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This document was updated using version SOLIDWORKS 2022 SP04. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.

1. Preface:

The SOLIDWORKS weldments functionality makes it possible to design a weldment structure as a single multibody part. The structure system is an advanced weldments environment that allows you to create and modify structural members of different profiles in one feature. This SolidPractice document provides information about the functionalities available for SOLIDWORKS weldments, and troubleshooting tips to for common weldment issues.

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1. Introduction

A weldment structure is a body that consists of multiple metallic structural members that are welded together. This structure is useful as a supporting structure in different types of constructions. Weldment structures are found in a wide variety of products that include automation equipment, scientific machinery, industrial equipment, and many other specialized products.

A weldment part in SOLIDWORKS is a specialized part, with certain features available to facilitate the functional needs of a weldment structure. Features on the Weldments toolbar help to streamline the design and manufacture of welded structures, frames, and bases that form the backbone of products developed in many industries.

The SOLIDWORKS weldment design functionality makes it possible to design a weldment structure as a single multibody part, from sketching the basic framework and creating structural members with groups of sketch segments, to adding elements like gussets and end caps to complete the structure. Users can quickly create designs that have extrusions and generate the cut lists and bills of materials (BOMs) required for manufacturing. SOLIDWORKS accelerates the design process, saving time and development costs, and increasing productivity.

The purpose of this document is to demonstrate the importance of the different functionalities of weldment features, along with weldment sketch tips and information about working with weldment groups. This document also discusses some important weldment features that help in reaching the design intent of a weldment design, as well as tips on troubleshooting common weldment issues.

1. Overview of Weldment Design

The SOLIDWORKS weldments functionality makes it possible to design a weldment structure as a single multibody part by using either 2D or 3D sketches to define the basic framework. The primary features are called structural members, which are created using sketch segments in groups. These sketch entity groups can be from the same sketch, or the designer can take them from different sketches. You can create the cross section of the structural geometry by using different customizable profiles. Once the basic structural members are in place, the designer can add ends caps, gussets and other finishing features.

After creating the first structural member in a part, SOLIDWORKS adds a Weldment feature

feature. You can assign custom properties to these items. Lastly, the software prepares a weldment cut list that appears as a table in the drawing. The weldment cut list contains all information similar to a BOM. The cut list groups bodies automatically based on similar geometry.

When you add a weldment feature to a part, the software also creates two configurations; a parent Default configuration, and a derived Default configuration.

Some of the SOLIDWORKS weldment features make it possible to:

• Work from a library of predefined structural shapes
• Automatically trim structural members at intersections
• Add stiffening plates, gussets, and end caps
• Add optional fillets and weld beads to the design
• Generate drawings, BOMs, cut lists, and other manufacturing documentation

1. Weldment File Locations

Before starting the design process, it is important to define correct paths for the various weldment related files (weldment profiles,weldment cut list templates, and weldment property files).

1. Weldment profiles

Weldment profiles define the cross section of the weldment structural member.. The default location for these profiles has been changed effective with the release of SOLIDWORKS 2022:

[install_directory]\..\SOLIDWORKS\data\weldment profiles

It is a common practice for users to create their own weldment profiles and add the profile paths to the location list under System Options > File Locations.

1. Weldment profile name mapping file

Instead of displaying the actual name of the directory or library file that holds weldment profiles, users can map to display a custom string by using the weldmentprofiles.txt file. The custom strings in this file appear in the drop-down list of the structural members. The default location for this file is:

[install_directory]\..\SOLIDWORKS\lang\[language]\weldmentprofiles.txt

1. Weldment cut list template

The weldment cut list template defines the weldment cut list in a drawing. The default template name is cut list.sldwldtbt. The default location for this file is:

[install_directory]\..\SOLIDWORKS\lang\[language]\cut list.sldwldtbt

You cannot modify this template directly. Instead, use the default template to create a cut list, add new columns as necessary, and then save the table as a template. The information that appears in the weldment cut list table comes from the cut list properties.

