A Student’s Guide to the INP Analyzer
Learning FEA from the Input File
A Student’s Guide to the INP Analyzer
With Runnable Example Files for Abaqus Student Edition
Joseph P. McFadden Sr | The Holistic Analyst
www.McFaddenCAE.com | McFadden@snet.net
Before You Begin
Most FEA courses teach you how to use the GUI: click here to create a part, click there to assign a material, click this to mesh. That is necessary but not sufficient. The GUI generates an input file. The solver reads that input file. The results come from whatever is in that file. If you do not understand what is in the file, you do not understand your simulation.
This guide takes a different approach. Instead of starting with the GUI, we start with the input file itself. You will read INP files, process them in the analyzer, run them in Abaqus Student Edition, and see how each keyword translates to a physical concept. By the time you go back to the GUI, you will know exactly what every button does because you will have seen what it writes into the file.
The five example INP files included here are intentionally simple: a 100 mm beam with 24 nodes and 5 elements. Simple enough to read every line, but complete enough to teach every fundamental concept. You can submit them directly to Abaqus Student Edition and view the results.
What You Need
• The INP Analyzer (AbaqusINPAnalyzer.exe or the Python script)
• The 5 student INP files (student_01 through student_05)
• A text editor (Notepad++, VS Code, or even plain Notepad)
• Abaqus Student Edition (optional but recommended for running the models)
• The 5 full-size reference INP files (example_01 through example_05) for reading
ℹ️ The student INP files (24 nodes, 5 elements) are designed to run in Abaqus Student Edition which limits model size to 1000 nodes. The full-size files (44 nodes, 10 elements) are for reading and analyzer practice only.
FEA Fundamentals Through the INP File
What Is a Node?
A node is a point in space defined by coordinates. In the INP file, nodes are defined under the *NODE keyword with an ID number and X, Y, Z coordinates. Every node is a location where the solver will calculate displacement, velocity, acceleration, and reaction forces. The more nodes in your model, the finer the resolution of your results.
ℹ️ Open student_01_modal_analysis.inp in a text editor. Find the *NODE block. Notice 24 nodes arranged in a 6×2×2 grid. Node 1 is at the origin (0,0,0). Node 6 is at (100,0,0). The beam is 100 mm long.
What Is an Element?
An element connects nodes into a shape that the solver can compute stresses and strains for. In this kit, we use C3D8R elements: C means Continuum (3D solid), 3D means three-dimensional, 8 means 8 nodes per element, R means Reduced integration (one integration point instead of eight). Each element line lists the element ID followed by its 8 node IDs in a specific order.
ℹ️ In the same file, find the ELEMENT block. Element 1 connects nodes 1, 2, 8, 7, 13, 14, 20, 19. Trace these node IDs back to the NODE block — they form a cube from (0,0,0) to (20,10,10).
What Is a Material?
A material definition tells the solver how the substance behaves under load. At minimum, you need ELASTIC (stiffness) and DENSITY (mass). The ELASTIC keyword takes Young’s modulus (E) and Poisson’s ratio (ν). The DENSITY keyword takes mass per unit volume. In the tonne-mm-s unit system, Steel has E=200,000 MPa, ν=0.3, and density 7.8×10⁻⁹ tonne/mm³.
ℹ️ Open the file in the analyzer. Click the Materials tab. Select Steel. The Property Viewer tab shows the numerical values. Verify they match what is in the text file.
What Is a Section?
A section assignment connects elements to materials. The *SOLID SECTION keyword takes two parameters: ELSET (which elements) and MATERIAL (which material definition). This is the critical linkage: elements belong to an element set, the section assigns that set to a material, and the material defines the physical behavior. If any link in this chain is broken, the solver does not know what the elements are made of.
ℹ️ Find SOLID SECTION in the file. It says ELSET=Beam, MATERIAL=Steel. Now find ELEMENT — it says ELSET=Beam. The chain is: Elements → ELSET “Beam” → Section → Material “Steel.”
What Is a Boundary Condition?
