HyperMesh and BatchMesher

Special Realization Types

Special Realization Types

 Previous topic Next topic Expand/collapse all hidden text  

Special Realization Types

 Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  
hmtoggle_plus1greyHiLock

hilock_spotpanel

The HiLock realization type is available for Nastran and OptiStruct.

It can be used for any more or less parallel combination of PSHELL and PCOMP elements, and creates a 1D element construct consisting of RBAR, CBAR and CBUSH elements.

hilock_example_diagram

 

hilock_component_table

The outer extensions represent the thicknesses of the outer shell elements. The inner nodes of the RBAR element are connected to the shell elements whereas the inner nodes of the CBAR elements are coincident to the shell nodes. Between the appropriate connected and coincident nodes CBUSH elements are created. Each outer node connects one CBAR and one RBAR.

Each HiLock connection gets its own coordinate system with the z-axis collinear to the HiLock direction. All affected nodes are assigned to this coordinate system, which is taken into account for the DOF definition of the CBAR elements, the stiffness calculation of the CBUSH elements, and the DOF of the node constraint.

This realization uses the shell properties and materials (PSHELL or PCOMP) and a definable HiLock material to calculate the exact position of the outer nodes and the stiffness of the PBUSH elements.

Certain conditions must be met for reliable realization:

•In the case of composites, only PCOMP cards in which the laminate option is either blank or set to SYM (symmetric) are supported.  MEM, BEND, SMEAR, and SMCORE options are not supported for HiLock realization, and will cause realization to fail if used.
•The joined shells should be parallel to each other and planar.
•The fastener should be perpendicular to the shells.
•The z-axis of the element system, the material system, and the fastener system should be collinear.
•Stiffness is calculated assuming that the shells are perfectly planar and parallel. Small deviations will produce insignificant changes in predicted stiffness, but larger ones would require a system transformation.
•The shell elements which share a node with the HiLock (separate for each layer) should have the same properties, same materials, same material orientations, and similar sizes. The attributes of the element upon which the projection falls is assumed to be the same as the other surrounding elements (no averaging method is used.)

 

If attributes necessary for the stiffness calculation are missing, the connector fails and an error message displays in the status bar.

The realization requires available nodes near the connector position. If sufficient nodes are not available, the created elements are not collinear anymore and the HiLock gets a questionable geometry.

 

All HiLock elements (RBARs, CBARs, CBUSHs) created during the realization process are organized into a component named HiLock.

The following property collectors are created:

•HiLock_PBAR_<diameter>: This property collector is created with the PBAR card associated with it. The RBAR elements reference this property. The attributes are calculated depending on the diameter specified in the Spot panel during realization.
•HiLock_PBUSH_<translational stiffness>_<rotational stiffness>: These property collectors are created with the PBUSH card associated with them. The CBUSH elements reference this property. The attributes are calculated depending on the chosen HiLock material and the properties and materials of the connected shells (PSHELL and/or PCOMP).

 

The following load collector is created:

•HiLock_SPC6: the SPCs which are created for each HiLock are moved into it.

 

The following system collector is created:

•HiLock: Systems created during the realizations will be moved into this collector. If this system collector already exists, any newly created systems will be moved into the same collector.

 

If a HiLock material is not selected, a default material is created:

•HiLock_MAT1: This material will be assigned to the PBAR cards, and can be found in the following folder of the installation directory: [hm_scripts_dir]/connectors/HiLock_Mats.

The predefined values are:

set E 1.8+07

set G 4.7e+04

set NU 0.330

set RHO 8.9e-09set A 1.7e-05

 

When defining a HiLock connector, the HiLock Material Option can be selected for individual connectors using the Connector Entity Editor.

