Define a bolt pre-load (ANSYS)

Define the bolt

1. In the FEM file, use the 1D Mesh command to create PRETS179 elements to model the axial pretension within the bolt shank. Ensure that the meshes that the PRETS179 elements connect match exactly.For more information, see 1D meshing.

2. (Optional) Use the 1D Connection command to connect the PRETS179 elements to the mesh on the surrounding part using either MPC184 type elements or BEAM4 type elements (defined with very stiff properties). For more information, see 1D Connection and MPC184 or BEAM4 in the ANSYS Element Reference Manual.

3. Define an appropriate pre-tension node for the bolt.In the Simulation Navigator, right-click the PRETS179 mesh and choose Edit Mesh Associated Data.In the Mesh Associated Data dialog box, use the Select Pretension Node option to select the appropriate pretension node from the graphics window.In the PRETS179 dialog box, use the SECDATA options to other options for the pre-load. For more information, see Defining the pre-tension section options.

After you specify the pretension node, you can either use the options in the Pretension load (SLOAD) group in the PRETS179 dialog box or the Bolt Pre-Load command to complete the definition of the bolt pre-load. See Defining the bolt pre-load options for a discussion of the criteria you should use to determine where to define the bolt pre-load.

Define the bolt pre-load in the PRETS179 physical properties

1. Use the Force/Displacement key (KFD) option to specify the type of pre-load to create. Select FORC to apply a concentrated load (force) to the bolt.Select DISP to apply a tightening adjustment to change the length of the bolt.

2. Depending upon the KFD option you selected, use the FDVALUE option to specify the value of either the pre-tension force or displacement.

3. Use the Initial Action Key (KINIT) option to control how the software applies the pre-load.Select LOCK to have the software apply the specified pre-load in the current load step and then lock the load value in the next load step.Select SLID to have the software apply the specified pre-load in the current load step and then not maintain the specified preload in the next load step.Select TINY to have the software apply a very small pre-tension load (equal to 0.1% of the specified Force) to the bolt. Do this if you selected FORC from the KFD list.For more information, see Bolt Pre-Load dialog box (ANSYS).

4. Use the LSLOAD option to specify the number of the load step to which to apply the defined FDVALUE.

5. If you selected FORC from the KFD list, use the LSLOCK option to specify the number of the load step in which the software locks the displacement value resulting from the pre-tension force.

Define the bolt pre-load as a load on selected elements

1. Click OK in the PRETS179 dialog box.

2. Switch to the Simulation file and make the appropriate solution step active.

3. Choose Home tab→Loads and Conditions group→Bolt Pre-Load .

4. In the Bolt Pre-Load dialog box, select the Type of pre-load to create. Select Force on 1D elements to apply a concentrated load (force) to the bolt.Select Adjustment on 1D elements to apply a tightening adjustment to change the length of the bolt.

5. [Optional] Specify a name for the load from the Bolt Pre-Load dialog box.

6. In the Model Objects group, click Select Object and select the PRETS179 elements or curves to which to apply the pre-load.

7. In the Magnitude group, define the pre-load force or the tightening adjustment in one of these ways:Select Expression to use a constant value or expression to define the magnitude. For more information, see Expressions. Select Field to define magnitude that varies with frequency, time, or temperature. For more information, see Using fields and expressions to define boundary conditions.

8. Use the KINIT option to control how the software applies the pre-load.Select LOCK to have the software apply the specified pre-load in the current load step and then lock the load value in the next load step.Select SLID to have the software apply the specified pre-load in the current load step and then not maintain the specified pre-load in the next load step.If you selected Force on 1D elements from the Type list, select TINY to have the software apply a very small pre-tension load (equal to 0.1% of the specified Force) to the bolt.For more information, see Bolt Pre-Load dialog box (ANSYS).

9. Click OK.The load is applied to the model.

How do I

Define a bolt pre-load for a bolt modeled with beam elements (Abaqus)

Learn more

Bolt pre-load

Bolt pre-loads with Simcenter Nastran and Simcenter 3D Multiphysics

Pre-loaded bolts modeled with beam elements (Nastran)

Pre-loaded bolts modeled with solid elements (Nastran)

Bolt pre-loads with Abaqus

Constraining bolts to their pre-loaded lengths (Abaqus)

Pre-loaded bolts modeled with solid elements (Abaqus)

Pre-loaded bolts modeled with beam elements (Abaqus)

Bolt pre-loads with ANSYS

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Define a bolt pre-load (ANSYS), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });