FreeCAD For Beginners: CAD Thinking Part 2

Step-by-Step FreeCAD CAD Thinking Tutorial Part 2: Modeling a Latch Part

Introduction

This tutorial supports the video that guides you through modeling a latch part in FreeCAD (version 0.21) using the Part Design workbench. You’ll learn to select an optimal side profile to minimize operations, create a sketch with additive geometry, remove negative space with a pocket, and add fillets for finishing. The tutorial compares the side profile approach (fewer operations) with the front profile approach (more operations) to emphasize model stability. It’s designed for intermediate FreeCAD users familiar with sketching and part design. Prerequisites include FreeCAD 0.21 and a previously modeled reference part (e.g., Part 1) for alignment.

Click here for video

Part 1, 2, 3 and 4 have been released.  Part 5 will be coming soon.

Step 1: Set Up a New Document and Link Reference Part

• Description: Create a new FreeCAD document and link a reference part to guide the latch’s placement.
• Instructions:
  1. Open FreeCAD 0.21 and select File > New to create a new document.
  2. Save the document as “Latch_Part.fcstd” (File > Save As).
  3. Open the reference part file (e.g., “Part1.fcstd”) in FreeCAD.
  4. In the reference part’s Tree View, select the main body (e.g., “Fillet”).
  5. Hold Alt, drag the selected body, and drop it into the new document’s tab to create a link.
  6. Alternatively, in the new document, switch to the Part workbench, click Make Link, select the reference part’s body, and confirm.
  7. Right-click the linked part, select Transform, and adjust its position (e.g., rotate or translate) to align with the intended latch position. Click OK.
  8. Go to View > Toggle Axis Cross to display the coordinate system for reference.
• Tips:
  • Save both files in the same folder to avoid broken links.
  • Use the linked part as a visual guide to ensure the latch aligns correctly in 3D space.

Step 2: Create the Base Sketch (XZ Plane)

• Description: Sketch the side profile of the latch part using additive geometry to form the main shape.
• Instructions:
  1. Switch to the Part Design workbench.
  2. Click Create Body and then Create Sketch on the XZ_Plane.
  3. Enable Auto Constraints and Avoid Redundant Auto Constraints in the sketcher settings.
  4. Use the Center and Endpoint Arc tool to create an arc with a Radius of 3 mm, starting from the origin.
  5. Use the Line tool to add a 17 mm horizontal line from the arc’s endpoint.
  6. Use the Endpoint and Rimpoint Arc tool to add an arc with a Radius of 16 mm, connecting to the line.
  7. Add a vertical Line of 2 mm from the second arc’s endpoint.
  8. Add a horizontal Line of 23 mm to connect back toward the origin.
  9. Add another vertical Line of 2 mm downward.
  10. Add a final Line to close the sketch, ensuring it aligns with the vertical axis using a Point on Object Constraint.
  11. Apply constraints:
      • Set the total length from the origin to the farthest point to 30 mm using a Horizontal Distance Constraint.
      • Apply Coincident Constraints to ensure all lines and arcs connect.
      • Apply Horizontal and Vertical Constraints to keep lines aligned.
  12. Verify the sketch is fully constrained (no degrees of freedom).
  13. If constraints fail, adjust points (e.g., ensure the final line connects to the vertical axis).
  14. Add two Circles for holes:
      • Set one circle’s Diameter to 3 mm and the other to 2 mm.
      • Position each 7 mm from the sketch’s endpoints using Horizontal Distance Constraints.
  15. Close the sketch and save the document.
• Tips:
  • Use additive geometry (building the shape piece by piece) for clarity, as opposed to subtractive methods (e.g., trimming a slot).
  • Measure distances on the technical drawing or screen if dimensions are unclear.

Step 3: Pad the Sketch

• Description: Extrude the sketch to create the latch’s solid geometry.
• Instructions:
  1. Select the sketch in the Tree View and click Pad.
  2. Set the Length to 21 mm (per the technical drawing).
  3. Disable Symmetric to Plane to pad in one direction only, as symmetry is unnecessary here.
  4. Click OK.
  5. Check the 3D view to confirm the pad aligns with the linked reference part.
• Tips:
  • Avoid symmetry in the pad to reduce operations, as mirroring isn’t needed yet.
  • Verify the pad direction matches the latch’s orientation.

