Navigating in 3D Space

When drawing a line in a 3D sketch, the cursor and origin initially look like those shown in Figure 36.1. The large red origin is called the space handle, with the red legs indicating the active sketching plane. Any sketch entities that you draw lie on this plane. The cursor also indicates the plane to which the active sketching plane is parallel. The XY graphic shown in Figure 36.1 doesn't mean that the sketch is going to be on the XY plane, just parallel to it.

Pressing the Tab key causes the active sketching plane to toggle between XY, YZ, and ZX. The active sketching plane indication doesn't create any sketch relations; it just lets you know the orientation of the sketch entities that are being placed. If you want to create a skew line that isn't parallel to any standard plane, you can do this by sketching to available endpoints, vertices, origins, and so on. If there are no entities to snap to, then you need to accept the planar placement, turn off the Line tool, remove any automatic relations, rotate the view, and move one end of the sketch entity in a different plane.

An excellent tool to help you visualize what's happening in a 3D sketch is the Four Viewport view. This view divides the screen into four quadrants, displaying the front, top, and right views in addition to the trimetric or isometric view. You can sketch in any of the viewports, and the sketch updates live in all the viewports simultaneously. This arrangement is shown in Figure 36.2. You can easily access the divided viewport screen by clicking buttons on the Standard Views toolbar. You can also manually split the screen by using the splitter bars at the lower-left and upper-right ends of the scroll bar areas around the graphics window.

When you move unconstrained entities in a 3D sketch, they move in the plane of the screen. You can use this to your advantage to create or edit lines in 3D space, but it can also lead to unexpected results. When you view the sketch at an angle, move it, and then rotate the view, you may notice that the sketch has shot off into deep interplanetary space. This is another reason for using the Four Viewport view, which enables you to see what's going on from all points of view at once, thereby avoiding any surprises.

Understanding Sketch Relations in 3D Sketches

Several relations are available in 3D sketches that aren't found in 2D sketches, such as AlongX, AlongY, AlongZ (which act as replacements for horizontal and vertical), and OnSurface.

Relations in 3D sketches are not projected as they are in 2D sketches. For example, an entity in a 2D sketch can be made coincident to an entity that's out of plane. This is because to make the relation, the out-of-plane entity is projected into the sketch plane, and the relation is made to the projection. In a 3D sketch, “coincident” means coincident, with no projection.

Keep in mind that solving sketches in 3D is more difficult than it is in 2D. You'll see more situations where sketch relations fail or flip in the wrong direction. Angle dimensions are particularly notorious in 3D sketches for flipping direction if they change and go across the 180-degree mark. When possible, you should work with fully defined sketches and be careful (and conservative) with sketch relations.

For example, the sketch shown in Figure 36.3 cannot be fully defined without also overdefining the sketch. The main difficulty is that the combination of the tangent arc and the symmetric legs of the end brace cannot be located rotationally, even using the questionable reliability of 3D planes that are discussed next. The only workable answer to this problem is to create a separate 2D sketch on a real 2D sketch plane, where the plane is defined by the elements of the 3D sketch.

Creating Planes in Space

It's possible to create planes directly inside 3D sketches. These planes are defined by constraints and selections rather than selecting a type of method to define a plane. Sketches can be created on these planes and move with the planes. Having planes in the sketch also enables planar sketch entities such as arcs and circles in 3D sketches.

Unfortunately, you must watch out for many things with 3D planes. Be aware that they don't follow their original definition like normal reference-geometry-type planes. Planes inside 3D sketches act more like sketch entities in that if they are underdefined, they can move around inside the sketch. Watching sketch planes move in a sketch is very unsettling for most SolidWorks users. Figure 36.4 shows the PropertyManager interface for creating 3D planes; however, keep in mind that the plane doesn't maintain the original relation to these initial references. The parent-and-child relations that SolidWorks users are used to are suspended for this one function, or they work in the reverse from what you normally expect.

