FEM software — NASTRAN, ABAQUS (concepts and use): Question bank

3.6.20 · D5 · Physics › Spacecraft Structures & Systems Engineering › FEM software — NASTRAN, ABAQUS (concepts and use)

Intuition Is page ko kaise use karein

Neeche har line ek trap hai. Left side padho, apna jawab zor se bolo, phir right side reveal karo. Agar tera reasoning hollow tha ("mujhe lagta hai... sahi?"), toh yahi woh misconception hai jise yeh page pakadne ki koshish kar raha hai. Har jawab tumhe kyun batata hai, sirf verdict nahi.

Shuru karne se pehle, vocabulary pakki kar lo. Jab hum DOF (degree of freedom) kehte hain toh matlab hai ek number jise solver change kar sakta hai — 3D mein ek single node ke liye woh 3 translations plus 3 rotations hote hain, yani 6 numbers. Jab hum mesh kehte hain toh matlab hai structure ko chhote pieces (elements) mein kaatna jo nodes par jodte hain. Jab hum $Ku = F$ kehte hain, toh padho "stiffness times displacement equals force" — machine ko $K$ aur $F$ pata hai, aur woh unknown displacements $u$ solve karta hai. Yeh teen pictures apne dimaag mein rakho.

Related vault topics: parent topic, Vibration and Modal Analysis, Stress Analysis and Margins, Model Correlation, Composite Materials.

True or false — justify

A finer mesh always gives a more accurate answer

False. Finer mesh usually exact answer ki taraf converge karta hai, lekin ek badly shaped element (ek "sliver" jisme tiny angle ho) ya galat jagah refined mesh cost waste karta hai aur conditioning worsen kar sakta hai; accuracy mesh convergence se aati hai, sirf raw element count se nahi. Hamesha check karo ki refine karne par answer change hona band ho jaata hai.

A modal analysis needs no applied force

F

True. Modes structure ki khud ki property hain — tum eigenvalue problem

(K - ω^{2} M) ϕ = 0

solve karte ho, jiske right side par zero hai. Frequencies aur mode shapes exist karte hain chahe koi structure par push kare ya na kare. Dekho Vibration and Modal Analysis.

NASTRAN cannot do dynamics, only static

Ku = F

False. NASTRAN ki heritage precisely launch dynamics hai — modal, frequency response, aur random vibration (PSD). Static toh sirf uska simplest solution sequence hai, uska ek maatra solution nahi.

A linear static solution scales exactly: double the load, double the stress

True — linearity ki definition se. Linear matlab

K

constant hai, toh

u = K^{- 1} F

F

ke proportional hai. Jis moment yeh sach nahi rehta (contact opening, plasticity, buckling) tum linear world mein nahi ho aur nonlinear solver switch karna padega.

Newton-Raphson gives the exact nonlinear answer in one solve

False. Yeh iterative hai: har step ek linearised system

K_{T} Δ u = R

solve karta hai aur residual

R

ko shrink karta hai. Tum repeat karte ho jab tak

∥ R ∥

tolerance se neeche na giraye — ek solve tabhi exact answer deta hai jab problem pehle se linear ho.

ABAQUS is simply a "better NASTRAN" — always use it

False. 5-million-DOF linear launch model ke liye, NASTRAN ke optimised linear solvers kaafi faster hain aur unke paas decades ki flight heritage hai. ABAQUS tabhi use karo jab physics genuinely nonlinear ho (contact, plasticity, large rotation, composite damage).

Fixing all six DOF at one node is enough to make a static run solve

Usually false for a full 3D body. Ek single fully-fixed node baaki structure ko uske around hinge ya spin karne deta hai agar load line allow kare; solver ko enough constraints chahiye ki sab rigid-body motion remove ho sake, warna

K

singular rehta hai aur solve fail hota hai.

The stiffness matrix

K

depends on the applied load

False linear analysis mein —

K

sirf geometry aur material se aata hai (

\int B^{T} DB d V

). Yeh load/displacement-dependent (tangent stiffness

K_{T}

) tabhi banta hai jab tum nonlinear ho jaate ho.

Spot the error

"My model has no boundary conditions, but static solved fine and gave huge displacements."