1. Weldment property file

The weldmentproperties.txt file contains all of the custom properties for a weldment, and for the cut list within it. Users can add more properties to this file. The default location for this file is:

C:\ProgramData\SOLIDWORKS\SOLIDWORKS[version]\lang\[language]\weldments\weldmentproperties.txt

1. Weld table template

The weld table in a drawing provides information about the weld beads in the model. It includes weld bead custom properties such as weld material, weld process, weld mass, weld cost, weld time, and others. Similar to the weldment cut list template, you can customize this table by adding columns and then saving the table as template. The default weld table file has the name weldtable-standard.sldwldtbt. The default location for this file is:

[install_directory]\..\SOLIDWORKS\lang\[language]\weldtable-standard.sldwldtbt

1. Weldment Profiles

Weldment profiles are sketches that define the cross-section shape of a structural member. Weldment profiles include attributes for Standard, Type, and Size.

1. Default profile

The default profiles are the weldment profiles that are available with a new SOLIDWORKS installation. The default profiles are in the following location:

[install_directory]\..\SOLIDWORKS\data

Till SOLIDWORKS 2020, the installation directory of SOLIDWORKS includes ANSI inch and ISO standard profiles by default.

Effective with the release of SOLIDWORKS 2021, the additional weldment profiles for other standards (ANSI, AS, BSI, CISC, DIN, GB and JIS) alongwith the ANSI inch and ISO will also be available at same location. Users can add or change locations for weldment profiles by going to Tools > Options > System Options > File Locations > Weldment Profiles.

Weldment profile files have the *.sldlfp file extension, and consist of library feature sketches.

The size list sorts numerically from the smallest size to the largest. In addition, the two most recently used profile sizes appear at the top of the size selection list. Users can also transfer material from a weldment profile by selecting the Transfer Material from Profile option in the PropertyManager.

1. Custom profile

SOLIDWORKS allows users to create a custom weldment profile for use while designing weldment structural members. Users need to create the custom profile as a library feature part (*.sldlfp) file, and then add the location of this custom profile path to Tools > Options > System Options > File Locations > Weldment Profiles. By default, the profile origin becomes the pierce point on the sketch for the structural member. While creating a weldment structural member, the name given to the library feature part appears in the Size list in the Structural Member PropertyManager.

1. Configured weldment profile

Effective with the release of SOLIDWORKS 2021, all weldment default profiles are configured profiles.

Custom profiles with one configuration have a three-level folder path. For example:

\..\SOLIDWORKS\data\weldment profiles\ansi inch\angle iron.

Wherease, configurable profiles have a two-level folder path. For example:

\..\ SOLIDWORKS\data\weldment profiles\ansi inch\

1. Profile positioning

While creating weldment structures, the following settings are available to position the profile sketch according to the design intent:

• Mirror Profile: Use this setting to flip the profile about on the horizontal or vertical axis.
• Alignment: Aligns an axis of the group profile to any vector (edge, construction line, etc.) that you select. Select which axis of the profile to align:
  • Horizontal axis
  • Vertical axis
• Rotation Angle: Use this option to rotate the profile. The profile rotates with respect to the pierce point.
• Locate Profile: This option allows you to define the position of the weldment profile. By default, the location of the weldment profile is at the origin of its sketch.

The Weldments folder of the Design Library contains additional weldment profiles for other standards. (Design Library > SOLIDWORKS Content > Weldments). To download the standards files, press the Ctrl key on the keyboard and then click a standard.

• When using custom profile weldment structures, remember that another user cannot reuse a custom profile to create a new weldment model if the custom profiles are not available to other users. In such circumstances, the best practice is to use a common shared location for custom profiles.

1. Sketch Tips

In SOLIDWORKS, you can use both 2D and 3D sketches as layout sketches. An advantage to using a 3D sketch is that all of the sketch entities and its parametric relation is under one sketch. This is the reason that many users prefer a 3D sketch for weldment layout.

