Contents

1. Overview

This workflow provides a clear process for carrying out crack analysis of a concrete bridge pier using MIDAS FEA NX. It starts with setting analysis conditions, building the model, and defining reinforcement and material properties to capture nonlinear behavior of concrete and steel. The model is then meshed, boundary conditions and loads are applied, and nonlinear analysis cases are run. Finally, the results are reviewed to study crack initiation, growth, widths, stresses, and overall deformation, giving a realistic understanding of the pier’s performance.

2.Model Description

Structure Type:
Reinforced Concrete Vase-Shaped Pier

Materials:

• Concrete: C40
• Prestressing Tendons: Steel Strands (15.2 mm)
• Longitudinal Rebar: HRB400
• Stirrups: HPB300

Pier Height:
6400 mm

Boundary Conditions:
Fixed at the base of the pier

Loads:

• Self-weight
• Reaction force from the superstructure: 8000 kN/m²
• Braking force: 250 kN

Figure 2.1 Reinforced Concrete Bridge Pier

3.Operation Procedure

3.1 Setting Analysis Conditions

Set the model type, gravity direction, and initial variables. The unit system can be modified during the modeling process or when checking the analysis results. Input parameters will be automatically converted based on the selected unit system.

1. Launch midas FEA NX.
2. Click "File" > "New" to open the Analysis Settings dialog box, as shown in Figure 3-1.
   In this dialog, set up a 3D model with the Z-axis as the gravity direction.
   Use the dropdown menu to select the unit system. For this model, use "kN" and "m".
   Then click "OK" to confirm.

Figure 3.1 Analysis Settings Dialog Box

Note:
The unit system can also be modified using the dropdown menu at the bottom right corner of the program interface.   

3.2 Creating the Model

3.2.1 Import the Pier Outline

1. Click the icon from the toolbar , or right-click in the model window and select "Move Work Plane."

   Choose the reference plane XZ, then click "OK" to confirm.

Figure 3.2-1 Moving Work Plane

2. Select "File" > "Import" > "DXF 2D (Wireframe)" to open the Parasolid File. Choose the file named "pier.X_T", and finally click "OK" to confirm.

Figure 3.2-2 Importing Pier Parasolid File

3.2.2 Generate the Pier Edges and Surface

1. Go to Geometry > Sub Shape > Explode   ,then click "Select Curve".
   Select the Pier Geometry and explode it into “Edge” first and then into “Face”, then click "Apply." Select appropriate name for the Geometry Sets.

Figure 3.2-3 Exploding Edges and Faces from Solid

4. Defining Tendons and Regular Reinforcement

1. In the model window, right-click and select "Move Work Plane", then click "Reset to GCS".
   Next, move the work plane to the plane where the top tendons are located:

• Click "Select Plane", then in the model window, set the filter to "Face" and select the top surface of the pier beam.
• In the Offset field, enter "-0.15" (m).
• Check "Origin" and input the coordinates (0, 0.8, 6.1).
• Finally, click "OK" to confirm.

Figure 4.1 Modifying Work Plane

2. In the main menu, go to Geometry > Point & Curve > Line to open the Line dialog box.

• Under the 2D tab, in the Position field, first enter "3.395, 0.35", then click "Geometry Group".
• In the "Name" field, enter "Tendon", click "Add" , then click "Close".
• In the Geometry Group dropdown menu, select "Tendon", then click "Apply".
• Next, in the Position field, enter "-6.79, 0", and click "OK" to complete the line creation.

Figure 4.2 Defining Tendon Line

Note:
The coordinates entered in the "Position" field are relative to the current work plane.
Make sure to use a comma ( , ) in English input mode to separate the values.

3. In the main menu, go to Geometry > Transform > Move/Copy to open the Move dialog box.

• Click "Select Target", then select the recently created tendon line in the model window,
  or go to the Project Tree > Geometry > Tendon > Curve > Line and double-click the line.
• For Direction, select the Y-axis in the model window.
• Under Method, check "Copy (Uniform)".
• Enter a Distance of 0.7 m and Number of Copies as 1.
• Set the Geometry Group to "Tendon", and then click "OK" to confirm.

Figure 4.3 Copying Tendon Line

4. In the Model Tree, go to Geometry and check only "Curve". 

Then, in the main menu, go to Geometry > Transform > Move/Copy to open the Move dialog box.

• Click "Select Target", switch to the Front View , and select the left edge outline of the pier in the model window.
• Set the Direction to the X-axis of the model.
• Under Method, check "Copy (Uniform)", enter a Distance of 0.06 m, and Number of Copies as 1.
• Add and select a Geometry Group named "Rebar", then click "Apply."