Huge displacements khud bata rahe hain. Bina constraints ke

K

singular hai (rigid-body modes ki zero stiffness hoti hai); ek "solved" run jo numerically survive karta hai woh round-off noise par chal raha hai. Woh displacements meaningless hain — pehle rigid-body motion pin down karo.

"I ran SOL 103 (modal) and asked why the stresses look wrong."

Modal analysis mode shapes output karta hai, jo unscaled motion patterns hain (often unit mass se normalise kiye gaye). Unke "stresses" relative shapes hain, real stress values nahi. Real stress ke liye tumhe actual forces ke saath static ya response run chahiye.

"I found a mode at 850 Hz but the launch environment has no energy there, so I ignored it."

Yeh actually us mode ke liye sahi call hai — lekin poora spectrum check karo. Resonance tabhi hoti hai jab environment ki energy kisi natural frequency se overlap kare, toh har low mode ko launch PSD ke against compare karo, sirf pehle wale se nahi.

"I modelled a bolted joint in NASTRAN linear static and trusted the contact pressure."

Contact (surfaces ka touch karna, separate hona, slide karna) inherently nonlinear hai — contact area load ke saath change hoti hai. Linear NASTRAN gap open ya close nahi kar sakta; woh ya toh surfaces glue karta hai ya free chhod deta hai. True pressure distribution ke liye ABAQUS contact use karo.

"Failure index came out 0.8, so the part failed."

Failure index 1.0 matlab failure ki onset; 0.8 matlab 80% tak pahuncha — part fail nahi hua hai lekin margin thin hai. Dekho Stress Analysis and Margins; factor of safety ke saath 1 se neeche index wahi chahiye.

"My composite ply directions are all 0°, and I'm surprised the panel is weak in the 90° direction."

Single-direction layup sirf fibres ke along strong hota hai. Quasi-isotropic strength ke liye mixed orientations chahiye (0/45/-45/90); all-0° plies ke saath transverse (matrix-dominated) direction design se kaafi weaker hoti hai. Dekho Composite Materials.

"I switched the mesh from coarse to fine and the frequency dropped, so the coarse one was wrong and I'm done."

Tumne sirf do points dikhaye hain. Coarse meshes over-stiffen karte hain (frequencies thodi zyada), toh drop expected hai — lekin tumhe phir se refine karna hoga aur confirm karna hoga ki frequency move karna band ho gayi. Do points convergence nahi hai.

"I applied the bolt torque directly as a load in the model."

Torque ek structural load nahi hai jise mesh samjhe; tum ise equivalent axial preload

F = T / (k d)

mein convert karte ho aur woh apply karte ho. Galat DOF mein raw torque dene se nonsense milta hai.

Why questions

Why formulate FEM through virtual work instead of solving the PDE directly?

Stress-equilibrium PDE

\nabla \cdot σ + f = 0

odd geometries par exact solutions maangta hai — haath se impossible. Virtual work ise ek integral (weak) form mein badal deta hai jisme sirf approximate shape functions per element chahiye, jo cleanly matrix

Ku = F

mein discretise ho jaati hain.

Why does the tangent stiffness

K_{T}

appear specifically as a derivative

\partial F_{int} / \partial u

Kyunki Newton-Raphson residual ko Taylor step se linearise karta hai:

R (u + Δ u) \approx R (u) + K_{T} Δ u

. Derivative local slope hai jo predict karta hai ki residual kaise change hoga, toh prediction ko zero set karne se best correction

Δ u

milta hai.

Why is the Riks (arc-length) method needed for post-buckling instead of ordinary load stepping?

Peak load ke baad structure snap through kar sakta hai — displacement badhta hai jabki load girta hai. Load-controlled stepping decreasing-load path follow nahi kar sakta (woh jump kar deta). Riks equilibrium curve ki arc length ke along advance karta hai, load aur displacement dono track karta hai, toh turnaround survive karta hai.

Why do spacecraft engineers prefer text input decks over pure GUI clicking?

Text decks (.bdf, .inp) diffable aur version-controllable hain, aur tumhe parametric studies script karne dete hain — 50 runs mein automatically plate thickness sweep karo. GUI clicks ko usi tarah replay ya audit nahi kiya ja sakta. Yeh Model Correlation ko bhi underpin karta hai.

