Choose the right container for parts, assemblies, and drawings, then check templates, units, and references.
Choose a part, assembly, or drawing for the work you need to do
Choose a part, assembly, or drawing for the work you need to do
A part describes geometry. An assembly positions components relative to one another. A drawing communicates that design through views, dimensions, and notes. Start by deciding which job you need the document to do.
SOLIDWORKS part: .sldprt
Contains part geometry and its modeling features. A part can contain one body or multiple bodies; the file extension does not mean there is exactly one solid.
SOLIDWORKS assembly: .sldasm
References components, including parts and subassemblies, and stores their arrangement and assembly relationships.
SOLIDWORKS drawing: .slddrw
Usually references a part or assembly to generate drawing views. It is a separate document from the model.
An Onshape document is a container for related design information. Open a workspace to edit that information, then select the tab for the task.
Part Studio: create geometry using sketches and features. One Part Studio can produce several related parts.
Assembly: insert and position part or subassembly instances and define their relationships.
Drawing: create drawing sheets and views of models.
Tabs and tab folders: organize the document's contents. Use the Tab Manager to find a tab when the row becomes crowded. A tab folder organizes tabs; it does not mate parts together.
Supporting detail: Addendum 1 — Vendor help for the document model.
Check the template and units before entering dimensions; Checklist
Check the template and units before entering dimensions
A template supplies starting settings. In SOLIDWORKS, part, assembly, and drawing templates use .prtdot, .asmdot, and .drwdot. Choose the appropriate template, then verify the new document's units. A familiar template name is not proof that its settings are right.
In Onshape, check workspace units; account preferences provide defaults for new documents. Choose a suitable drawing template when creating a drawing, and check that drawing's units and sheet settings too.
Confirm the active document or workspace and the tab you are editing.
Check length and angle units before entering bare numbers.
Enter a known dimension and verify its displayed value and units.
Check drawing units and sheet scale separately from the model.
Changing the display from inches to millimeters should express the same physical length in another unit. It does not repair geometry created at the wrong size. Display precision controls how many digits you see; it is not a manufacturing tolerance.
Supporting detail: Addendum 2 — Template and unit references.
Keep referenced files together when you transfer a design; Practice
Keep referenced files together when you transfer a design
For a typical file-based SOLIDWORKS design, the assembly points to component files, and a drawing points to its model. Sending only the assembly file may leave the recipient without the parts. Renaming or moving files outside a reference-aware workflow can break those connections.
Use Pack and Go to gather a design's related files. Review the package contents, including required drawings, then open the transferred design and check for missing references. Files can be reorganized when references are updated; they do not have to remain permanently in the original folder.
Practice choosing a complete reference package; Interactive
Practice choosing a complete reference package
A reference is a stored relationship from one design document to another. In this lesson's declared graph, an arrow A → B means document A requires document B. A drawing may require a model; an assembly may require parts and subassemblies; each subassembly may require more components.
Start with the document you intend to deliver, then follow every required arrow. This is the dependency closure: the starting document plus every directly and transitively required document. A shared component appears once even when two parents require it.
Static worked case — clamp drawing: the drawing requires the clamp assembly. The assembly requires left and right arm subassemblies plus the base. Both arm subassemblies require the same pivot pin, so the complete six-document set contains the pin once.
Available but omitted
The source file exists, but it was not selected for this package. Add the required document.
Unavailable at source
The declared required document cannot be obtained in the scenario. Checking its box cannot create it; locate or restore the actual source first.
Changed symbolic locator
The intended node still has the same stable identity, but one declared edge expects an old locator. Explicitly retarget that edge. A same-looking or same-named substitute is not automatically the intended document.
This graph is a teaching model, not actual CAD file management. It performs no file operations, uploads, downloads, renames, Pack and Go command, cloud lookup, or PDM action. Real CAD systems can use paths, internal identifiers, search locations, platform records, and workflow rules beyond this declared graph.
Use a reference-aware workflow to inspect and collect the real design. In SOLIDWORKS, Find References can list documents referenced by the active file, Pack and Go can gather related files, and File Utilities can update references during supported rename, replace, or move operations. Review the result and open the transferred design to check it.
Supporting detail: Addendum 4 — Why this lab does not imitate a folder copy.
Engineering Graphics and CAD/CAD Modeling
CAD Model Views and Checks
Navigate a model, choose what edges to show, and check dimensions and mass without changing the design.
Zoom, pan, and rotate change your view of the model
Zoom, pan, and rotate change your view of the model
Zoom changes how large the model appears. Pan shifts it across the window. Rotate orbits the view so you can inspect another side. These viewing operations do not resize the part or move an assembly component.
