1. Chapter Nine
Bolt Pretension

2. Stresses due to specified pretension in bolt
Bolt Pretension
Whenever you model a bolted structure, it might be important to include the pretension (or preload) in the bolt caused by the tightening of the bolt.
ANSYS provides a convenient way to simulate bolt pretension:
Pretension elements PRETS179
Automatic pretension mesh generation
Load management for pretension sequence of multiple bolts
Stresses due to specified pretension in bolt
October 15, 2001
Inventory #
9-2

3. …Bolt Pretension
Although most pretension analyses involve contact elements to simulate contact between the bolt and the surrounding structure, we will avoid the contact issues here and focus on how to "pretension the bolt."
Topics covered:
A. PRETS179 Element
B. Typical Procedure
C. Workshop
October 15, 2001
Inventory #
9-3

4. Bolt Pretension A. PRETS179 Element
Pretension elements (PRETS179) apply the specified preload across a pretension section.
Surrounding Structure
Pretension Node
Preloaded Bolt
Nomenclature:
The bolt is subjected to a specified preload.
The surrounding structure resists the preload. Without the interaction with the surrounding structure, the preload could not be established.
The bolt is cut in two along the pretension section. This can be done automatically, using the PTSMESH command. Note that the mesh does not have to provide a planar pattern of nodes for the pretension section. In this example, PTSMESH was able to work with a free tet mesh.
PRETS179 pretension elements are used to tie the two surfaces together. These are similar to contact elements, but they act as hooks rather than as gaps.
All the pretension elements at a pretension section will share the same pretension node. This node is used to control the force in the bolt (somewhat similar to a contact pilot node).
Pretension Section
(brick or tet meshes)
October 15, 2001
Inventory #
9-4

5. Bolt Pretension …PRETS179 Element
Features of the pretension element:
A set of pretension elements is identified as a “section”.
2-D or 3-D line element that acts like a "hook" connecting two halves of a bolt.
Nodes I, J are the end nodes, usually coincident.
Node K is the pretension node:
Location is arbitrary.
Has one DOF: UX.
Used to define the preload, as an FX force or UX displacement.
Actual line of action is in pretension load direction
Preload direction J K
Node I
Pretension section
Bolt — solids, shells, or beams
October 15, 2001
Inventory #
9-5

6. Bolt Pretension …PRETS179 Element
Features of the pretension element (continued):
Preload direction is constant – it does not update for rotations
No material properties or key options
Underlying bolt elements may be solids, shells, or beams, lower or higher order.
Elements created automatically using GUI-based procedure.
October 15, 2001
Inventory #
9-6

7. Bolt Pretension B. Typical Procedure
Five main steps:
1. Import or create the geometry, including the bolt(s) and the surrounding structure.
2. Mesh all parts.
3. Create the pretension elements.
4. Apply loads and solve using multiple load steps:
Load step 1 for the bolt preload
Load step 2 to “fix” the bolt length
Load step 3 for other loads on the structure
5. Review results.
We will expand on steps 3 and 4 next.
October 15, 2001
Inventory #
9-7

8. Bolt Pretension ...Typical Procedure
Creating the Pretension Elements
After all parts of the structure, including the bolt(s), have been meshed, the next step is to create the pretension elements.
Two options:
Using PSMESH
Fastener must be meshed as one piece.
PSMESH will cut the fastener in two and generate the pretension section together with the pretension elements.
Elements at coincident nodes, EINTF (not discussed here)
The fastener must be meshed in two separate pieces.
Requires a matching node pattern.
October 15, 2001
Inventory #
9-8

9. Bolt Pretension ...Typical Procedure
The menus provide a wide variety of methods to create the pretension mesh.
Preprocessor > Create > Elements > - Pretension – Pretensn Mesh >
We will illustrate the procedure using the With Options > pick.
ANSYS splits the bolt shown and inserts the necessary pretension elements.
October 15, 2001
Inventory #
9-9

10. Bolt Pretension ...Typical Procedure
Select the option to – Divide at Node – Picked Elements +
Follow the menu prompts
Window the elements where the bolt should be split.
Pick a node to indicate where to section the bolt.
A pretension node will be created at this location.
October 15, 2001
Inventory #
9-10

11. Bolt Pretension ...Typical Procedure
Next, fill in the dialog box
Pressing OK will separate the elements of the bolt into two unconnected groups, tied together with pretension elements.
Assign a section number and name
Specify the preload direction (Y-axis points along the bolt axis in this case)
October 15, 2001
Inventory #
9-11

12. Bolt Pretension ...Typical Procedure
The output window will list a summary of the elements and the pretension node number.
Notice how the Bolt is split along existing element boundaries
October 15, 2001
Inventory #
9-12

13. Bolt Pretension ...Typical Procedure
You can “undo” a PSMESH operation as follows:
Preprocessor > Delete > Pre-tens Elements
The GUI automatically deletes the pretension elements and merges the nodes at the pretension section.
However, the pretension node (K node) is not deleted.
Note: if you don’t pick the pretension node, only individual pretension elements attached to that node will be deleted.
October 15, 2001
Inventory #
9-13

14. Bolt Pretension ...Typical Procedure
Pretension Load Application
When a physical bolt is pretensioned:
Turning the nut reduces the unstretched grip length of the bolt, thereby inducing pretension
When the desired pretension is achieved and the wrench is removed, the new unstretched grip length becomes ‘locked’
Typical ANSYS pretension loading procedure represents this same sequence
First, apply the specified pretension (usually a specified force) in one load step
Then, lock the pretension section displacement (lock the shortened grip length) in a subsequent load step.
Once all bolts are pretensioned and locked, apply external loads in the final load step
October 15, 2001
Inventory #
9-14

15. Bolt Pretension ...Typical Procedure
Stiff plate
Soft gasket
bolt1
bolt2
bolt3
Pretensioning and locking a large number of bolts in a specified sequence is made easy with the load-management tool.
Solution > Loads > Apply > Pretnsn Sectn …
Section to be preloaded first
Pretension load to be applied to this bolt
Semi-automated ‘locking’ of pretension displacement in the next load step
October 15, 2001
Inventory #
9-15

16. Bolt Pretension ...Typical Procedure
Continue the loading sequence for the other two sections:
Incrementing the loadstep number controls the pretensioning sequence
Semi-automatic restraint of the free-body bolt pieces
October 15, 2001
Inventory #
9-16

17. Bolt Pretension ...Typical Procedure
In solution, ANSYS automatically applies and locks the loads in the specified load step every time you issue a SOLVE.
For the three bolts shown in the previous example, you would need to solve four times to apply the specified pretension sequence.
SOLVE (LS1, applies the preload to bolt1)
SOLVE (LS2, fixes the preload displacement for bolt 1 and tightens bolt2)
SOLVE (LS3, locks bolt 2 and tightens bolt3)
SOLVE (LS4, locks bolt3)
With the preload applied, apply external loads acting on the overall structure.
October 15, 2001
Inventory #
9-17

18. Bolt Pretension ...Typical Procedure
Deformed geometry plot and bolt forces for the previous example
October 15, 2001
Inventory #
9-18

19. Bolt Pretension Workshop
Please refer to your Workshop Supplement for instructions on:
W13. Bolt Pretension.
October 15, 2001
Inventory #
9-19