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Weld bead feature types

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    Procedures | References

    Weld bead features in Autodesk Inventor include a cosmetic weld, a solid fillet weld, and a solid groove weld. All weld bead types reside only in the Welds feature group. Each is represented with a unique icon in the browser.

    Welds capture the weld specification, associate it with selected geometry, and display a weld symbol. Cosmetic and solid welding symbols can be recovered and created automatically in drawing views. You can also automatically generate caterpillar annotations for solid body fillet welds.

    You can create a welding symbol simultaneously with the weld bead or you can create it in a separate operation.

    How are cosmetic welds and solid welds different?

    Cosmetic welds are created as graphical elements. These graphical elements change the appearance of model edges to indicate they were welded. Cosmetic welds also create a standard weld symbol containing a full description of the weld feature. It does not create the actual weld bead geometry, and when calculated for mass properties, contributes an approximate mass. Because of these characteristics, cosmetic welds can easily represent a wide range of weld types.

    Solid welds use the weld specification to create a 3D representation of the weld bead and a weld symbol on the assembly weldment. The solid weld bead adds material to the model that contributes to the mass property calculations. Use solid welds for design cases where interference checking or the effects of welds on mass properties are a concern.

    Different weld types and values can be defined for both the arrow side and other side of a cosmetic weld. Arrow side and other side definitions for a solid weld can only differ in value.

    How is the workflow different for cosmetic welds and solid welds?

    Complete control of weld specification capabilities is available for all weld feature types. The main difference is that you select edges to create a cosmetic weld, and faces to create a solid weld.

    Weld preparations are optional for solid welds, but are not required for cosmetic welds. The cosmetic weld symbol contains the description of weld preparations required for the selected edges.

     

    Procedures

    Create weld bead features in weldments

    In a weldment assembly, use commands on the Weld tab to create fillet welds, groove welds, and cosmetic welds. Create intermittent or continuous fillet welds along the length of selected faces or use a groove weld to connect two faces with a solid weld bead.

    The following images show cosmetic, fillet, and intermittent fillet welds.

    Weld bead features are always affected by post-weld machining features, but are not affected by weld preparation features. Weld bead features are also not included in assembly feature participation lists.

    You can create a welding symbol when you create a weld bead or you can create it in a separate operation.

    Create a fillet weld feature

    Fillet welds build up corners by adding material between one or more faces of a single part or multiple parts.

    1. In a weldment assembly, double-click the Welds group in the browser to activate it.
    2. On the ribbon, click Weld tab Weld panel Fillet to open the Fillet Weld dialog box.
    3. In the graphics window, select one or more faces for the first selection set. Use the Shift key to cancel the selection of unwanted faces.
    4. Right-click and select Continue, and then select the second set of faces in the graphics window.
    5. If necessary, select the Chain check box to chain the faces together.
    6. Select the orientation of the weld bead and then enter corresponding values for the bead legs.
    7. Click the arrow to select the bead contour.
    8. If you choose a Convex or Concave contour, the Offset value is available. This value describes the amount the curve is offset from the flat as shown in the following image. The preview in the graphics window updates with the entered values.
    9. If creating an intermittent bead, set values according to the active standard. The preview image shows where the values are applied.
    10. Under Extents, click the down arrow and select the method to terminate the weld.
      • Use Extents All to cut through all faces. If some faces are removed from the feature, All remains a valid termination method because it does not rely on a specific distance or face.
      • Use Extents From-To only if you are sure the beginning and ending faces (or planes) remain intact throughout design changes. If the From or To face (or plane) disappears, the feature fails. Click the Start and End termination planes or faces. Selected termination planes and faces must be parallel.
      • Use Extents Start-Length when you want to specify a start point with or without an offset value and the overall length of the weld bead. Use Start-Length if the weld does not begin or end on an edge. Reverse the start point by selecting the Direction icon.
    11. If appropriate, click the Create Welding Symbol check box. Fillet weld beads are linked to values in the welding symbol unless you specifically break the link. Enter values to define the content and appearance of the welding symbol.

      For more information about the meaning of values in the welding symbol, see the Model welding symbol reference.

    12. Click Apply to create the fillet weld bead and, if selected, the welding symbol. Continue to create beads, if desired, or click Cancel to close the dialog box.