A 3D plane cannot be fully defined unless some sketch geometry on the plane is in turn related to something else. Limited types of sketch relations can be applied directly to the actual plane. Horizontal and vertical relations cannot be applied directly to the plane to orient it. Horizontal and vertical relations of entities on the plane are relative only to the plane and not to the rest of the part; therefore, making a line horizontal on the plane doesn't mean anything when the plane rotates (which it's free to do until it's somehow constrained to prevent this).

Beyond this, when a plane violates a sketch relation, the error isn't reported, which severely limits the amount of confidence that you can place in planes that are created in this way. The biggest danger is in the plane rotating, because that's the direction in which it is most difficult to fully lock down. The best recommendation here is to create reference sketch lines with relations to something stable, preferably outside of the 3D sketch.

If you choose to use 3D planes, you can activate them for sketching by double-clicking a plane. The plane is activated when it displays a grid. You can double-click in an empty space to deactivate the plane and return to regular 3D Sketch mode. The main thing that you give up when abandoning 3D sketch planes is the ability to use the Dynamic Drag options when all loft or boundary sketches are made in a single 3D sketch.

Limiting Path Segments

Some of the path segments that are allowed in 3D sketches can be used only if you sketch them on a plane. These entities include circles and arcs, and can include splines, although splines aren't required to be on a plane. To sketch on a 3D plane (a plane created within the 3D sketch), you can simply double-click the plane.

Some sketch entities and tools exist that you cannot create or use inside a 3D sketch, even if a sketch plane is activated. They include the following:

• Autodimension
• Fully Define Sketch
• Modify Sketch
• Sketch Slot
• Ellipse
• Polygon
• Dynamic Mirror
• Offset Entities
• Sketch text
• Sketch Picture

To sketch on a standard plane, planar face, or reference geometry plane, you can Ctrl+click the border of the plane with the Sketch Entity icon active or double-click the plane. The space handle will move, indicating that newly created sketch entities will lie in the selected plane.

Using Dimensions in 3D Sketches

Dimensions in 2D sketches can represent the straight-line distance between two points, or they can represent the horizontal or vertical distance, depending on the position of the cursor when you place the dimension. In 3D sketches, dimensions between points are always the straight-line distance. If you want to get a dimension that's horizontal or vertical, you should create the dimension between a plane and a point (the dimension is always measured normal to the plane) or between a line and a point (the dimension is always measured perpendicular to the line). For this reason, reference sketch geometry is often used freely in 3D sketches, in part to support dimensioning.

This is one of the differences between 2D and 3D sketches that users find difficult to manage. If you're used to visualizing dimensions within 2D sketches, direction-controlled dimensions in 3D sketches can be difficult to visualize and even more difficult to create.

Using the Weldment Feature

The Weldment button on the Weldment toolbar simply places a weldment placeholder in the FeatureManager. This placeholder tells SolidWorks that this part is a special weldment part—much in the way that the Sheet Metal feature in sheet metal parts is a placeholder—and denotes a special part type. The Weldment feature moves to the top of the tree, regardless of when you create it in the part history. If you don't create a Weldment feature manually, then one is automatically created for you and placed at the top of the tree when the first Structural Member feature is created. Structural members are discussed in the next section.

This feature offers only a few special default settings: You can set custom properties that transfer to all cut-list items that are created in the current part, and the Merge Result option is deselected by default in weldment parts. The ability to set custom properties is important when multiple weldments go together to make an assembly. To access the Custom Properties interface, shown in Figure 36.5, select the Properties option on the Weldment feature RMB menu.

The general workflow for creating weldment parts is as follows:

1. Create a new part and insert a Weldment feature.
2. Create a structural layout of 2D sketches, 3D sketches, or a combination of 2D and 3D sketches to represent a structure to be fabricated by cutting and welding structural shape stock.
3. Ensure that you have a library with appropriate structural shape sketches, properties, materials, and so on.
4. Make sure that you have allowed for sketch lines in the structural layout to represent a corner, centerline, or some other reference in the library structural shape sketch. This can greatly affect intersections between structural members.
5. Assign structural shapes to individual lines in the structural layout. Be sure you understand the rules on using groups.
6. Trim and miter intersections between structural members to suit your design.
7. Add plate entities such as end caps and gussets.
8. Add weld beads as needed.
9. Place the weldment into an assembly, and add castings and sheet metal parts, as well as holes and fasteners to attach nonwelded components.

