Step-by-Step FreeCAD Tutorial: Creating a Tray with Reference Images

This tutorial helps support the original video which guides you through creating a tray in FreeCAD (version 0.21) using reference images for accurate geometry. You'll learn to import images, sketch parts with symmetry, create bevels with subtractive pipes, mirror components, and assemble the final model using the A2Plus workbench. This tutorial is designed for intermediate FreeCAD users familiar with basic sketching and navigation. Prerequisites include FreeCAD 0.21 and the A2Plus workbench installed.

Reference image for the video tutorial FreeCAD: Picture Frame / Tray Tracing, Modelling, Assembly. This image is loaded in through file > import (FreeCAD v0.21 and above) or via the image workbench (FreeCAD v0.20 and below and some earlier development versions of 0.21)

Step 1: Set Up a New Document and Import Reference Image

• Description: Create a new FreeCAD document and import a reference image to guide your design.
• Instructions:
  1. Open FreeCAD 0.21 and select File > New to create a new document.
  2. Go to File > Import, select your reference image (e.g., a tray top view), and click Open.
  3. The image is placed on a plane (default may vary). Double-click the image in the Tree View to open its properties.
  4. Set the plane to XY_Plane in the properties panel.
  5. Calibrate the image scale by selecting two points on the image (e.g., a known dimension like the tray's inside width).
  6. Click a corner for the first point, then the opposite corner for the second point. Enter 500 mm as the calibration length and click OK.
• Tips:
  • Ensure the image aligns with the top view for accurate sketching.
  • Zoom in for precise point placement during calibration.

Step 2: Adjust Reference Image Placement

• Description: Reposition the reference image to align with the desired sketch origin.
• Instructions:
  1. Select the reference image in the Tree View and go to the Data tab.
  2. Adjust the Placement properties (X, Y, Z axes) to center the image appropriately for sketching.
  3. Click OK to confirm the new position.
• Tips:
  • Small adjustments can be made by entering numerical values or dragging the image.
  • Hide the image temporarily (press Spacebar) to check alignment with sketches.

Step 3: Create the Top Body Sketch

• Description: Sketch the top part of the tray using symmetry to reduce complexity.
• Instructions:
  1. Switch to the Part Design workbench.
  2. Click Create Body to start a new body, then Create Sketch on the XY_Plane.
  3. Use the Polyline tool to sketch a quarter of the tray’s top edge, starting at a corner and connecting to the vertical axis (e.g., a flat line, then a vertical line).
  4. Right-click or press Escape twice to exit the tool.
  5. Add an angle constraint of 135 degrees between the lines.
  6. Apply length constraints: set the horizontal line to 240 mm and the vertical line to 45 mm.
  7. Add a vertical distance constraint of 145 mm between key points to lock the shape.
  8. Use the B-Spline tool to sketch a curved edge, starting from an endpoint and placing points at curvature changes.
  9. Right-click to finish the B-Spline, then tweak control points for smoothness.
  10. Use B-Spline Tools > Insert Knot to add knots for finer adjustments.
  11. Apply a Constrain Block to lock the B-Spline in place.
  12. Close the sketch.
• Tips:
  • Enable Auto Constraints and Auto Remove Redundant Constraints in the sketcher settings for efficiency.
  • Use symmetry to sketch only a quarter of the part, mirroring later.

Step 4: Extrude the Top Sketch

• Description: Extrude the sketch to create the top part’s solid geometry.
• Instructions:
  1. Select the sketch in the Tree View and click Pad.
  2. Set the extrusion length to 30 mm and click OK.
• Tips:
  • Adjust the extrusion length later if needed by editing the Pad feature.
  • Hide the reference image (press Spacebar) to inspect the extruded part.

Step 5: Create a Bevel with a Subtractive Pipe (Inner Profile)

• Description: Add a curved bevel to the top part using a subtractive pipe.
• Instructions:
  1. Select the top face of the extruded part and click Create Sketch.
  2. Use the External Geometry tool to import the edge where the bevel will be applied.
  3. Sketch a Circle as the bevel profile, centered near the imported edge.
  4. Add a Diameter constraint of 30 mm to the circle.
  5. Close the sketch and rename it to “Inner Profile” for clarity.
  6. Select the sketch, then click Subtractive Pipe.
  7. Add the imported edge as the path. If the pipe stops prematurely, proceed to the next step.
  8. Create a new sketch on the same face, import the same edge, and draw a line extending beyond the part’s boundary.
  9. Close the sketch, select the “Inner Profile” sketch, and create a new Subtractive Pipe using the line sketch as the path.
  10. Click OK to complete the bevel.
• Tips:
  • Lock profile geometry with constraints to reuse it later.
  • Ensure the path extends fully across the desired edge.

Step 6: Create an Outer Bevel Profile

• Description: Add a custom outer bevel using another subtractive pipe.
• Instructions:
  1. Select the top face again and click Create Sketch.
  2. Import the outer edge using the External Geometry tool.
  3. Use the Polyline tool to create a scraper-like profile (e.g., two vertical lines connected by an arc).
  4. Add constraints: set the arc diameter to 45 mm, vertical lines to 20 mm, and distances from the edge (e.g., 4 mm and 5 mm).
  5. Make the sketch’s origin coincident with a reference point for mapping later.
  6. Close the sketch and rename it to “Outer Profile”.
  7. Select the sketch, click Subtractive Pipe, and add the outer edge as the path.
  8. Click OK to apply the bevel.
• Tips:
  • Fully constrain the profile to prevent unintended movement when reused.
  • Check the profile alignment visually by toggling the reference image.

