SOLIDWORKS

Model a sloped-front sheet-metal control box housing

Software: SOLIDWORKS
Platform: Windows
Length: 40 min
Resolution: 2560 × 1600
Output: SLDPRT, STEP, X_T

Samples play on a computer

40min

766clicks

220keys

Windows

Task

Model a control box housing as a single multibody sheet-metal part in millimetres. Use the supplied dimensioned diagrams diagram_01.png and diagram_01_detail01.png through diagram_01_detail04.png as the reference for size and feature layout.

Build the housing from a solid block, then convert it to sheet metal.

Block: Sketch a 280 × 350 mm footprint and extrude it 120 mm high.
Sloped front: Chamfer one top edge 60 × 100 mm. The side profile then shows a 102.77 mm sloped segment and a 247.23 mm flat segment.
Split lines: Add split lines that define the top opening and the two front window regions.
Fillet and shell: Round the bend edges with R10 fillets. Shell the body to 1 mm wall thickness.
Corner reliefs: Cut thin 8 mm corner reliefs and mirror them left-right and front-back.
Mounting holes: Add six Ø6 mounting holes, three on each side flange, using the Hole Wizard.
Bodies: Split off the two side panels so the part ends up with three bodies: the main housing and two side panels.
Sheet metal: Convert each body to sheet metal with flatten/process bends so that each has its own sheet-metal and flat-pattern definition.

Add the following features on the formed housing:

Rectangular flanges: Two 30 × 20 mm rectangular flange forms, placed as one instance plus its mirror.
Round flange: One Ø12.7 mm round flange form. It is centred between the rectangular flanges and dimensioned R8.85 on the top view.
Fan vent: A circular fan vent made with the Vent feature from a dimensioned vent sketch.
D cutouts: A D-shaped cutout inserted as a library feature and linearly patterned to 2 instances at 90 mm spacing.
D-sub cutout: A D-sub connector cutout inserted as a library feature.
Perforations: A hexagonal perforation pattern on both side panels, 227 instances each, with 10 mm hexagons at 15 mm spacing.

Assign Plain Carbon Steel as the material. Set these custom properties:

Description: "Control box housing - 1 mm sheet-metal enclosure with sloped front, perforated side panels, fan vent, D-sub and D cutouts"
PartNo: "Control-Box-Housing"
Material: "Plain Carbon Steel"

Give every sketch and feature a descriptive name, for example "Housing Block 280x350x120", "Housing Shell 1mm" and "Side Panel Perforation Pattern". Fully define all sketches. Keep a single Default configuration. Overall envelope: 280 × 350 × 120 mm.

ReferenceSheet 1

Loading the drawing

Rubrics17

R1
The model shall have an overall bounding box of 280 mm × 350 mm × 120 mm.
R2
The model shall be built from a 280 × 350 mm footprint sketch extruded 120 mm.
R3
The model shall include a 60 × 100 mm chamfer forming the sloped front.
R4
The model shall include R10 edge fillets and a 1 mm shell.
R5
The model shall contain three solid bodies: the main housing and two side panels.
R6
The model shall define three sheet-metal bodies, each with its own flat pattern feature.
R7
The model shall include six Ø6 mounting holes created with the Hole Wizard.
R8
The model shall include a 30 × 20 mm rectangular flange form tool instance and its mirror.
R9
The model shall include a Ø12.7 mm round flange form tool instance.
R10
The model shall include a fan vent created with the Vent feature from a dimensioned sketch.
R11
The model shall include a D cutout library feature linearly patterned to 2 instances at 90 mm spacing.
R12
The model shall include a D-sub connector cutout library feature.
R13
The model shall include a hexagonal perforation pattern of 227 instances at 15 mm spacing on each side panel.
R14
The model shall be assigned the material Plain Carbon Steel.
R15
The model shall carry custom properties Description, PartNo "Control-Box-Housing" and Material "Plain Carbon Steel".
R16
The model shall use descriptive feature names such as "Housing Block 280x350x120" and "Housing Shell 1mm".
R17
The model shall contain a single configuration named Default.