Use zoom to fit to recover the whole model, zoom to window to enlarge a boxed region, and zoom to selection when you need a selected detail. Mouse buttons, modifier keys, and wheel direction depend on your device and control preferences. Check those settings instead of assuming two platforms use the same gestures.
Use Onshape's view cube or SOLIDWORKS view-orientation controls to return to a known direction. The axis triad helps you keep track of model directions while orbiting.
Normal to looks straight at a selected plane
Normal to looks straight at a selected plane
Front, rear, top, bottom, left, and right are standard model directions. Normal to a planar face or sketch plane means looking along a direction perpendicular to it. An inclined face can therefore have a normal view that is different from every standard view.
The face marked F establishes the front. Normal to depends on the selected plane, not on the name of a standard view.
Isometric, dimetric, and trimetric are angled parallel-projection views. The three principal axes have equal foreshortening in isometric, two equal in dimetric, and three different in trimetric. Perspective adds apparent size change with distance; turn it off when comparing parallel projected shapes.
Supporting detail: Addendum 5 — Viewing direction is separate from drawing layout.
Choose a display style for the edges you need to inspect
Choose a display style for the edges you need to inspect
Keep the viewing direction fixed while comparing styles. Shading shows surfaces; edge settings decide which boundaries you can see. Labels differ between platforms, so read the option's effect.
Shaded without edges
Filled surfaces emphasize overall form without drawn edge outlines.
Shaded with edges
Filled surfaces plus visible edge outlines make face boundaries easier to follow.
Hidden lines/edges removed
An unshaded view shows visible edges and leaves concealed edges out.
Hidden lines/edges visible
Concealed edges are also shown, distinguished from visible edges. Useful for finding geometry behind the front surface.
Wireframe
Shows the edge framework through the model without opaque shaded faces. Overlapping edges can make depth difficult to read.
Original schematic: dashed lines mark concealed edges where they are distinguished. Colors and exact edge treatments vary with software settings.
Onshape also provides translucent display and shaded display with hidden edges. Translucency lets you see through faces; hidden-edge display highlights concealed boundaries. Neither removes material.
Supporting detail: Addendum 6 — Find the view options in vendor help.
A model section view reveals the inside without cutting the part
A model section view reveals the inside without cutting the part
Use a section view in the model window to clip away the near portion visually. Choose a plane or planar face, set the cut position and direction, and inspect the exposed interior. Turn the section off afterward to see the complete model again.
A viewing section does not create an extruded cut feature. It also does not automatically create a documented section view on a drawing sheet. See Onshape Section View help for the available section controls.
Check the selection before trusting a measurement; Checklist
Check the selection before trusting a measurement
Select the actual entities you need, then use Measure. An edge can provide length; a circular edge can provide radius or diameter; two suitable entities can provide distance or angle. Read the result label: minimum distance, center distance, and distance along an axis answer different questions.
Quick selection properties or status-bar values are useful checks, but they depend on what is selected. A face, an edge, a body, and an assembly component are different selections. Clear old selections before starting a new measurement. Measurement reports geometry; editing a driving dimension changes geometry.
Clear the previous selection and select the intended entities.
Confirm the highlighted face, edge, or component belongs to the intended part.
Read the measurement type and unit with the value.
Compare the result with a known dimension or a simple estimate.
Supporting detail: Addendum 7 — Measurement reference.
Mass needs material density as well as geometry; Practice
Mass needs material density as well as geometry
Assign a material to the intended part or body before relying on mass properties. A color or metallic appearance alone is not proof that the material density is correct. Check which bodies or components are included, the units, and any overrides before accepting mass or center of mass.
For a uniform solid, mass = density × volume. A correct volume with the wrong density still gives the wrong mass. Center of mass describes how mass is distributed; it need not lie inside the solid material of a hollow or curved part.
Supporting detail: Addendum 8 — Material assignment and mass-property help.
Separate feature order from edit history, preserve useful design states, and share the intended model with the right access.
The feature list describes how geometry is built
The feature list describes how geometry is built
The SOLIDWORKS FeatureManager design tree and the Onshape feature list help you find sketches and modeling features. Later features can depend on earlier geometry. Rename important features so another reader can tell what they do.
A tree also contains items such as planes, bodies, or components; not every row is a modeling operation. To understand how features build a part, continue with Feature-based Modeling.
A rollback bar lets you work at an earlier position in the feature sequence while later features are temporarily left out of regeneration. Move it forward again to evaluate the complete model and check dependent features. Rolling back does not retrieve an old saved revision, and it is not the same operation as separately suppressing one feature.
Supporting detail: Addendum 9 — Rollback follows the regeneration sequence.
