CATIA V5 to NX Conversion: The Short Version
A CATIA V5 to NX conversion carries geometry, assembly structure and most attributes reliably; feature history, parameters, publications and associative drawings survive only partly, and only through history-based tools. inteliScience’s Siemens NX engineers test translator, STEP AP242 and feature-based routes on your data. A 50-part sample shows what survives per part class.
The Problem: The Translator Says “Done”, the NX Engineer Says “Not Usable”
A CATIA V5 to NX conversion can finish without a single error message and still deliver parts nobody can work with: surfaces where solids were expected, skeleton links gone, design tables frozen into plain bodies, 3D annotations reduced to lines. A translator log records that a file was written. It does not record whether the data is fit for work in NX.
The reason is old and well documented. A CATIA V5 part is more than its shape. The specification tree, parameters and formulas, publications to other parts, knowledge rules and the Functional Tolerancing and Annotation (FT&A) captures all carry design intent. NIST researchers described in 2007 that CAD exchange standards were restricted to pure shape and left out construction history, parameters, constraints and features (NIST, 2007). Translators have improved since then. The gap has not closed.
So a conversion has to answer three questions per data type, not per file: what arrives in NX, through which route, and how you prove that it arrived correctly. This guide covers those three. What CATIA users have to relearn in NX, from the Part Navigator to WAVE links, is a different topic, covered in our guide on moving from CATIA to NX as a designer.
Both sides keep moving. As of October 2026, Dassault Systèmes ships CATIA V5-6R2026, and Siemens released the June 2026 version of its CAD system (2606) under the new name Designcenter (Siemens, June 2026); this guide keeps the name NX, as customer requirements still do. The exchange standards move too. The CAx Interoperability Forum, where CAD vendors test their STEP translators against each other, met for its Round 58J review near Frankfurt from 28 September to 2 October 2026, next to a STEP AP242 Day on 1 October (CAx-IF calendar).
What Survives a CATIA V5 to NX Conversion, Data Type by Data Type
Geometry and assembly structure survive every route. Feature history, parameters and links survive only a history-based tool, and only partly. PMI depends on the route: semantic 3D annotations travel through STEP only in AP242. Associative drawings come across only with dedicated migration tools, and even then they need a check before anyone releases from them.
| CATIA V5 data | NX CATIA V5 translator | STEP AP242 from CATIA | History-based tool | What to check in NX |
|---|---|---|---|---|
| Solids (PartBody, bodies) | Solid bodies | Solid bodies | Solid bodies, rebuilt from features | Body type, volume, area, centroid |
| Surfaces (Generative Shape Design) | Sheet bodies | Sheet bodies | Sheets or surface features, tool-dependent | Sheet count; sew where a solid is expected |
| Feature history (specification tree) | No | No | Partly; failed features arrive as bodies | Feature count, list of failed features |
| Parameters, formulas, design tables, knowledge rules | Not as working logic | No | Partly, depending on tool and feature types | Expressions that still drive the model |
| Publications and links between parts | Linked geometry as plain bodies | Linked geometry as plain bodies | Most links, if all referenced files are converted together | Links resolve, no broken parents |
| Assembly structure (CATProduct) | Structure and positions; constraints usually not | Structure and positions | Structure, positions, mating constraints advertised | Number of children, positions |
| 3D annotations (FT&A) | Depends on translator release; test | Semantic PMI with AP242 and 3D annotations enabled on export | Advertised by some tools | PMI count, view by view |
| Drawings (CATDrawing) | Not as associative NX drawings | No | Associative migration advertised | Views regenerate, match the released PDF |
| Properties and attributes | Many, with CATIA names | Part number and name; more depends on the exporter | Advertised | Mandatory attributes against the mapping table |
| Colors, layers, hidden elements | Arrive, rarely matching your NX standard | Depends on export settings | Tool-dependent | Layer and category check |
Two notes on reading it. The history-based column describes what vendors and Siemens publish about their tools, and published capability is not your result. Siemens itself describes failed or unsupported features arriving as intermediate bodies that have to be repaired one by one, from the first feature in the Part Navigator to the last (Siemens, 2018).
The second note is ours. Treat every cell that says “partly”, “depends” or “advertised” as a question for your sample, not as a yes.