Introducing the Structural Member Feature

A structural member is the basic building unit of weldments in SolidWorks. You can create a structural member by extruding or sweeping a profile along one or more path segments, and it may result in a single body or multiple bodies. The path segments may be in the form of 2D or 3D sketches.

When creating the sketch for the weldment, it's important to decide what the sketch represents. For example, does it represent the centerline of the structural elements or does it represent a corner? You can orient and position structural shape profiles relative to the frame sketch in several ways, with positioning at the shape centroid being probably the most intuitive for closed shapes and a corner being most intuitive for angle channels.

Figure 36.6 shows a single 3D sketch of a simple frame and a Structural Member feature in the process of creation. You must select the standard first, then the type, and finally the size. A limited number of profiles come with the software, and although you'll probably need to create some custom profiles, they're fortunately very easy to create.

To access a large number of weldment profiles in various standards, open the Design Library and click the SolidWorks Content icon. Under that, the Weldments folder has several zip files containing weldment profiles. Ctrl+click an icon to download the file, and then extract the contents of the zip file to the library location you have established for your weldment profiles.

GROUPING SELECTED PATH SEGMENTS

The concept of groups is simple. You can organize selected path segments within a structural member feature into two kinds of groups: parallel or contiguous. A single structural member may have multiple groups.

Parallel groups contain parallel path segments that don't touch. Parallel groups also require that you select the structural profile before you can select more than one path segment.

Contiguous groups contain path segments that touch end to end, two segments at a time. A contiguous group cannot have one path segment intersect in the middle of another or more than two path segments intersecting at a corner.

Each group can have only a single orientation of the structural profile. For example, if each frame leg needs the profile rotated to a different orientation, you need to rotate the legs in four separate groups instead of all in a single group.

Given those requirements, if the frame shown in Figure 36.6 were to be created entirely from the same structural profile—say, ANSI (American National Standards Institute) inch, square tube, 3 × 3 × 0.025—it would require a minimum of five groups, as shown in exploded form in Figure 36.7. The file used to create this image is included in the download materials from the website under the name Weldment groups.sldprt.

The main advantages of the groups functionality are that each member within the group is automatically trimmed to other members of the group, and you can control gaps within or between groups. The only trimming you need to take care of separately is the trimming between members of different groups.

LOCATING AND ORIENTING THE PROFILE

When you apply a profile to a path segment in a Structural Member feature, the profile must have some relationship to the path segment. The default point where the path “pierces” the profile is at the sketch origin. To change the pierce point, you can click the Locate Profile button at the bottom of the Structural Member PropertyManager, which zooms the view to present the profile sketch so you can select another sketch point to use as the pierce point. You can select any sketch point on the profile, including endpoints, sketch points, and virtual sharp points if they are present in the sketch.

Profile sketches are generally surrounded by several sketch points, which may seem unnecessary until you consider that you can use any of the points to position the profile. The Settings panel at the bottom of the Structural Member PropertyManager is shown in Figure 36.8 and displays a profile sketch with the interface.

In addition to locating the profile sketch, you can also rotate the profile using the Angle field in the Settings panel. This rotates all the bodies that are created by the Structural Member feature at the same time. In the example of the four-legged frame, if the legs are rectangular or circular, they can all be created in the same Structural Member feature because they're all rotated in the same way. However, if the legs are made from an asymmetrical shape such as an angle, then each leg needs to be made using a separate Structural Member feature, with each leg rotated differently.

USING CUSTOM PROFILES

Most of the custom profiles that you will need may be simply new sizes of existing profiles. You can easily create a custom profile by opening an existing profile, editing it, and saving it under a different name using the Save As command. You can also use configurations in the library part to create multiple sizes of the profiles, which can then be selected for use in weldment parts.