Gold outputControl-Box-HousingSLDPRT, STEP, X_T

Drag to turn, then scroll to zoom

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Events4,782

00:00.003Move830, 698 → 841, 718

00:00.860Click841, 718

00:01.122AppSolidWorks

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00:02.171Move1189, 806 → 850, 714

00:02.547Move843, 713 → 829, 710

00:02.571Move822, 709 → 808, 706

00:02.603Move803, 706 → 785, 705

00:02.723Move788, 705 → 1890, 1070

00:04.019Move1895, 1072 → 1820, 1135

00:04.860Click1820, 1135

00:04.987Move1820, 1133 → 1757, 1041

00:06.068Click1757, 1041

00:06.195Move1756, 1041 → 71, 428

00:07.772Click71, 428

00:07.987Move72, 429 → 96, 401

00:09.036Click96, 401

00:09.244Move96, 401 → 384, 602

00:10.292Move385, 603 → 155, 120

00:12.476Click155, 120

00:12.587Move154, 120 → 142, 174

00:13.052Click142, 174

00:13.123Move143, 175 → 779, 504

00:13.251Move1160, 634 → 1258, 667

00:13.275Move1384, 710 → 1434, 736

00:13.299Move1440, 741 → 1064, 637

00:15.196Move1065, 637 → 1066, 638

00:15.244Click1066, 638

00:15.356Move1066, 638 → 1066, 637

00:15.403Move1067, 637 → 1235, 475

00:17.036Move1235, 474 → 1234, 474

00:17.840KeyEsc

00:18.124Move1233, 476 → 140, 118

00:19.628Click140, 118

00:19.748Move140, 118 → 161, 140

00:19.812Move178, 154 → 199, 175

Loading events

Narration224

00:00
Opened SOLIDWORKS and brought Part1 into view, dismissing the New SOLIDWORKS Document screen and returning to the empty part workspace.
Prepare the SOLIDWORKS part document for modeling.
00:09
Entered Sketch1 and created a centered rectangular sketch with diagonal construction lines, leaving the rectangle under-defined.
Create the base profile for the part.
00:29
Edited the rectangle’s horizontal dimension in the Modify box, entering 280 and confirming the value.
Set the sketch width to 280 mm.
00:33
Selected the rectangle’s vertical dimension and edited it in the Modify box, entering 250.
Set the sketch height to 250 mm.
00:37
Confirmed the 250 mm height, exited the dimension edit, and selected sketch geometry while reviewing the fully defined 280-by-250 rectangle.
Finalize and inspect the rectangular sketch dimensions.
00:53
Edited the vertical dimension to 350 mm, confirmed it, and initiated Boss-Extrude from the sketch; the preview shows a solid extrusion with an 81.00 mm blind depth.
Create a 3D boss from the dimensioned rectangular profile.
01:10
Entered a 20 mm blind Boss-Extrude depth and confirmed it, creating the rectangular solid from Sketch1. Opened the feature menu and moved toward the Chamfer command.
Create the base extruded solid and begin applying an edge treatment.
01:28
Opened Chamfer and set the first chamfer distance to 60 mm, then entered a second distance of 10 mm.
Configure a two-distance chamfer on the part.
01:32
Entered and reviewed the chamfer parameters, selected an edge, and displayed the preview on the front portion of the block with 60 mm and 100 mm distances.
Select the chamfer edge and verify the asymmetric chamfer preview.
01:41
Confirmed the chamfer, producing the sloped front face, then opened Fillet and prepared the part for a radius feature.
Apply the chamfer and begin rounding a remaining edge.
02:00
Set the Fillet radius to 10 mm and selected an edge, showing the radius callout and preview on the chamfered block.
Configure a 10 mm fillet on the selected edge.
02:08
Confirmed the fillet and rotated the completed part through several viewing angles, leaving Boss-Extrude1, Chamfer1, and Fillet1 in the feature tree.
Finalize the model and inspect the resulting geometry.
02:21
Switched to SOLIDWORKS, entered Sketch2, and changed to a front-facing sketch view of the part.
Continue editing the part sketch.
02:34
