Convert DWG to SLDPRT

A supplier’s DWG profile may need to become an .sldprt file before it can be extruded, machined, added to a SOLIDWORKS assembly, or released as a native part. A 2D drawing supplies sketch geometry, not the thickness, feature sequence, materials, or manufacturing intent required for a complete 3D part.

What DWG contains

DWG is Autodesk’s native CAD drawing format, used primarily by AutoCAD and supported by products including BricsCAD, DraftSight, and many architectural, CAM, and engineering applications. It can store 2D entities such as lines, arcs, polylines, layers, blocks, dimensions, hatches, layouts, and external references; some DWG files also contain 3D solids, surfaces, meshes, or proxy objects.

Most fabrication DWGs are 2D drawings. A closed outline can become a SOLIDWORKS sketch, but it does not automatically define an extrusion depth, hole specification, fillet radius, bend allowance, tolerance, or parametric design history.

What SLDPRT contains

SLDPRT is the native part-file format of SOLIDWORKS. A part can contain sketches, feature history, solid and surface bodies, materials, configurations, equations, custom properties, and references used by SOLIDWORKS assemblies and drawings.

Saving imported geometry as .sldprt creates a native SOLIDWORKS file, but it does not necessarily create editable native features. A 3D body imported from SAT, STEP, or another exchange format is normally an imported, or “dumb,” solid until critical features are rebuilt or recognized.

Create a part from a 2D DWG

SOLIDWORKS Desktop is the preferred tool for a 2D source because its DWG/DXF Import Wizard can place selected drawing geometry directly in a part sketch.

1. Open the DWG in AutoCAD, BricsCAD, or DraftSight. Remove title blocks, notes, dimensions, hatches, viewport borders, duplicate lines, and other geometry that is not part of the required profile.
2. Place the required closed profiles in model space. If the geometry is only in a paper-space layout, copy or recreate it in model space. Explode or simplify blocks when they prevent clean import.
3. In SOLIDWORKS, select File → Open, choose the DWG file, and start the DWG/DXF Import Wizard.
4. Select Import to a new part as 2D sketch. Select model space, set the source units, and import only the layers needed for the profile.
5. Inspect the sketch before making a feature. Use Tools → Sketch Tools → Check Sketch for Feature to locate open contours, overlaps, and self-intersections. Close gaps, remove duplicates, and convert unwanted entities to construction geometry.
6. Add driving dimensions and sketch relations where design changes are expected. DWG dimensions usually import as annotations or drawing entities, not as SOLIDWORKS driving dimensions.
7. Create the required solid with Features → Extruded Boss/Base, Revolved Boss/Base, or another feature. Add holes, cuts, fillets, chamfers, and patterns as separate native features where practical.
8. Use File → Save As and save the completed part as .sldprt.

Import a 3D DWG solid

If the DWG contains actual AutoCAD ACIS solids, export the model to SAT rather than importing it as a 2D sketch. SAT preserves boundary-representation solid geometry more reliably than a drawing import, but not the original feature history.

1. Open the file in an AutoCAD edition that supports ACIS export. Confirm that the model contains ACIS solids rather than proxy objects or faceted meshes.
2. Run ACISOUT and save the selected solid bodies as a .sat file.
3. In SOLIDWORKS, use File → Open to import the SAT file as a solid body.
4. Run Tools → Evaluate → Import Diagnostics if SOLIDWORKS reports faulty faces or gaps. Heal the body before adding downstream features.
5. Save the imported body as .sldprt. Rebuild holes, patterns, fillets, and other features that must remain editable.

Online conversion and compatibility limits

For a small, non-confidential file, CloudConvert offers browser-based DWG-to-SLDPRT conversion. Upload the source, select SLDPRT as the output format, then open the result in the target SOLIDWORKS version and inspect the geometry before using it in production.

Online conversion cannot infer missing 3D intent from a 2D drawing and should not be expected to produce a clean parametric feature tree. Do not upload controlled drawings, customer models, or export-controlled data unless the service’s security terms and retention settings are acceptable. Desktop SOLIDWORKS remains the appropriate option for editable parts and sensitive files.

• DWG unit metadata can be absent or unreliable. Measure a known edge after import and correct the scale before creating features.
• Bind external references in the source CAD system, or provide every referenced file. Missing Xrefs can omit required geometry.
• Dense polylines, splines, and traced geometry can create thousands of sketch entities, causing slow rebuilds or failed extrusions. Simplify the source profile before import.
• Newer SOLIDWORKS versions cannot normally be opened directly in older versions. Confirm the recipient’s version; use STEP or Parasolid for neutral 3D exchange when a native SLDPRT is not required.
• An imported body may be valid for mass properties, assemblies, and CAM, but saving it as SLDPRT does not make it parametric.