Contents

1. Overview

This tutorial outlines the procedure for conducting a detailed Bridge Joint Analysis using Midas CIVIL NX and Midas FEA NX. The process involves exporting a specific joint from a Midas CIVIL NX model, performing a detailed solid element analysis in FEA NX, and then importing the results back into CIVIL NX to observe the behaviour within the global structure. 

2.Step-by-Step Procedure

Detailed Step to do Truss Joint Analysis

2.1 Export Joint from Midas CIVIL NX 

The first step is to isolate and export the specific joint from the main bridge model in Midas CIVIL NX. Procedure:

1. In your Midas CIVIL NX project, select the joint members you wish to analyze. 

2. Navigate to the Export menu. 

3. Choose the option Frame Section for Solid. 

4. In the export dialog, set Divisions in element to 0. 

5. Select the target elements for export. Click OK. 

6. Save the file with the name Arch_bridge.mcs.

2.2 Model Setup and Geometry in Midas FEA NX

With the joint exported, we will now set up the Midas FEA NX environment and import the geometry for detailed modification.

2.2.1 Initial Setting 

1. Launch Midas FEA NX & Create a New file. 

In the "Analysis Setting" window, ensure the Model Type is 3D. 

2. Set the Unit System to kN, m, sec. and Click OK. 

3. Save As... to save your new project file.

2.2.2 Import Model 

1. From the main ribbon, select Frame to Solid.

2. Browse and select the Arch_bridge.mcs file you exported from CIVIL NX. 

3. Click Open. 

4. Click OK in the import dialog to generate the solid geometry from the frame elements.

2.3 Geometry Modification

This phase involves refining the imported geometry to accurately represent the joint and add necessary components like gusset plates. 

2.3.1 Initial Set-up

1. Move Work Plane: Right-click on the Work Plane in the model tree and select Move. Set the offset to 0.25. 

2. Define Grid: Click the Define Grid icon. Set Number to User Defined and enter 50 and Click OK. 

2.3.2 Divide and Delete Overlapping Solid

1. Divide Solid: Go to Geometry Divide Solid. Select the main members as the Target Solids. For the Dividing Tool, use the Dividing Plane option, set to the Z plane at a position of 1.1 m & Click OK. 

2. Delete Coinciding Portion: Select the unnecessary portion of the divided solid and press the Delete key.

2.3.3 Create Gusset Plate

1. Create Points for Gusset Plates: Use the Geometry >Point & Curve >Point tool to create points that will define the layout of the gusset plates. 

2. Translate Points: Use the Geometry >Transform >Translate tool to copy these points to create the required layout. For the first translation, use a distance of 2.5/2. Repeat this for distances of 2.5/4, -2.5/4, and -2.5/2.

3.Go to Geometry > transform > Translate and select the nodes as in fig below  & Copy at Distance = 1.5 and Times =1 , Click OK.

4.Select “a” node Click on 2 points shown in fig Below.Now Method > MOVE and Distance >  0.3 >Click on APPLY

Repeat the process for “b” node and Distance > -0.3

5. Create Polylines: Go to Geometry > Point & Curve > Polyline. Connect the points you created to form the outline of the gusset plates. 

6. Create Gusset Plate Face: Go to Geometry>Surface & Solid > Make Face. Select the edges of the polyline you just created to form a surface. Assign this to a new Geometry Set named "Gusset". 

7. Extrude Gusset Plate: Go to Geometry > Protrude > Extrude. Select the face of the gusset plate. Use the 2-Point Vector to define the extrusion direction and set the Length to 0.02. Ensure Make Solid and Fuse are checked.

2.3.4 Fuse the Solid

1. Final Geometry with Boolean Operations: Use the Geometry Boolean Solid tool. Use the Fuse option to merge all the individual solid components (arch members, gusset plates) into a single, continuous solid body. Ensure Merge faces and Delete Tool are checked.

2.Remove additional part and Fuse: Geometry > Divide > Solid and Select Target object.