Repeat the same step, this time you need to select the top left outermost layer.

• Click "Select Target", switch to the Front View , and select the top edge outline of the pier in the model window.
• Set the Direction to the Z-axis of the model.
• Under Method, check "Copy (Uniform)", enter a Distance of -0.06 m, and Number of Copies as 1.
• Assign to Geometry Group “Rebar", then click "Apply."

Figure 4.4 Creating Regular Rebar

In the main menu, go to Geometry > Point & Curve > Intersect & Trim .

• Click "Select Curve", then select the two recently copied curves in the model window, and click "OK."
• Next, press the Delete key in the model window to remove the unnecessary top segments, as shown in Figure 4.5.
• In the pop-up "Delete Object" dialog box, click "OK" to confirm the deletion.

Figure 4.5 Using Intersect Option

Figure 4.6 Deleting the undesired geometries

Figure 4.7 Final Left pier outline

5. To create the remaining regular rebars, go to Geometry > Transform > Move/Copy from the main menu to open the Move dialog box.

• Click "Select Target", switch to the Front View , and select the existing regular rebar line in the model window.
• Set the Direction to the X-axis of the model.
• Under Method, check "Copy (Uniform)".
• Enter a Distance of 0.09 m, and Number of Copies as 1.
• Add and select the Geometry Group named "Rebar", then click "Apply."

Continue by clicking "Select Target" again, then select the regular rebar line in the model window.

Set the Direction to the model’s X-axis, check "Copy (Uniform)", enter a Distance of 0.1 m, and set the Number of Copies to 17. Click "OK" to confirm.

Figure 4.8 Generation of Longitudinal rebars

6. In the model window, right-click and select "Move Work Plane", then click "Reset to GCS".

• Click "Select Plane" and choose the reference XZ plane in the model window.

Go to Geometry > Point & Curve > Line from the main menu. In the Line dialog box, under the 2D tab:

• Enter "-0.55, 0" in the Position field, select the "Rebar" group from the dropdown, and click "Apply".
• Then enter "0, 2" in the Position field and click "OK."

Now go to Geometry > Transform > Move/Copy, and in the Move dialog box:

• Click "Select Target" , then select the newly created rebar line in the model window.
• Set Direction to the X-axis, check "Copy (Uniform)", set Distance to 0.1 m, and Number of Copies to 5.
• Add and select the "Rebar" group, and click "Apply."

Click "Select Target" again, then select the curved line in the middle part of the pier as shown below.

Figure 4.9 Generation of Longitudinal rebars

Set Direction to the Z-axis, check "Copy (Uniform)", enter a Distance of -0.06 m, and Number of Copies to 1. Click "OK."

In the main menu, go to Geometry > Point & Curve > Intersect & Trim .
Click "Select Curve", and in the model window, select the lines highlighted in Figure 4.10, then click "OK."

Figure 4.10 Translation of top edge

 

Press the Delete key to remove the top segments as shown in the figure. In the pop-up "Delete Object" dialog box, click "OK" to confirm.

Figure 4.11 Deleting the undesired geometries

7. Go to Geometry > Transform > Move/Copy. In the Move dialog box:

• Click "Select Target", then select all longitudinal rebar lines in the model window.
• Set the Direction to the Y-axis, check "Move", enter a Distance of 0.06 m,
• Set the Geometry Group to "Rebar", and click "Apply."

Next, go to Move/Copy again:

• Click "Select Target", select all longitudinal rebar lines,
• Set Direction to Y-axis, check "Copy (Uniform)",
• Enter a Distance of 1.48 m, Number of Copies as 1,
• Add and select the "Rebar" group, then click "Apply."

Figure 4.12 Creating Longitudinal rebars at opposite face

Repeat the Move/Copy process again:

• Select the outermost longitudinal rebar,
• Set Direction to Y-axis, check "Copy (Uniform)",
• Enter a Distance of 0.148 m, Number of Copies as 9,
• Add and select the "Rebar" group, then click "OK."

Figure 4.13 Creating Longitudinal rebars at left face

Finally, go to Geometry > Transform > Mirror:

• In the Mirror dialog box, click "Select Target", and select all longitudinal rebar lines in the model window.
• Set Mirror Type to "Plane", click "Plane Selected", then choose the YZ plane in the model window.
• Check "Copy Object", set the Geometry Group to "Rebar", and click "OK."