•From current model. Select an existing material from the current model.

connector_hilock_material_option

•From search folder (default). For HiLock realizations the material search folder is HiLock_Mats. HyperMesh searches for this folder in the following locations and in the following order:
1.Installation: [hm_scripts_dir]/connectors/Hilock_Mats
2.User directory: [USER_HOME]/HiLock_Mats
3.HyperWorks Configuration Path folder: [HW_CONFIG_PATH]/Hilock_Mats
4.Current working folder: [CURRENTWORKINGDIR]/HiLock_Mats

connector_hilock_material_option_current_working_folder

In the Connector Entity Editor, the HiLock Material Folder field is populated with the name of the folder that was found last. Only the files in this HiLock_Mats folder are considered and can be selected in the HiLock Material File field.

By default, the first file listed (alphabetical order) in the folder is automatically populated in the HiLock Material File field, and will be used when realizing a connector from the panel. For this reason, it is important that you only keep valid material files in the HiLock_Mats folders.

•From connector metadata: Once a connector is realized with the HiLock Material Option “From Search Folder”, the folder and file name is written as metadata to the connector. Folder data is saved in a relative manner to allow the exact same rerealization in a different work environment as long as the materials are saved in according folders.

If the materials are not available as the metadata states, the realization will fail and the following message with be displayed: Material file/id not found.

connector_hilock_material_option_from_conn_metadata

 

Combined translational bearing stiffness at composite plate with the fastener contact

(these values are defined for every composite plate in the joint).

After summation of bearing stiffness of plies where n = number of plies in the composite plate:

hilock_summation_of_bearing_stiffness

 

Combined translational bearing stiffness of the joint at ply i location in directions x and y.

hilock_Combined_translational_bearing_stiffness

 

Transformed reduced stiffness in x and y-direction for ply i.

hilock_Transformed_reduced_stiffnesses

Where

hilock_mi_ni_def

(theta = angle of orientation for ply i)

And

nonzero components of the reduced stiffness matrix for ply i are:

hilock_nonzero_components

 

Angle of ply i orientation in a CQUAD4 element.

hilock_angle_ply_orientation_cquad4

 

Material orientation of a CQUAD4 defined by a coordinate system.

hilock_material_orientation_CQUAD4_coordinate_system

 

Rotational bearing stiffness in plate-fastener contact.

hilock_rotational_stiffness_plate_fastener

 

 

Combined translational bearing stiffness at metallic plate with the fastener contact

After summation of bearing stiffness of plies where n = number of plies in the composite plate:

hilock_combined_translational_bearing_stiffness_at_plate

Where

 t = thickness of metallic part

 E = elastic compression modulus of metallic (isotropic) part

 v = Poisson's ratio

 

Rotational bearing stiffness at metallic plate with the fastener contact

hilock_rotational_bearing_stiffness_metallic_plate

Where

 t = thickness of metallic part

 E = elastic compression modulus of metallic (isotropic) part

 v = Poisson's ratio

 

 
hmtoggle_plus1greyRBE3 Load Transfer

Connectors allow you to create MPC’s using RBE3 elements between the nodes of shell-shell, shell-solid or solid-solid groups by using spot connectors. This realization type is supported for OptiStruct, Nastran and Abaqus user profiles.

The following use cases are supported:

rbe3_load_transfer_solidsolid

 

rbe3_load_transfer_face_face

 
Note:For successful realization of these connectors, the non-normal projection option needs to be active. Otherwise the projection onto an edge does not work.

rbe3_load_transfer_edge_face

 
Note:For successful realization of these connectors, the non-normal projection option needs to be active. Otherwise the projection onto an edge does not work.

rbe3_load_transfer_edge_edge

 
Note:This situation is a very specific one and needs some preparation to be successful, since the projection onto 1D elements is not supported. Here the non-normal projection option needs to be activated for the projection onto the edge. In addition, the node of the 1D element needs to be defined directly as a link. Normally this is done during connector creation by activating add node location as link. This option is only available for nodes as connector location and only if the center definition is set to use connector position for center.

rbe3_load_transfer_shellbeam

Center definition:

There are three different options for the center available:

•use shortest projection for center

The closest node becomes the center of the RBE3 element.