2D sketch:

• SOLIDWORKS creates 2D sketch geometry on a reference plane or face.
• Using a 2D sketch for sketching complex geometry is time consuming, and might require the creation of additional reference planes.

3D sketch:

• A 3D sketch does not require the creation of additional reference planes.
• It is relatively quick and easy to sketch complex geometry using a 3D sketch.
• You can create the complete geometry in a single 3D sketch .

The following image compares the number of sketches necessary to create a similar sketch profile using 2D and 3D sketches.

1. Importance of Weldment Groups

A weldment group is a collection of structural segments that have the same cross section. When creating a structural member, users can select sketch segments within the same group or from different groups. Users can create a group that contains a particular feature to affect all segments without affecting other segments or groups in the structural member. Selecting sketch segments in the same group ensures application of the same settings for corner treatment, weld gap, alignment, etc. The advantage of working with groups is that bodies never intersect with each other and the software automatically trims and extends them.

1. Types of groups

• Contiguous group: A continuous contour of segments that join end-to-end. You can control how the segments join to each other. The end point of the group can optionally connect to its beginning point.

• Parallel Group: Includes a discontinuous collection of parallel segments. Segments in this group cannot touch each other.

It is possible to create weldment structures by using either a single group or multiple groups. The following examples describe the advantages and disadvantages of the different behaviors.

1. Working with a single group

When all sketch segments connect with each other, the recommendation is to create a single group. With a single group, you can use multiple options for corner treatments, as shown in the following image. In this case, SOLIDWORKS applies the same corner treatment in all corners of the weldment.

Single groups also require less rebuild time when compared to multiple groups. When working with a complex geometry, use of multiple groups can increase the rebuild time and affect the overall performance of the model.

1. Working with multiple groups

When sketch segments do not connect, it becomes necessary to use multiple groups. In this case, you can create multiple groups in the same structural member feature by using the New Group option. Be aware that the weldment profile will be same across all groups, however settings such as corner treatment, weld gap, alignments, etc. can be different between the groups.

The following example depicts the existence of multiple groups, and each group consists of a single sketch line segment.

Unlike a single group, it is not possible to apply the corner treatment in this weldment structure.

1. Limitations of multiple groups

• Limited availability of corner treatment options
• You must specify the corner treatment at every corner separately
• You must define the settings for each group separately

Because of the limited corner treatment option, if SOLIDWORKS does not create the corners you want, you need to use the Trim/Extend command. This increases the number of features and therefore affects performance.

Selecting a group in the PropertyManager highlights only that group in the graphics area.

 

When using the End Miter corner treatment, an additional Merge miter trim bodies option becomes available in the PropertyManager. As the name implies, this option combines miter trim bodies, and the cut list displays the length of all combined bodies.

option

Before the release of SOLIDWORKS 2013, this was the default option. However, having this option active by default creates a cut list showing a single body with a combined length. This creates problems if left unnoticed. Therefore, the behavior changed effective with the release of SOLIDWORKS 2013 SP03. The Merge miter trimmed bodies option is now inactive by default.

1. Weldment Configuration

In SOLIDWORKS, the addition of a weldment feature creates two default configurations. The default configurations are:

• Default
• Default , which is a derived configuration

This allows a user to keep machining features (such as hole, fillet, chamfer, etc.) active in the As Machined configuration. Whereas, the As Welded configuration suppresses the machined features to show the part as it appears prior to the machining operations.

Users can deactivate the automatic creation of derived configurations by going to Tools > Options > Document Properties > Weldments and then clearing the Create derived configurations option. The Assign configuration Description strings option controls application of the As Machined and As Welded suffix text.

1. Weldment Cut List – Configurations

Whenever SOLIDWORKS creates a cut list in a drawing, the cut list always links to the Default configuration. In a scenario where a user deletes this configuration, then SOLIDWORKS creates the cut list with the Default configuration.