Other sources for custom profiles include 3D Content Central, which has a large number of erector-set aluminum extrusion profiles and the accessory hardware for those systems. Toolbox also has a Structural Steel sketch generator, shown in Figure 36.9, which enables you to generate most standard shapes. If you have Toolbox installed on your system, you can find this tool in the Toolbox menu.

Weldment profiles are great candidates for storing in your special library folder, separate from the SolidWorks installation directory. To establish this library location, you can choose Tools ➢ Options ➢ File Locations ➢ Weldment Profiles. Also keep in mind that if you share design duties with other users, either the library location should be shared among users on a network or the libraries should be copied to each user's local library. You can also share library data through a Product Data Management, or PDM, program.

If you are creating completely new custom profiles, remember that when locating the profile relative to the path segments, you can use any sketch point. As a result, you should provide ample selections for pierce points. Virtual sharps function well around filleted corners, as well as sketch points at the centroid of a shape.

In addition to sketch geometry, the library part files should also contain custom property information about the structural shape, such as part number, supplier, material, and so on. This information propagates to the cut list.

ADDING CORNER TREATMENTS

Any intersection of sketch lines at mutual endpoints within a single group, except as noted in this section, creates a situation that requires that the corners be cut to match. Figure 36.10 shows an example of the options available when lines meet at right angles. Notice that within a group, you have the option to set a weld gap at the intersections.

To access the toolbar with the Corner Treatment options, you can click the pink dot at the intersection of the path segments. The default Corner Treatment settings are found in the Structural Member PropertyManager, but you may need to adjust them individually.

Two situations don't require corner treatments. The first situation is when a line intersects another line at some location other than an endpoint in the same Structural Member feature—for example, a support meeting the main member in the middle. In this situation, the member that ends in the middle of the other member is trimmed to a butt joint. The second situation is when an intersecting member is created by a later Structural Member feature. You deal with this situation by using the Trim/Extend function, which is described later in this chapter.

USING ARC SEGMENTS

When arc sketch segments are part of the selection for a Structural Member, a Merge Arc Segment Bodies option appears after the selection box in the Selections panel. This means that any tangent arc segment will be joined to the entities to which it's tangent, but any nontangent entities will create separate bodies.

Figure 36.11 shows a tangent arc in the curved leg brace, along with the Merge Arc Segment Bodies option in the PropertyManager.

If the Merge Arc Segment Bodies option isn't selected, then a separate body is created for arc segments. The Merge Arc Segment Bodies option applies to the whole feature and cannot be set selectively for individual arc segments within the selected sketch entities; it's either selected for all or deselected for all. If some arc segment bodies are merged and others are not, then you should create separate Structural Member features.

It's also a curious limitation that only one arc may be selected if the selected path segments are disjointed. For example, you cannot select the two arcs for two J-shapes that don't touch in the same Structural Member feature. The obvious workaround is to create two separate groups.

Using the Trim/Extend Feature

In situations where you must create multiple Structural Member features, thereby creating intersecting bodies, you must deal with the interferences using the Trim/Extend feature. An example of this is shown in Figure 36.12. The legs and braces shown are all being trimmed by a single face on the bottom side of the rectangular section of the frame, where a small arrow will appear.

Bodies can be trimmed by planar faces or other bodies. Bodies can also be trimmed before they are mirrored or patterned. Although trimming with faces is faster, it may not give the same geometrical results.

The Extend option enables either trimming or extending, as appropriate. If the Extend option isn't selected, then trimming is the only action available.

Using the End Cap Feature

The End Cap feature closes off an open-ended structural member. You can add multiple end caps in a single End Cap feature. The PropertyManager and the end product are shown in Figure 36.13.

The end cap using the Outward option sits on the outside face of the member and overlaps the thickness of the member by the inverse of the thickness ratio that's applied in the Offset panel. If the Use Thickness Ratio option is turned off, it functions as an offset from the outer faces of the member from which it is created. When this option is turned on, the thickness ratio can range from zero to one. For a value of zero, it's flush with the outer faces of the member, and for a value of one, it's flush with the inner faces of the member. Using the Inward option, the cap fits inside the hole in the member.

