Create Pretension Bolt

Create pretension loads in 1D and 3D bolts.

ANSYS: Create Pretension Bolt

Create pretension loads in 1D and 3D bolts of ANSYS models using the ANSYS PRETS179 element type.

Element PRETS179 is a bar element with a third node used for pre-loading. Use the Pretension Bolt tool to get a pre-loaded bolt with PRETS179 elements created at the desired location with a third node. A pretension section is created and associated with the pretension elements created. Also, the pretension load card SLOAD is created with the defined load in the utility, as well as a load steps on and off values. You can edit this load card after completing this process.

Restriction: The Pretension Bolt tool is only available in the ANSYS solver interface.

From the menu bar, click Tools > Pretension Bolt.
The Pretension Bolt dialog opens.
For Pretension Type, select the type of bolt to create.
In the Node ID field, enter the node ID for the third node of the pretension element.

Note: If you do not enter a node ID, a default node number will be assigned.
In the Section Name field, enter a name for the pretension section to be created.

Note: If you do not enter a section name, a default name will be assigned.
Toggle the type of method for loading the bolt to either Force or Displacement, then enter a corresponding value.
In the Loadstep ID to activate [LSLOAD] field, enter the load step ID to which the load is to be applied.
In the Loadstep ID to lock [LSLOCK] field, enter the load step ID to which the displacements or force loads needs to be locked.
Click Create.

Select source entities for the pretension bolt.

Option	Description
1D pretension bolt	In the panel area, use the Nodes selector to select the nodes of the 1D elements where the pretension element needs to be created and then click proceed.
3D pretension bolt	In the panel area, use the Comps selector to select the bolt component and then click proceed. Note: Multiple components are not allowed to be selected. If more than one bolt is selected, they will all be placed under one component. Use the elems selector to select the elements which form the cut section of the bolt and then click proceed. Pretension elements are created at this section. Figure 1. Example of a Typical Section Use the node selector to select two or three nodes that define the load direction for the pretension load and then click proceed.

Option

Description

1D pretension bolt

In the panel area, use the Nodes selector to select the nodes of the 1D elements where the pretension element needs to be created and then click proceed.

3D pretension bolt

In the panel area, use the Comps selector to select the bolt component and then click proceed.
Note: Multiple components are not allowed to be selected. If more than one bolt is selected, they will all be placed under one component.
Use the elems selector to select the elements which form the cut section of the bolt and then click proceed.
Pretension elements are created at this section.

Figure 1. Example of a Typical Section
Use the node selector to select two or three nodes that define the load direction for the pretension load and then click proceed.

For 1D pretension bolts, PRETS179 elements are created at the node locations, with the pretension section created and associated to these elements. A SLOAD card with the given pretension load is also created.

For 3D pretension bolts, PRETS179 elements are created at the cut section with the pretension section created and associated to these elements. A SLOAD card with the given pretension load is also created.

To edit the SLOAD card, click Edit SLOAD.

Samcef: Create Pretension Bolt

Create and edit 1D and 3D pretension bolt loads and bolt sections.

Use the Pretension Manager to create and edit pretension bolts. Existing bolts and newly created bolts are displayed in the table within the Pretension Manager dialog. The card attribute's of every bolt present in the model are displayed. You can edit the output codes for each bolt in the Output column. Any changes made to the Output column will be automatically updated in the respective BOLT cards.

Restriction: The Pretension Bolt tool is only available in the Samcef solver interface.

Create a 1D Pretension Bolt

From the menu bar, click Tools > Pretension Manager.
The Pretension Manager dialog opens.
Click Create New.
Set the Bolt type to 1D.
In the Name field, enter a name for the bolt.
Click Element > Select Existing Element.

Figure 2.
In the panel area, use the elems selector to select a single beam, bar, or rod element and click proceed.
The ID of the selected element is displayed in the field to the right of the Element definition button.
To automatically generate a pretension node at the second node of the selected 1D element, select the Auto generate pretension node checkbox.

Figure 3.

Once the 1D element is selected, the generated pretension node's ID is displayed in the Node ID field.

Figure 4.
Select whether to apply a Force or Displacement load on the bolt, then enter a corresponding magnitude.