    Create a groove weld feature

    1. In a weldment assembly, double-click the Welds group in the browser to activate it.
    2. On the ribbon, click Weld tab Weld panel Groove to open the Groove Weld dialog box.
    3. If required, select the Chain Faces check box to pick multiple tangent faces.
    4. Click Face Set 1, and in the graphics window select one or more faces for the first selection set. Use the Shift key to cancel the selection of unwanted faces. The selected faces match the colored line on the button face.
      • Select the Full Face Weld check box if you want the weld bead to extend the full length of the selection set.
      • Select Chain Faces to include all tangent faces in the selection.
      • Select the Ignore Internal Loops check box to extend the weld bead across internal loops, such as holes or cuts.
    5. Right-click and select Continue and then select the second set of faces in the graphics window. Selected faces match the colored line on the button face.

      Select Full Face Weld and Ignore Internal Loops check boxes to specify the treatment for the second selection set.

    6. Click Fill Direction. In the graphics window, click an edge or face to indicate the weld direction.
    7. If a direction pick is not required, such as a cylinder in a hole, select the Radial Fill check box to define the direction.
    9. If required, click the Create Welding Symbol check box. Enter values to define the content and appearance of the welding symbol.

      For more information about the meaning of values in the welding symbol, see the Model welding symbol reference.

    10. Click Apply to create the groove weld bead and, if selected, the welding symbol. Continue to create beads, if desired, or click Cancel to close the dialog box.

    Show Me how to create a groove weld bead

     

    Create a cosmetic weld feature

    1. Open a weldment assembly. If necessary, convert a regular assembly to a weldment. For more information, click Convert an assembly to a weldment.
    2. In the browser, right-click the Welds folder and select Edit.
    3. On the ribbon, click Weld tab Weld panel Cosmetic.
    4. Specify the Select Mode. Select one or more edges, or select a chain of contiguous edges or a closed loop.
    5. Under Extents, click the arrow to select the method to terminate the cosmetic weld bead:
      • Use All to cut through all faces. If some faces are removed from the feature, All remains a valid termination method because it does not rely on a specific distance or face.
      • Use From To only if you are sure the beginning and ending faces (or planes) remain intact throughout design changes. If the From or To face (or plane) disappears, the feature fails. Click the Start and End termination planes. Selected planes and faces must be parallel.
    6. In Area, click to select the area or use the Measure command or Show Dimensions.
    7. Select the Create Welding Symbol check box to create the welding symbol together with the cosmetic weld bead. For more information, click Model welding symbol reference.

      If you prefer, you can create the weld symbol later. The cosmetic weld bead is nested below the weld symbol in the browser Weld folder.

    Add end fills to beads in weldments

     

    You can add a weld end fill in a model to represent the filled region indicating the end of a weld bead. The end fill may be recovered in the drawing view. An end fill is automatically added to a fillet weld bead.

    1. In a weldment assembly, double-click the Weld folder to enter the weldment environment.
    2. On the ribbon, click Weld tab Weld panel End Fill. Existing end fill faces are highlighted..
    3. Click any face of a solid weld bead to add an end fill.
    4. Continue to add end fills. Right-click and select Done to quit.

    To remove an end fill, click End Fill and then click the face again to turn off the face highlight.

    TipTo change the appearance of an end fill, right-click the Welds folder in the browser and select Properties. In the Properties dialog box, click the Weld Bead tab. In the End Fill Appearance box, click the arrow to list available appearances and select. Click OK to close the dialog box.

    Export weld bead properties to spreadsheets

    To help you determine accurate weld rod usage, fabrication time, and bead weights, you can export weld bead physical properties to a spreadsheet. You can query the mass, volume, length, type, and name of individual beads in the weldment assembly. Or you can list all the weld beads in the current assembly and in all referenced weldment files. The names of the referenced files are included in the report. You can generate a weld bead report from any assembly document.

    Length and Area values are not reported for groove welds.

    Once the weld bead properties are exported to the spreadsheet, you can insert your own formulas to obtain cost information or paste the table into a drawing for reference.

    1. On the ribbon, click Weld tab Weld panel Bead Report in a weldment assembly.
    2. In the Report Location dialog box, accept the default name or enter a different one.
    3. Browse to the location where you want to place the file.
    4. Click Save.

