Simcenter 3D Solutions How to model thermal connections of bolts, nuts, holes, and flanges

Open the Simulation file 

You will open the Simulation file and reset the dialog box settings to ensure that they are in the expected initial state. 

1. Choose File→Open and open bolts_nuts_connection\nuts_and_bolts.sim. 

2. Choose File→Preferences→User Interface and on the Dialog and Precision page, reset the dialog box memory. 

3. Click OK. 

The model consists of two parts: 
    - The 3D model of two flanges fastened together by 8 bolts and nuts. 
    - The 2D axisymmetric representation of the 3D model. 

Stitch free edges in a 2D model  

You will inspect and stitch free edges for a 2D model within solid bodies of bolts, and flanges to correctly model heat conduction through the bodies.  

1. Choose Home tab→Tools group→Model Display Preferences. 

2. On the Polygon Edges page, in the Free Edges group, select the Display Free Edges check box. 

3. Click OK. 
   The free edges are displayed in the graphics window. Notice that the flange bodies have free edges that are not connected. You must connect geometrically disconnected parts to model heat conduction through the bodies. You can thermally connect the bodies by stitching the edges or creating thermal coupling between them. In this example, you will stitch free edges between flanges.   
    

4. In the Simulation Navigator, expand the  assembly1_aasyfem1.afm node, right-click the model3_fem1.fem node and choose Make Work Part. 

5. Choose Home tab→Polygon Geometry group→Stitch Edge . 

6. In the graphics window, select the two flange bodies. 

7. Click OK. 

8. Choose Home tab→Tools group→Model Display Preferences. 

9. On the Polygon Edges page, in the Stitched Edges group, select the Display Stitched Edges check box. 

10. Click Apply. 
    Notice that the stitched edge of the two flanges is displayed in blue. 
     

11. Clear the Display Free Edges and Display Stitched Edges check boxes. 

12. Click OK. 

Mesh the flange with axisymmetric elements 

You will create a mesh collector and define the mesh for two flanges using axisymmetric elements since the geometry of flanges is a solid of revolution.  

1. Choose Home tab→Mesh group→2D Mesh . 

2. In the graphics window, select the four faces of two flanges. 
    

3. From the Type list, select Axisymmetric Linear Quadrilateral. 

4. In the Element Size box, type 0.5. 

5. In the Destination Collector group, click New Collector . 

6. In the Physical Properties sub-group, from the Solid Property list, select Solid 1, which is the predefined solid with the AISI_310_SS material. 

7. In the Name box, type AXI. 

8. Click OK to close both dialog boxes. 

Mesh the hole with plane stress elements 

You will create a mesh collector and define the mesh for holes in the flanges. You will create the mesh using plane stress elements for the holes with associated thickness. 

1. Choose Home tab→Mesh group→2D Mesh . 

2. In the graphics window, select the three faces as shown in this example.  

3. In the Element Properties group, in the Type box, select Plane Stress Linear Quadrilateral. 

4. In the Destination Collector group, click New Collector . 

5. In the Physical Properties sub-group, from the Plane Property list, select Plane Property 1, which is predefined plane property with the material AISI_310_SS material. 

6. In the Name box, type PS_HOLES. 

7. Click OK. 

8. In the Advanced Parameters group, from the Create Separate Meshes list, select On-For Each Face to create separate meshes per associative thickness. This will ensure correct thermal coupling between the bodies. 

9. Click OK. 

10. In the Simulation Navigator, expand the model3_fem1.fem→2D Collectors→ PS_HOLES mesh collector. 

11. Under the PS_HOLES mesh collector, click SHIFT and select three meshes, then right-click and choose Edit Mesh Associated Data. 

12. In the Element Properties group, from the Thickness Source list, select Hole to instruct the software to compute the thickness of material minus pattern of holes. 

13. From the Centerline Definition list, select Vector and Point to define centerline using the vector and point. 

14. From the Specify Vector list, select ZC-axis. 

15. In the Exclude Edges Transverse to Centerline sub-group, click Select Edge and select the two highlighted edges to exclude them from the thickness calculations. 
     

