Nastran Weld Failure Determination

If the following five conditions are satisfied, you can analyze weld failure between adjacent parts of your model:

• The analysis type is Static Stress with Nonlinear Material Models.
• You explicitly define all contact pairs where you want to determine weld damage. (Weld damage criteria cannot be defined for the default contact setting.)
• You define the basic contact type in the browser as Bonded or Welded for contact pairs where you want to determine weld damage.
• You define at least a minimal set of weld bonding material failure parameters, as detailed on this page.
• You run the simulation using the Autodesk Nastran solver, or you export the model to the Autodesk Nastran Editor and run it there.

To access the weld failure settings:

1. Define one or more Bonded or Welded contact pairs.
2. Double-click an explicitly defined contact pair heading in the browser, or select one or more contact headings, right-click, and choose Edit Settings from the context menu.
3. Select Nastran contact (BSCONP) options from the drop-down menu at the top of the Contact Options dialog.
4. Go to the Weld Damage Model tab.

   Options and values that you specify here are output to the Nastran deck as parameters of BSCONP cards.

Attention: The Nastran-specific contact options contained within the General and Advanced tabs of the Contact Options dialog are the same for all analysis and contact types (including nonlinear analyses). Please refer to the Nastran Contact Options page in the General Information (Common to Multiple Analysis Types) branch for the settings in these two tabs.

Weld Damage Model Tab

The parameters within the Weld Damage Model tab of the Contact Options dialog are as follows:

Failure theory: For applicable contact types, there are three options for determining weld bond failure available from this drop-down menu:

• None: Do not perform weld bond failure calculations. This is the default choice.
• Weld failure model: There are two damage models used for modeling weld failure when this option is selected—stress-based and deformation-based. The damage model that is used depends upon the additional parameters that you define within the Weld Damage Model tab (see Table 1).

  Stress-based weld failure is supported only for Welded contact (symmetric or unsymmetric). It is not supported for Offset weld contact.

  Deformation-based weld failure is supported for Welded and Offset weld contact (symmetric or unsymmetric).

  Parameters that you Specify (see definitions below):			Weld Failure Damage Model and Defaults Values
  SDMAXT and/or SDMAXS	UDINITT and/or UDINITS	UDMAXT and/or UDMAXS
  ✓			Stress-based damage model where UDINITi is calculated using SDMAXi and the equivalent weld stress and displacement from the first load increment. UDMAXi is the incremental deformation to failure after damage initiation and is set to 0.1% of the calculated UDINITi value.
  ✓		✓	Stress-based damage model where UDINITi is calculated using SDMAXi and the equivalent weld stress and displacement from the first load increment. UDMAXi is the incremental deformation to failure after damage initiation.
  	✓	✓	Deformation-based damage model.
  	✓		Deformation-based damage model where UDMAXi is defaulted to 2 * UDINITi.
  		✓	Deformation-based damage model where UDINITi is defaulted to 0.5 * UDMAXi.
  			No damage model is used if the none of the required parameters are specified.
  Note: SDMAXi values are ignored if UDINITi values are specified.

• Cohesive zone failure: This failure theory requires that you specify one of the following two sets of parameters:
  • SDMAXT and UDMAXT, or
  • SDMAXS and UDMAXS

  The UDINITT and UDINITS parameters are ignored.

  The Cohesive zone failure theory is only supported when the Contact type is Welded (symmetric or unsymmetric). It is not supported for Offset weld contact.

Tensile stress (damage initiation): (Nastran SDMAXT parameter; Real number ≥ 0.0; Default = 0.0) – This parameter is the tensile stress of the weld bonding material when damage initiates.

Shear stress (damage initiation): (Nastran SDMAXS parameter; Real number ≥ 0.0; Default = 0.0) – This parameter is the shear stress of the weld bonding material when damage initiates.

Separation normal (damage initiation): (Nastran UDINITT parameter; Real number ≥ 0.0; Default = 0.0) – This parameter is the separation normal to the master weld surface when bond damage initiates.

Slip tangential (damage initiation): (Nastran UDINITS parameter; Real number ≥ 0.0; Default = 0.0) – This parameter is the slip tangential to the master weld surface when bond damage initiates.

Separation normal (complete failure): (Nastran UDMAXT parameter; Real number ≥ 0.0; Default = 0.0) – This parameter is the separation normal to the master weld surface when bond damage results in complete failure.

Slip tangential (complete failure): (Nastran UDMAXS parameter; Real number ≥ 0.0; Default = 0.0) – This parameter is the slip tangential to the master weld surface when bond damage results in complete failure.

Weld Failure Results

Elements along welded contact interfaces are free to pull apart where weld bonding material failure has been determined. In other words, you can see weld failure by the separation that occurs in the displaced model results.

In addition, there are three Nastran output vectors produced when weld failure calculations have been performed (detailed below). However, these three results are not currently supported within the Simulation Mechanical Results environment. To see the results contours associated with weld damage, you must export the model to the Autodesk Nastran Editor and then run the simulation and post-process the results there. The additional weld failure results are as follows:

• SSHL CONTACT EQUIVALENT STRESS: This output vector reports the equivalent stress state at the surface contact interface and is calculated at the nodes along the contact surface using the following equation:

  σ_eqv = [σ_normal² + 3(τ_x² + τ_y²)]^1/2

  Where:

  • σ_normal is the SSHL CONTACT NORMAL STRESS
  • τ_x is the SSHL CONTACT SHEAR STRESS–X
  • τ_y is the SSHL CONTACT SHEAR STRESS–Y
• SSHL BOND EFFECTIVE DISPLACEMENT: This output vector reports the effective displacement quantity for the nodes at the contact surface. SSHL BOND EFFECTIVE DISPLACEMENT is a nodal quantity for the relative displacement of the slave nodes with respect to the master surface. The effective displacement is calculated using the following equation:

  D_EFF = [D_Z² + (D_X² + D_Y²) / 3]^1/2

  Where:

  • D_Z is the normal displacement of the slave node from the master surface in the local coordinate system
  • D_X is the X directional displacement of the slave node with respect to the local coordinate system
  • D_Z is the Y directional displacement of the slave node with respect to the local coordinate system
• SSHL BOND DAMAGE: This output vector reports the amount of damage occurring on the contact surface. It is the ratio of the effective displacement versus the allowable bond displacement.