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How to change font size on SolidWorks drawing?

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Engineering drawings are the main communication link between design, manufacturing, and quality. Even a perfectly modeled part can cause mistakes if the drawing is crowded, unreadable, or uses inconsistent text sizes. That’s why controlling font size in SolidWorks drawings is important both for readability and for complying with your company or industry drafting standards.

In SolidWorks you can control fonts at three levels:

  • Title block / sheet format – company name, drawing title, revision, etc.
  • Document defaults – global font for dimensions, notes, balloons, and other annotations.
  • Individual annotations – override the font for one specific dimension or note.

This article walks through all three, using a simple drawing of a plastic gear motor as an example. We’ll start from a common problem – an oversized title block – then cover dimensions, notes, and how to save your settings into templates so you only do this once.

1. Where font size is controlled in SolidWorks drawings

Before changing anything, it helps to understand where the settings live:

  1. Sheet format (title block)
    The sheet format controls everything “in the background”: title block, border, company logo, static notes. You edit this with
    Edit Sheet Format. Any fonts you change here affect the title block on that sheet.
  2. Document Properties
    Go to Tools > Options > Document Properties. Here you can define default fonts for:

    • All dimensions (and each type of dimension)
    • Notes, balloons, weld symbols, surface finish, etc.

    New annotations use these fonts as long as “Use document font” is enabled for them.

  3. Individual overrides
    Selecting a dimension, note, or balloon lets you override the document font for just that one item. This is useful for emphasis, but overusing it makes drawings harder to maintain.

The rest of the article uses this same structure: first fix the title block, then set defaults, then adjust specific annotations where needed.

2. Example: oversize title block text

Below is a drawing of a plastic gear motor showing only the outer dimensions of the product. In the title block, the drawing title is oversized and shifted out of place by default, which makes it unclear which part the drawing refers to.

We’ll start by fixing the title block font and position, then move on to dimension text and other annotations.

3. Changing the font size of text in the title block

Title block text belongs to the sheet format, so you must edit the sheet format, make your changes, and then return to the normal sheet.

3.1 Entering sheet-format editing mode

  1. Open your drawing.
  2. In the FeatureManager design tree, right‑click on Sheet Format1 (highlighted in yellow in the image) and choose
    Edit Sheet Format.Alternatively, you can right‑click in an empty area of the sheet (not on any view) and choose Edit Sheet Format.

You are now editing the background entities: border, title block, fixed notes, etc. Regular model views are “ghosted out” and cannot be selected.

3.2 Editing the title block text and font

  1. Click once on the title text in the title block to select it.
  2. Double‑click the text to activate editing. A text box and a formatting toolbar / PropertyManager will appear.
  3. Either:
    • Use the Formatting toolbar above the text, or
    • In the PropertyManager, find the Font button.
  4. Click Font…, then choose the desired:
    • Font family (e.g., Arial, ISO, or your company’s standard)
    • Style (regular, bold, italic)
    • Size (in points or document units, depending on your setup)
  5. Click OK to apply the change.
  6. Drag the text’s bounding box to reposition the title so it sits cleanly inside the title-block cell.

After adjusting the font size and moving the text, the drawing title now fits the title block and is easy to read.

3.3 Exiting sheet-format editing

  1. Right‑click in an empty area of the sheet.
  2. Select Edit Sheet to return to normal drawing-editing mode.

Your title block font changes now apply to this sheet. Later, we’ll see how to save this as a sheet-format file so every new drawing uses the same title-block fonts automatically.

4. Changing the font size of dimensions

Dimension fonts can be changed:

  • Globally for the entire drawing via Document Properties, or
  • Individually for just one dimension via its PropertyManager.

Best practice is to set a sensible global default and only override individual dimensions when there is a clear reason (for example, a key dimension you want to highlight on a manufacturing drawing).

4.1 Setting the default font for all dimensions

To change the default font size for all dimensions in a drawing:

  1. Open the drawing whose dimension fonts you want to adjust.
  2. Click Tools > Options (gear icon on the Standard toolbar).
  3. In the dialog, click the Document Properties tab.
  4. In the left-hand tree, select Dimensions.
  5. At the top of the right-hand side, click the Font… button.
    (You can also set fonts for specific dimension types, such as Linear, Angular, Diameter, etc., if you want them to differ.)
  6. In the font dialog, choose the required:
    • Font name
    • Style (regular, bold, italic)
    • Size (height) appropriate for your drawing scale and plotting standard
  7. Click OK to confirm the font, and OK again to close Options.

All dimensions that still have Use document font enabled will update to the new size. Any dimensions that were manually overridden will keep their individual settings.

4.2 Overriding the font size of a single dimension

Sometimes you need one dimension to stand out, or you’re working on a legacy drawing where only a few dimensions are wrong. In that case, change the font just for that dimension:

  1. Click on the dimension whose font size you want to change.
  2. In the PropertyManager on the left, go to the tab named Other.
  3. Find the Dimension font section.
  4. Uncheck Use document font.
  5. Click the Font… button.
  6. In the font dialog, set the new size (and any other style changes you need), then click OK.

A formatting window similar to the one used for title block text appears, but this time it controls only the selected dimension.

Here the dimension text size has been increased successfully, making it easier to read or to emphasize as a key value.

If later you want to return that dimension to the global setting, simply select it, go back to the Other tab, and re‑check Use document font.

5. Changing font size for notes, balloons, and other annotations

Notes and other annotations (surface finish symbols, weld symbols, balloons, etc.) work similarly to dimensions: there is a document-level default and per-annotation overrides.

