How to Create a Drawing Template in SolidWorks and CATIA V5

A well-built drawing template in SolidWorks or CATIA V5 is a one-time investment that pays back every time a drawing is created — consistent title blocks, automatic BOM linkage, and company-standard annotations eliminate rework and ensure every drawing that leaves the department meets the same quality standard.

Drawing templates are the foundation of a consistent engineering documentation system. Without a template, every engineer recreates the title block from scratch, chooses their own annotation standards, and formats views differently — resulting in a drawing library that looks like it was made by entirely different companies. With a well-built template, the drawing framework is automatic, the BOM is pre-linked to model properties, and the revision block is ready to receive ECO entries. This article walks through the key elements of building a production-quality drawing template in both SolidWorks and CATIA V5, covering title block setup, sheet format vs. template, layer and annotation standards, and BOM configuration.

Sheet Format vs Drawing Template: Understanding the Distinction

In both SolidWorks and CATIA, two separate elements define the drawing environment:

Sheet format (SolidWorks) / Frame and Title Block (CATIA): The background layer of the drawing sheet — the border, title block, revision block, and company logo. This is non-editable in the normal drawing environment. Engineers view it but cannot accidentally modify it. Changes require explicitly editing the sheet format. In SolidWorks, these are .slddrt files; in CATIA V5, these are Frames and Title Blocks stored in the CATDrawing file or in a separate catalog.

Drawing template (SolidWorks) / Drawing standard (CATIA): The initial state of the drawing file — which sheet format is applied, what drawing standard is used (ASME, ISO, JIS), what font and text height are set, which layers exist, and what annotation styles are defined. In SolidWorks, templates are .drwdot files; in CATIA V5, they can be standard .CATDrawing files used as starting points or configured through the drafting standards XML files.

The workflow: the template loads the sheet format automatically. Engineers open the template to create a new drawing, and the sheet format/border/title block are already in place.

Title Block Setup: Required Fields

The title block should contain linked fields (notes) that automatically populate from model or drawing properties, and static fields that are manually filled in:

Automatically populated fields (linked to properties):

• Part number / drawing number (linked to the model’s “PartNumber” or “DrawingNumber” custom property)
• Description / title (linked to “Description” property)
• Material (linked to “Material” property)
• Revision (linked to “Revision” property)
• Sheet number and total sheets (built-in variables — “$SHEET” and “$SHEETTOTAL” in SolidWorks; auto-filled in CATIA)
• Scale (linked to the sheet scale setting)
• File name (as backup reference)
• Date created / date modified (can be linked to file system date or custom property)

Static or manually filled fields:

• Company name and logo (placed as a picture or vector graphic in the sheet format)
• Projection angle symbol (first or third angle — a standard element placed once in the sheet format)
• General tolerances note (standard company tolerance class — e.g., “UNLESS OTHERWISE NOTED: ±0.1 mm LINEAR, ±0.5° ANGULAR”)
• Signature fields (designed by, checked by, approved by) with date lines — manually signed or digitally signed per company procedure
• Weight field (can be linked to SolidWorks mass properties; requires configuration)

SolidWorks: Building the Sheet Format

To create or modify a sheet format in SolidWorks:

• Step 1: Open a new drawing (or existing drawing). Right-click the sheet tab → Edit Sheet Format. The background elements become editable.
• Step 2: Draw the border using lines (or import an existing DXF border). Use the Sheet Properties to set the sheet size (A4, A3, A1, etc.) and match border dimensions to the sheet.
• Step 3: Draw the title block table in the lower-right corner using lines. Ensure all cell boundaries are aligned precisely — misaligned title blocks look unprofessional and reflect poorly on the engineering organization.
• Step 4: Add notes in each cell. For linked fields: Insert → Annotations → Note, then in the note text, type $PRPSHEET:”PropertyName” to link to a custom property from the drawing or $PRP:”PropertyName” to link to the referenced model’s property. For example: $PRPSHEET:”DrawnBy” links to a drawing-level property; $PRP:”Material” links to the material property of the model referenced on the sheet.
• Step 5: Insert the company logo using Insert → Picture. Scale and position in the designated logo cell. Embed the image (not link) for portability.
• Step 6: Add the projection angle symbol. Draw a simple first-angle or third-angle symbol using lines and circles in the title block, or insert a saved symbol block.
• Step 7: Exit sheet format edit mode (right-click → Edit Sheet). Save as .slddrt in the designated company template folder.

SolidWorks: Building the Drawing Template (.drwdot)

• Step 1: Open a new drawing, selecting the sheet format created above.
• Step 2: Set the drawing standard: Tools → Options → Document Properties → Drafting Standard. Select ASME, ISO, or custom. This controls dimension style, text height, arrowhead style, and GD&T symbol appearance.
• Step 3: Configure dimension styles: set font, text height, decimal places, and tolerance display format per company standard.
• Step 4: Configure annotation styles: note font, balloon style, surface finish symbol version (ISO 1302:2002 or earlier), GD&T frame style.
• Step 5: Set layer definitions (see Layer Setup section below).
• Step 6: Add standard notes to the drawing (not the sheet format) — the general tolerance note, material note placeholder, and any other company-standard notes that appear on every drawing. These are editable when the template is used.
• Step 7: File → Save As → .drwdot (Drawing Template). Save to the designated company template folder registered in Tools → Options → System Options → File Locations → Document Templates.