Selected the upper rectangular face and opened Offset Entities; edited the offset distance field and confirmed the value as 20.
Create an inset or offset rectangle in Sketch2.
02:43
Completed the offset operation, leaving an inner rectangle on the upper face with a visible 20.00 dimension, then zoomed the sketch view.
Define and inspect the inset sketch geometry.
02:52
Opened Split Line with Projection selected, kept the current sketch as the curve, and selected the upper face as the target face.
Project the sketch onto the selected part face.
03:02
Confirmed the Split Line feature and returned to the part model, where Split Line1 appears in the FeatureManager; adjusted the view and selected the lower chamfered region.
Create the projected split-line feature and review the resulting model.
03:15
Zoomed out and expanded Split Line1 in the FeatureManager, revealing Sketch2, then selected the inset rectangular geometry on the upper face.
Inspect the created split-line feature and its source sketch.
03:27
Dragged across the SolidWorks model area and clicked, leaving the lower rectangular face selected and the front rectangular sketch visible.
Manipulate and inspect the part geometry.
03:37
Clicked and scrolled to zoom in on the front face, enlarging the rectangular sketch and lower section.
Adjust the model view for closer inspection.
03:44
Scrolled and clicked the feature tree, then dragged and clicked near the lower model area, leaving the lower face highlighted.
Select and inspect a model feature or face.
03:54
Scrolled repeatedly and clicked Sketch2 in the feature tree, zooming and repositioning the view until the sketch rectangle and 20.00 dimension were prominent.
Open or inspect Sketch2 geometry and its dimension.
04:06
Clicked and dragged through the feature tree and graphics area, then entered Sketch2 editing mode; the rectangular contour became shaded and selected.
Edit and review the Sketch2 contour.
04:16
Clicked within the sketch and then clicked the confirmation control to exit Sketch2, returning to the part view with the upper face highlighted.
Finish sketch editing and return to the part model.
04:26
Activated Offset Entities and selected the lower rectangular contour, leaving a yellow offset preview around it.
Create an offset sketch contour around the lower rectangular region.
04:36
Adjusted the sketch view, then selected the Line tool and began drawing a line from the lower rectangular region.
Add a reference or construction line to the sketch.
04:44
Exited the in-progress line operation with Escape, then reactivated the Line tool and started another line along the center area of the lower rectangle.
Create a vertical sketch line in the lower rectangular feature.
04:54
Opened Mirror Entities, selected sketch lines, and mirrored them about the center reference line, producing two vertical lines within the lower rectangle.
Create a symmetric pair of sketch lines across the centerline.
05:09
Edited the selected sketch dimension, entered 30, confirmed it, and then activated the Trim Entities tool.
Set the spacing of the central sketch lines and prepare to trim geometry.
05:20
Dragged the Trim tool across the central sketch geometry, adjusted the view, and exited sketch editing to the Features tab.
Trim the sketch geometry and finish the sketch operation.
05:30
Selected the current sketch and completed the Split Line operation, returning to the part with the newly created split feature visible in the feature tree.
Create or apply a split-line feature to the part.
05:40
Rotated and adjusted the part view, then opened the Shell feature and selected the part for shelling; the Shell PropertyManager displayed a 10.00 mm thickness field.
Prepare and configure a shell operation on the modeled part.
05:57