During the realization, based on the connector position and the tolerance the closest links are determined up to the number of required layers (num layer). All other link candidates are not taken into account for the next step. The closest node is also determined and becomes the center of the RBE3 element. Based on this center position, all nodes within the given tolerance (distance center to node) and belonging to the remained links are attached to the RBE3 element.

Note:If the connector has been created with the option add location node as link the option use shortest projection for center is ignored and the linked node becomes the center of the RBE3 element.

rbe3_load_transfer_shellbeam_useshortestprojection

•use connector position for center

The exact position of the connector becomes the center of the RBE3 element.

rbe3_load_transfer_shellbeam_useconnectorposition

•use coarse mesh for center

During the realization, based on the connector position and tolerance, the closest links are determined up to the number of required layers (num layer). All other link candidates are not taken into account for the next step.

From the remaining links, the one with the coarsest mesh is identified and a node on this mesh (close to the perpendicular connector projection) becomes the center of the RBE3 element. Based on this center position all nodes within the given tolerance (distance center to node) and belonging to the remaining links are attached to the RBE3 element.

Note:If the connector has been created with the option add location node as link, the option use shortest projection for center is ignored and the linked node becomes the center of the RBE3 element.

rbe3_load_transfer_shellbeam_usecoarsemesh

 

 
hmtoggle_plus1greySeam Hexa Adhesives

This realization type creates a continuous or discontinuous hexa weld with a predefined pattern. All defined information is stored on the connector, and can be exported into the connector XML file.

seam_hexa_adhesive

Seam Hexas are created from the Seam panel, using settings such as the ones shown in the image below.

special_realizations_seamhexa_panel

 

The parameters to be set are:

1.The hexa dimension depends on the following settings:
•The length of a hexa is predefined by the distribution of the test points along the seam connector. This is defined by spacing or density during the connector creation.
•The width of the single hexa depends on the number of strips and the defined total width of the seam, which is measured perpendicular to the seam direction. See the picture above.
•The thickness of a single hexa depends on the number of defined coats and the selected thickness option described below.
2.The available thickness options listed below interact with the general option consider shell thickness and offset for hexa positioning. In the pictures below, the green seams on the left take into account the thickness as well as the shell offset. This information is used for dimensioning and positioning the hexas. For the pink seams on the right side, the hexas are always positioned around the exact middle between the current shell positions. The shell thicknesses are taken into account only for the hexa height, but not for the positioning. Pay attention to the orange lines and arrows in the pictures below; they illustrate the dependencies for the positioning.
•shell gap

The seam completely and exactly fills the gap between the two shells. Shell thicknesses and offsets are not considered.

seam_hexa_adhesive_shellgap

•maintain gap

The seam is positioned in the exact middle between the shells. The seam thickness is adjusted, that on both sides the gap between shell and seam fits the defined gap size. Shell thicknesses and offsets are not considered.

seam_hexa_adhesive_maintaingap

•(t1+t2)/2

The seam thickness is calculated by averaging both shell thicknesses. On the left side the offsets and thicknesses are taken into account, so that the seam is positioned around the middle of the air gap. On the right side the seam is just positioned around the middle of the shell positions.

seam_hexa_adhesive_t1_t2_2

•midthickness

On the left side the exact air gap is determined and filled with the seam. On the right side the seam thickness is calculated by subtracting half the thickness of both shells from the total distance of the shells.

seam_hexa_adhesive_midthickness

•const. thickness

The thickness of the seam is predefined for both; on the left side the seam is positioned around the middle of the air gap, on the right side around the middle of the two shells.

seam_hexa_adhesive_constantthickness

 

Remarks

•The HEXA elements will be centered about the seam connector if the seam connector is not close to a free edge. If the distance between the seam connector and free edge of a component is less than half the width of the HEXA, then the realization of HEXA elements will start from the seam connector and will be extruded in the direction away from the edge.