Be aware that the drawing cut list is an exact replica of the cut list table in the part. In many cases, users think that the drawing cut list is wrong when they compare it with the As Machined configuration in the model. However, users should always compare the As Welded configuration in part to the drawing weldment cut list. The following image demonstrates the case where the cut list in the drawing is pointing to the As Welded configuration, and the active configuration in the model is As Machined.

1. Bill of Materials – Indented – Detailed cut list

The BOM – Indented cut list is similar to the weldment cut list. Users can also insert cut list information by going to using Insert > Tables > Bill of Materials > Indented > Detailed cut list. This cut list is further customizable as Flat numbering, Detailed numbering or No numbering.

The advantage of an Indented BOM is that the user can switch between the Default and Default configurations. The design intent of the weldment cut list is that you can only select Default configurations because the structural member bodies from this configuration are what companies buy from their hardware vendors.

Another important advantage in a BOM is the use of equations, which is a limitation in a cut list.

1. Weldment Properties and Cut List Properties

Similar to the custom properties in a SOLIDWORKS file, every weldment or sheet metal part contains cut list properties. The key difference between custom properties and cut list properties is that custom properties are created at the document level, whereas cut list properties are created in the cut list item. By default, cut list properties are inserted when you create a weldment or a sheet metal feature. The template file that drives the weldment cut list properties has the name cut list.sldwldtbt. The location of this file is:

[install_directory]\..\SOLIDWORKS\lang\[language]

Users can edit the cut list property template to add more properties that then become available in the drop-down list.

The Description property value can also govern then name of the cut list folder. To change this value, go to Tools > Options > Document Properties > Weldments and then activate the Rename cut list folders with Description property value option. These folder names help to identify the profile in use.

The default cut list properties are Length, Angle, Description, and Material. You can also get the bounding box properties of a body by selecting the Create bounding box option.

Effective with the release of SOLIDWORKS 2018, you can copy and paste the properties from cut list to custom, and vice versa.

1. Properties in detail

• Description: This value is evaluated from the information in the profile's (.sldlfp) file properties. To add or modify properties that appear in the cut list, go to File > Properties and modify the Custom properties of the .sldlfp format file..
• Length: This property value is derived by measuring the normal distance between end faces.
• Angle: This is the angle between the normal of the cut face and the centerline of the body.
• Quantity: This property reflects the quantity in each cut list folder. If the Detailed cut list option is not active while creating the BOM, the BOM quantity shows the length value.
• Total Length: This value displays the combined length of all items that have the same profile, material, and size. From SOLIDWORKS 2016 onward, derived parts display the Total Length in the cut list properties.

Effective with the release of SOLIDWORKS 2020, two new cut list properties are available for structural members:

1. Angle Direction: This property indicates whether the two ends face of the body are along the same direction or not. You can specify:

• Same
• Opposite
• Out of Plane
• None

1. Angle Rotation: The Angle Twist property indicates the angle between the normals of two end cut planes for out of plane trimming. You can set the angle from 0–180 degrees.

 

To exclude display of the cut list item, select the Exclude from cut list option.

Cut list update:

• Before the release of SOLIDWORKS 2015, it was a requirement that all bodies under the cut list must be grouped as items. SOLIDWORKS provides automatic and manual options for the grouping. As shown in the following image, the Automatic option is the default active setting. This option groups the bodies automatically on the basis of geometrical similarity whenever the Update option is active. The Update option also rearranges the cut list when there is a change to the part design. When a cut list requires an update, the ‘Update’ symbol appears in the cut list as shown in the following image:

An common observance is that when there are modifications to weldment sketches or profiles in quick succession, a user might complain that a drawing cut list does not display the correct information. In such cases, the first thing to try is to select the Update option in the Cut list feature of the part.