Confirmed the shell command, selected the two front rectangular faces, and left the Shell PropertyManager open with the thickness set to 1.00 mm.
Define the faces to remove and set the shell thickness.
06:07
Accepted the shell feature and manipulated the view with middle-button rotations and zooming, inspecting the resulting open-top enclosure and front rectangular openings.
Review the completed shell geometry from multiple viewpoints.
06:17
Continued rotating and zooming the shelled model, moving from an angled enclosure view to an edge-on orientation for inspection.
Inspect the shell result and surrounding geometry.
06:26
Rotated the part back to an angled view, selected the upper face, and opened Sketch4 for editing; the sketch view showed the large upper rectangular region and two lower rectangles.
Create or edit a new sketch on the shelled part.
06:34
Adjusted the sketch view with clicks and scroll gestures, then left the rectangular sketch visible at a different zoom.
Inspect or reposition the sketch geometry.
06:45
Exited the active rectangle tool, selected sketch geometry, and created or edited a line near the upper edge; dimensioning activity left a visible 9.58 mm measurement.
Add and dimension sketch geometry.
07:00
Opened the dimension Modify dialog, replaced the value 9.58093265 mm with 8, and confirmed it; the sketch then displayed an 8.00 dimension and became fully defined.
Set the sketch offset dimension to 8 mm.
07:10
Exited sketch editing and opened the Cut-Extrude feature panel, leaving a 3D preview of the enclosure with the selected thin cut contour and blind depth controls visible.
Create a cut feature from the completed sketch.
07:20
Opened the Thin Feature Units dropdown, reviewed the available unit choices, and navigated the cut preview while leaving the dropdown open.
Review or adjust thin-feature settings and units.
07:28
Confirmed the unit dropdown, adjusted the Cut-Extrude settings, and completed the feature; the model tree gained Cut-Extrude-Thin1 and the resulting cut geometry appeared on the part.
Finalize the thin cut-extrude feature.
07:38
Scrolled and clicked through the Mirror feature controls, then completed the operation; the model returned to the normal view with Mirror1 added in the feature tree.
Create or confirm a mirrored feature on the part.
07:48
Zoomed and panned around the part, inspecting the large recessed area and highlighted edges, then opened the Reference Geometry menu.
Inspect the mirrored result and prepare to create reference geometry.
07:58
Selected Plane from the Reference Geometry menu and entered the Plane PropertyManager, then zoomed and adjusted the model view while selecting geometry for the plane.
Define a new reference plane using model geometry.
08:10
Continued selecting and reviewing plane references while zooming and panning; the Plane PropertyManager showed a fully defined result with Face<1> as the first reference.
Constrain and validate the new reference plane.
08:19
Selected additional model faces and manipulated the view with middle-button navigation and scrolling; the plane definition remained fully defined with Face<1> and Face<2> references.
Add or verify additional references for the reference plane.
08:31
Rotated and zoomed the model while reviewing the fully defined plane, then accepted the operation; Plane1 appeared in the feature tree and the model returned to a clear isometric view.
Finish creating the reference plane and inspect the result.
08:47
Switched to the SOLIDWORKS window, opened the Mirror feature, and selected the mirror plane and feature entries in the PropertyManager.
Set up a mirrored feature on the part.
08:56
Selected the mirror feature and adjusted the preview, then exited the active command and returned to the part view.
Create and review the mirrored geometry.