Translator Options: The NX Translator, STEP AP242 or a History-Based Tool
There are three routes, and they differ in what they keep, what they need and who has to run them. The CATIA V5 translator in NX is the shortest path for geometry and structure. STEP AP242 is the neutral path that also carries semantic PMI. History-based tools rebuild features and links, at the price of extra licences and repair work on everything that fails.
The CATIA V5 translator in NX
NX reads CATPart and CATProduct files directly through File > Import > CATIA V5, and Siemens lists point-to-point translators for CATIA V5 and CATIA V4 among its interoperability options (Siemens, CAD interoperability). What you get is bodies and assembly structure, with names, colors and many properties. What you do not get is the CATIA specification tree.
That is enough for more data than most teams expect: released parts, purchased components and parts that change once a year are fine as bodies, edited with Synchronous Modeling when needed. Check early whether your NX license bundle includes the translator. Then agree on the import options once and write them down, so the hundredth batch behaves like the first.
STEP AP242 exported from CATIA V5
The STEP route takes two steps: CATIA writes the file, NX reads it. On the CATIA side, STEP export needs the STEP interface add-on licence (ST1); the protocol, AP203 ed2, AP214 ed3 or AP242, is chosen under Tools > Options > General > Compatibility > STEP, and 3D annotations must be enabled in the General section of the same options (Rand 3D). Choose AP242. The CAx-IF states that semantic PMI in STEP is supported by AP242 only, while AP203 and AP214 carry annotations at most as polyline presentation (PMI recommended practices, version 4.1, June 2024). AP242 itself is now in its fourth edition, ISO 10303-242:2025.
STEP has one advantage the direct translator lacks: AP242 files can carry geometric validation properties, meaning volume, surface area and centroid computed by the sending system, so the receiving side can check itself. The import settings that decide between solid and surface on the NX side, and a pre-check that shows whether a file carries validation properties, are in our guide to NX STEP import.
History-based conversion tools
These tools replay the CATIA features as NX features instead of copying the final shape. Siemens described in 2017 that its Content Migration Manager (CMM) migrates part features from CATIA V5 and other systems, while the geometry-level NX Migration does not, and that both migrate drawings associatively to their parts and assemblies and run fidelity checks on the result (Siemens, 2017). In 2018 Siemens added that CMM turns CATIA geometrical sets into feature groups and keeps most links, as long as all supporting files are included. Today Siemens lists migration services that “migrate, verify, report 2D and 3D bulk data”.
Third-party tools make similar promises. Elysium’s CADfeature converts history between CATIA V5, NX, Creo, SOLIDWORKS, Inventor and Solid Edge and advertises associative drawings, assembly mating relationships and PMI (Elysium). CoreTechnologie’s 3D_Evolution offers feature-based conversion for CATIA, NX, Creo, SolidWorks and Inventor (CoreTechnologie).
How much history comes through depends on which CATIA features your designers used: pads, pockets and fillets are one thing, multi-sections, ordered geometrical sets and knowledge rules another.
Which route we would choose
Our clear recommendation: run the NX translator and STEP AP242 on the same sample and compare the results before anyone buys a history-based tool. If the sample shows that only a small share of your parts will keep changing in NX, rebuilding those few by hand costs less than licences plus repair of every failed feature. If a large, cleanly modeled part family will change for years, a history-based tool earns its place, and the sample tells you how many features you will repair per part.
Before You Convert: Prepare the CATIA V5 Data
A conversion inherits every problem the CATIA data already has. Parts that do not update in CATIA convert badly, products with broken links convert incomplete, and a vault without reference values cannot be checked afterwards. An hour of preparation per part family saves days of repair in NX.
- Update everything in CATIA first. A part with update errors in the specification tree converts with the same errors, or with silently missing features.
- Resolve broken links. File > Desk shows which documents a CATProduct points to. A missing CATPart becomes a missing component, and a missing source part breaks every publication that depends on it.
- Convert complete sets. File > Send To > Directory copies a document together with the files it points to. History-based tools keep links only when all referenced files are converted in the same run.
- Decide what should not arrive. Hidden construction geometry, deactivated features, old bodies kept “just in case”: decide per part family whether NX gets them, before the first batch.
- Settle the naming rule. CATIA keeps the part number separate from the file name. Your NX rule has to say which of the two becomes the NX file name or item ID.
- Measure reference values in CATIA. Volume, wetted area and center of gravity per part (Measure Inertia), and the number of instances per product, written to a CSV. Without them, nobody can prove the conversion was right.