If the Automatic option is not active, you must perform the grouping of items in “manual” mode by right-clicking a body (or multiple bodies) and then creating a cut list item. You can then drag and drop bodies to rearrange them in the cut list.

• Effective with the release of SOLIDWORKS 2015, a modification to the cut list update operation introduced the Automatically update cut lists option under Tools > Options > Document Properties > Weldments. This option also appears as Update Automatically on the context menu of the Cut list feature. When active, this option updates the cut list after any modification. However, users still have the ability to control this behavior manually. If the Update Automatically option is not active, then users can select the Update option to update the cut list manually.

• Linking cut list properties: It is possible to add a cut list item name in the BOM. To acomplish this, add a new property, and then under Text/Expression, select the Cut list name option. Thereafter, when you insert a BOM, you can select the cut list folder name under the BOM column.
• Cut list sorting options: Effective with the release of SOLIDWORKS 2017, there is an option available to sort cut list items. Using this option, you can collect the identical bodies by excluding the faces generated from holes, fillets, and chamfers. A minor difference in the bodies caused the cut list to use different groups for similar bodies. This was once a problem when generating a stock list for such items.

• Mirror or Derived part: It is common practice of users to create derived weldment parts (mirror weldment part or by performing Insert part in a weldment part ). This imports cut list properties from the parent (base) part to the derived part. When inserting a weldment part, a Cut-list properties option is available in the Insert Part PropertyManager. Cut list properties display as linked to parent part- under Value / Text Expression for properties that link to the parent part. You cannot modify such properties without breaking the external reference link.

1. Editing Weldment Features

In addition to the Structural Member feature, there are many additional features in weldments to complete the weldment part design. These features are applied on the structural members to achieve the required geometry. Effective with the release of SOLIDWORKS 2016 onward, the feature name for a structural member is based on the type and size of the structural members inserted. Some of these features include the following:

1. Trim/Extend

Use the Trim/Extend command to trim and (or) extend bodies. When creating structural members using separate features, the bodies do not produce the proper ‘corner’ geometry. In such situations, the Trim/Extend feature is very helpful.

There are four corner trim options.

After selecting the bodies to trim, you also have the ability to specify whether to keep or discard individual bodies as shown in the following image.

In many cases, it is preferable to trim by using the Face/Plane option because it offers better performance. Select the Bodies option when trimming against a non-planar entity such as a round pipe or a stepped surface.

Keep in mind that use of the Trim/Extend feature creates a new set of bodies, which might cause the cut list to update. Users often ask why weldment cut list items lose their manually added cut list properties when trimmed. This occurs because when the Trim/Extend feature creates a new body, the cut list items and properties change. Users should add these properties again for the trim or extend bodies.

• Avoid using multiple faces to trim and extend bodies. Using multiple faces when trimming or extending bodies can create multiple unwanted bodies.

For example, the previous image depicts the selection of multiple faces as the trimming boundary. In this case, after the trim operation, the user might expect that the creation nine bodies. However, the Trim/Extend feature creates 13 bodies. Because of the selection of multiple faces, the bodies get trimmed as well as extended because the Allow extension option is active and the user did not select whether to keep or discard bodies. Therefore, the operation creates eight trimmed bodies instead of four.

The following image displays the assignment of the keep and discard tags to each body. Bodies that receive the keep tag will result in the creation of many bodies. In this case, there are eight. Therefore, be watchful of the number of bodies. As an option to avoid such problems, you might deactivate the Allow extension option.

1. Sub-weldment

A sub-weldment is a subset of items in a weldment cut list. In simple terms, a sub-weldment is a folder that is created in the cut list by selecting the required cut list bodies.

Sub-weldment fuctionality exists to help manage large and complex weldment cut lists. To create a sub-weldment, right-click one body or multiple bodies in the cut list, and then click Create sub-weldment.

In the folder structure for sub-weldments, each unique body has its own cut list item. This helps to differentiate between the different bodies.