09:08
Rotated and zoomed the 3D part, selected Plane1, and opened its context controls for further operations.
Inspect the model and prepare the reference plane for another operation.
09:18
Opened Hole Wizard and zoomed out to review the part with the hole specification panel displayed.
Begin configuring a hole feature.
09:27
Changed the Hole Wizard hole type to a plain hole and adjusted the displayed hole specification fields.
Configure the hole feature parameters.
09:37
Opened the hole size dropdown and scrolled through the available diameter options without confirming a new selection.
Review available hole sizes.
09:47
Adjusted the SolidWorks view and selected the Hole Position tool, changing the model from an isometric view to a top-oriented sketch view.
Prepare the part for defining hole positions.
09:57
Zoomed the sketch view in and out, then opened the view-orientation control and changed the displayed model orientation.
Set an appropriate working view for sketch editing.
10:06
Closed the view-orientation popover and adjusted the zoom, leaving the part centered in a smaller top view.
Reframe the model while continuing hole-position editing.
10:16
Zoomed into the upper portion of the part and selected Sketch5 in the FeatureManager, activating the Rectangle tool.
Begin creating or editing rectangular sketch geometry.
10:25
Drew or selected a large construction rectangle in Sketch5 and interacted with its sketch geometry and dimensions.
Define rectangular reference geometry for the sketch.
10:41
Opened the dimension Modify dialog, entered 20, and confirmed the value, updating the displayed dimension to 20.00.
Set the selected sketch dimension to 20.00.
10:49
Entered 10 in the Modify dialog and confirmed the dimension change, then scrolled and clicked within the SolidWorks sketch view.
Adjust a sketch dimension and inspect the updated sketch.
10:58
Entered 10 in another Modify dialog and confirmed it, then scrolled the sketch view and pressed Escape to exit the active interaction.
Set another sketch dimension and review its placement.
11:07
Pressed Escape several times, selected sketch geometry, and activated the Hole Position tool; the sketch became fully defined.
Prepare the sketch for positioning hole features.
11:17
Clicked in the sketch and zoomed far out with repeated scroll actions, leaving the fully defined sketch visible at a small scale.
Reframe the sketch for selecting hole-position geometry.
11:25
Scrolled repeatedly to zoom and pan around the sketch, then clicked near the lower-left feature area.
Navigate the sketch and select a location for hole positioning.
11:35
Continued zooming and clicking sketch geometry, selecting the left vertical edge and then the right vertical edge in the Hole Position workflow.
Select opposing sketch references for hole positioning.
11:45
Adjusted the view of Sketch5 with middle-button navigation and scrolling, then rotated and zoomed out to inspect the dimensioned sketch on the part.
Inspect the sketch geometry and hole-position layout.
11:55
Exited the sketch-editing view and used middle-button navigation and scrolling to rotate and zoom the modeled part, leaving the hole features visible on the upper panel.
Review the resulting part geometry and hole locations.
12:06
Continued rotating and zooming the part with middle-button navigation, moving from an angled exterior view to a close-up of the enclosure and its selected edges and faces.
Inspect exterior faces and edge geometry.
12:18
Activated SOLIDWORKS and continued orbiting and zooming around the part, selecting different faces and edges while inspecting the enclosure and circular opening.
Examine candidate faces and split-related geometry.
12:27
Changed to the Direct Editing tools, adjusted the model view, and opened the Split command; selected geometry is shown in blue in the Split property panel.
Set up a split operation on the part.
12:37
Resized and repositioned the SOLIDWORKS window, then continued the Split setup by selecting additional faces and inspecting the resulting body preview labels.
Define and review split faces and resulting bodies.
12:46
Selected split result bodies in the Split tool, changing the highlighted body selection in the model.
Review and adjust the bodies produced by the split operation.
12:58
Selected additional resulting bodies in the Split PropertyManager, leaving multiple body checkboxes enabled.
Configure which split bodies should be retained.
13:10
Accepted the Split operation and returned to the model tree, then selected a model feature and opened its context menu.
Finalize the split feature and inspect feature or body commands.
13:24
Entered Isolate mode and used zoom or view navigation to inspect the isolated geometry, changing from a single plate view to a close-up of the enclosure.
Inspect individual split geometry in isolation.
13:37
Continued navigating the isolated model, zooming out to show a long perforated strip and then restoring the enclosure view before selecting another feature.