8. In the model window, right-click and select "Move Work Plane", then click "Reset to GCS."

• Click "Select Plane" and choose the XY reference plane, then enter an offset distance of 6.03 m.

Go to Geometry > Point & Curve > Line   from the main menu. In the Line dialog box under the 2D tab:

• First, enter "-2.85, 0.07" in the Position field.
• Click "Geometry Group", enter "Tie Beam Rebar" as the Name, click "Add" , then "Close."
• In the Geometry Group dropdown, select "Tie Beam Rebar", then click "Apply."
• Next, enter "-5.7, 0" in the Position field and click "OK."

Then, go to Geometry > Transform > Move/Copy. In the Move dialog box:

• Click "Select Target" and select the newly created tie beam rebar in the model window.
• Set the Direction to the Y-axis, check "Copy (Uniform)",
• Enter a Distance of 0.1 m, Number of Copies as 1,
• Add and select the "Tie Beam Rebar" group, then click "Apply."

Go to Geometry > Transform > Move/Copy. In the Move dialog box:

• Click "Select Target", then select the tie beam rebars created in the previous step.
• Set the Direction to the Y-axis, check "Copy (Uniform)",
• Enter a Distance of 0.12 m and Number of Copies as 11,
• Choose the "Tie Beam Rebar" group, then click "Apply."

Next, again go to Move/Copy:

• Click "Select Target", and select all tie beam rebars in the model window.
• Set the Direction to the Z-axis, check "Copy (Uniform)",
• Enter a Distance of -0.66 m, Number of Copies as 1,
• Add and select the "Tie Beam Rebar" group, then click "Apply."

One more time, go to Move/Copy:

• Click "Select Target", then select the two outermost tie beam rebars on the top layer.
• Set the Direction to the Z-axis, check "Copy (Uniform)",
• Enter a Distance of -0.08 m, Number of Copies as 7,
• Select the "Tie Beam Rebar" group, and click "OK."

Figure 4.14 Regular Rebar in the Bridge Pier

5 Defining Materials and Properties

5.1 Defining Structural Material

1. In the main menu, go to Mesh > Property/Coordinate/Function > Material to open the Add/Modify Material dialog box.
   Click "Create" > "Isotropic" to open the Material dialog box.

Figure 5.1-1 Defining Materials

In the Name field, enter "Concrete", and select the "Concrete Smeared Crack" as the material model type.

Under the "General" tab:

• Elastic Modulus: 34,500,000
• Poisson's Ratio: 0.2
• Unit Weight: 26
• Thermal Expansion Coefficient: 1e-005

This example uses the smeared crack model for crack analysis, where cracks are distributed throughout the element without element separation. It is typically used for reinforced concrete structures with a dense rebar layout.

Under the "Nonlinear" tab:

• Click the icon next to "Tension Function".
  • Enter "Tension Function" as the name
  • Set the Model Type to "Constant"
  • Input Ft = 2400 kN/m², then click "OK"
• Then click the icon next to "Compression Function"
  • Enter "Compression Function" as the name
  • Set the Model Type to "Constant"
  • Input Fc = 26,800, then click "OK"

Finally, assign the defined Tension Function and Compression Function,
Set Stiffness to Secant, and click "OK" to confirm.

Figure 5.1-2 Defining Nonlinear Concrete Material

2. In the Name field, enter "Tendon", and select "Elastic" as the model type.
Under the "General" tab:

• Elastic Modulus: 200,000,000
• Poisson's Ratio: 0.3
• Unit Weight: 78.5
• Thermal Expansion Coefficient: 1.2e-005
  Click "Apply" to confirm.

3. In the Name field, enter "Rebar", and select "Elastic" as the model type.
Under the "General" tab:

• Elastic Modulus: 206,000,000
• Poisson's Ratio: 0.31
• Unit Weight: 78.5

• Thermal Expansion Coefficient: 1.2e-005

  Click "OK" to confirm.

5.2 Defining Properties

1. In the main menu, go to Mesh > Property/Coordinate/Function > Property to open the Add/Modify Property dialog box.

   Click "Create" > "3D" to open the Create/Modify 3D Property dialog box.

Figure 5.2-1 Defining Property

In the Name field, enter "Concrete".

In the Label field, also enter "Concrete", and select "Concrete" as the material.

Then click "OK" to confirm.