5.1 Change the default font for notes (document level)

  1. Open a drawing.
  2. Click Tools > Options, then go to the Document Properties tab.
  3. Under Annotations, select Notes.
  4. Click Font… and set the desired typeface, style, and size.
  5. Click OK to apply, then OK again to close Options.

All new notes (and any existing notes that still use the document font) will now use this size. You can repeat the same process under Annotations > Balloons, Surface Finish, Weld Symbols, etc., to standardize all annotation fonts across the drawing.

5.2 Override the font of a specific note or label

  1. Select the note or label in the drawing.
  2. In the PropertyManager, look for the Document font (or similar) checkbox.
  3. Clear that checkbox.
  4. Click the Font… button that becomes active.
  5. Choose the desired size and style, then click OK.

This changes only the selected note or label. Use this sparingly so your drawing doesn’t end up with a patchwork of different text sizes.

6. Controlling how big text looks on screen (text scale & high‑resolution displays)

Sometimes the printed text size is correct, but on a high‑resolution monitor dimensions look tiny when you zoom out and huge when you zoom in. SolidWorks offers a setting that affects how annotations scale on screen:

  • Tools > Options > Document Properties > Detailing > Always display text at the same size

When this is enabled (primarily for parts and assemblies and 3D views), annotations are drawn at a nearly fixed screen size regardless of zoom level, which can improve readability during modeling. When it is disabled, text scales more strictly with the model, which can be important when exporting 3D PDFs or using model-based definition workflows.

Keep in mind:

  • This setting affects screen display, not the actual printed height of text on a 2D drawing.
  • The real control of drawn/printed text size is still the font size you choose for dimensions and notes in Document Properties and per-annotation overrides.

7. Saving your font settings to templates and sheet formats

If you only change fonts in a single drawing, every new drawing will revert to the old defaults. To make your settings stick, you should:

  • Save a customized sheet format (for the title block), and
  • Save a customized drawing template (for document-level font defaults).

7.1 Save the sheet format (title block fonts)

  1. Open a drawing where the title-block fonts are set the way you want.
  2. Right‑click in the sheet and select Edit Sheet Format.
  3. Confirm that the border, title block layout, and fonts are correct.
  4. Click File > Save Sheet Format….
  5. Save the file as a .slddrt sheet-format file in the folder SolidWorks uses for sheet formats (check under
    Tools > Options > System Options > File Locations > Sheet Formats).

From now on, when you create a new drawing or change sheet properties, you can choose this custom sheet format and get the same title-block fonts every time.

7.2 Save the drawing template (document font defaults)

  1. Open a new or existing drawing.
  2. Set up all Document Properties the way you want (dimensions, notes, balloons, Detailing options, etc.).
  3. Click File > Save As….
  4. In Save as type, choose Drawing Template (*.drwdot).
  5. Save the template in the folder listed under Tools > Options > System Options > File Locations > Document Templates.

When you start a new drawing using this template, it will automatically use the fonts and other settings you configured, so you don’t have to adjust them manually every time.

8. Choosing sensible font sizes for engineering drawings

Most companies base their drawing practices on standards such as ISO, ASME Y14.2/Y14.5, or a company-specific drafting standard. Those standards typically recommend minimum printed text heights for different types of text.

As a practical guideline (always check your local/company standard):

  • Dimensions & general notes: around 2.5–3 mm (≈0.10–0.12 in) when printed at full scale.
  • Title block info (part name, drawing title): often larger, e.g. 5–7 mm, so it stands out.
  • Sub-headings & section titles: typically between the two, e.g. 3.5–5 mm.

In SolidWorks, that means:

  • Choose font sizes so that, at the intended paper size (A4, A3, ANSI B, etc.), the printed text height meets these values.
  • Use one main font family (e.g., an ISO-style or Gothic block font) for all annotations to keep the drawing visually consistent.
  • Reserve bold or larger fonts for a few key items: drawing title, major section headers, or critical dimensions.

9. Quick FAQ & troubleshooting

Q: I changed the dimension font in Document Properties, but some dimensions didn’t update. Why?

Those dimensions probably have Use document font unchecked and an individual font override. Select each dimension, open the Other tab in the PropertyManager, and re‑enable Use document font to make them follow the global setting again.

Q: My title-block font keeps reverting when I start a new drawing.

You likely updated the sheet format in just one drawing. Make sure you edit the sheet format, change the fonts, and then use File > Save Sheet Format to save a reusable .slddrt file. Also ensure your drawing template is set up to use that sheet format.

Q: Do I have to change fonts on every sheet in a multi‑sheet drawing?

Each sheet can reference the same sheet format file, so the title block fonts will be consistent. If a sheet is using a different sheet format, switch it in the sheet’s Properties dialog to your standard format.

Q: The dimension text looks tiny on my 4K monitor but prints fine. What should I change?

If the printed size is correct, leave the drawing fonts alone. Instead adjust how text is displayed on screen: check the Always display text at the same size or Text scale settings under Document Properties > Detailing in parts/assemblies or adjust your Windows display scaling. That way you don’t break your plotted drawing standard just to make dimensions easier to see on screen.

Q: Is it better to use points or document units for font size?

Points are consistent across documents (1 pt = 1/72 inch), which some users prefer. Using document units can be more intuitive when you’re thinking in millimeters or inches for printed height. The most important thing is to pick values that produce readable printed text and then keep them consistent in your templates.

With these tools – sheet formats, Document Properties, and a few targeted overrides – you can make your SolidWorks drawings far more readable and professional, and you only have to do the setup once if you save everything into templates and sheet formats.

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