Add Welds

Table of contents

• About
• Usage
• Weld Section
• Reference Face
• Weld Geometry
  • Weld Mesh
  • Intermittent weld parameters
  • Visualization of weld mesh
• Graphics
• Contact adjustment
• Debugging tips
• Weld Geometry Export
• Model assembly
• App default material
• Add Butt Welds

About

The Add Fillet Welds and Add Butt Welds are load feature where weld seams are created and placed in a group folder in the current static or modal analysis. The Welds are constructed of linear SOLID185 or quadratic SOLID186 brick elements. Bonded contacts at the weld legs uses “projection-based method” and contact morphing for robust contact results, see CONTA174 in Ansys help for more information.

The Welds can also be added in a thermal analysis using linear SOLID278 or quadraticSOLID279 elements. The temperatures will be mapped to the structural if using the “Imported Loads”.

The Modal analysis must have “Pre-Stress Environment = None” for the weld group to be added.

Usage

Click on “Add Fillet Welds” (or “Add Butt Welds”) in the toolbar inserts the Fillet Welds Group folder in the current static analysis and creates the first Fillet Welds load object.

To add additional welds right click on the Fillet Welds Group folder and select “Add Fillet Welds” or click on the “Add Fillet Welds” in the toolbar again. You can also use “Duplicate” on an existing Weld and modify the properties.

Inputs to define the Fillet/Butt Welds are:

(*) Default values

Default values for these properties are defined in the Weld Settings (or the preference file).

(i) Reference Face

If selecting additional faces these are used as target faces only and plotted in turquoise color. See Reference Face below for examples.

(ii) Intermittent

Selecting Type = “… intermittent” displays these properties.

(iii) Material

The following material properties (and corresponding MAPDL MP Lab) are supported: Young’s Modulus (EX), Poisson’s Ratio (NUXY), Density (DENS), Coefficient of Thermal Expansion (ALPX), Thermal Conductivity, (KXX), Specific Heat (C), Isotropic Hardening (BISO & MISO), Kinematic Hardening (BKIN, KINH). If orthotropic properties are defined the X component is automatically used (EX, NUXY, ALPX & KXX).

A property file is also written to the solver files directory that is used by the Weld Report feature.

Weld Section

This is the location where the weld seam root is placed. The edge cannot be a shared edge in a multi-body part. Also make sure that there are no bonded or no separation contacts defined between the solid parts (from “Auto Detection”). It is recommended to use solid shell mesh method on thin solids.

Reference Face

The weld geometry will follow Planar or Curved geometry. The weld Angle is derived from the angle between the Reference face and the opposite face connected to the Weld section edge. The property Min weld angle (weldElementMinAngle *) and Max weld angle (weldElementMaxAngle *) will control if a weld can be placed.

In the picture below only parts of the full edge length fulfil the angle criteria. An error message is shown if no weld elements are created for a group of edges.

The Target face is automatically detected from solid element nodes within a bounding box with padding size Gap_max around the weld contact face nodes. A small Gap between the parts is also allowed as the weld mesh is morphed onto the target faces using contact adjustment. The maximum gap size, Gap_max, is defined as a fraction (default 50%) of the Throat thickness a; Gap_max = weldElementGapRatio·a (*). This value is also used as the pinball radius, “PINB”, for the weld contact.

The reference face for one section edge cannot be the “target” face for another section edge in the case of defining multiple weld chains in the same weld object. Separate the edge chains so they do not belong to parts for the “target” face. Defining welds for multiple flange parts to one common target face in one Fillet Weld object is OK.

If additional faces not connected to any section edge are selected these are used as target face only. For complex thin-walled geometry this is recommended to avoid that contacts are created on both sides of the target plate.

Partial penetration welds can be defined by using the “chamfer” face as the reference face.

The Throat thickness, a, is always defined from the section edge out to the free weld surface for each node along the weld line, see example of pipe connection in the section “Visualization of weld mesh and weld stress results”.

(*) weldElementGapRatio, weldElementMinAngle and weldElementMaxAngle are defined in the Add Weld Settings (or preference file).