    Set visibility of weld bead features and symbols

    Weld bead features and symbols are on by default when they are first created. They remain on until you change their visibility. When a weldment is placed in another assembly, its weld bead features and symbols are visible in the assembly.

    You can control the visibility of weld bead features and symbols for an entire weldment, for the Welds feature group, and for individual weld bead features.

    You can turn off both the symbol and the weld bead feature or just the symbol. Turning off weld bead feature visibility automatically turns off the associated weld symbol as well.

    Weld bead feature and symbol visibility are reflected in design view representations.

    To set visibility for the Welds feature group

    You can change visibility for all assembly weld bead features or weld symbols in the Welds feature group using an option on the context menu.

    1. In the browser select the Welds feature group.
    2. Right-click and select the needed visibility option. Clear the check mark to turn off.
      • To change weld bead feature visibility, select Visibility.
      • To change symbol visibility, select Symbol Visibility.
    3. To turn on visibility, select the feature group in the browser, right-click, and select the needed option.

    To set visibility for selected weld bead features

    At the feature level, you can set visibility for symbols only. Weld bead feature visibility is not available.

    1. In the browser or the graphics window, select one or more weld bead features.
    2. Right-click and select Symbol Visibility. Clear the check mark to turn off.
    3. To turn on visibility , select one or more weld bead features in the browser, right-click and select Symbol Visibility.
    NoteTo select multiple weld bead features, hold down the Ctrl key and select.

    To set visibility for an entire weldment or assembly with subweldments

    The View tab sets visibility for the entire weldment.

    1. On the ribbon, click View tab Visibility panel Object Visibility.
    2. On the drop-down menu, clear the check mark to hide all weld bead features or weld symbols. Select the option to turn on visibility.

    Browser symbols show the visibility state selected on the View tab.

    NoteTo reset visibility on or off in the browser or graphics window, first set the option on the View tab.

    Delete weld features

    You can delete individual features from any of the three weld feature groups . You cannot delete the actual weld feature groups.

    When you delete a weld bead feature , its associated welding symbol is also deleted. The weld bead feature annotations and any drawing welding symbols associated with the weld bead feature will be deleted the next time the drawing updates.

    When you delete assembly features from a weld feature group, you might need to reapply constraints or recreate features.

    1. In the browser, expand the feature group containing the feature to delete.
    2. Select the feature to delete in the graphics window or the browser, and then choose one of the following actions:
      • Press the Delete key.
      • Right-click and select Delete.

     

    References

    Fillet weld features

    Creates a fillet weld feature in a weldment assembly. A welding symbol may be created simultaneously with the feature or it may be created in a separate operation.

    The weld bead and the welding symbol are separate features in the welds folder of the browser. The welding symbol can be associated with the fillet bead feature so that changes to the fillet bead update the welding symbol values. Changes to the welding symbol cannot update the fillet bead feature. When consumed by a welding symbol, the fillet weld is a child node of the welding symbol.

    Access:

    		Right-click the Welds folder in the browser and select Edit. On the ribbon, click Weld tab Weld panel Fillet.

    The Bead box specifies the parameters for constructing the fillet weld.

    Selection and Size

    Selects the faces to define the fillet weld. Select the Chain check box to select tangent contiguous faces automatically.

     

    Leg Length constructs a fillet weld based on leg length (height and width). If only one value is entered, leg lengths are equal.

     

    Throat constructs a fillet weld based on the distance between the weld root and the face of the fillet weld.

       
    		Direction changes the start position of an offset weld.

    Contour

    		  

    Specifies Flat, Convex, or Concave weld bead process shape and if appropriate, an offset distance. Offset is used with Concave or Convex contours to control the inward or outward bow of the weld bead face.

    Intermittency

    		  

    Specifies intermittency of a fillet weld bead, specific to the active standard.

    ANSI standard specifies bead length and the distance between bead centers.

    ISO, BSI, DIN, and GB standards specify bead length, spacing between beads, and the number of beads.

    JIS standard specifies bead length, the distance between bead centers and the number of beads.

    Extents

    Determines the method for starting and ending a fillet weld. A fillet weld can terminate on a work plane, on a planar face, or extend across all selected geometry for a full-length weld. The start and end position of a fillet weld can also be offset from a model edge. Click the arrow to select the extent method.

    • All creates the weld bead across all selected geometry in the specified direction.
    • From-To selects the beginning and ending faces or planes on which to terminate the weld feature. In a weldment, the faces or planes may be on other parts, but must be parallel.
    • Start-Length creates a weld bead with a user specified offset distance and a fixed length. If the weld does not begin or end on an edge, use Start Offset to specify the set back distance.

    Select Create Welding Symbol to expand the dialog box to set welding symbol parameters. Click this link to go to the Model Welding Symbol Reference.

    Groove weld feature

    Creates a groove weld feature in a weldment assembly that connects two face sets with a solid weld bead. A welding symbol can be created simultaneously with the feature or it can be created in a separate operation.

    The weld bead and welding symbol are separate features in the welds folder of the browser. There is no association between the welding symbol and the weld bead feature so you can specify any welding symbol values for the weld bead feature. When consumed by a welding symbol, the groove weld is a child node of the welding symbol.

    Access:

    		Right-click the Welds folder in the browser and select Edit. On the ribbon, click Weld tab Weld panel Groove.

    The Bead box specifies the parameters for constructing the groove weld.

    Face Sets 1 and 2

    Selects the two sets of faces to connect by a groove weld bead. Each face set must consist of one or more contiguous part faces.

    Full Face Weld specifies how the weld bead appears for both face sets.

     

    Clear the check box to specify that the weld bead ends at the extents of the smaller face set.

     

    Select the check box to specify that the weld bead extends to consume both face sets. If face sets 1 and 2 are different lengths, the weld bead expands to fit both faces.

    Chain Faces selects multiple tangent faces.

    Ignore Internal Loops determines if a selected face set results in a hollow groove weld or a solid weld.

     

    Clear the check box to specify that the weld bead extends along the loop, but not the face.

     

    Select the check box to specify that the weld bead spans the internal loop to cover the entire face.

    Fill Direction

    Sets the direction in which groove weld face sets are projected onto one another when connected by the groove weld bead. To define the fill direction, you can select:

    • Planar faces and work planes (specifies direction normal to the chosen face or plane)
    • Cylindrical, conical, or toroidal faces (specifies direction of the surface axis)
    • Work axes
    • Part edges
    • Two points (work axis, model vertex)
     
    		 

    Projects the weld bead at the angle of the first selected face set.

     
    		 

    Projects the weld bead perpendicular to the second selected face set.

     

    Radial fill

    		Projects the weld bead around a curve. Fill Direction is not available when the Radial Fill check box is selected.

     

    Select Create Welding Symbol to expand the dialog box to set welding symbol parameters. Click this link to go to the Model Welding Symbol Reference.

    Cosmetic welds

    Creates a cosmetic weld feature in a weldment assembly. A welding symbol may be created simultaneously with the feature, but may be created in a separate operation.

    The weld bead and the welding symbol are separate features in the welds folder of the browser. The welding symbol and the weld bead feature are not associated, so you can specify any welding symbol values for any weld bead feature. When consumed by a welding symbol, the cosmetic bead is a child node of the welding symbol.

    Cosmetic weld beads are useful when the design does not require interference analysis or the aesthetic appearance of solid weld beads. Their approximate physical properties can be included in mass properties.

    Access:

    		Right-click the Welds folder in the browser and select Edit. On the ribbon, click Weld tab Weld panel Cosmetic.

    The Bead box specifies the parameters for constructing the cosmetic bead.

    Select Mode

    Sets the selection preference for areas on which to apply the cosmetic weld bead. Edge is the default. Chain automatically selects tangent, contiguous edges. Loop selects a closed loop.

    Extents

    Determines the method for ending a cosmetic weld. A cosmetic weld can terminate on a work plane or extend across all selected geometry for a full-length weld. Click the arrow to select the extent method.

    All creates the weld on all features and sketches in the specified direction.

    From-To select beginning and ending faces or planes on which to terminate the weld feature. In a weldment, the faces or planes may be on other parts, but must be parallel.

    Area

    Sets the cross-sectional area for a cosmetic weld bead so the physical properties of the cosmetic bead can be calculated.

    Select Create Welding Symbol to expand the dialog box to set welding symbol parameters. Click this link to go to the Model Welding Symbol Reference .

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