Step 7: Mirror the Top Body

• Description: Mirror the top part to complete its symmetrical geometry.
• Instructions:
  1. Select the Pad, Subtractive Pipe (Inner Profile), and Subtractive Pipe (Outer Profile) in order.
  2. Click Mirrored in the Part Design toolbar.
  3. Set the mirror plane to Base YZ Plane and click OK.
  4. Select the Mirrored feature, set Refine to True in the properties, and click OK to clean edges.
• Tips:
  • Select features in the correct order to avoid mirroring errors.
  • Check for overlapping faces; adjust the sketch if needed.

Step 8: Create the Side Body Sketch

• Description: Sketch the side part of the tray, referencing the top body.
• Instructions:
  1. Create a new Body and rename it “Side Body”.
  2. Click Create Sketch on the XY_Plane.
  3. Hide the Mirrored feature of the top body and show the Pad’s sketch (press Spacebar).
  4. Adjust the top body’s sketch placement by lowering it along the Z-axis (e.g., -1 mm) for visibility.
  5. In the side body sketch, use a Sub Shape Binder to import the top body’s sketch into the active body.
  6. Set the binder’s Make Face property to False.
  7. Import key points from the binder using the External Geometry tool.
  8. Use the Polyline tool to sketch a quarter of the side part, connecting to the horizontal axis.
  9. Add a B-Spline to create a curved edge, connecting to the imported points.
  10. Adjust B-Spline knots for smoothness.
  11. Create tangency by sketching a construction line between B-Spline control points and applying Point on Object constraints.
  12. Lock the B-Spline with a Constrain Block and set helper geometry to Construction mode.
  13. Close the sketch.
• Tips:
  • Use the sub shape binder to reference geometry across bodies safely.
  • Ensure tangency for smooth transitions between parts.

Step 9: Extrude the Side Sketch and Apply Bevels

• Description: Extrude the side sketch and reuse the top body’s bevel profiles.
• Instructions:
  1. Select the side sketch, click Pad, and set the length to 30 mm.
  2. Go to the top body, select the “Inner Profile” sketch, and adjust its Map Mode to attach to a vertex and edge on the Pad (use Normal to Edge).
  3. Switch to the Draft workbench, select the “Inner Profile”, and click Clone.
  4. Drag the clone into the “Side Body” and remap it to a vertex and edge on the side body’s pad (use Normal to Edge).
  5. Switch to Part Design, select the clone, and create a Subtractive Pipe using the side body’s edge. If it stops short, create a sketch with an extended line as the path.
  6. Repeat for the “Outer Profile”: constrain it fully, clone it, remap to the side body, and create a Subtractive Pipe.
  7. For the outer bevel, create a duplicate of the “Outer Profile” (use Edit > Duplicate Selection), remap it to another vertex, and create a Subtractive Sweep with both profiles as sections.
• Tips:
  • Disable Skip Recomputes (right-click project) before major updates to avoid errors.
  • Use multi-section sweeps for complex bevels.

Step 10: Mirror the Side Body

• Description: Mirror the side body to complete its geometry.
• Instructions:
  1. Select the Pad, Subtractive Pipe (Inner Profile), and Subtractive Sweep (Outer Profile) in order.
  2. Click Mirrored, set the plane to Base YZ Plane, and click OK.
  3. Set the Mirrored feature’s Refine property to True.
• Tips:
  • Verify no overlapping faces appear; adjust sketches if necessary.
  • Save frequently to preserve progress.

Step 11: Assemble the Tray with A2Plus

• Description: Use the A2Plus workbench to assemble the top and side bodies into a complete tray.
• Instructions:
  1. Install the A2Plus workbench via Tools > Add-on Manager if not already installed.
  2. Create a new file (File > New) and save it as “Tray_Assembly.fcstd”.
  3. Switch to the A2Plus workbench.
  4. Click Add Shapes from External File, select the tray file, and import the “Top Body” and “Side Body”.
  5. One body is fixed (check Fixed Position in Data tab). Select a vertex on the fixed body and a matching vertex on the movable body.
  6. Click Point Identity Constraint to align them.
  7. Duplicate the side body (Duplicate Part), right-click the duplicate, and select Transform to rotate it into position.
  8. Align vertices with another Point Identity Constraint.
  9. Repeat duplication and constraint application to position additional side body copies, forming the tray.
  10. Save the assembly.
• Tips:
  • Increase Point Size in View settings to see vertices clearly.
  • Save parts and assembly in the same folder for easier management.

Conclusion

You’ve created a tray in FreeCAD by importing reference images, sketching symmetrical parts, applying custom bevels, mirroring components, and assembling them with A2Plus. If issues arise, revisit sketches for constraints or check mapping modes. Handles and a base can be added using similar workflows. Save your work and experiment with refinements for precision.

Additional Resources

• FreeCAD Documentation
• A2Plus Workbench Tutorial
• FreeCAD Forum: https://forum.freecad.org/