How to Create a New Title Block in SOLIDWORKS

A SOLIDWORKS title block identifies a drawing and gives manufacturing, inspection, purchasing, and revision teams the information they need to use it correctly. A useful title block normally includes the drawing number, part or assembly name, revision, material, scale, sheet number, drawn-by and checked-by fields, dates, units, tolerances, and company information.

The safest way to create one is to edit a drawing’s sheet format, build the border and notes, link repeatable fields to properties, define the editable title block area, and then save both the sheet format and drawing template. The sheet format controls visible items such as the border, logo, and title block. The drawing template stores document settings and points a new drawing to the chosen sheet format.

Before you edit the title block

Decide what information the drawing must communicate before drawing boxes and adding notes. A small internal drawing may need only basic identification and revision data. A released manufacturing drawing may also need general tolerances, projection method, surface-finish requirements, approval fields, proprietary notices, and a reference to the governing standard.

Keep the title block readable at the final printed size. Do not add fields merely because another company uses them. Every field should have an owner and a clear source. Information that already exists in model or drawing properties should usually be linked instead of typed manually on every sheet.

1. Create or open a drawing

1. Click File > New.
2. Select Drawing.
3. Choose a sheet size and an existing sheet format that is close to the result you need.
4. Confirm units, drafting standard, projection type, and document properties before investing time in the layout.

If you are updating an existing company format, work on a copy. That preserves the released template while you test note links, line weights, logo placement, and printing.

2. Enter Edit Sheet Format mode

Right-click a blank area of the sheet or the Sheet Format item in the FeatureManager design tree, then choose Edit Sheet Format. You can also use the Sheet Format CommandManager. In this mode, you edit the border, title block geometry, static notes, linked notes, and other background items rather than drawing views.

A common source of confusion is editing the drawing sheet instead of the sheet format. If drawing views can still be selected but the border cannot, you are probably not in Edit Sheet Format mode.

3. Build the border and title block grid

Use sketch lines, rectangles, dimensions, and relations to create the border and divide the title block into logical fields. Put the title block where your organization expects it, commonly in the lower-right corner. Keep line weights and spacing consistent, and leave enough room for the longest expected values.

Use a restrained layout. Drawing number, title, revision, and sheet number should be easy to find. Secondary information can use smaller fields, but it still needs to remain legible in PDF output and on a printed shop copy.

4. Add static and property-linked notes

Choose Annotations > Note and place the required labels and values. Static notes are appropriate for labels such as “DRAWING NUMBER,” a fixed company address, or a standard notice. Values that change between drawings should be linked to properties.

Use Link to Property in the Note PropertyManager to connect a note to a drawing property or to a property from the model shown in the drawing. Typical links include description, part number, material, revision, mass, finish, and drawn-by information. Choose the property source deliberately: a drawing-level property and a referenced-model property are not interchangeable.

Test every linked field with a sample model. A note that displays correctly in the template may become blank when the drawing has no referenced model, uses a different configuration, or lacks the expected custom property. For more on reusable metadata, see the guide to the SOLIDWORKS custom properties folder.

5. Define the editable title block fields

SOLIDWORKS can define a hotspot and a controlled list of notes that users edit when completing the title block. While editing the sheet format, choose Title Block Fields. Resize the rectangle over the intended title block area, then select the notes users should be able to enter or change.

Use the up and down controls in the Title Block Table PropertyManager to set the field order. That order controls how users move through the fields with the Tab key. Add clear tooltip text so someone completing the drawing knows what belongs in each field.

6. Save the sheet format and drawing template

Exit Edit Sheet Format mode and test the title block on a normal drawing. Then save the reusable pieces:

• Sheet format: save the visible border and title block as an .slddrt file.
• Drawing template: save the drawing document as a .drwdot file so document properties, units, drafting standard, layers, and the sheet-format reference are retained.

Store company-controlled formats and templates in a shared, backed-up location with clear names for paper size, units, standard, and revision. Configure the corresponding file locations in SOLIDWORKS so users do not browse to personal folders or outdated copies.

Test the title block before release

Create a new drawing from the template and verify the full workflow:

• Insert a part and an assembly that contain realistic custom properties.
• Check that model-linked and drawing-linked values populate from the intended source.
• Click the title block hotspot and tab through editable fields in the expected order.
• Confirm sheet number, sheet count, scale, units, and revision behavior.
• Export a PDF and inspect line weights, clipping, text size, and logo quality.
• Open a second sheet if the template supports multi-sheet drawings and confirm the format behaves consistently.

The final PDF is the practical test. A title block that looks acceptable at high zoom can still become cramped, faint, or clipped when printed.

Common title block problems

A linked value is blank

Confirm the property exists, check whether the note points to the drawing or referenced model, and verify the correct model or configuration is active in the drawing view.

The border cannot be selected

Enter Edit Sheet Format. Normal drawing mode is for views and annotations; sheet-format mode is for the border and title block background.

Changes affect only one drawing

Editing a drawing does not automatically update the reusable source files. Save the corrected .slddrt and, when needed, the .drwdot template in the controlled location.

The title block changes when the sheet size changes

Maintain separate sheet formats for the paper sizes your organization uses. A title block designed for one format may not scale or reposition cleanly on another.

Users overwrite values that should be automatic

Link repeatable values to properties and include only genuinely manual notes in the editable Title Block Fields list.

Bottom line

A reliable SOLIDWORKS title block is more than a rectangle with text. Build it in the sheet format, link changing values to the correct properties, define a clear hotspot and field order, save both the .slddrt and .drwdot files, and test the result on real drawings and exported PDFs. For broader drawing practice, see SOLIDWORKS detailing and drawing techniques and how to change a SOLIDWORKS sheet format.

Official references: Defining or Editing Title Blocks and Title Block Management.