Step 4: Create a Pocket for Negative Space (YZ Plane)

• Description: Remove material from the front profile using a pocket to form the latch’s inner geometry.
• Instructions:
  1. Switch to the front view (YZ_Plane) using the view toolbar.
  2. Create a new sketch on the YZ_Plane.
  3. Enable Sketch View Section to see inside the padded part.
  4. Use the External Geometry tool to import the top and side edges of the pad (e.g., the 2 mm wall).
  5. Use the Rectangle tool to sketch a rectangle enclosing the area to keep (e.g., a 2 mm wide wall).
  6. Apply constraints:
     • Set the rectangle’s width to 2 mm to match the wall.
     • Set the height to 6 mm (ensuring it exceeds the part’s height to remove all excess material).
     • Apply Symmetry Constraints to center the rectangle on the part’s midline.
     • Use Coincident Constraints to align with imported edges.
  7. Close the sketch.
  8. Select the sketch, click Pocket, and set it to Through All with Symmetric to Plane enabled to remove material on both sides.
  9. Click OK.
• Tips:
  • The pocket acts like a “cookie cutter,” keeping the sketched area and removing the rest.
  • Ensure the rectangle’s height is sufficient to avoid leftover faces.

Step 5: Add Fillets

• Description: Apply fillets to round off the latch’s top edges for pivoting functionality.
• Instructions:
  1. Select the top edges of the pocketed part (two edges where the latch will pivot).
  2. Click Fillet in the Part Design toolbar.
  3. Set the Fillet Radius to 1 mm (per the technical drawing).
  4. Click OK.
• Tips:
  • Select only the edges needing fillets to avoid unnecessary operations.
  • Check the technical drawing to confirm fillet placement and size.

Step 6: Verify with Reference Part

• Description: Ensure the latch aligns correctly with the linked reference part.
• Instructions:
  1. Unhide the linked part (press Spacebar in the Tree View).
  2. Visually inspect the latch’s alignment with the reference part in the 3D view.
  3. If misaligned, right-click the latch body, select Transform, and adjust its position or rotation. Click OK.
  4. Save the document.
• Tips:
  • Use the axis cross to guide transformations.
  • The linked part helps visualize the latch’s position for the upcoming assembly.

Step 7: Compare with Front Profile Approach

• Description: Highlight the efficiency of the side profile approach by comparing it to the front profile.
• Instructions:
  1. Note the side profile workflow used 3 operations: Pad, Pocket, and Fillet.
  2. The front profile approach requires more operations:
     • Pad for the initial shape.
     • Pocket to remove material for the inner profile.
     • Pocket for holes and arcs.
     • Fillet for the pivot edge.
     • Fillet to clean up another edge.
     • Mirror for symmetry.
  3. Recognize that the side profile reduces operations (3 vs. 6), improving model stability by minimizing the dependency chain.
• Tips:
  • Fewer operations reduce the risk of errors when modifying early features.
  • The side profile leverages negative space removal for simplicity.

Step 8: Finalize the Model

• Description: Verify the model and prepare for assembly.
• Instructions:
  1. Inspect the latch for errors (e.g., incorrect dimensions or missing features).
  2. Adjust sketches or constraints if needed to match the technical drawing.
  3. Save the file (File > Save).
• Tips:
  • Toggle the Axis Cross to confirm orientation.
  • Hide the linked part or sketches to reduce clutter in the Tree View.

Conclusion

You’ve modeled a latch part in FreeCAD using a side profile approach, creating a sketch with additive geometry, removing negative space with a pocket, and adding fillets. This method uses only three operations, making the model more stable than the front profile approach, which requires six operations. The linked reference part ensures proper alignment for assembly. If issues arise, check sketch constraints or pocket settings. The latch is now ready for assembly in the A2Plus workbench, as covered in a future tutorial. Save your work and refine as needed for precision.

Additional Resources

• FreeCAD Documentation
• FreeCAD Forum
• Support the creator: Ko-fi, Patreon