1. Fillet Beads

Fillet beads are the geometry in the welded portion. Users can create full length, intermittent, or staggered fillet weld beads between any intersecting weldment entities such as structural members, plate weldments, or gussets.

Fillet beads create solid bodies in the cut list, however they are not added to any cut list folder. Fillet beads are considered for the mass calculations. To ignore fillet beads for a mass calculation, create a folder that contains all fillet bead features inside, and then suppress the folder.

 

1. Weld Beads

Weld beads are the cosmetic representation of welded geometry. Unlike fillet beads, weld beads do not create a solid body. Instead, they create a geometry-like display that simplifies the part design. You can use either the Weld Geometry option or the Weld Path option to create weld beads. Use the Weld Geometry option when specifying single-body and multibody welds. The Weld Path option provides a single selection box where you select the faces and edges to weld.

Because this is only a display representation, the weld beads do not affect performance to the same extent as fillet beads. Therefore, to improve the performance, use a weld bead instead of a fillet bead wherever possible.

The benefits of using weld beads include:

• Uniform implementation in parts and assemblies
• Compatibility with all types of geometry, including bodies with gaps
• A lightweight and simplified weld bead display
• Inclusion of weld bead properties in drawings using weld tables
• The Smart Weld Selection Tool for face selection of weld bead paths
• Association of weld bead symbols with the weld beads
• Handles that assist in defining weld paths (lengths)

1. Gussets

Gussets are the supporting members for structural members. They act as reinforcement for the area between two intersecting structural members. You can create gussets between disjointed planar surface bodies that are separated by a structural member. Gussets are also supported on cylindrical faces. You can set the color for gusset features from Options > Document Properties > Model Display > Gusset. To can add multiple gussets, select the Keep Visible (

In the FeatureManager design tree for a gusset, there are options available to create a Polygonal Profile

property.

1. End Caps

An end cap is used to close the ends of structural members such as pipes, square tubes, and rectangular tubes. Be aware that it is possible to add end caps only to profiles with linear edges.

Like a gusset, end caps receive only the Material property in the cut list.

1. Weldment Document Properties

Effective with the release of SOLIDWORKS 2015, some of the weldment options are available in the document properties. These document properties options allow users to create part templates for weldment parts. The weldment options include the following:

• Automatically create cut lists: This is the default option, which enables the automatic creation of cut lists. This setting groups similar bodies together. If the option is not active, you can enable it by right-clicking on the Cut list item in the FeatureManager tree.
• Automatically update cut lists: This default option activates the automatic update of cut lists. You can also control this behavior by selecting the Update Automatically option on the Cut list context menu. Consider turning this option off if you experience performance problems with large weldments.
• Rename cut list folders with Description property value: As the name implies, this option renames cut list folders with a description property value. This option is active by default when using a blank template to create a weldment part in SOLIDWORKS 2015 or later. The description property values are embedded through the weldment profile.
• Create derived configurations: This option manages if a user wants to create derived configuration Default . The advantage of this option is that the cut list in the drawing is created for the only configuration (default) in the part.
• Assign configuration description strings: This option is available only if the Create derived configurations option is active. This option adds As Welded or As Machined the suffix text to the configuration name. Before the release of SOLIDWORKS 2015, this behavior was managed by using the Disable additional weldment configuration description strings option under Tools > Options > System Options > General.
• Collect identical bodies: This option collects all bodies that are geometrically identical in a specified Cut-List-Item folder, but are generated by different features. This option is useful to collect identical bodies and choose faces and features to exclude in sorting.
• Bounding Box Properties: This option is available effective with the release of SOLIDWORKS 2018. The option allows customization of the bounding box properties. To customize these properties, deactivate the Use default description option, and then enter values in the respective fields. When appropriate, you can also select to change the existing bounding box properties in legacy parts. Be aware that you cannot reverse changes that you make to existing bounding box descriptions.