- Pick a sample with your worst cases. 30 to 50 files: large surface parts, parts with publications, design tables and FT&A, the biggest products. The easy parts tell you nothing.
Step 6 is the one teams skip, and it is the one that makes everything after the import measurable.
After the Import: Check NX Against the CATIA Source
Never accept a converted batch on the translator log. Measure each converted part in NX and compare it with the values measured in CATIA before the conversion: body type, volume, surface area and centroid for parts, the number of components for assemblies, plus the attributes your mapping table promises.
The CAx-IF publishes thresholds that work as a starting point: 0.5 percent for solid volume and surface area, and 0.02 mm plus a 0.1 percent ratio of part size for the centroid of parts larger than 20 mm, as proven industry examples (geometric validation properties, version 4.6, April 2023). The same document defines the number of children as a validation property for assemblies.
The first script is an NX journal. It opens every converted part in a folder, measures it and writes one CSV row per file. It changes and saves nothing, uses only the public NXOpen API, and runs interactively or in batch with run_journal from the NX installation.
# NX journal (Python): measure converted CATIA V5 parts for the comparison with CATIA.
# Opens each .prt in CONVERTED_DIR, writes one CSV row per file, changes and saves nothing.
# Interactive: Developer tab > Journal > Play. Batch: run_journal.exe from the NXBIN folder.
import csv
import glob
import math
import os
import NXOpen
import NXOpen.UF
CONVERTED_DIR = r"D:\migration\batch-01\nx" # adjust
OUT_CSV = r"D:\migration\batch-01\nx_values.csv" # adjust
REQUIRED_ATTRS = ["PART_NUMBER", "DESCRIPTION", "MATERIAL"] # from your mapping table
FIELDS = ["file", "solids", "sheets", "features", "pmi", "children",
"volume", "area", "cx", "cy", "cz", "diag", "missing_attrs", "error"]
session = NXOpen.Session.GetSession()
uf = NXOpen.UF.UFSession.GetUFSession()
def measure(part):
bodies = list(part.Bodies)
solids = [b for b in bodies if b.IsSolidBody]
root = part.ComponentAssembly.RootComponent
row = {
"solids": len(solids),
"sheets": sum(1 for b in bodies if b.IsSheetBody),
"features": sum(1 for _ in part.Features), # about one per body: no history arrived
"pmi": sum(1 for _ in part.PmiManager.Pmis),
"children": len(root.GetChildren()) if root is not None else 0,
"missing_attrs": " ".join(a for a in REQUIRED_ATTRS if not part.HasUserAttribute(
a, NXOpen.NXObject.AttributeType.String, -1)),
}
if solids:
uc = part.UnitCollection # base units of the part, mm for metric parts
units = [uc.GetBase("Area"), uc.GetBase("Volume"), uc.GetBase("Mass"), uc.GetBase("Length")]
mp = part.MeasureManager.NewMassProperties(units, 0.999, solids)
boxes = [uf.Modl.AskBoundingBox(b.Tag) for b in solids]
low = [min(bb[i] for bb in boxes) for i in range(3)]
high = [max(bb[i + 3] for bb in boxes) for i in range(3)]
row.update(volume=mp.Volume, area=mp.Area, cx=mp.Centroid.X, cy=mp.Centroid.Y,
cz=mp.Centroid.Z, diag=math.dist(low, high))
return row
rows = []
for path in sorted(glob.glob(os.path.join(CONVERTED_DIR, "*.prt"))):
row = {"file": os.path.splitext(os.path.basename(path))[0]}
try:
_, status = session.Parts.OpenBaseDisplay(path)
status.Dispose()
row.update(measure(session.Parts.Work))
except NXOpen.NXException as ex:
row["error"] = ex.Message
finally:
session.Parts.CloseAll(NXOpen.BasePart.CloseModified.CloseModified, None)
rows.append(row)
with open(OUT_CSV, "w", newline="") as fh:
writer = csv.DictWriter(fh, fieldnames=FIELDS)
writer.writeheader()
writer.writerows(rows)
The second script needs no NX. It reads the CATIA reference values from preparation step 6 and the NX values, applies the CAx-IF thresholds and prints a verdict per file.
