Siemens NX Drafting, PMI, and MBD Complete Guide

NX · Drafting & PMI

Overview

The Siemens NX documentation pipeline is built on two axes: 2D Drafting and 3D PMI (Product Manufacturing Information).

Drafting produces traditional drawings under ISO, ANSI, JIS, DIN, GB, and ESKD standards, while PMI implements Model-Based Definition (MBD) per ASME Y14.41.

This page covers everything from creating Base/Projected/Section/Detail views and dimensioning/GD&T work, to the MBD workflow where PMI is placed on Model Views and then consumed automatically downstream (CMM, CAM).

For the Drafting shortcut Ctrl+Shift+D and application switching, see 01-shortcuts-ui.md.

Entering Drafting and Setting the Sheet

Open the Drafting application with Application → Drafting or Ctrl+Shift+D.

NX drawings are not a separate .drw file; they are either embedded as a Drawing Sheet inside the same .prt or kept in a dedicated drawing part ({partname}_dwg.prt) that references the component. Choose according to your organization's standard.

Sheet Size and Drafting Standard

Options you choose in the New Drawing Sheet dialog:

Item	Value
Sheet size	A0–A4, B, C, D, E, ANSI, ISO, JIS
Drafting Standard	ISO, ANSI, JIS, DIN, GB, ESKD
Template	Custom template containing the company title block and logo
Scale	Base scales such as 1:1, 1:2, 1:5

The Drafting Standard changes arrow style, default tolerances, dimension placement rules, and how units are displayed.

Korean and Japanese manufacturing shops mainly use JIS or ISO, US-based OEMs use ANSI, and Russia/CIS regions use ESKD.

> Tip: Instead of drawing the company title block every time, pre-embed it in a template part registered under UGII_DRAFTING_TEMPLATE_DIR — it is applied automatically at New Drawing time.

Drawing View System

Base View and Projected View

Base View: the first reference view placed on the sheet. Pick a Model View (Front, Top, Right, Iso, etc.).
Projected View: dragged out from the Base View to create an orthographic projection. The four cardinal directions and Iso view can all be pulled freely.

Section View and Detail View

Sections and local blow-ups are the most frequently used auxiliary views on the shop floor.

View Type	Description
Simple Section	Straight-line section
Stepped Section	Stepped section with multiple jogs
Revolved Section	Rotational section (round parts)
Aligned Section	Unfolds sections of differing angles onto a single plane
Half Section	Half-cut
Broken-out Section	Local partial cutaway
Detail View	Local magnification inside a circular, rectangular, or custom boundary
Broken View	Omits the middle of long parts
Auxiliary View	View along the normal of an inclined face
Overlay View	Overlays two states for comparison (pre/post assembly, unfolded/folded)

Since NX 11 the Section Line itself can be sketch-defined, so non-standard sections update just by editing the sketch.

> Note: Do not forget to set the Detail View scale differently from the parent view. NX auto-infers it, but to avoid dimension display errors, specify Scale explicitly in Detail View Preferences.

Dimensioning

Rapid Dimension: clicking an object auto-detects the type (linear/angular/radius).
Supports all traditional types — Linear, Angular, Radial, Diameter, Ordinate (from an origin), Chain, Baseline, etc.
Auto Dimension: pulls and places sketch dimensions that exist in the view. Useful for semi-automatic dimensioning.
Dimension Style: manages details like arrow style, extension line gap, and text placement.

GD&T / Feature Control Frame

GD&T supports both ASME Y14.5 (US) and ISO 1101 (international).

Tolerance types that go inside a Feature Control Frame (FCF):

Category	Item
Form	Flatness, Straightness, Circularity, Cylindricity
Orientation	Perpendicularity, Parallelism, Angularity
Location	Position, Concentricity, Symmetry
Profile	Profile of Line, Profile of Surface
Runout	Circular Runout, Total Runout

Modifiers supported include MMC (Ⓜ), LMC (Ⓛ), RFS, Free State (Ⓕ), Projected (Ⓟ), and Tangent Plane (Ⓣ), and Datum Feature Symbol and Datum Target can be created alongside them.

Symbols & Notes

Surface Finish: ISO 1302 / ASME Y14.36 symbols
Weld Symbol: ISO 2553 / AWS A2.4
Note / Label / Balloon: free-form annotations and balloons
Parts List (BOM Table): exclusive to assembly drawings. Component Item IDs, quantities, and materials are tallied automatically, and Balloons in the view are linked to the same item numbers.
Hole Callout: reads hole parameters from the feature and auto-generates standard text like ⌀6.5 THRU, ⌴⌀11 ▽5.5.

