation>;<min_variation>
• FIT_TOLERANCE_ONLY;<class>;<hole_fit>;<shaft_fit>;<type>;<max_variation>;<min_variation>

The values for the tolerance variation can also be linked to other cells in Excel. For example, if it is desired to have the tolerance shown on the Inspection Report then enter the variation on the Inspection Report sheet and then link the values to the tolerance specification cell. The screenshots below will make this clearer.

Once the tolerance values are entered into the Design Table it is best to save and close the file and return to SolidWorks to test the settings. If everything is correct the tolerance values should be shown on the dimension and should be modifiable through the design table.

Once the design table is functioning the rest is just Excel work. One caveat is that the first sheet in the Excel Design Table must be named Sheet1 and must remain the first sheet in the Design Table file for the connectivity to the SolidWorks model to remain intact.

Create a new sheet in Excel and create the form per company standards, if applicable. In addition to the dimensions and tolerances users can add file properties to the Design Table which in turn control the SolidWorks model as well as propagate to the Inspection Report sheet if mapped correctly. For example, a SolidWorks Custom Property named ‘Part_Number’ would be controlled in a Design Table with the syntax of ‘$prp@Part_Number’.

Additionally, in order to get the Inspection Report to be functional some creative formula writing will be required. The example was done using cell references in certain areas and concatenating values in other areas.
Here are some example concatenate formulas:

=CONCATENATE(‘Inspection Report’!C11,’Inspection Report’!D11)
‘Inspection Report’!C11 = Symmetric
‘Inspection Report’!D11 = 0.004

=CONCATENATE(‘Inspection Report’!C12,’Inspection Report’!J7,’Inspection Report’!D12,’Inspection Report’!J7,’Inspection Report’!E12)
‘Inspection Report’!C12 = Bilateral
‘Inspection Report’!J7 = ; (this character can be hidden in any cell on the inspection report; it is required as a separator in the Excel Concatenate  formula).
‘Inspection Report’!D12 = 0.010 (serves as the Max Variation)
‘Inspection Report’!E12 = 0.005 (serves as the Min Variation)