Designing Irregular Shapes in SolidWorks

by rypan27 in Design > 3D Design

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Designing Irregular Shapes in SolidWorks

In this project, I modeled a forked mounting bracket in SOLIDWORKS. The part has a stepped base, a taller rear block, a circular through-hole, rounded fork tips, a U-shaped slot, a 30° angled side recess, and beveled front edges. I used sketches, Extruded Boss/Base, Extruded Cut, Fillet, Draft, and Chamfer to build the shape one feature at a time.

The nine photographs below are my own SOLIDWORKS screenshots, arranged in the order the features appeared in my model. Each image shows the result of its corresponding step.

Downloads

Supplies

Computer with SOLIDWORKS installed

Mouse (recommended for sketching and rotating the model)

My dimensioned bracket drawing (for reference)

Dimensions and reference

All dimensions are in inches (IPS). The values below combine the engineering drawing with geometric measurements from the submitted STL. Coordinates are an explicitly reconstructed way to reproduce the part; they are not a claim about the exact original sketch constraints.

Create the Base and Left Rear Step

1. Open SolidWorks and choose File → New → Part. Change the unit system at the bottom-right of the window to IPS (inches).

2. Select Top Plane → Sketch, then choose Sketch → Line. Press Ctrl + 8 to look straight at the sketch.

3. Draw a closed six-sided outline by connecting these points in order (X, Y, inches): (0.20, 0.00), (4.20, 0.00), (4.20, 2.50), (0.00, 2.50), (0.00, 1.25), and (0.20, 1.25). Connect the last point back to the first.

4. Use Sketch → Smart Dimension to set the main outside width to 2.50 in and the total reach to 4.20 in. Confirm the short rear step is 0.20 in deep and stops at Y = 1.25 in.

5. Exit Sketch. Select Features → Extruded Boss/Base; set End Condition = Blind and Depth = 0.75 in. Accept the feature.

Expected result: The solid base is 0.75 in thick, with a 0.20 in step at its left end. The drawing’s 4.00 in reach runs from X = 0.20 to X = 4.20; the full envelope is 4.20 in.

Build the Raised Rear Block

1. Click the large top face of the base, then click Sketch and press Ctrl + 8.

2. Choose Sketch → Corner Rectangle. Draw a rectangle in the left rear area of the part.

3. Use Smart Dimension to set its boundaries to X = 0.00–0.75 in and Y = 1.25–2.50 in (rectangle size 0.75 × 1.25 in).

4. Exit Sketch. Select Features → Extruded Boss/Base.

5. Set End Condition = Blind, Depth = 0.75 in, and keep Merge result checked. Accept the feature.

Expected result: The raised rear block reaches 1.50 in above the bottom of the part (0.75 in base + 0.75 in additional extrusion).

Cut the Circular Through-Hole

1. Select the flat top face of the main plate, not the top face of the raised block. Choose Sketch.

2. Select Sketch → Circle and click near the left-middle area of the plate to place its center.

3. Use Smart Dimension to set Diameter = 0.80 in.

4. Dimension the center point relative to the model origin: X = 1.25 in and Y = 1.50 in.

5. Exit Sketch, choose Features → Extruded Cut, and set End Condition = Through All. Accept the cut.

Expected result: You should see one circular hole, 0.80 in in diameter, passing all the way through the 0.75 in plate.

Round the First Fork-End Corner

1. Open the Features tab and select Fillet.

2. Set Fillet Type = Constant Size Fillet and Radius = 0.50 in.

3. Rotate the model if needed. Select ONLY the vertical outer edge at the far-right corner of the upper arm (plan-view corner X = 4.20, Y = 2.50).

4. Check the preview. The sharp 90° corner should turn into a quarter-circle while the top and bottom faces remain flat.

5. Click the green checkmark to accept.

Expected result: One outer corner on the right end is rounded; the other remains square, as shown in the photo.

Round the Second Fork-End Corner

1. Choose Features → Fillet again.

2. Set Radius = 0.50 in, the same as the first corner.

3. Select ONLY the vertical outer edge at the remaining far-right corner (plan-view corner X = 4.20, Y = 0.00).

4. Check the preview to make sure it rounds the outside corner, not the future slot.

5. Accept the feature.

Expected result: Both outside corners on the right side now have matching R0.50 in rounds.

Create the U-Shaped Fork Slot

1. Click the plate’s top face → Sketch. Choose Sketch → Circle.

2. Place the center at X = 2.20 in, Y = 1.25 in and use Smart Dimension to set Diameter = 0.50 in.

3. Exit Sketch and use Features → Extruded Cut → Through All to create the rounded inner end of the slot.

4. Select the top face again → Sketch → Corner Rectangle.

5. Draw a rectangle from X = 2.20 in to X = 4.40 in, between Y = 1.00 in and Y = 1.50 in. The right end must extend beyond the physical right edge of the plate.

6. Exit Sketch and select Features → Extruded Cut → Through All. The rectangle should join the existing round opening.

Expected result: The right side is now a two-pronged fork. The slot is 0.50 in wide and has a semicircular left end.

Cut the Side Recess

1. Click the main plate’s top face and enter Sketch → Corner Rectangle.

2. Draw a rectangular cutter crossing the lower outside edge of the part (the Y = 0 edge).

3. Dimension its left and right boundaries to X = 0.75 in and X = 1.75 in. Position its inner edge at Y = 0.25 in; put its other edge below Y = 0 so the rectangle crosses the plate edge.

4. Exit Sketch. Choose Features → Extruded Cut, with End Condition = Through All.

5. Check the preview, then accept the cut.

Expected result: The lower side now has a 1.00 in-long notch. At this stage its inside wall is vertical, not angled.

Apply the 30-Degree Draft

1. Rotate the model to show the side recess made in Step 7.

2. Choose Features → Draft, and set the draft method to Neutral Plane.

3. Set Draft Angle = 30°.

4. For Neutral Plane, select the main plate’s underside (the face at Z = 0).

5. For Faces to Draft, select the vertical inner wall of the side notch (the wall that was at Y = 0.25 in).

6. Examine the preview. Reverse the draft direction if necessary: the lower edge should remain at Y = 0.25, while the upper edge moves inward toward the plate.

7. Accept the draft only after the preview matches the sloped wall in your photograph.

Expected result: The recess wall is now slanted by 30°. The top edge moves inward by approximately 0.43 in over the 0.75 in plate thickness.

Chamfer the Front Ends and Finish

1. Rotate the model to an isometric view so both fork arms are visible.

2. Choose Features → Chamfer (under the Fillet dropdown if Chamfer is not shown).

3. Select an Equal Distance chamfer. Use 0.35 in as the STL-based reconstruction value; this produces a 45° chamfer between perpendicular faces.

4. Select the intended upper outside edges near the two rounded fork ends. Confirm the preview follows the edges shown in the final photograph rather than the inner wall of the U-slot.

5. If SolidWorks automatically selects too many connected edges, disable Tangent Propagation and select only the necessary edges or perform the chamfers separately.

6. Accept the chamfer. Press Ctrl + 7 for Isometric View; rotate to inspect the hole, U-slot, side recess, rounded corners, and beveled ends.

Expected result: The bracket matches your final photograph. The part should be a single solid body. The 0.35 in chamfer is inferred from the STL; the separate drawing also includes a 0.25 in callout, so verify that callout before claiming this is the original design setting.