Onshape history records edits; versions preserve milestones; Interactive
Onshape history records edits; versions preserve milestones
Onshape records completed edits in document history. The feature list shows the modeling sequence; history records changes to the document over time. Editing an early sketch today changes the history today even though the sketch remains early in the feature list.
A version captures the design state of the workspace, including its tabs, at a named point. That captured design state is read-only. Use a meaningful milestone name and description so a reviewer knows which state you mean.
A branch starts from a version and provides a separate workspace for further edits. Use it to explore an alternative while preserving the starting version. Compare changes before merging; merging needs review, not just a button click.
Supporting detail: Addendum 10 — Viewing history, restoring, and branching serve different purposes.
Worked symbolic timeline: feature order stays put while edits accumulate
What: the feature list remains Mounting sketch → Base extrude → Edge fillet. Why: editing the first feature later should add a new history event, not move that feature to the end of the regeneration sequence.
Start Main workspace: sketch width 60 mm, extrude depth 12 mm, fillet radius 2 mm.
Edit the early Mounting sketch now: width 60 → 72 mm. It remains feature 1.
Create the fixed Design review snapshot: 72 / 12 / 2 mm.
Edit Main again: sketch width 72 → 84 mm. The snapshot still reads 72 / 12 / 2 mm.
Create Lightweight branch from Design review, then edit only its extrude depth 12 → 8 mm.
1 · Mounting sketch — width starts at 60 mm.
2 · Base extrude — depth starts at 12 mm.
3 · Edge fillet — radius starts at 2 mm.
State after the worked actions
Sketch width
Extrude depth
Fillet radius
Main workspace · editable
84 mm
12 mm
2 mm
Design review · fixed snapshot
72 mm
12 mm
2 mm
Lightweight branch · editable
72 mm
8 mm
2 mm
This is a symbolic in-memory model, not Onshape or SOLIDWORKS. It performs no rollback, restore, merge, save, file operation, or permission change.
A SOLIDWORKS save or file copy needs its own revision plan
A SOLIDWORKS save or file copy needs its own revision plan
In a local file workflow, Save writes the current document to disk. A deliberate copy can preserve an earlier state, but a filename alone does not establish a managed revision or capture all referenced files. Keep descriptive names and know which copy is the active design.
Before copying an assembly or drawing for an alternative, check what its references will point to. Two assembly copies can still use the same part file; editing that shared part can affect both. Use the transfer checks in CAD Files and Documents.
SOLIDWORKS installations may use PDM or connected data management for version and revision control. Follow that system's workflow when present; local Save and Save As are not a universal replacement for it.
Share the intended state and check the recipient's access; Checklist; Practice
Share the intended state and check the recipient's access
In Onshape, decide whether the recipient needs to inspect a fixed version or collaborate in an editable workspace. A link to a changing workspace can show later edits; a version identifies a fixed design state. Grant access using the document's sharing controls.
Confirm the document, workspace or version, and tab you intend to share.
Review document visibility and the intended recipient.
Choose view or edit access and inspect additional permissions such as export, copy, and resharing.
Check that the recipient can open the intended state with the intended access.
Do not assume that sending a URL grants access, or that view access prevents copying or exporting. Available sharing options depend on the account and organization. Review Onshape Share Documents for those permissions.
A component may live outside the folder you copied. SOLIDWORKS File Utilities describes Pack and Go and tools that update references when files move or change names.
Addendum 4. Why this lab does not imitate a folder copy
A plain folder copy can omit a component stored elsewhere, but real reference resolution is more complicated than matching visible filenames. This local in-memory lesson predicts a declared graph only. It does not claim that copying these names would repair a real design, and it does not model Onshape documents, cloud permissions, or PDM-managed identities.
Addendum 5. Viewing direction is separate from drawing layout
A standard view tells you where you look from. First-angle or third-angle projection tells you where that view belongs on a drawing sheet. Explore the geometry in Orthographic Projection and the Glass Box. An angled model view is useful for recognizing shape but is not a substitute for dimensions.
Onshape camera and render options links to navigation and display controls. Current browser controls can separate shading choices from hidden-edge choices; older outlines may list them as combined styles.
Addendum 9. Rollback follows the regeneration sequence
SOLIDWORKS Rollback Bar help explains moving through the feature sequence. A file can be saved with its bar rolled back, so inspect the bar's position when reopening a model.
Addendum 10. Viewing history, restoring, and branching serve different purposes
Viewing an earlier state is inspection. Restoring changes a workspace back to an earlier state. Branching gives you a separate place to continue editing. Check the active workspace before any restore or merge. See Onshape Versions and History and Document Management.