seam_hexa_adhesive_remarks1

•For OptiStruct and Nastran solvers, the HEXA elements are tied to a shell using RBE3’s at locations where the HEXA nodes and shell nodes are non-coincident. If the HEXA nodes and shell nodes are coincident then RBE2's will be used to tie them.
•For the LS-DYNA solver only, the shell gap thickness option is supported. If the HEXA nodes are coincident with shell nodes, then those shell nodes will be used to create HEXA elements. The HEXA elements at some or all nodes will be tied directly to the shells.
•This realization type is intended to work on meshes--both shells and solids.

 
hmtoggle_plus1greyRADIOSS acm(shell gap contact and coating)

This realization creates hexa clusters between shell components. Contacts get defined between the shell components and the appropriate hexa nodes. A heat affected zone for the shells from ultra high strength steel material is also created. It can be used for any amount of parallel combinations of shell components.

The heat affected zone dimensions are defined with the parameters shown below.

radioss_acm_shell_gap_contact_coating

You must specify which materials are considered as ultra high strength materials.

1.For each connected link the contact /inter/TYPE2/ gets created and is named TYPE2_CONTACT_PID_<link ID>. The following sets are created and referenced.
a.MASTERPART_SET_PID_<link ID>: In this set, which is referenced as the master by the above mentioned contact, the link entities like the component get organized.
b.SLAVENODE_SET_PID_<link ID>: In this set, which is referenced as the slave by the above mentioned contact, the hexa nodes projecting onto the master entities get organized.
2.For each link combination the hexa clusters are organized into separate components and named RAD_SOLID_SPOTWELD_PID_<link1 ID>_<link2 ID>. All components are assigned the following material and property:
a.RAD_SOLID_SPOTWELD_DEFAULT_MAT. This material is defined as /MAT/LAW59/.
b.RAD_SOLID_SPOTWELD_DEFAULT_PROP. This property is defined as /PROP/CONNECT/.

The default values are read from uhss_washersolid_matprop.rad in the installation.

3.The heat affected zone elements (washer) are organized into one separate component for each link from the ultra high strength steel material and named RAD_WASHER_PID_<link ID>. All components are assigned the following material and property:
a.RAD_WASHER_MAT. This material is defined as /MAT/PLAS_JOHNS/.
b.RAD_WASHER_PROP. This property is defined as /PROP/SHELL/.

The material and property values are read from uhss_washersolid_matprop.rad in the installation.

 

When defining an acm(shell gap contact and coating) connector, the UHSS Material Option can be selected for individual connectors using the Connector Entity Editor.

•From current model. Select an existing material from the current model.

radioss_acm_shell_gap_contact_coating_material_define

•From search file (default). For acm(shell gap contact and coating) realizations the material search file name is materialsnippets.txt. HyperMesh searches for this file in the following locations and in the following order:
1.Installation: [hm_scripts_dir]/connectors/materialsnippets.txt
2.User directory: [USER_HOME]/materialsnippets.txt
3.HyperWorks Configuration Path folder: [HW_CONFIG_PATH]/materialsnippets.txt
4.Current working folder: [CURRENTWORKINGDIR]/materialsnippets.txt

radioss_acm_shell_gap_contact_coating_material_define_2

In the Connector Entity Editor, the UHSS Material File field is populated with the name of the file that was found last.

The text file contains snippets from the materialnames, which need to recieve heat affected zones during the realization.

•From connector metadata: Once a connector is realized with the UHSS Material Option “From search file”, the folder name is written as metadata to the connector in a relative manner to allow the exact same rerealization in a different work environment as long as the same materialsnippets.txt files are saved in according folders.

radioss_acm_shell_gap_contact_coating_material_define_3

 

 

 

 

See Also:

Connector Module

Spot Panel

Seam Panel