NX Sheet Metal: The Short Version
NX sheet metal is the NX application that keeps a constant-thickness part associated with its flat pattern. inteliScience uses it with DACH shops whose press tables live outside the default K-factor. On Designcenter NX 2606 the 3D and the unfold update together. The shop still loses when Customer Defaults and the bend table do not match the brake.
| What Siemens shows | What the shop still owns |
|---|---|
| Tab, Flange, Jog, Contour Flange | Thickness, radius, inset, relief |
| Live flat pattern in a second window | Neutral factor vs the press |
| Inherit Flat Pattern PMI checkbox | Template, layers, callout order |
The Problem: YouTube Ends at the Flange
Search “NX sheet metal” and you get a bike bracket: 2 mm tab, 12 mm flanges, a 1.5 mm bead. Siemens’ How-to (14 August 2025) is honest about that demo. It is also honest about the drawing trap: PMI does not ride onto the flat view until File > Preferences > Drafting > Flat Pattern View > PMI > Inherit Flat Pattern PMI is on, and you place the view again.
DACH still googles Abwicklung. The English command is Flat Pattern. Same job. The laser and the brake do not care which language the ribbon used.
We advise against modeling sheet as a solid shell “because it looks like a cover.” Convert-to-Sheet-Metal is a different article. This one stays on native features and the unfold.
A 2606 session that actually unfolds
Application > NX Sheet Metal (Designcenter still labels it that way after the June 2026 CAD rename). Set Customer Defaults for thickness, bend radius, and Neutral Factor before the first Tab. Changing them later is a fight with every feature.
Sketch the base Tab. Confirm thickness in the dialog, not in a later Extrude. Flange the edges you will bend. If the part hits a tube, Jog is the offset, not a sketch fight. Contour Flange is for a sketched profile around a tube; Unite bodies first or the contour hangs off the wrong solid. That sequence is the Siemens How-to, not folklore.
Open a second window, split screen, Flat Pattern. Add a flange. The unfold should move. If it does not, you are not in Sheet Metal features. You are looking at a solid that NX cannot unfold.
In current releases the bend callouts are PMI notes, not leftover drafting text, and the drawing view reads them from the model view. Designcenter 2606 did not change that. The toggle still has to sit in the company template, or every designer switches Inherit on by hand and the callouts shuffle.
# After a sheet metal part exists: count bodies (NXOpen, NX 2606).
import NXOpen
session = NXOpen.Session.GetSession()
work = session.Parts.Work
n = 0
for b in work.Bodies:
n += 1
print("bodies:", n)If you expected one sheet body and you have two, you skipped Unite. The flat pattern will only tell the truth about the body you picked.
Where the default K-factor dies
Resize Neutral Factor on one part is a dialog. The press has a table over thickness, angle, die opening, and sometimes the coil. We would rather you keep that table in NX (or in a file NX reads) than in a spreadsheet on a shared drive that three people edit.
A flat pattern that is 1.2 mm too long is not an NX bug. It is a table the last job never updated. Command Prediction can suggest the next Sheet Metal click. It cannot sign the blank size.
Drawing: Base View > model view Flat Pattern. Inherit PMI, place the view, check the callouts against the bend order the brake operator expects. Section views and exploded views are ordinary drafting and not the point here. If the plant still ships a 2D master, that is a methods decision, not a ribbon click. We wrote the trade-off as MBD vs 2D.
Neutral factor, bend allowance, bend table: which one NX is using
NX lets you define bends in Customer Defaults in more than one way: a fixed neutral factor value, a bend allowance formula, or a bend table read from a file. The default is a single neutral factor. It is also the one the demo used, and the one the press does not respect.
- Neutral factor (K-factor). One number between 0 and 1 for the position of the neutral line. Good enough for one material, one thickness, one die. Wrong the moment the shop swaps the V opening.
- Bend allowance formula. The same physics as an expression, with the factor as a variable. Better when you want the maths visible and versioned.
- Bend table. Values per material, thickness, radius and angle, measured on your machine. This is what the brake actually does. It is also the one most shops never load into NX, because the numbers live in a spreadsheet next to the press.
The method is a part attribute once the first feature exists. Changing it later means re-checking every flat pattern the part ever exported. That is why it belongs in Customer Defaults and in the part template, decided once by methods, not by whoever models the next cover.
This runs as a POC. What’s missing for production: Company defaults, a bend table that matches the brake, Inherit PMI in the drafting template, and a check that every flange pair has a corner treatment. NX CAD design services is that pack, not a weekend of Tabs.
What to look for in an NX sheet metal setup
- Defaults first. Thickness and Neutral Factor in Customer Defaults, not tribal memory.
- Native features. Tab / Flange / Jog / Contour Flange, not shell-from-solid unless you meant Convert.
- Live unfold. Split screen. If it does not update, the feature tree is wrong.
- Inherit PMI in the template. A checkbox per user is not a process.
- One table. NX, Excel, or the control: pick a master. Two tables is scrap.
- DXF layers. What the laser sees must match what the template exports.
Our clear recommendation: NX sheet metal over a solid mock-up whenever the part will be lasered and bent. NX is strong here. The gap is the press, not the command.
Siemens NX consulting is where we put those defaults and the NXOpen checks (constant thickness, untreated corners) so the next cover does not invent a new K-factor.
If flat patterns are a recurring problem in your team, our NX sheet metal training covers bends, bend tables and flat patterns on your own parts.
Frequently Asked Questions
What is NX sheet metal?
The NX / Designcenter application for constant-thickness parts with an associative flat pattern. Features such as Tab, Flange, Jog, and Contour Flange carry bend data. A shelled solid does not, until you convert it.
NX sheet metal vs modeling a solid cover?
Use NX sheet metal when you need an unfold, bend notes, and a blank the laser can cut. Use ordinary modeling when the part is machined from plate and never bent. Mixing both on one body is how unfolds fail.
Why is my NX flat pattern empty of PMI?
Inherit Flat Pattern PMI is off in Drafting preferences, or the view was placed before you turned it on. Place the Flat Pattern view again. Put the toggle in the company template so it is not a per-user surprise.
How much does getting the unfold wrong cost?
Blank scrap plus a brake setup is the cheap day. A cover that does not close on the cabinet is the expensive one. We have seen shops reprint a nest because NX and the press disagreed by a millimetre. The seat is not the bill. The table is.
Flat pattern vs bend table?
The flat pattern is the shape. The bend table is why that shape matches the machine. NX can unfold with a neutral factor, a bend allowance formula, or a bend table; only the table carries what your brake measured. Load it once, in Customer Defaults, and stop re-typing K-factors per part.
Next Step
Want the unfold to match your brake, not the demo K-factor? Book a free 60-minute strategy call. Book a strategy call about NX sheet metal