16. In the Number of Instances box, type 8. 
    Each instance represents a copy of the hole as the mesh is rotated around the rotational axis. 

17. Click OK. 

Mesh the bolt with plane stress elements 

You will create a mesh collector and define the mesh for bolts in the flanges. 

1. Choose Home tab→Mesh group→2D Mesh . 

2. In the graphics window, select three faces of the bolt geometry. 
   Tip: To facilitate the selection of the bolt face, deselect the nut polygon geometry. 
    

3. In the Element Properties group, make sure that Plane Stress Linear Quadrilateral is selected. 

4. In the Destination Collector group, click New Collector . 

5. In the Physical Properties sub-group, from the Plane Property list, select Plane Property 1. 

6. In the Name box, type PS_BOLTS. 

7. Click OK to close both dialog boxes. 

8. In the Simulation Navigator, under the PS_BOLTS mesh collector, click SHIFT and select three meshes, right-click and choose Edit Mesh Associated Data. 

9. In the Element Properties group, from the Thickness Source list, select Bolt to instruct the software to compute the thickness of a pattern of bolts. 

10. From the Centerline Definition list, select Vector and Point. 

11. From the Specify Vector list, select ZC-axis. 

12. In the Exclude Edges Transverse to Centerline sub-group, click Select Edge and select the two highlighted edges to exclude them from the thickness calculations. 
     

13. In the Number of Instances box, type 8. 
    Each instance represents a copy of the bolt as the mesh is rotated around the rotational axis. 

14. Click OK. 

15. In the Simulation Navigator, right-click PS_BOLTS and choose Plot Thickness Contour to verify if the bolt thickness is correctly defined. 
     
    Note that the thickness is zero on the edges of the bolt, and the highest thickness is 280 mm in the centerline of the bolt head. 

16. Chose Home tab→Context group→Return to Model . 

Mesh the nut with plane stress element and define its thickness 

You will create a mesh collector and define mesh for nuts.  

1. Choose Home tab→Mesh group→2D Mesh . 

2. In the graphics window, select three faces of the nut geometry. To facilitate the selection, you can deselect the PS_BOLTS mesh collector and Bolt geometry. 
    

3. In the Element Properties group make sure that Plane Stress Linear Quadrilateral is selected. 

4. In the Destination Collector group, click New Collector . 

5. In the Physical Properties sub-group, from the Plane Property list, select Plane Property 1. 

6. In the Name box, type PS_NUTS. 

7. Click OK to close both dialog boxes. 

Determine area factor for modeling nut thickness 

Since there is no predefined thickness source for the nut, you will define the nut thickness with an expression. You must determine the area factor for the 2D nut mesh so that the total nut mass is the same in 3D and 2D.  

1. In the Simulation Navigator, under the PS_NUTS mesh collector, click SHIFT and select nut mesh under PS_NUTS, right-click and choose Edit Mesh Associated Data. 

