CAD Files and Documents
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.
Continue with Feature-based Modeling, Assembly Files and Mates, or Orthographic Projection and the Glass Box for the modeling and drawing methods.
An Onshape document holds tabs inside a workspace
An Onshape document holds tabs inside a workspace
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.
Several parts created together in a Part Studio are not automatically an assembly with motion relationships. See Sketch Entities and Planes to begin geometry and CAD History, Versions, and Sharing to distinguish a workspace from a version.
Vendor help for the document model
Onshape Documents describes the container and its contents. Interface layout and available tools can vary by platform.
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.
Template and unit references
See SOLIDWORKS file locations and template types and Onshape account preferences. Changing an Onshape account unit preference does not retroactively change existing documents.
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.
Why a folder copy needs checking
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.
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.
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.