CATIA V5: Drafting Standards and Title Block Setup

CATIA V5 drawing standards are defined in XML files under the CATDraftingStandards catalog. To configure a company standard:

• Step 1: Navigate to the CATIA installation’s DraftingStandards folder and copy an existing standard XML (e.g., ISO.xml) to a company-specific file (e.g., CompanyISO.xml).
• Step 2: Edit the XML to configure: dimension text height, line types and weights, GD&T frame style, annotation styles, and tolerancing standards. These settings govern the appearance of all annotations created in CATIA drawings using this standard.
• Step 3: Register the company standard in Tools → Options → Mechanical Design → Drafting → Standard File, pointing to the custom XML.
• Step 4: For the title block, CATIA uses a “Frame and Title Block” approach. The title block is created in a dedicated CATDrawing or as a template in the drawing frame catalog. Use Insert → Drawing → Frame and Title Block → Manage Frames and Title Blocks to assign the company frame.
• Step 5: Title block fields in CATIA can be linked to Part Properties via formulas. In the title block text, reference document properties that were set on the 3D part (Part Number, Nomenclature, Description, Material, Revision). CATIA passes these properties to the drawing automatically when the part is projected.
• Step 6: Save a .CATDrawing file with the company frame applied, company standard set, and standard layers configured as the template. Distribute to all users via a shared network location or PDM system.

Layer Setup for Drawing Templates

Layers allow different annotation types to be shown or hidden and printed in different line weights. A standard layer scheme for engineering drawings:

Layer Name	Content	Line Weight	Color
0 or DEFAULT	Visible part outlines (auto-generated views)	0.5 mm	Black
HIDDEN	Hidden lines	0.25 mm	Black (dashed)
CENTERLINE	Center lines, axes	0.18 mm	Black (chain)
DIMENSIONS	Dimension annotations	0.25 mm	Black
NOTES	Text notes and callouts	0.25 mm	Black
GDT	GD&T feature control frames	0.25 mm	Black
SURF_FINISH	Surface texture symbols	0.25 mm	Black
TITLE_BLOCK	Title block (read-only in drawing)	0.35 mm	Black
CONSTRUCTION	Construction geometry (non-printing)	Any	Gray (no print)

BOM Template Linkage

A BOM (Bill of Materials) table pre-configured in the drawing template saves significant time on assembly drawings:

SolidWorks BOM setup in template:

• Insert → Tables → Bill of Materials. Select BOM type (Top-Level Only, Parts Only, or Indented). Choose which columns appear (Item Number, Qty, Part Number, Description, Material, Mass, etc.) and set column widths.
• Save the BOM table format as a .sldbomtbt (BOM template) file. Reference this template file in the drawing template via Insert → Tables → Bill of Materials → select saved template.
• BOM entries auto-populate from model custom properties. Ensure the part models set the same property names that the BOM template expects (e.g., “PartNumber” not “Part Number” — SolidWorks property names are case-sensitive and space-sensitive).

CATIA V5 BOM setup:

• CATIA’s Bill of Material function (Analyze → Bill of Material) generates the BOM from the product structure. For drawings, a BOM table can be inserted via Insert → Table → Bill of Material (Drafting workbench).
• Configure the BOM table format — columns (Part Number, Nomenclature, Description, Quantity, Material) and link each column to the corresponding product attribute.
• Save the BOM table as a saved view or as part of the drawing template to ensure consistent format on all assembly drawings.

Revision Block Setup

The revision block should be pre-formatted with the correct columns (Rev, Description, Date, By, ECO#) and have rows ready for the first few revisions. Including at least 5–7 blank revision rows in the template avoids reformatting on every drawing that undergoes revisions. The revision block should be in the sheet format (non-editable background) but with the data cells accessible when editing the sheet format.

In SolidWorks, the current revision can be stored as a drawing custom property and linked to the “REV” field in the title block. When the revision is updated (via ECO process), updating the drawing property automatically updates the title block revision indicator.

Distributing and Maintaining Templates

• Store template files in a shared network location accessible to all engineers, registered in each workstation’s CAD system file locations settings
• Control templates under version control — treat template files like controlled engineering documents with revision history
• When the company logo, standard, or title block format changes, update the template centrally and communicate to all users with the effective date
• Include a “drawing created from template version” property in the drawing to track which template was used for each drawing — useful during template transitions

Conclusion

A well-built drawing template in SolidWorks or CATIA V5 is infrastructure investment that pays back immediately and continuously. Title blocks auto-populated from model properties eliminate manual entry errors; consistent annotation standards ensure every drawing communicates the same way; pre-configured BOM tables and revision blocks save setup time on every new drawing. The one-time effort to build the template correctly — with proper property linkages, layer structure, company logo, projection symbol, and BOM format — results in a drawing department that produces consistent, professional documentation at higher speed with fewer errors. Templates should be treated as controlled engineering documents, updated through a governed process, and distributed centrally to ensure the entire organization is always working from the same standard.