Why does the modal problem take the form

(K - ω^{2} M) ϕ = 0

with a mass matrix

M

Free vibration matlab inertia stiffness balance kare:

M \ddot{u} + Ku = 0

. Sinusoidal motion

u = ϕ e^{iω t}

assume karne par

\ddot{u}

- ω^{2} u

ban jaata hai, toh mass

M

ke roop mein enter karta hai aur poori cheez us eigenvalue equation mein collapse ho jaati hai.

Why check the mode shapes, not just the frequency numbers?

Do designs ek frequency share kar sakte hain phir bhi bilkul alag vibrate kar sakte hain — ek solar panel twist kar raha, doosra bracket flex kar raha. Shape batati hai kahan stiffen karna hai aur kya mode load path ke liye relevant bhi hai. Frequency akele yeh hide kar deti hai.

Why does a bolt preload increase joint stiffness (geometric nonlinearity)?

Plates ko hard press karne se gaps close hote hain aur members ek stressed state mein aa jaate hain jo further motion resist karta hai — stiffness ab deformed, preloaded geometry par depend karti hai, jo exactly wahi hai jo NLGEOM=YES capture karta hai. Ek linear model, isse blind, joint ki rigidity understate kar deta.

Edge cases

What frequencies does a completely unconstrained (free-free) structure show first?

Chhe rigid-body modes (near) zero Hz par — teen translations, teen rotations jo koi strain energy nahi lete. Yeh physically correct hain orbit mein float karte spacecraft ke liye; pehla flexible mode woh hai jise tum loads ke against compare karte ho.

What happens to

Ku = F

if the structure is a mechanism (has an internal hinge with no stiffness)?

K

mechanism direction mein singular hai, toh koi unique

u

exist nahi karta — solve ya toh fail hoga ya unbounded motion return karega. FEM ek load-carrying structure assume karta hai; ek free mechanism ko constraints ya wahan stiffness chahiye.

A material's Young's modulus is entered as zero by mistake — what does the solve do?

Woh element koi stiffness contribute nahi karta, effectively load path mein ek hole. Neighbouring elements over-deform karte hain, displacements blow up karte hain, aur

K

singular ho sakta hai. Output trust karne se pehle hamesha material cards sanity-check karo.

At exactly the failure index = 1.0, has the part broken?

Yeh damage ki onset par hai — criterion abhi sirf satisfy hua hai. Progressive failure ke liye (jaise composites mein Hashin) yeh mark karta hai kahan cracking shuru hoti hai, total collapse nahi; structure tab bhi load carry kar sakta hai jab tak fibre breakage na ho jaaye.

A load is applied but no motion results (

u = 0

) — is this a bug?

Zaruri nahi. Agar load line seedha ek fully constrained node mein jaata hai jiske direction mein koi free DOF nahi, toh reaction use absorb kar leta hai aur displacement genuinely zero hota hai. Confirm karo ki reaction forces applied load balance kar rahe hain.

The nonlinear solve won't converge — the residual

∥ R ∥

plateaus instead of dropping. What's the physical reading?

Structure ne likely ek instability hit ki hai (buckling, snap-through, ya full contact separation) jahan tangent stiffness

K_{T}

singular ya negative-definite ho jaati hai. Newton-Raphson wahan ruk jaata hai; tum arc-length (Riks) scheme switch karo ya stabilisation add karo.

Two identical meshes give slightly different frequencies on two machines — real error?

Usually physical nahi — tiny differences floating-point round-off aur solver ordering se aati hain, engineering significance se kaafi neeche. Tabhi chinta karo jab gap itna bada ho ki resonance decision change ho jaaye, jo ill-conditioned model ki taraf point karta hai, real design difference nahi.

Recall Quick self-test

Modal analysis right-hand side is... ::: Zero — modes structure ki property hain, koi external force nahi. Linear analysis assumes $K$ is... ::: Constant (load aur displacement se independent). Failure index of 1.0 means... ::: Failure ki onset, zaruri nahi ki total collapse. A free-free structure's first six modes are at... ::: Near-zero Hz — rigid-body modes. Contact and plasticity force you into... ::: Nonlinear analysis (e.g. ABAQUS, Newton-Raphson).