Skip to content
Sign in
Menu

How to export a STEP file that makes a good drawing

A drawing cannot carry what the file never brought. These are the export settings for each CAD system, with the dialog drawn out and the checkbox that matters pointed at.

Six rules that hold for every CAD system

  1. Pick AP242 if your version offers it, AP214 otherwise. AP203 works, but it arrives with no colour, no material and no tolerances.
  2. Export solids. Wireframe and loose surfaces have no volume, and without volume there are no views and no dimensions.
  3. Keep the assembly structure. Do not merge everything into one solid or flatten the tree: that structure is what lets you pick which part gets drawn.
  4. One single file. The «one STEP per component» option splits the assembly into dozens of files, and only one file can be uploaded.
  5. Use the real manufacturing names for your parts. That name ends up in the title block and is how each part is found inside the assembly.
  6. Work in millimetres and orient the part the way it is made: the views come from the model coordinate system.

SOLIDWORKS

AP242

File ▸ Save As ▸ STEP AP242 (*.step) ▸ Options

  1. Open the part or assembly and go to File ▸ Save As. Under file type pick STEP AP242; if your version does not offer it, STEP AP214 will do.
  2. Click Options before saving. It is the only place where what the file carries is decided, and by default it does not carry everything.
  3. Under Output as, leave Solid/Surface geometry. Wireframe exports curves, not volume, and curves make no drawing.
  4. Tick Export face/edge properties so colours travel, and leave Export assembly components as separate STEP files clear: that box splits the assembly into one file per part.
  5. If you work with MBD, export through File ▸ Share ▸ STEP242: it is the only route that carries custom properties and 3D annotations.

What your drawing gains

The real name of every part so you can pick what gets drawn, colour in the viewer and, with MBD, the drawing number and revision already filled into the title block.

GD&T on your 2D drawings does not travel into STEP with any version. Only dimensions and tolerances created on the model with DimXpert or MBD come across.

STEP Export Options
  • File FormatSTEP AP242Choose
  • Solid/Surface geometryTick
  • Wireframe (3D curves)
  • Export face/edge propertiesTick
  • Export appearances
  • Split periodic faces
  • Export assembly components as separate STEP filesLeave clear
  • Output coordinate system-- default --
Rendering of the SOLIDWORKS export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

Creo Parametric

AP242

File ▸ Save As ▸ STEP ▸ Options ▸ Configure Export Profiles

  1. Save as STEP and, before accepting, go into Options ▸ Configure Export Profiles.
  2. Switch the protocol to ap242_e3, or to ap214_is if whoever receives it runs older software. The factory profile is ap203_is and it leaves out material, properties and annotations.
  3. For geometry, export solids. Facets turn the part into a mesh and the exact geometry is gone.
  4. Tick colour, layers and groups; material definition with name and density; and geometric and assembly validation properties.
  5. If the model carries PMI, leave it ticked: with ap242 the annotations travel with their meaning, not just as drawn symbols.

What your drawing gains

Material and density in the title block without typing them, the model volume to check it was read correctly, and real tolerances on the dimensions.

Measured on real production files out of Creo: with the factory profile you get geometry, names, colour and layers, and not a single property. Changing the profile is the whole job.

STEP Export Profile
  • Protocolap242_e3Choose
  • Export as solidsTick
  • Export as facetsLeave clear
  • Colour, layers and groupsTick
  • Material definition (name and density)Tick
  • Geometric and assembly validation propertiesTick
  • Annotations and PMI
Rendering of the Creo Parametric export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

Autodesk Inventor

AP242

File ▸ Save Copy As ▸ STEP (*.stp) ▸ Options

  1. Use Save Copy As and pick STEP as the file type.
  2. In Options, set the application protocol to 242. It has been available since Inventor 2022; on older versions pick 214.
  3. Export solids and leave Include sketches clear: loose curves clutter the views and add nothing to the drawing.
  4. Fill in the document name with the real part reference. That is what shows in the title block and what identifies the part inside the assembly.

What your drawing gains

Each part reference exactly as you keep it in Inventor, the model colour and, with 3D annotations, tolerances on the dimensions.

PMI comes from the model annotation environment. Anything living in the .idw drawing stays in the drawing.

STEP File Save As Options
  • Application protocol242Choose
  • Export solidsTick
  • Include sketchesLeave clear
  • Design doc nameREF-0001
Rendering of the Autodesk Inventor export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

Siemens NX

AP242

File ▸ Export ▸ STEP242

  1. Open File ▸ Export and pick STEP242. If that option misbehaves in your installation, STEP214 is the safe fallback.
  2. Under Data To Export, pick the entire assembly. By default only the active component may come out.
  3. Tick solids, PMI and attributes. Attributes are what carry your part data into the file.
  4. Check that the model unit is the millimetre before exporting.

What your drawing gains

The full assembly tree with its references, annotations with meaning, and whatever part attributes you have defined.

Material and density travel poorly from NX into other systems. Check them at the far end and, if they did not make it, declare them when launching the job.

Export to STEP
  • STEP versionAP242Choose
  • Data To ExportEntire AssemblyChoose
  • SolidsTick
  • PMI
  • AttributesTick
Rendering of the Siemens NX export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

CATIA V5

AP242

Tools ▸ Options ▸ General ▸ Compatibility ▸ STEP, then File ▸ Save As ▸ .stp

  1. The setting is not in the save dialog: go first to Tools ▸ Options ▸ General ▸ Compatibility ▸ STEP.
  2. In the export section, set the application protocol to 242 ed1.
  3. Tick 3D Annotations if the model carries them. Without that box the PMI does not come out even though the protocol supports it.
  4. Save as .stp from the complete product, not from a single part opened on its own, or you lose the assembly tree.

