Samcef Pretension Manager

Location: Tools menu > Pretension Manager

Use the Samcef Pretension Manager to create and edit 1D and 3D pretension bolt loads and bolt sections.

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.

pretension_manager_samcef

1.	From the menu bar, click Tools > Pretension Manager.

2.	In the Pretension Manager dialog, click Create New.

3.	Set the Bolt type to 1D.

4.	In the Name field, enter a name for the bolt.

5.	Click Element and select Select Existing Element.

pretension_manager_samcef_select_existing_element_1d

6.	In the panel area, use the elems selector to select a single beam, bar, or rod element.

7.	Click proceed. The ID of the selected element is displayed in the field to the right of the Element definition button.

8.	To automatically generate a pretension node at the second node of the selected 1D element, select the Auto generate pretension node checkbox.

pretension_manager_samcef_auto_generate_1d

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

pretension_manager_samcef_auto_generate_pretension_node_1d

9.	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.

pretension_manager_samcef_apply_load_1d

10.	Click Function Time.

11.	In the panel area, use the curves selector to select the required curve for the load.

12.	Click proceed. The selected curve and its corresponding ID are displayed in the field to the right of the Function Time definition button.

13.	Click Load Collector and select whether to Select Existing Collector or Create New Collector to store the defined load.

•	Select Existing Collector

Directs you to the panel area where you can use the loadcol selector to select an existing load collector.

•	Create New Collector

Creates 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.

pretension_manager_samcef_load_collector_1d

14.	To create a FIX parameter, select the FIX parameter checkbox and enter a FIX value.

15.	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)

16.	Click Create. A BOLT is created as a group entity.

Export Deck of a 1D Bolt

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.

1.	From the menu bar, click Tools > Pretension Manager.

2.	In the Pretension Manager dialog, click Create New.

3.	Set the Bolt type to 3D.

4.	In the Name field, enter a name for the bolt.

5.	Click Contact Surface and select whether to Create New Surface or Select Existing Surface.

•	Create New Surface

Directs you to 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.

pretension_manager_samcef_3d_create_new_surface

•	Select Existing Surface

Directs you to the panel area where you can use the contactsurf selector to select an existing contact surface.

6.	Select a Method for defining the bolt.

•

Creates a .MCT contact between the two faces of the cut.

•

Creates a MEAN element and a new node on each side of the cut.

7.	Select a pretension node.

•

Manually

Clear the Auto generate pretension node checkbox, then 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.

•	Auto-Generate

Select the Auto generate pretension node checkbox. A pretension node will be automatically generated in the center of the contact surface.

8.	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. 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.

9.	Click Function Time.

10.	In the panel area, use the curves selector to select the required curve for the load.

11.	Click proceed. The selected curve and its corresponding ID are displayed in the field to the right of the Function Time definition button.

12.	Click Load Collector and select whether to Select Existing Collector or Create New Collector to store the defined load. The load collector is created along the 3D bolt.

•	Select Existing Collector

Directs you to the panel area where you can use the loadcol selector to select a load collector.

•	Create New Collector

Creates 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.

13.	To create a FIX parameter, select the FIX parameter checkbox and enter a FIX value.

14.	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)

15.	Click Create. A BOLT is created as a group entity.

Export Deck of a 3D Bolt

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.