A boundary condition constrains specific degrees of freedom at specific nodes. The *BOUNDARY keyword takes a node set name and a DOF range. DOFs 1, 2, 3 are translations in X, Y, Z. DOFs 4, 5, 6 are rotations. Specifying DOFs 1 through 6 means the node is completely fixed — it cannot move or rotate. This is called encastré (built-in) support.
ℹ️ Find BOUNDARY in the file. It says FixedEnd, 1, 6. Now find NSET, NSET=FixedEnd — it contains nodes 1, 7, 13, 19. These are the four nodes at X=0 (one face of the beam). They are all locked in all 6 directions.
What Is a Step?
A step defines what the solver does with the model. A STATIC step solves for equilibrium under load. A FREQUENCY step finds natural frequencies. A DYNAMIC step integrates equations of motion through time. The step also contains the loading, output requests, and solver controls. Everything before the STEP block defines the model. Everything inside the *STEP block defines the analysis.
Exercises
Work through these exercises in order. Each builds on the previous one. For each exercise, process the INP file in the analyzer, read the file in a text editor, and (if you have Abaqus) run it and examine the results.
Exercise 1: Static Analysis (student_03)
Objective
Understand the most basic FEA analysis: linear static. A 10N downward force is applied at the free end of a cantilever beam. You will compare the FEA tip deflection to the exact analytical solution.
Steps
1. Process student_03_static_analysis.inp in the analyzer
2. Examine Summary tab: confirm Static step, 1 load, 1 boundary condition
3. Examine Parts tab: note the volume and mass of the steel beam
4. Open the file in a text editor. Read the HAND CALCULATION CHECK comment block
5. Calculate the analytical deflection: PL³/3EI = 10 × 100³ / (3 × 200000 × 833.33) = 0.020 mm
6. Run in Abaqus Student Edition. Compare the FEA tip deflection to 0.020 mm
ℹ️ The FEA result will not be exactly 0.020 mm because beam theory assumes slender beams and we only have 5 elements. The difference teaches you about mesh convergence — more elements = closer to the analytical answer.
Exercise 2: Gravity Loading (student_04)
Objective
Learn how body forces work. Gravity applies acceleration to every element that has density defined. This exercise demonstrates why the *DENSITY keyword is not optional for any analysis involving mass.
Steps
7. Process student_04_gravity_loading.inp in the analyzer
8. Note the mass shown in the Parts tab (should be ~7.8×10⁻⁸ tonne = 0.078 grams)
9. Open the file. Find the *DLOAD keyword. The GRAV load type applies acceleration
10. Run in Abaqus. Check the tip deflection under self-weight
11. Now try this: edit the file in a text editor. Delete the *DENSITY block. Save and run again. What happens?
ℹ️ Without density, the elements have no mass. Gravity produces zero force. The beam does not deflect. This is the single most common unit error in FEA: forgetting density or using wrong units for density.
Exercise 3: Two-Material Beam (student_05)
Objective
Understand how multiple materials are assigned in a single model. This is the fundamental concept behind every multi-component assembly: the ELSET → SECTION → MATERIAL chain must be defined separately for each material region.
Steps
12. Process student_05_two_material_beam.inp in the analyzer
13. Check the Parts tab: you should see 2 parts with different materials
14. Check the Materials tab: both Steel and Aluminum should appear
15. Check the Sections tab: 2 solid sections with different material references
16. Open the file. Find the two *ELEMENT blocks with different ELSET names
17. Find the two *SOLID SECTION blocks. Trace the ELSET→MATERIAL chain for each
18. Run in Abaqus. Observe the stress discontinuity at the material interface
ℹ️ The steel portion (3 elements) will have lower stress than the aluminum portion (2 elements) under the same load because steel is stiffer. The analyzer correctly identifies both parts with their individual masses.
Exercise 4: Modal Analysis (student_01)
Objective
Understand eigenvalue analysis. The solver finds natural frequencies and mode shapes without any applied load. These are the frequencies at which the structure wants to vibrate. Every subsequent dynamic analysis depends on this result.