2. In the Element Properties group, in the Thickness sub-group, from the Thickness Source list, select Field/Expression. 

3. In the Thickness box, type 2*pi()*radius to define the thickness of the nut, disregarding the hole inside. 

4. In the Number of Instances box, type 8.  

5. Click OK.  

6. In the Simulation Navigator, under PS_NUTS, right-click the first nut mesh and select Solid Properties. 

7. In the Information window, check the total mass. It shows that the total mass is 8.24843 kg. 

8. Close the Information window. 

9. Repeat steps 6-8 for each nut mesh to verify the masses of each nut and sum them. The sum is 31.373724 kg. 

10. To verify the total mass in 3D model, right-click model2_fem1.fem x 8 and select Open in Window. 

11. In the opened window, expand 3D Collectors→Nut, right-click the nut mesh and select Solid Properties. 

12. In the Information window, verify that the total mass is 0.09338785 kg. 

13. Compute the area factor as 0.09338785/31.373724=0.002976626. 

Define the correct nut mesh thickness 

1. Return to the Simulation file window. 

2. Select the nut mesh under PS_NUTS mesh collector, right-click and choose Edit Mesh Associated Data. 

3. In the Thickness box, type 0.002976626*2*pi()*radius to add the correction factor. 

4. Click OK. 
   Verify that the total mass now is the same as in 3D model. 

Explore predefined boundary conditions for 3D and 2D models 

1. In the Simulation Navigator, right-click the nuts_and_bolts.sim node and choose Make Work Part. 

2. Expand the Simulation Object Container and Constraint Container. 
   The following boundary conditions are defined: 
      Advanced Controls simulation object with the PLOT BC SUMMARY advanced parameter, that generates HTML file that displays convective area for thermal couplings. 
      Advanced Controls simulation object with the DISPLAY BC SUMMARY TABLES advanced parameter, that describes the data stored for each thermal coupling in the model. 
      Thermal coupling simulation objects to model thermal connection between bolt and the first flange, nut and bolt, nut and second flange, nut and flange face, bolt head and flange for 3D model.  
      Temperature constraints on the surface of the flanges and top of the bolts to model thermal conduction through the model. 

Connect the bolt and flange faces for the 2D model 

You will model the thermal connection between the bolt face meshed with plane stress elements, and the flange face meshed with the axisymmetric elements. 

1. In the Simulation Navigator, right-click the Simulation Object Container node and choose New Simulation Object→ Thermal Coupling. 

2. Deselect all mesh collectors and under the Polygon Geometry node, select the Bolt check box. 

3. In the Name group, type 2D_Bolt-Flange. 

4. For the primary region, select the bolt face as it is smaller face than the face of the flange. 
    

5. For the secondary region, select the two flange faces that are in contact with the bolt. 
    

6. In the Magnitude group, from the Type list, select Heat Transfer Coefficient. 

7. In the Coefficient box, specify 100 W/(m2·°C). 

8. In the Additional Parameters group, make sure that the Only Connect Overlapping Elements check box is selected to instruct the solver to connect elements in terms of proximity and an overlap check. 

9. Click OK. 

Connect the nut and bolt faces for the 2D model 

You will model the thermal connection between the nut face meshed with plane stress elements and the bolt face meshed with plane stress elements. 

1. In the Simulation Navigator, right-click the Simulation Object Container node and choose New Simulation Object→ Thermal Coupling. 

2. In the Name group, type 2D_Nut-Bolt. 

3. For the primary region, select the bolt face that is in contact with the nut. 
   Tip: Deselect the nut geometry to select the correct bolt face.  
    

4. For the secondary region, select the nut face that is in contact with the bolt. 
   Tip: Deselect the bolt geometry to select the correct nut face.  
    

5. In the Magnitude group, from the Type list, select Heat Transfer Coefficient. 

6. In the Coefficient box, specify 100 W/(m2·°C). 

7. In the Additional Parameters group, make sure that the Only Connect Overlapping Elements check box is selected. 

8. Click OK. 

Connect the nut and flange edges for the 2D model 

You will model the thermal connection between the nut edge meshed with plane stress elements and the flange edge meshed with axisymmetric elements. 

1. In the Simulation Navigator, right-click the Simulation Object Container node and choose New Simulation Object→ Thermal Coupling. 

2. In the Name group, type 2D_Nut-Flange. 

3. For the primary region, select the three highlighted nut edges. 
   Tip: Use filter Polygon Edge. 
    

4. For the secondary region, select the three flange edges that are in contact with the nut. 
    

5. In the Magnitude group, from the Type list, select Heat Transfer Coefficient. 

6. In the Coefficient box, specify 100*5184/785 W/(m2·°C). 
   Tip: This area correction is found by solving the model once with 100 W/m²°C. In the BC data summary, we get an area of 783 mm² for this BC. The convection area is supposed to be equal to the side of the nut, 5184 mm². 