What your drawing gains

The product tree with every part name, colour, and 3D annotations with their meaning.

Options ▸ Compatibility ▸ STEP
  • Application Protocol242 ed1Choose
  • 3D AnnotationsTick
  • Export as solids
Rendering of the CATIA V5 export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

Solid Edge

AP242

File ▸ Save As ▸ Save Copy As ▸ STEP (*.stp) ▸ Options

  1. Pick Save Copy As and choose STEP as the type.
  2. Go into Options and set the protocol to AP242.
  3. Keep the assembly structure: it is what lets you pick afterwards which part gets drawn.
  4. Leave colour export ticked so parts stay recognisable in the viewer.

What your drawing gains

The assembly with its hierarchy and names, and the colour of every part.

STEP Export Options
  • ProtocolAP242Choose
  • Keep assembly structureTick
  • Export colours
Rendering of the Solid Edge export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

Fusion

AP242

File ▸ Export ▸ STEP (*.step)

  1. Check the component names in the tree first: those are what travel into the file and what you will see when picking parts.
  2. Export the whole design from File ▸ Export, with STEP as the type.
  3. Check that the document units are millimetres before exporting.

What your drawing gains

Component names and the design structure; Fusion exports AP242 on its own, so there is no protocol to choose.

Export
  • TypeSTEP (*.step)Choose
  • What is exportedDesignChoose
Rendering of the Fusion export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

Onshape

AP242

Document menu ▸ Export ▸ STEP

  1. Open the document or assembly menu and pick Export.
  2. Choose STEP as the format and AP242 as the version.
  3. Keep the assembly structure. The flattened option loses the hierarchy and the subassemblies with it.
  4. If the model carries MBD, enable it in the export; on large models it pays to set the annotation text height.

What your drawing gains

The assembly tree with every part reference and, with MBD, tolerances that carry meaning.

Export
  • FormatSTEPChoose
  • STEP versionAP242Choose
  • Keep assembly structureTick
  • Export as flattened structureLeave clear
Rendering of the Onshape export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

Rhino

AP214

File ▸ Save As ▸ STEP (*.stp) ▸ Options

  1. Before exporting, join the surfaces and check the result is a closed solid with no naked edges.
  2. Save as STEP and open Options.
  3. Pick AP214: AP242 support in Rhino is still partial.
  4. Drop the export tolerance to 0.001 mm so curved surfaces arrive clean.

What your drawing gains

Exact geometry instead of a mesh, which is what decides whether diameters and radii are dimensioned correctly.

The usual failure coming from NURBS modelling is exporting loose surfaces instead of closed solids. If the model does not close, the drawing comes out with incomplete views.

STEP Export Options
  • ProtocolAP214Choose
  • Export closed solidsTick
  • Export tolerance0.001 mm
Rendering of the Rhino export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

FreeCAD

AP242

Edit ▸ Preferences ▸ Import-Export ▸ STEP, then File ▸ Export

  1. The settings live in the preferences, not in the export dialog: open Edit ▸ Preferences ▸ Import-Export ▸ STEP.
  2. Set the scheme to AP242 and the units to millimetres.
  3. Turn on Use LinkGroup so the assembly hierarchy arrives complete.
  4. Select the assembly in the tree and export it with File ▸ Export. Select a single body and a single body is all you get.

What your drawing gains

The document hierarchy with every object name and the colour assigned to it.

Preferences ▸ Import-Export ▸ STEP
  • SchemeAP242Choose
  • UnitsmmChoose
  • Use LinkGroup (keep hierarchy)Tick
  • Merge compoundsLeave clear
Rendering of the FreeCAD export dialog, with the settings that matter highlighted. Option names may vary slightly between versions.

What each STEP version carries

STEP is not a single format: the application protocol decides what fits inside the file. Whatever does not fit is not lost through a fault, it was simply never written.

DataAP203AP214AP242
Exact solid geometryYesYesYes
Part names and assembly treeYesYesYes
Body and face colourNoYesYes
Layers and groupsNoYesYes
Material and densityNoYesYes
Validation properties (volume, area, centre of mass)NoYesYes
Your own data: drawing number, revision, customer, finishNoRarelyYes
Machine-readable tolerances and GD&TNoNoYes

One warning that costs many hours: the dimensions and tolerances living in your 2D drawing do not travel into the STEP file with any version. Only what was created as an annotation on the 3D model makes the trip.

Frequently asked questions

Which STEP version should I upload if I am not sure?
AP242 if your CAD offers it, AP214 otherwise. An AP203 file is processed just as well: the geometry and the dimensions come out right, but the file arrives with no colour, no material and no tolerances, so those have to be typed in when the job is launched.
Should I upload the whole assembly or a single part?
The whole assembly, in one file. You then pick by name which parts you want drawings of, and each one gets its own sheet. What does not work is the option that exports one STEP file per component, because it scatters the assembly across dozens of separate files.
Why do my parts show up unnamed or numbered?
Because the file was exported with the tree flattened or merged into a single solid, or because the model still carries the automatic names from the CAD system. Export again keeping the structure, with the manufacturing names set in the model.
My tolerances are on the 2D drawing, do they count?
No. Dimensions on a 2D drawing stay in the drawing file and never enter the STEP file, whichever version you pick. Only GD&T created as a 3D annotation on the model travels: DimXpert or MBD in SOLIDWORKS, Model Annotation in Inventor, 3D annotations in CATIA, PMI in Creo and NX.
What if all I have is an STL?
It is processed too, but an STL is a triangle mesh: curved surfaces are dimensioned by approximation and diameters depend on the resolution it was exported with. If you get to choose, export STEP.

Export one part and see for yourself

The quick way to know whether your settings are right is to upload the file and look at the drawing. If something did not make it, we say so in the job itself.

Start for freeTalk to us