Weld Geometry

Weld Mesh

Intermittent welds will be correctly placed on open and closed edge chains. An open chain will always have a weld segment in the beginning and the end of the edge chain. A closed chain will have evenly spaced weld segments. You may also mix open and closed edge chains in one weld object. The first edge in a chain selection is used to define the start vertex and the second edge is used to define the direction of the section path.

For a weld seam with free ends (an open chain) the start and end of the weld can be offset from the start and end vertex using the property “Free end offset”. The default value is defined in the Add Weld Settings (or by the parameter “weldElementEndOffset” in the preference file).
If the angle between the tangents of two connected sections or individual weld segments is greater than 45 degrees the weld seam is split to avoid warped elements, see the weld corners in the picture below.

The weld seam is also checked for negative volume elements that may occur if the throat thickness is greater than the section edge curvature at an inner radius. Combining “Add fillet weld” with standard contacts between the connected parts may cause contact constraint forces resulting in un-realistic weld results. For the same reason creating fillet welds on both the inside and outside corner is not recommended. It is “impossible” to weld when only the corners touch.

Intermittent weld parameters

For intermittent welds the parameters “Weld fraction”, “Number of Welds”, “Weld Length” and “Weld Spacing” have relations to each other. When updating one parameter the others are updated automatically as well. Assigning a new Weld fraction will recalculate the number of welds needed based on the current Weld Length and then adjust to the actual Total Weld Length and Section Length. The resulting Weld fraction is then re-calculated based on the discrete number of welds from Total Weld Length and Section Length (Example below: Weld Fraction = 96·0.1/24.06 = 0.399).

Also note that the minimum “Weld Length” and the maximum “Weld Spacing” are defined in the Add Weld Settings (or preference file). If using Design Explorer to analyze different weld parameters use “Throat thickness”, “Number of Welds” and “Weld Length” as input parameters and “Total Weld Length”, “Section Length” and “Total Weld Mass” as output parameters. The resulting weld fraction can be derived as a new output parameter using an expression for “Total Weld Length” divided by “Section Length”; “P5/P6”.

Visualization of weld mesh

The mesh (and results) can be visualized using a “User Defined Result” with Scoping Method: “Result File Item”. See the section Mesh Results on how to plot.

In case of complex geometry with curvature and gaps the weld contact status can be verified by a “Rst Contact Status”. The contact status values have the following meaning; 0: Open far, 1: Open near, 2: Closed sliding, 3: Closed sticking (Bonded).

Graphics

A graphic representation is created once valid inputs are given.

• Weld Section edges are plotted as red lines.
• Reference Faces are plotted in dark blue.
• Optional Target Faces are plotted in turquoise.
• Weld geometry wire frame is plotted in green lines.
• Weld throat thickness is plotted with a red line.
• Weld seam is plotted with a thick purple line on top of the Weld Section.

The weld section Id number is printed at the center of each section edge.
This number is used in the result tables.
The printing of Id number can be turned on/off in the General Settings (or preference file “showWeldId = False”).

Contact adjustment

By default the CNCHECK,MORPH option is used in order to align the weld mesh contact nodes with the target elements for improved contact convergence.

If you have planar geometry and no gaps or for some other reason don’t want to morph the weld contact nodes to the target face you may tag the weld object with the tag “FilletWeldNoMorph” to exclude that weld object from morphing. The default value for the new welds is defined in the Add Weld Settings (or preference file). The tag is automatically added to the project when adding a Fillet Welds Group.

Debugging tips

If the green lines that define the weld geometry is not displayed at the expected location the surface geometry quality may be poor.
Solution: Try to simplify the geometry in SpaceClaim, e.g. replace a face with a new planar or cylindrical face.

If the lines are “translated” or “scaled” the saved geometry information has been corrupted.
Solution: Open SpaceClaim and “cut and paste everything” (CTRL+A, CTRL+X, CTRL+V) and then close SpaceClaim. This trick forces a geometry update that usually will resolve any graphical issues.