Note: A load is not created until a load collector is specified.
Click Function Time.
In the panel area, use the curves selector to select the required curve for the load and click proceed.
The selected curve and its corresponding ID are displayed in the field to the right of the Function Time definition button.
Click Load Collector and select where to store the defined load.
- Choose Select Existing Collector to open the panel area where you can use the loadcol selector to select an existing load collector.
- Choose Create New Collector to create a new load collector with the prefix PRETENS_#. The number appended to the end of the load collector name depends on the number of load collectors currently present in the model.
The load collector is created along the 1D bolt.

Figure 5.
To create a FIX parameter, select the FIX parameter checkbox and enter a FIX value.
Select where the different codes will be internally written in the solver deck.
- Total axial force in the bolt (9524)
- Relative displacement in the cut (9530)
Click Create.

A BOLT is created as a group entity.

The macro element ID for the first bolt that was created is written out as the maximum element ID in the model + the number of nodes present in model. 1000 is added to the macro element ID for consecutive bolts, that is, if the first bolt’s macro ID is 3, then the next bolt will be 1003 (3 + 1000).

The macro element ID of a bolt is reflected in its .SAI command, which is written along with the bolt’s corresponding output-code. It is preceded by the comment !!HM_TEMP_OUTPUTBLOCK, which enables the model-reader to ignore the output block upon import and not create any output blocks in HyperMesh. A bolt card that does not contain an output definition will not have a .SAI command written out.

All such commented commands are automatically exported out again upon re-export in the same format.

The load applied on a bolt is written out in the solver deck. A load’s magnitude is written out after VAL, and any curve attached to the load using Function Time is written after the keyword NF.

Create a 3D Pretension bolt

From the menu bar, click Tools > Pretension Manager.
The Pretension Manager dialog opens.
Click Create New.
Set the Bolt type to 3D.
In the Name field, enter a name for the bolt.
Click Contact Surface and select where to create a new surface or select an existing surface.
- Choose Create New Surface to open the panel area where you can use the node list selector to select two consecutive nodes to generate a contact surface. The first node should be a base node in the desired contact surface. The second node should lie in the direction of the contact surface's normal. A default name is assigned to the new contact surface with the prefix PRETENS_#. The number appended to the end of the name depends on the number of contact surfaces currently present in the model.
  
  Figure 6.
- Choose Select Existing Surface to open the panel area where you can use the contactsurf selector to select an existing contact surface.
Select a Method for defining the bolt.
- Choose 1 to create a .MCT contact between the two faces of the cut.
- Choose 2 to create a MEAN element and a new node on each side of the cut.
Select a pretension node.
- Choose Manually, then clear the Auto generate pretension node checkbox and click Select. In the panel area, use the nodes selector to select two consecutive nodes. The first node should be a base node in the desired contact surface. The second node should lie in the direction of the contact surface's normal. The approximate center of the contact surface where the pretension node will be created on is automatically estimated.
- Choose Auto-Generate, then select the Auto generate pretension node checkbox. A pretension node will be automatically generated in the center of the contact surface.
Select whether to apply a Force or Displacement load on the bolt, then enter a corresponding magnitude.
A load is not created until a load collector is specified. The load acts in the direction normal to the contact surface. A load (force and displacement) is always created for bolts in the X-direction (COMP1), regardless of the model.
Click Function Time.
In the panel area, use the curves selector to select the required curve for the load and click proceed.
The selected curve and its corresponding ID are displayed in the field to the right of the Function Time definition button.
Click Load Collector and select where to store the defined load.
- Choose Select Existing Collector to open the panel area where you can use the loadcol selector to select an existing load collector.
- Choose Create New Collector to create a new load collector with the prefix PRETENS_#. The number appended to the end of the load collector name depends on the number of load collectors currently present in the model.
The load collector is created along the 3D bolt.
To create a FIX parameter, select the FIX parameter checkbox and enter a FIX value.
Select where the different codes will be written internally in the solver deck.
- Total axial force in the bolt (9524)
- Relative displacement in the cut (9530)
Click Create.

A BOLT is created as a group entity.

The macro element ID of the first bolt that was created is written out as the maximum element ID in the model + the number of nodes present in model. 1000 is added to the macro element ID for consecutive bolts, that is, if the first bolt’s macro ID is 117653, then the next bolt will be 118653 (117653 + 1000).

All such commented commands are automatically exported out again upon re-export in the same format.

The load applied on a bolt is written out in the solver deck. A load’s magnitude is written out after VAL, and any curve attached to the load using Function Time is written after the keyword NF.