1. Unlinking and Relinking Cut List Properties

Effective with the release of SOLIDWORKS 2018, the Link column in the Cut-List Properties dialog box allows you to select properties where the text in the Value/Test Expression column can link to a parent part or to a cut list folder. If the check box in the Link column is clear, you can override the value in the Value/Test Expression column. Be aware that a linked check box is active only for the system-defined properties.

1. Configuring Cut Lists

In the Cut-List Properties dialog box, you can configure cut lists by making a selection from the Configuration drop-down list in the upper left corner of the Cut List Summary tab.

You can also apply a configuration to a cut-list property. To do this, in the Properties Summary tab, click the Configuration icon next to the text in the Value/Text Expression column, and select one of the following:

• This Configuration
• All Configurations
• Specify Configurations

Selecting a configuration option updates the evaluated value.

If a property links to a parent configuration, clear the link before assigning a configuration to the Value/Text Expression property.

1. Tips for Troubleshooting Weldments

The following topics represent some commonly reported problems and possible troubleshooting tips.

1. Cut Lists
2. Part cut list properties do not match drawing cut list

By default, a weldment part creates an and an configuration. In a weldment model, the default active configuration is . The configuration is used for a drawing cut list.

The most likely reason for a mismatch of cut list property values in a part and drawing is the use of different configurations. A primary troubleshooting tip is to verify the cut list properties by activating the configuration in the part.

1. Newly created structural members do not appear in a drawing cut list

In this case, a part consists of multiple configurations that also include the derived configuration. A structural member is added to another configuration and the weldment cut list refers to a different configuration.

For example, the previous image depicts the addition of a new structural member to the Same feature configuration, while the cut list refers to the Separate Feature configuration.

 

1. Length and Angle values in the drawing weldment cut-list do not match the same values in a part:

This is similar to the case for the previous issue. Users work primarily in the active configuration of the part, and modify the length and angle values there. While modifying the dimension, the configuration option is set to This Configuration. The user might expect the dimension to change in the drawing cut list also, however this is not the case. The reason is that the dimension modification happened only in the configuration. Therefore, make sure to also apply the change to the configuration.

1. Bodies do not group together
2. Mirror bodies do not group together

In the following example, the bodies are mirrored. Therefore, users expect them to be grouped together.

SOLIDWORKS only groups bodies when they are geometrically identical. However in this case, these bodies are not geometrically identical because the geometry of the hole is in a different position in both bodies. To verify if the bodies are identical, use the Move/Copy command to align the bodies and overlap the bodies as shown in the next image.

In the example, the holes are on the same side but at a different location in both bodies. Therefore the parts are not identical and SOLIDWORKS groups them separately.

1. Geometrically similar bodies do not group together

Consider the same example if we remove the holes from the bodies, and yet SOLIDWORKS still groups the bodies separately.

This behavior occurs because the bodies do not use the same material. Different materials have a different density, which creates a difference in mass. This makes the bodies asymmetrical, and so the software groups these bodies separately.

1. Weldment Performance
2. Weldment part is taking more rebuild time

To verify which feature is taking more rebuild time, go to Tools > Feature statistics. The Performance Evaluation dialog box lists all of the features in the model and the amount of time it takes to rebuild each feature. Analyse the feature that is taking the most amount of rebuild time, and determine if there are externally referenced features that are contributing to the performance problem.

One of the commonly known delaying factors is the presence of a large number of weld beads. Sometimes creation of a weld bead can take a lot of time even for simple geometry when the faces and edges being welded are very long. The reason for such delays remain under investigation as of the most recent update to this document.

1. Performance issues due to many number of bodies and weldment cut list

Editing a feature or sketch and then rebuilding the model might also be affected by the cut list presence when there are a large number of bodies. In addition, the number of bodies also influence interactive operations such as zoom, pan, and rotate. More recent versions of SOLIDWORKS demonstrate great improvement in the handling of a large number of weldment bodies. If you experience similar issues in an older version, it is a recommendation to verify the problem in the latest version.

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