Flat Pattern Drawing

For sheet metal parts, Insert → View → Flat Pattern View auto-generates the unfolded view.

Bend Lines and Bend Notes (UP/DOWN, R, angle) are added automatically, and a separate Bend Table can also be inserted — shop-floor essential for blank size verification and laser cutting input.

> Tip: If the Flat Pattern does not refresh, run View → Update Views manually. If the bend radius changed but blank size did not, nine times out of ten the view update is stale.

Drawing Automation and Templates

Drawing Template (.prt): template pre-loaded with title block, standard view layout, and company logo. New Drawing starts from this template.
Part Family Drawings: with a single drawing attached to a Part Family, the same drawing is auto-regenerated for each size variant.
Drafting Preferences / Object Preferences: distribute organization standards as .nxd files.
Retained Annotations: if a view is deleted and recreated, existing dimensions auto-reconnect to the new view.

Drawing Field Tips

Layer separation: place dimensions, notes, centerlines, and hatching on separate layers, and simplify what is shown by toggling layers during reviews.
For complex sections, sketch-define the Section Line so it is easy to edit later.
When 3D PMI exists, use Inherit PMI to auto-inherit it into drawing views and make the MBD→2D transition seamless.
In a Teamcenter environment, always Check Out before editing a drawing. This is basic discipline against revision tangles.
Fill part numbers and title block fields from Expressions so they stay in sync with the Part Family.

Drawing View Properties and Display Control

Each Drawing View has independent properties. Right-click → Settings to adjust:

Item	Content
Scale	View scale (independent from the parent view)
Reference Set	Which Reference Set the view displays
Hidden Lines	Whether hidden lines are shown and their line style
Smooth Edges	Whether tangent edges are shown
Threads	Thread representation (Simplified/Symbolic/Detailed)
Centerlines	Auto-center line generation
Section Line Appearance	Section line weight and arrow size

The most commonly missed item on the shop floor is thread representation. Unless the company standard (whether Simplified or Symbolic) is preset in the Template, representations drift from view to view.

View Dependent Edit

Use this when you want to hide or highlight edges only in a specific view. The edit is applied at the view level without touching the model, so other views are unaffected.

It is useful to visually hide edges of rear parts in an assembly drawing.

Drawing Revision Control

Three axes for managing drawing Revisions:

Revision Block: a Revision table next to the title block (ECO number, date, author).
Revision Clouds: encloses changed regions in a cloud.
Balloons / Delta Symbols: flags change locations with Δ1, Δ2 markers.

In a Teamcenter environment, when the Item Revision increments, the drawing Revision also auto-advances, and Structure Manager lets you trace which Revision is tied to which assembly.

PMI Overview

PMI (Product Manufacturing Information) is a capability that embeds the dimensions, tolerances, and notes needed for manufacturing, inspection, and assembly directly into the 3D model.

The ultimate goal is MBD (Model-Based Definition), where the 3D alone fully defines the product without a 2D drawing, and ASME Y14.41 / ISO 16792 are the governing standards.

PMI Components

Dimensions: Linear, Angular, Radial, Diameter
Feature Control Frame (geometric tolerance)
Datum Feature, Datum Target
Surface Finish
Weld Symbol
Note / Callout
Material Specification
Custom Symbol

Model Views and PMI Placement

If PMI is placed anywhere, annotations overlap and become unreadable. NX groups PMI with the concept of a Model View.

Menu → View → Operation → New Model View creates a view
Specify view name, orientation, and visible-object set
Each view can be configured with its own PMI set to display

A common naming convention in automotive and aerospace is process-based, such as MV-INSPECTION (inspection), MV-ASSY-TOP (assembly top), and MV-MACHINING-OP10 (per machining operation).

Creating PMI

In Menu → Insert → Annotation → Dimension, set Mode to 3D (PMI) and click a dimension — it is saved to the current Model View.

The Annotation Plane is the plane the dimension will sit on, and usually the Model Plane is auto-selected, but you can specify it manually when needed.

Semantic PMI

PMI that goes beyond visual representation and stores the GD&T Datum–Tolerance relationships in a machine-readable form is called Semantic PMI. Semantic PMI is consumed automatically downstream.