Figure 5.2-2 Defining 3D Property

2. Click "Create" > "1D" to open the Create/Modify 1D Property dialog box.
Select the "Tendon" tab.

• In the Name field, enter "Prestressed Tendon"
• Set Constitutive Model to "Linear Elastic"
• Select Material: 2 - Tendon
• Input Tendon Area: 0.0021
• Check the box for Relaxation Factor

Code: JTG3362-2018

Relaxation Factor: 0.2

• Characteristic Strength: 1,860,000
• Wobble Friction Coefficient: 0.3
• Sliding Friction Coefficient: 0.0015
• Initial Stress (Start): 0.006

• Initial Stress (End): 0.006

  Click "Apply" to confirm.

3. Next, select the "Embedded Truss" tab.

• In the Name field, enter "Rebar"
• Set Constitutive Model to "Linear Elastic"
• Select Material: 3 - Rebar

• Input Cross-Sectional Area: 4.91e-4

  Click "OK" to confirm.

Figure 5.2-3 Defining Tendon Property

5.3 Mesh Generation

1. In the main menu, go to Mesh > Generate > 3D to open the Generate Mesh (Solid) dialog box.
   Click the "Auto - Solid" tab.

• In the model window, select the pier.
• Set Seeding Method to "Size", and enter 0.5.
• In the dropdown menu, select "Hybrid Mesh Generator" and check "Match Adjacent Faces".
• Set Property to "Concrete".
• Enter "Pier" as the Mesh Group Name, then click "OK" to generate the mesh.

Figure 5.3-1 Generating Solid Mesh

Note:

• Matching adjacent faces is based on the global coordinate system.
• When generating solid mesh, you can click the button at the bottom right of the Generate Mesh (Solid) dialog box to enable options such as higher-order elements and mid-side node generation.

2. In the main menu, go to Mesh > Generate > 1D to open the Generate Mesh (Line) dialog box.

In the Model Tree > Geometry, check only "Rebar" and "Tie Beam Rebar".

In the model window, select the rebars.

• Set Seeding Method to "Division" and enter 10
• Set Property to 3: Rebar
• Enter "Rebar" as the Mesh Group Name, then click "Apply."

3. In the Model Tree > Geometry, check only "Tendon".

In the model window, select the two tendon lines.

• Set Seeding Method to "Division" and enter 10
• Set Property to 2: Prestressed Tendon
• Enter "Tendon" as the Mesh Group Name, then click "OK."

Note: You can select geometry or mesh elements either directly from the model window or via the "Geometry" section in the Model Tree – Model Tab for mesh generation.

Figure 5.3-2 Generating Mesh for Rebars

5.4 Setting Boundary Conditions

In the main menu, go to Static/Slope Analysis > Boundary > Constraint to open the Constraint dialog box.

• Select the "Basic" tab
• In the Name field, enter "Pier Base Fixity"
• Set Type to "Node"
• In the model window, select all nodes at the base of the pier
• Set the Condition to "Fixed"
• Enter "Boundary Group - 1" as the Boundary Group Name
• Click "OK" to confirm.

Figure 5.4-1 Defining Boundary Conditions

Note:

• In the "Advanced" tab of the Constraint dialog box, boundary conditions can be defined based on degrees of freedom or stacked planes.

  You can also use the "Auto" tab to automatically assign boundary conditions.

5.5 Defining Loads

1. To add self-weight, go to Static/Slope Analysis > Static Load > Self Weight   from the main menu.

   In the Self Weight dialog box:

• Enter “-1” in the Gz component
• Set the Load Group Name to "Self-Weight"
• Click "OK" to confirm.

Figure 5.5-1 Applying Self-Weight Load

2. To apply the weight of the superstructure, go to Static/Slope Analysis > Static Load > Pressure from the main menu.

In the Pressure dialog box:

• Select the "Surface" tab
• Enter "Superstructure Weight" as the Name
• Set the Type to "3D Element Face"
• Set Direction to "Normal"
• Check the "Uniform Load" option
• In P or P1, enter 5000
• Set the Load Group Name to "Uniform Load"
• Click "OK" to confirm.

Figure 5.5-2 Applying Pressure Load

Note:
In the Model Tree – Analysis tab, right-click on Pressure and select Display Options.

In the pop-up Options dialog box, under Load/Boundary Conditions, click "Pressure" and check "Display Values" on the right to view the applied load magnitudes.

3. To apply prestressing to tendons, go to Static/Slope Analysis > Static Load > Prestress from the main menu.
In the Prestress dialog box:

• Set Element Type to "Tendon"
• Set Target Type to "Mesh Group"
• Select the two tendon mesh groups
• Under Post-Tensioning Method, choose "Stress Input"
• For Initial Tensioning, select "Both" (Start and End)
• Enter 1,200,000 in both Start and End fields
• Set the Load Group Name to "Prestressing"
• Click "OK" to confirm.