Review another isolated split result and return to the main model.
13:48
Opened the Combine tool, kept Add selected, and selected Split1 bodies for the combine list, adding a second split body.
Prepare to combine selected split bodies into one feature.
13:58
Adjusted the SolidWorks view and manipulated the Combine feature selections, changing the highlighted body and rotating the model to inspect the result.
Inspect and refine the combined solid bodies.
14:09
Rotated and zoomed the SolidWorks model, moving from a top-front view to an angled underside view while inspecting the split and combined features.
Review the part geometry from multiple orientations.
14:19
Rotated and zoomed the model through several orientations, ending with a more frontal view of the enclosure and its two front openings.
Inspect the enclosure geometry and feature appearance.
14:30
Continued rotating and zooming the part, then moved to an isolated side-like view showing a single tapered solid body.
Examine individual geometry and orientation.
14:41
Returned to the enclosure view, switched to the Sheet Metal tools, opened the Bends command, and selected a face/edge so the model highlighted the bend region.
Create or configure a sheet-metal bend on the part.
15:00
Entered and confirmed values in the Bends PropertyManager, changing the active face selection and editing a visible relief value while leaving the bend preview active.
Set bend parameters for the selected sheet-metal face.
15:15
Switched to SolidWorks, adjusted the view, and selected faces on the sheet-metal part while the Bends parameters panel remained open.
Inspect or prepare sheet-metal bend selections.
15:27
Exited the active bend-selection state, zoomed and panned around the enclosure, and inspected its edges and upper-right area.
Review the model geometry and bend-related selections.
15:36
Rotated and zoomed the 3D model repeatedly, moving from a close-up corner view to broader views of the enclosure and then into another close inspection.
Examine the enclosure from multiple viewpoints.
15:48
Waited through window resizing, then right-clicked the model and switched back to SolidWorks with the Shell1 context menu open.
Open commands for the selected shell feature.
15:58
Entered isolate mode for Shell1 and adjusted the view slightly while inspecting the remaining isolated sheet-metal geometry.
Inspect the shell feature separately from the rest of the part.
16:15
Selected a face while the Bends panel was active and rotated the isolated model through several viewpoints, leaving the base face highlighted blue.
Inspect and select a face for bend parameters.
16:25
Scrolled briefly, restored the SolidWorks window, and left the isolated sheet-metal part visible while the view refreshed.
Continue inspecting the isolated part.
16:35
Rotated and adjusted the model view, then interacted with the feature tree to select the flat-pattern area and related geometry.
Inspect the sheet-metal part and its flat-pattern features.
16:45
Rotated, zoomed, and repositioned the isolated model; selected geometry and changed the view to show the formed enclosure with its two rectangular front openings.
Review the part from multiple angles.
17:05
Exited the isolated view, rotated and zoomed the complete part, and selected the two rectangular front features, highlighting their outlines.
Inspect front-panel features on the complete part.
17:14
Rotated and zoomed the model through several orientations, selected a flat-pattern item in the feature tree, and displayed a mostly flat side panel with bend-line references.
Inspect another flat-pattern configuration.
17:27
Exited the isolated view, rotated and zoomed the part, and ended on a front-facing oblique view showing the enclosure, upper panel, side holes, and two rectangular front openings.
Return to and review the complete part from the front.
17:37
Rotated and zoomed the sheet-metal enclosure model, bringing the top opening, front cutouts, and mounting holes into a close view.
Inspect the enclosure geometry from different orientations.
17:46
Rotated and zoomed the model through side and front views, ending with the enclosure shown in a centered isometric view.
Review the completed enclosure from multiple angles.
17:54
Opened the Design Library task pane and expanded its library categories while leaving the enclosure model visible.
Browse available SOLIDWORKS library content.
18:03
Navigated the Design Library to forming tools and selected the rectangular flange item, opening the Library Feature placement mode.
Prepare a forming-tool feature for placement on the part.

Model a control box housing as a single multibody sheet-metal part in millimetres.

Model a detailed sheet-metal control-box enclosure in SOLIDWORKS, adding extrusions, chamfers, fillets, shelling, vents, holes, patterns, forming tools, and mirrored features. Flatten and export the part to DXF, then save the completed model as “Control-Box-Housing.”