Working with the Gusset Feature

The Gusset feature creates a three-, four-, or five-sided gusset in a corner between structural members, as shown in Figure 36.14. You can place the gusset at specific locations along the edge in the corner, or you can offset it by a specific dimension in a specific direction by using the settings in the Parameters panel. You can control the size and thickness of the gusset in the Profile panel. There's no sketch for this feature type; it's simply created from the parameters that you enter in the PropertyManager interface. Again, if you need to make multiple Gusset features in succession, you can use the pushpin icon to keep the interface displayed until you close it by clicking the red X icon.

Using Cut-List Properties

In addition to the custom properties for the document, SolidWorks weldments also utilize Cut-List Properties. You can access Cut-List Properties by right-clicking a Cut List Item folder (other than the top-level Cut List folder) at the top of the FeatureManager and selecting Properties. The Cut-List Properties may not be available for a newly created weldment until you have updated the cut list (right-click the top-level Cut List icon and select Update).

Figure 36.17 shows the Cut-List Properties dialog box, which allows users to enter data such as length and material for BOMs and cut lists.

Notice the Properties Summary tab, which enables you to look at each property and see the value for each cut-list item. This is where you would select a property such as Description, assign descriptions for each cut-list item, and then go on to the next property—say, Material—and assign values for that property.

The Cut List Table tab shows you a preview of the cut list and enables you to use cut-list templates that might have different default columns established. Figure 36.18 shows the Cut List Table tab of the Cut List Properties dialog box.

As Figure 36.18 shows, you may need to enter information for items added to the weldment such as end caps or gussets. Cut-list properties are also added when you insert a bounding box for nonstructural members.

Excluding and Reordering Cut-List Items

To exclude a feature in the FeatureManager from the cut list, you can select Exclude From Cut List from the feature's RMB menu. The next time the cut list is updated, the members that were created by that feature will be listed at the bottom of the Cut List folder with the weld beads. To include the item again in the cut list, select Include In Cut List from the feature's RMB menu and update the cut list again. Figure 36.19 shows a folder that has been excluded from the cut list.

Only entire Cut List folders can be eliminated from the cut list, not individual bodies. To reorder items in the cut list, just drag and drop the folder to where you want it to be in the list.

Using Weld Beads and Fillet Beads in Weldments and Assemblies

The icons for Weldment, Fillet Bead, and Weld Bead look very similar. The Weldment tool is used to proclaim the part as a Weldment part. The difference between a fillet bead and a weld bead is that the Fillet Bead feature creates actual solid geometry, which shows up in a weldment part as a feature, while the Weld Bead feature creates a cosmetic representation of a weld bead. Figure 36.20 shows the Fillet Bead features in the FeatureManager and the actual fillet bead between a plate and a structural member.

To create a weld in an assembly, you still use the Weld Bead tool. The Weld Bead feature produces a cosmetic display of a weld and keeps track of it in a folder at the top of the assembly FeatureManager or the Weldment Part FeatureManager.

Figure 36.21 shows the Weld Bead PropertyManager and the preview it applies to a weldment part.

The Weld Bead feature doesn't show up in the part or assembly FeatureManager as a feature (even though you access the command at Insert ➢ Assembly Feature ➢ Weld Bead), and it doesn't create geometry that adds mass. It does produce a cosmetic weld bead on the part, and it creates a new folder in the FeatureManager right below the Annotations folder. The entries in the folder show how many weld beads of what length are applied to the entire weldment. Fillet beads add nothing to the Weld folder. As a result, the type of information you need to have in your model will help you determine if you want to use the Fillet Bead or Weld Bead feature. If you need to show welds in an assembly, you have to use the cosmetic display of weld beads.

The Weld Bead PropertyManager also gives you the option to define the ANSI weld symbol before the feature is complete. The interface for defining the weld symbol is shown in Figure 36.22. Use the Define Weld Symbol button in the Settings panel of the Weld Bead PropertyManager to access this interface.