Figure 5.5-3 Applying Prestress to Tendons

4. To apply the braking force, first create a node at the center of the bearing surface.

• Click the "Top View" icon from the toolbar.
• Then go to Mesh > Node > Create Node from the main menu to open the Node Control dialog box.
• In the "Node" tab, select "Between Two Nodes",
  then click "Select Node 1" and choose Node 1 and Node 2 in the model window, as shown in Figure 4.5-4.
• In the Mesh Group field, enter "Pier Top Center".

Figure 5.5-4 Creating Center Node at Bearing Surface

5. From the main menu, go to Mesh > Property/Coordinate/Function > Property to open the Add/Modify Property dialog box.

• Click "Create" > "Etc." to open the Create/Modify Other Property dialog box.

• Select "Rigid Link", enter "Rigid Connection" as the name, and under Common Type, choose "Rigid Body".

  This will automatically check all degrees of freedom under Property.

Next, go to Mesh > Element > Create to open the Create/Delete Element dialog box.
In the "Etc." tab, select "Rigid Link" from the dropdown list.

• Click "Select Node 1" and select the center node created at the bottom of the bearing surface.
• Then click "Select Node(s)" below it and choose the remaining 20 nodes at the top of the pier.
• Set Property to "Rigid Connection"
• In the Mesh Group field, enter "Rigid Connection" and click OK to create.

Figure 5.5-5 Creating Rigid Connection Between Bearing

Surface Center Node and Other Nodes

Go to Static/Slope Analysis > Static Load > Nodal Force from the main menu to open the Nodal Force dialog box.

• In the Name field, enter "Braking Force"
• Set Target Type to "Node"
• Select the two center nodes created at the bottom of the bearing surface
• Leave the default settings in Reference Target, Type, and Coordinate System
• Enter 250 (kN) in the Y field
• Set the Load Group Name to "Braking Force", then click OK to confirm.

5.6 Defining the Analysis Case

From the main menu, go to Analysis > Analysis Case > New to open the Add/Modify Analysis Case dialog box.

• In the Title field, enter "Crack Analysis of Concrete Bridge Pier"
• Set the Solution Type to "Nonlinear Static"
• Click "All Groups" to move all relevant mesh groups, boundary conditions, and static loads to the "Activated Groups" section.

Then click the shortcut button next to "Analysis Control":

• In the Nonlinear tab:
  • Under Load Step, set Number of Steps to 10
  • Under Convergence Criteria, check only "Displacement", and set the value to 0.01

Click the shortcut next to "Output Control" ,

• In the Output Type, check the desired output options as shown in the figure,
• Finally, click "OK" to confirm.

Figure 5.6-1 Analysis Case

Figure 5.6-2 Analysis Case

From the main menu, go to Static/Slope Analysis > Options.

In the "Analysis/Results" tab, check "Standard (Stable)" under Element Processing Method, then click "OK" to confirm.

6. Post-Processing of Analysis Results

In the main menu, go to Analysis > Run.
In the FEA NX Solver dialog box, check the case titled "Crack Analysis of Concrete Bridge Pier" with the type set as "Nonlinear Static", then click "OK" to run the analysis.

After the analysis is complete, go to the Results tab in the Model Tree, where you can view 3D Element Crack Results.

The Crack Status is categorized as follows:

• Fully open during loading/unloading
• Partially open during loading/unloading
• Closed cracks
• No cracks formed

In the main menu, go to Results > General > No Result Display , and you can choose "Feature Line" as the display mode.

Figure 6.1 3D Element Crack Results

Note:
Differences in mesh type and mesh size can lead to variations in the crack status and 3D element crack stress results after nonlinear analysis.
The screenshots provided in this example reflect the outcomes based on the current mesh configuration and element size.

"CRACK STRESS/STRAIN/WIDTH" is categorized into three directions:

• NN (Normal): Perpendicular to the crack plane (disk face)
• NS (Shear): Along a line within the crack plane (disk edge)
• NT (Tangential): Along the arrow direction within the crack plane

These directions are shown as illustrated below.

Figure 6.2 3D Element Crack Stress Results

In the Model Tree, under "Property", select "Legend".
Change the "Decimal Places" setting to 3 to adjust the number of decimal places shown in the legend.
Then click "Apply" to confirm.

Figure 6.3 Display Value Settings