Auto-generates CMM inspection programs (Siemens Quality Planner, Mitutoyo MCOSMOS+, etc.)
CAM reads tolerance information and adjusts machining strategy and tool selection
When exported via 3D XML, JT, or STEP AP242, PMI travels with the file for supply chain sharing

> Tip: If PMI is authored in graphic-only form, automated CMM programs cannot read it. Explicitly set the Tolerance Type and always specify Datum references to reach the Semantic level.

MBD Workflow

Complete the 3D model.
Place every dimension, tolerance, and note directly on the 3D as PMI.
Create multiple Model Views for different purposes (inspection, assembly, machining).
Deliver to downstream systems via Teamcenter or JT (no drawing).
The CMM reads the PMI and auto-generates the inspection program.
CAM auto-selects machining strategy from the PMI tolerances.

The core benefit of MBD is a Single Source of Truth: no drawing-interpretation error, less confusion from language or notation differences in international collaboration, and automation of inspection and machining.

Since FAA/EASA regulations formally recognized ASME Y14.41, MBD is effectively standard for aerospace parts.

PMI Field Tips

Document which PMI standard (ASME Y14.41 or ISO 16792) the organization follows.
Name Model Views by process (MV-FINAL-INSPECTION, MV-ASSY-STEP1).
For PMI color, keep the default blue and use red only for special tolerances — this is a common shop convention.
Cramming too many PMIs into a single view clutters the model. Filter per view.
Display Instances: attach PMI to a single instance of a pattern feature and have the "show repeated instances" option propagate automatically.
Treat PMI placement as carefully as a drawing review. Readability in 3D depends heavily on camera angle.

> Note: PMI auto-updates when the model is modified, but if the referenced face is deleted, it remains broken. Run the Check for Broken PMI utility regularly to check integrity.

Running PMI and Drafting in Parallel

Many organizations cannot drop 2D drawings at once. A realistic transition path:

Phase 1: 2D-drawing-led, PMI added only as reference information
Phase 2: PMI as Single Source of Truth, 2D auto-generated by PMI Inherit
Phase 3: 2D drawings abolished, MBD-only distribution

In Phase 2, using the Inherit PMI option in Drafting auto-displays PMI placed in 3D inside the view. Not having to enter dimensions twice is a big advantage.

Drafting & PMI Shared Tips

Arrow and text sizes are governed by the Drafting Standard, so to override with the company standard, manage it with the .nxd Preferences file.
For the Parts List in assembly drawings, configure Include/Exclude filters carefully. It is common to aggregate standard parts (bolts) as a group and keep special parts as individual items.
Connect the Item ID, Revision, and Date fields of the Title Block to Attribute references so manual entry disappears.
A common review color convention: red for changes, green for reference notes, blue for dimensions.

Adoption Case Studies

Among Korean vehicle OEMs, some Powertrain divisions have already reached Phase 3 (2D abolished), while Body/Chassis divisions remain at Phase 2.

For suppliers, delivering a JT + PMI package as the baseline, with a PDF drawing attached only when needed, is spreading.

In aerospace, the Phase 3 transition is fastest after the FAA/EASA's MBD recognition. Since Boeing 787 and Airbus A350, a PMI-centric data package has effectively become the supply-chain standard.

Field Checklist

Confirm the Drafting Standard is set to the team standard (ISO/JIS/ANSI, etc.)
Verify that title block Expressions are linked to Item ID and Revision and auto-update
Sketch-define Section Lines so future edits are possible
When Detail View scale differs from the parent view, specify it explicitly
Arrange GD&T consistently in the order Datum Feature Symbol → Datum Reference → FCF
Verify that Parts List Balloon numbers match BOM table item numbers
For Flat Pattern Views, run View Update after design changes to check blank size
Standardize PMI Model View names on a process basis
Verify PMI is authored as Semantic PMI so CMM/CAM can consume it automatically
Sample-test that PMI carries through correctly on JT/STEP AP242 Export

PDF / 2D DWG Export

No matter how far MBD progresses, 2D PDF and DWG are still required at the external supply-chain handoff. NX provides these export paths.

PDF: File → Export → PDF. Creates one file per sheet; the model itself can also be exported as 3D PDF (U3D embedded).
DWG/DXF: converts Drafting views into AutoCAD-compatible layers. Line types and dimension styles map according to the Drawing Standard.
3D PDF with PMI: creates a 3D PDF that preserves PMI, allowing external viewers to rotate and inspect PMI without CAD.

> Tip: PDFs sent to suppliers should be converted with Adobe standard fonts (Helvetica, Times) so the layout does not break on other PCs. Embedding NX's internal fonts as-is inflates file size unnecessarily.