Steps
19. Process student_01_modal_analysis.inp in the analyzer
20. Note the *FREQUENCY step type in the Summary tab
21. Run in Abaqus. Open the results in Abaqus/Viewer
22. Step through the mode shapes. Mode 1 is first bending. Mode 2 may be lateral bending or torsion depending on the aspect ratio
23. Record the first 5 natural frequencies from the .dat file
24. Now modify the file: change the material from Steel to Aluminum (E=70000, density=2.7e-09). Run again. How do the frequencies change?
ℹ️ Aluminum has lower stiffness and lower density than steel. The frequency depends on the square root of stiffness/mass. Work out which effect dominates.
Exercise 5: Shock Analysis (student_02)
Objective
Understand transient dynamic analysis. A shock pulse is applied as base acceleration, and the solver integrates the equations of motion through time to find the response. This is where all of the previous concepts come together: mesh, materials, boundary conditions, and dynamic loading.
Steps
25. Process student_02_shock_analysis.inp in the analyzer
26. Note the Dynamic step and amplitude curve in the Summary
27. Open the file. Find the *AMPLITUDE block and plot the 12 data points on paper. It should be a half-sine shape
28. Find the *BOUNDARY with type=ACCELERATION. The value 981000 mm/s² = 100g
29. Run in Abaqus. Plot the tip displacement (U2) and tip acceleration (A2) versus time
30. Identify the peak displacement. Does it occur during the pulse or after?
ℹ️ For many structures, the peak response occurs AFTER the pulse ends, during the ring-down phase. This is why total simulation time must extend well beyond the pulse duration. A simulation that stops when the pulse stops misses the worst case.
File Reference
Student Files (Runnable in Abaqus Student Edition)
24 nodes, 5 elements each. These run within the Abaqus Student Edition limits.
File
Analysis Type
Key Concept
student_01_modal_analysis
Modal
Eigenvalue extraction
student_02_shock_analysis
Shock
Transient dynamics
student_03_static_analysis
Static
Force-displacement, hand calc
student_04_gravity_loading
Static + Gravity
Body forces, density requirement
student_05_two_material_beam
Static
ELSET-Section-Material chain
Full-Size Reference Files (Read-Only / Analyzer Practice)
44 nodes, 10 elements. Richer models for reading and analyzer inspection. These include SRS, Random Vibration, and Harmonic Response which are multi-step analyses.
File
Analysis Type
Steps
example_01_modal_analysis
Modal
1: Frequency extraction
example_02_shock_analysis
Shock
1: Implicit dynamic
example_03_srs_analysis
SRS
2: Frequency + Modal Dynamic
example_04_random_vibration
PSD/Random
3: Freq + SS + Random Response
example_05_harmonic_response
Harmonic
2: Frequency + Steady-State
Using the Learning Center Tab
The Learning Center is the last tab in the analyzer. It provides comprehensive educational content for each analysis type and best practice topic. Use it alongside the example files for complete coverage.
How to Navigate
• Filter by Category: “Analysis Types” for the 5 dynamics topics, “Best Practices” for general FEA guidance
• Filter by Difficulty: Start with Beginner (green dot), progress to Intermediate (yellow), then Advanced (red)
• Click any topic to see its full content in the right panel
• For Analysis Type topics, click Generate Example INP to create custom versions with your choice of material, element type, and boundary conditions
Recommended Learning Path
31. Exercise 1 (Static) → no Learning Center topic needed, this is fundamental mechanics
32. Exercise 2 (Gravity) → read the Millisecond Unit Systems topic to understand unit traps
33. Exercise 3 (Two-Material) → read the Output Requests topic to learn what to request
34. Exercise 4 (Modal) → read the Modal Analysis topic in the Learning Center
35. Exercise 5 (Shock) → read the Shock Analysis topic
36. Then read SRS, Random Vibration, and Harmonic topics alongside the full-size reference files
37. Finally, explore the Best Practices topics: mesh quality, contact, mass scaling
ℹ️ The Learning Center also lets you generate custom INP files from each analysis type topic. Try generating a free-free modal analysis (no boundary conditions) and compare the results to the cantilever version.
The input file is the truth. Learn to read it.
— Joe McFadden, The Holistic Analyst