# compare_conversion.py: CATIA V5 reference values vs. measured NX values, per file.
# catia_values.csv columns: file,volume,area,cx,cy,cz,children
# file = name without extension; same units as NX (mm); children only for CATProducts.
# Thresholds: CAx-IF industry examples, GVP recommended practices v4.6 (April 2023).
# Usage: python compare_conversion.py catia_values.csv nx_values.csv
import csv
import math
import sys
VOL_AREA_TOL = 0.005 # 0.5 percent for volume and surface area
CENTROID_ABS = 0.02 # mm
CENTROID_REL = 0.001 # 0.1 percent of the bounding-box diagonal (parts above 20 mm)
def load(path):
with open(path, newline="") as fh:
return {row["file"]: row for row in csv.DictReader(fh)}
def check(ref, got):
if got is None:
return ["not in the NX batch"]
if got["error"]:
return [got["error"]]
reasons = []
if ref.get("children"): # assembly: compare the structure
if got["children"] != ref["children"]:
reasons.append(f"children {ref['children']} in CATIA, {got['children']} in NX")
elif not got["volume"]:
reasons.append(f"no solid, {got['sheets']} sheet bodies")
else:
for key in ("volume", "area"):
dev = abs(float(got[key]) - float(ref[key])) / float(ref[key])
if dev > VOL_AREA_TOL:
reasons.append(f"{key} off by {dev:.2%}")
shift = math.dist([float(got[k]) for k in ("cx", "cy", "cz")],
[float(ref[k]) for k in ("cx", "cy", "cz")])
if shift > max(CENTROID_ABS, CENTROID_REL * float(got["diag"])):
reasons.append(f"centroid moved {shift:.3f} mm")
if got["missing_attrs"]:
reasons.append("missing attributes: " + got["missing_attrs"])
return reasons
catia, nx = load(sys.argv[1]), load(sys.argv[2])
print("file;verdict;reasons")
for name in sorted(catia):
reasons = check(catia[name], nx.get(name))
print(f"{name};{'NOT OK' if reasons else 'OK'};{', '.join(reasons)}")
Read the result by pattern, not by file. When forty parts fail on the same attribute, the mapping table is wrong, not the parts. When surface parts all report “no solid”, that is expected for Generative Shape Design data and needs its own rule, or a sew step; the options are in our guide to turning imported surfaces into NX solids. The feature column tells you at a glance whether a history-based tool delivered history or just bodies with extra steps.
Numbers cannot see everything. PMI has to be checked view by view on a sample, drawings have to regenerate and match the released PDF, and links have to resolve in the assembly that uses them. The full catalog of checks for migrated data, from naming to standard parts, and how to run them in batch, is in our guide to CAD data quality after a migration to Siemens NX.
Two scripts on one sample folder are a pilot. What a production conversion needs: a tested route per part class, an NX target standard the data lands in, a mapping table for attributes and layers, the same checks on every batch, and NX engineers for the parts that fail. We start with an NX Migration Check on up to 50 of your parts.
Parts Without History: Edit, Rebuild or Leave Alone
Most converted parts will arrive without a usable feature history, whatever route you choose, and most of them do not need one. Decide per part class: leave released, frozen parts as bodies, edit occasional changes with Synchronous Modeling, and rebuild with features only the parts that will keep changing or become the base for variants.
We’d advise against rebuilding every converted part. It feels thorough and burns the budget on parts nobody will open again. The opposite mistake is just as expensive: keeping a master part as a body and paying for every change with direct edits that nobody can trace.
At inteliScience, a Siemens NX engineering partner with NX engineers in Cluj-Napoca, we sort part classes on the sample before the bulk move, so the rebuild list is short and justified. The ways from a history-free body to a parametric NX part, and an acceptance test for the rebuilt part, are compared in our guide from STEP to parametric in NX.
Frequently Asked Questions
How do you verify that a CATIA V5 to NX conversion is accurate?
Compare values measured in NX with the same values measured in CATIA before the conversion, part by part: body type, volume, surface area, center of gravity and, for assemblies, the number of components. The CAx Interoperability Forum cites 0.5 percent for volume and area and 0.02 mm plus 0.1 percent of part size for the centroid as proven industry thresholds. PMI, drawings and links still need a visual check on a sample, because mass properties cannot see them.
Can CATIA V5 publications and external references be kept when converting to Siemens NX?
Only with a history-based migration tool, and only when every referenced file is converted in the same run. Direct translators and STEP files bring the linked geometry as independent bodies without the link. Siemens described in 2018 that its Content Migration Manager keeps most links of a CATIA file as long as all supporting files are included. In NX, associative links between parts are WAVE links, so the converted structure needs the same linking rules as new NX work.