7. In the Additional Parameters group, make sure that the Only Connect Overlapping Elements check box is selected. 

8. Click OK. 

Connect the nut and flange faces for the 2D model 

You will model the thermal connection between the nut face meshed with plane stress elements and the flange face meshed with axisymmetric elements. 

1. In the Simulation Navigator, right-click the Simulation Object Container node and choose New Simulation Object→ Thermal Coupling. 

2. In the Name group, type 2D_Nut-Flange_faces. 

3. For the primary region, select the three nut faces that are in contact with the flange. 
   Tip: Use filter Polygon Face. Deselect Bolt geometry if it is selected. 
    
    

4. For the secondary region, select the flange face that is in contact with the nut. 
    
    

5. In the Magnitude group, from the Type list, select Heat Transfer Coefficient. 

6. In the Coefficient box, specify 100*8796/2800 W/(m2·°C). 
   8796/2800 is the area correction factor, where 2800 mm2 is the area of the nut's polygon surface multiplied by the number of instances. 8796 mm2 is the area of the interior of the nut.  

7. In the Additional Parameters group, make sure that the Only Connect Overlapping Elements check box is selected. 

8. Click OK. 

Connect the bolt head and flange edges for 2D model 

You will model thermal connection between the bolt edge meshed with plane stress elements and the flange edge meshed with axisymmetric elements. 

1. In the Simulation Navigator, right-click the Simulation Object Container node and choose New Simulation Object→ Thermal Coupling. 

2. In the Name group, type 2D_Bolt_Head-Flange. 

3. For the primary region, select three highlighted bolt head edges. 
   Tip: Use filter Polygon Edge. To facilitate the selection, deselect the flange geometry. 
    

4. Deselect the bolt geometry and for the secondary region, select the three flange edges in contact with the bolt. 
    

5. In the Magnitude group, from the Type list, select Heat Transfer Coefficient. 

6. In the Coefficient box, specify 100 W/(m2·°C). 

7. In the Additional Parameters group, make sure that the Only Connect Overlapping Elements check box is selected. 

8. Click OK. 

Solve the model 

1. In the Simulation Navigator, double-click the assembly1_assyfem1.afm node to make work part.  

2. Right-click the assembly1_assyfem1.afm node and select Assembly Check→Assembly Label Manager to resolve label conflicts in your assembly file. 

3. In the Automatic Label Resolution group, click Automatically Resolve. 

4. Click OK. 

5. Right-click the nuts_and_bolts.sim node and select Make Work Part. 

6. Right-click the Solution node and choose Solve. 

7. Click OK. 
   When the solution is complete, the Analysis Job Monitor displays the status as Completed Successfully.   

8. Close the Information window. 

9. Click Cancel in the Analysis Job Monitor dialog box. 

Display results 

Display the temperature results. 

1. In the Post Processing Navigator, double-click the Thermal node to load the results. 

2. Expand Thermal and double-click Temperature - Element. 
    

3. Expand the Post View 1→Mesh Collectors→assembly1_assyfem1.afm→model3_fem1.fem node and clear AXI, PS_HOLES, model1_fem2.fem, 2D Elements check boxes to compare the temperature for bolts and nuts. 
    

4. To display nut results for 2D model, deselect the PS_BOLTS, check box. 

5. To display nut results for 3D model, clear all eight model2_fem1.fem check boxes. Expand first model2_fem1.fem and select Nut check box. 
    

Investigate thermal coupling areas in the HTML file 

The model contains the PLOT BC SUMMARY advanced parameter. You will compare the coupling areas for 3D nut and bolt coupling with 2D nut and bolt coupling. 

1. From the solution directory, open the nuts_and_bolts-Solution_data.html file. 

2. In the graphics, select Thermal Coupling. 

3. From the Property Type list, select Area. 

4. From the Select Thermal Coupling list, select 3D_Nut-Bolt. 

5. From the Select Second Thermal Coupling list, select 2D_Nut-Bolt. 
    
   Note that convective areas are in good agreement between 3D model and 2D axisymmetric representation. 

You have completed this lab.