Part 1: Setting a Quick Model
Full step-by-step Abaqus/CAE walkthrough for the plate-with-hole: geometry, materials, meshing, BCs, run, and results.
2D Plate with a Hole
Now that we have covered some fundamentals and learned how to operate within Abaqus/CAE, let’s walk through a complete example: a plate with a central hole under tension, as shown in Figure 1.
| ⚙️ Parameter | 📏 Value |
|---|---|
| Plate length, $L$ | 100 mm |
| Plate height, $H$ | 20 mm |
| Hole diameter, $D$ | 10 mm |
🗂️ Sketch & Setup
Open Abaqus/CAE, set the working directory, and start a Standard/Explicit Model. You can also launch from a terminal in the target folder with:
abaqus cae
In the Start Session dialog, choose Standard/Explicit Model to begin.
🧩 Geometry
The first step of any model is defining the geometry.
In the Part module, select:
This means we are creating a 2D deformable part using the Shell option, which defines an area. If we had chosen Wire instead, we would have created a 1D part (for example, a truss).
First, select the 🟦 rectangle tool (Create Lines: Rectangle (4 Lines)) and draw it roughly at the center. Next, add horizontal and vertical construction lines ➕ through the midpoint of the sketch. These construction lines serve as auxiliary references and do not form part of the geometry.
At this point, your sketch should look similar to Figure 2.
Now, add a circular hole at the center by selecting the circle tool and clicking in the middle of the plate. Ensure the sketch forms a closed contour - Abaqus requires closed profiles for part creation. Open profiles will cause an error.
Next, apply the dimensions according to Table 1.
Use the dimension tool (second column, fourth row) from the sketch toolbar.
Finally, center the sketch at the origin. Create a point at $(0,0)$, apply the Fixed constraint to it, and then use the Coincident constraint to align the circle center with this point.
When a sketch is fully defined, all lines appear green (see Figure 3). If it becomes overdefined ⚠️ (e.g., due to conflicting constraints), the lines turn yellow and the conflicting constraints appear in purple.
Press Done ✔️ at the bottom of the sketch window to create the part.
At this point, you have your part created inside the Part module, as shown in Figure 4. With this, the geometry section of the model is complete.
🧪 Material and Section
In Abaqus, material properties are defined within the Property module 🧱. So let’s create a PMA material with the following elastic properties (isotropic): $E=3 \; \text{GPa}$ ; $\nu = 0.4$. For this we are going to create a material and then select:
\[\text{Mechanical} \; \rightarrow \; \text{Elasticity} \; \rightarrow \; \text{Elastic}\]as shown in Figure [[Files/material_property.png]]. Then, select “Isotropic” (as shown in [[Files/material_prop2.png]]) as the type and insert the young’s modulus and the poison coefficient. Pay attention to the units ⚠️! Since we are working in millimeters (mm) and newtons (N), our elastic properties must be in megapascals (MPa) to maintain dimensional consistency 📏.
The second step is defining a section. A section is, in essence, the middle layer between the material definition and the geometry. While the material defines how a material behaves, the section specifies how that material will be represented or simplified in your model. For instance, with the same material, you could create a solid, shell, or beam section - each producing different structural behaviors depending on the modeling assumptions. So even if this feels a bit abstract now, it’s enough to remember that the section combines both the material and the modeling approach. Every element in your model must be assigned a section, and this step ensures that Abaqus knows how to interpret the material response of your geometry.
🧩 Assembly and Mesh
Moving on to the assembly and mesh steps. The assembly module represents what the solver actually sees . You might create several parts in the Part module, but only those you create instances of it in the assembly will be used for simulation. Even if you have just one part, you still need to create an assembly instance. You’re essentially telling the solver: “here’s the part I want to analyze.
To do this, create an Instance. An instance is a placed copy of a part within the assembly. You can have multiple instances of the same part, for example, a connection with 10 identical bolts can be modeled using one bolt geometry and section, but repeated as multiple instances.
When creating an instance, Abaqus will ask whether it should be dependent or independent. A dependent instance means the mesh is created at the part level, while an independent instance allows meshing at the assembly level.
The distinction mainly affects how nodes and elements are numbered:
-
In an independent instance, all nodes and elements share a global numbering system across the entire assembly (no duplicates).
-
In a dependent instance, each part maintains its own numbering (so, for example, Element ID = 1 could exist in multiple parts).
See Figure 5 for a quick visual.
At this stage you can change element types, meshing schemes, or seed sizes; we’ll keep the defaults for this intro run.
🧷 Boundary Conditions
First, create a static general step (General → Static, General). Static time is a loading parameter, not real time; dynamic analyses track physical time. Name it (e.g., loading_step) and keep the default ramp amplitude unless you need a custom loading curve.
Apply displacement BCs on left and right edges: $u_x = -1.5$ mm (left) and $u_x = +1.5$ mm (right) to apply tension.
Extra detail screenshot
🚀 Job and Output
Create and submit a job (e.g., plate_with_hole), monitor it in the Job Monitor, then open the Visualization module to inspect results (e.g., von Mises stress).