Select Tool as mentioned in fig. and Check on Delete Original , Geometry set > gusset >Click on OK

Select and Delete the “B” member and Go to Geometry > Boolean > Solid , Click on Fuse > Select all objects and Check on Merge faces and Delete tool >Click on OK

2.4 Define Materials and Properties 

2.4.1 Define Material

Navigate to Mesh Material and Click Create Isotropic. 

Select the DB (Database) and choose Steel of grade S355 from the EN05(s) standard. > Click OK. 

2.4.2 Define 3D Property

Navigate to Mesh Property and Click Create 3D. 

Name the property (e.g., "3D_Property") and assign the steel material you just created and Click OK.

2.5 Meshing the Solid

1. Navigate to Mesh > Generate > 3D. 

2. Select the Auto-Solid option. 

3. Select the entire structure. 

4. Set the mesh Size to 0.1. 

5. Assign the 3D Property you created. and Click OK to generate the tetrahedral mesh.

2.6 Create Rigid Links 

Rigid links are used to apply the nodal displacements from the 1D frame model in CIVIL NX to the 3D solid faces in FEA NX. 

2.6.1 Create Center Points

For each of the 6-member faces, create diagonal lines using Geometry > Line. Then, create a point at the center of each diagonal using Geometry > Point. 

2.6.2. Create Center Nodes

Go to Mesh > Node > Create and create a node at each of the central points you just made. 

2.6.3. Create Rigid Links

 Go to Mesh > Element > Create > Other. 

Select Rigid Link. For each member face, use a polygon selection to select all the nodes on that face. ○ Deselect the central node you created. For the Master Node, select the central node. 

Define a new "RIGID" property for the rigid body.Click OK and repeat for all 6 member faces.

2.7 Assign Displacements 

1. Get Displacements from CIVIL NX:  Return to your original Midas CIVIL NX model.  Go to Results > Result Tables > Displ. ○ Extract the nodal displacements (Tx, Ty, Tz, Rx, Ry, Rz) for the relevant load case (e.g., LCB1) at the nodes corresponding to the joint. 

2. Assign Displacements in FEA NX: In FEA NX, go to Static Analysis > Static Load > Disp.  For each of the 6 central nodes (the master nodes of your rigid links), create a new displacement load. Copy the corresponding displacement values (Tx, Ty, Tz, Rx, Ry, Rz) from the CIVIL NX results table and paste them into the dialog. Click Apply and repeat for all 6 nodes.

2.8 Perform Analysis Procedure 

1. Navigate to Analysis > Analysis Case > General. 

2. Give the analysis case a Title (e.g., "Joint Analysis"). 

3. Ensure all load and boundary sets are moved to the Active Sets and Click OK.

4. Click the Perform icon to run the analysis.

2.9 Review Results 

1. Solid Stresses: In the results tree, go to Solid Stresses and select S-Von Mises to view the stress distribution in the joint. 

2. Displacements: In the results tree, go to Displacements and select Total Translations to view the displacement pattern.

2.10 Import Results Back to Midas CIVIL NX 

1. Export from FEA NX: Click Export midas civil and save the results as a .mct file. 

2. Prepare CIVIL NX Model:  In your Midas CIVIL NX project, delete the original frame members of the joint.Go to Properties Material Properties. Modify the existing material by giving it a new ID (e.g., 11) to avoid conflicts. 

3. Renumber Nodes and Elements: Go to Node/Element Renumbering. Renumber all existing nodes to start from a high number (e.g., 10000) and all existing elements to start from a high number (e.g., 30000). This prevents overlap with the imported data. 

4. Import MCT File: Go to APPS MCT COMMAND SHELL. Open the JOINT ANALYSIS.mct file you exported from FEA NX. Delete any unnecessary data (like REBAR data if present) and click RUN. 

5. Merge Nodes: Go to Node/Element Merge. Select the intersecting nodes between the imported solid model and the existing frame model and merge them. Repeat for all 6 connection points. 

6. Perform Final Analysis: Run the global analysis again in Midas CIVIL NX (Analysis Perform Analysis).

2.11 View Final Results in Midas CIVIL NX 

1. Navigate to Results Stresses Solid Stresses. 

2. Select the desired load case (e.g., Dead Load). 

3. Click Apply to view the detailed stress results of the joint integrated within the full bridge model.