There is a debug option in the Weld Strength Settings (preference file) that will plot the weld nodes coordinate system when evaluating a weld result. The triad has the same orientation as the “Weld Csys” plotted at the beginning of each edge. When changing between evaluated results the node triads will not be visible anymore.

In case the model does not solve you may open the model in MAPDL to review the mesh before solving by adding a MAPDL system to the “Setup” component of your analysis and the select “Edit in Mechanical APDL…”.

This allows you to inspect the weld mesh and element quality etc. prior to solving. There is a component (Named Selection) named “FILLETWELDGROUPELEM” that contains all fillet welds created by the app.

Weld Geometry Export

The fillet weld mesh and weld lines can be exported prior to solving the model using the context menu option “Export all Fillet Welds” on the “Fillet Welds Group”. The mesh is written to the ANSYS cdb file “FilletWeldGroupExport.cdb” in the “Solver Files Directory” subfolder “WeldStrength”. This weld mesh will not be morphed onto the reference and target faces and allows for easy conversion to solids using the steps below.

The fillet weld mesh (Solid185/Solid186) and the needed weld contacts are created during solution. Set “Export Weld Group Cdb = Yes” in the Add Weld Settings (or the option “writeFilletWeldCdb = True” in the preference file) to export the weld mesh from the “Fillet Welds Group” to the Ansys cdb file “FilletWeldGroup.cdb” in the “Solver Files Directory”. Read the cdb file in an “External Model” and link the “Setup” cell to the “Model” cell of a “Mechanical Model” and finally link it to a “Geometry” system to export to a target geometry format.

Individual weld lines can also be imported into Space Claim or Design Modeler. See the “Export Weld Line” option for the weld objects.

Model assembly

The Mechanical model of the welds can also be used in a model assembly with the original geometry for other analyses, e.g. “Transient Thermal”.

The “Fillet Weld” object can be defined in thermal analysis prior to the structural analysis without using model assembly, see the analysis system A & B in “WeldToolkit-StrengthDemos_V2XY.Z.wbpz”.

App default material

Weld Toolkit contains a list of default materials for use with weld. The material properties are saved in a “dictionary” in the app installation folder in the file “Materials.json” (same location as the preference file). This file can be edited using e.g. Visual Studio Code or other text editors with plugins for “json” format.

The selected weld material (from Engineering Data) can be exported and included in the app default materials.

Right-click on a weld and select “Export Weld Material” to export the selected weld material (from Engineering Data) to be included in the app default materials and be available for future analyses.

Keep a backup copy of the file. When installing a new version of Weld Toolkit you may replace the default file with your custom version.

If the Engineering Data material name already exists in the bolt material list you get the option to update the material with the new properties defined in Engineering Data. If exporting a default material, e.g. “S235-BISO” nothing happens.

The properties “Tensile Yield Strength” (Ry) and “Ultimate Yield Strength” (Rm) if defined are used in Rivets/Bolts Result when post processing Eurocode 3. These properties are not to be confused with the yield limit used in isotropic and kinematic hardening plasticity material models.

The structural material properties for the default materials are listed in the following table.
The material “None” is used to not modify the existing material of the bolt part assigned by Mechanical.
All bolt materials uses the same linear properties.

• Young’s modulus: 200 GPa
• Poisson’s ratio: 0.3
• Density: 7850 kg/m³
• Coefficient of Thermal Expansion: 1.2e-05 -/C
• Thermal Conductivity: 60.5 W/(m*C)
• Specific Heat: 434 J/(kg*C)

The “Bilinear Isotropic Hardening” (BISO) uses the “Tensile Yield Strength” (Ry) as the yield limit and a tangent modulus of 1000 MPa.

Add Butt Welds

The “Add Butt Weld” is identical to “Add Fillet Weld” in all properties except for the “Weld Geometry Type”. Two geometries are available: “V-Butt Weld” and “Bevel Butt Weld”. In both cases the base geometry is assumed to have a chamfer where the weld material is placed, and a face connected to the weld section edge that defines the weld direction. The weld geometry is identified based on the angle between these two faces. The graphics display the throat thickness from the weld root up to the surface.

Curved and cylindrical geometry is also supported.