NX CATIA V5 translator vs third-party conversion software: when is the extra tool worth it?
When a large share of your CATIA parts will keep changing in NX and was modeled with a clean feature history. The translator in NX brings geometry and assembly structure, which is enough for released parts and occasional direct edits. History-based tools such as Siemens Content Migration Manager, Elysium CADfeature or CoreTechnologie 3D_Evolution rebuild features, but failed features still arrive as bodies, so run the tool on your own sample before buying licences for the whole vault.
How much does a CATIA V5 to NX conversion cost per part?
There is no reliable per-part price, because the translation itself runs in batch while the real cost sits in parts that fail the checks and in parts that must be rebuilt with a feature history. The share of those parts decides the budget, and it differs from one CATIA vault to the next. inteliScience measures it in an NX Migration Check on up to 50 of your parts, which ends with an effort range per route and part class.
Which CATIA V5 data should be cleaned up before converting to Siemens NX?
Everything that does not update cleanly in CATIA: parts with update errors, products with missing or broken document links, deactivated features and leftover construction geometry. Settle the naming rule too, because CATIA keeps the part number separate from the file name and NX needs one rule for file names or item IDs. Then measure volume, area and center of gravity of each part in CATIA, so the converted result has something to be compared against.
Next Step
If you have a CATIA V5 vault and a date for native NX data, the most useful next hour sorts the data: how many parts, which programs still change, which part classes need a feature history. inteliScience NX engineers, working nearshore from Cluj-Napoca one hour ahead of CET, go through that with you and tell you plainly which route fits and what to test first.
Related Topics
- CATIA to NX Migration Check for up to 50 parts
- CATIA to NX training for experienced designers
- NX Engineering Services overview
References
- NIST, “Standardized data exchange of CAD models with design intent” (2007): https://www.nist.gov/publications/standardized-data-exchange-cad-models-design-intent (retrieved 2026-10-09)
- Siemens Designcenter blog, “Sizing up Content Migration Manager (CMM) and NX Migration (NXM)” (4 December 2017): https://blogs.sw.siemens.com/designcenter/sizing-up-content-migration-manager-cmm-and-nx-migration-nxm/ (retrieved 2026-10-09)
- Siemens Designcenter blog, “CMM: Migrating to NX From Catia” (19 March 2018): https://blogs.sw.siemens.com/designcenter/cmm-migrating-to-nx-from-catia/ (retrieved 2026-10-09)
- Siemens, “CAD interoperability” (point-to-point translators and migration services): https://www.siemens.com/en-us/products/designcenter/cad-software/cad-interoperability/ (retrieved 2026-10-09)
- Siemens Designcenter blog, “Designcenter: a new name for the future of engineering” (26 June 2026): https://blogs.sw.siemens.com/designcenter/designcenter-a-new-name-for-the-future-of-engineering/ (retrieved 2026-10-09)
- Rand 3D, “Exporting STEP and IGES files in CATIA V5”: https://resources.rand3d.com/catia-tips/exporting-step-iges-files-in-catia-v5 (retrieved 2026-10-09)
- CAx-IF, “Recommended Practices for the Representation and Presentation of Product Manufacturing Information (PMI) (AP242)”, version 4.1 (20 June 2024): https://www.mbx-if.org/home/wp-content/uploads/2024/06/rec_pracs_pmi_v41.pdf (retrieved 2026-10-09)
- CAx-IF, “Recommended Practices for Geometric and Assembly Validation Properties”, version 4.6 (21 April 2023): https://www.mbx-if.org/home/wp-content/uploads/2024/05/rec_prac_gvp_v46.pdf (retrieved 2026-10-09)
- MBx Interoperability Forum, “Dates and Events” (CAx Round 58J review, 28 September to 2 October 2026; STEP AP242 Day, 1 October 2026): https://www.mbx-if.org/home/mbx/dates/ (retrieved 2026-10-09)
- ISO 10303-242:2025, edition 4: https://www.iso.org/standard/84300.html
- Elysium, “CADfeature”: https://www.elysium-global.com/en/product/cadfeature/ (retrieved 2026-10-09)
- CoreTechnologie, “3D_Evolution”: https://www.coretechnologie.com/products/3d-evolution/ (retrieved 2026-10-09)

