Chapter 22
Working with Large Scale Design

According to SolidWorks marketing materials, “Large Scale Design brings together the tools you need to effectively design machinery, heavy equipment, plants, small ships, and other large objects.”

Large Scale Design encompasses topics exclusively covered in this chapter: Walk-through animation, GridSystem, IFC export, Large Design Review, and Facility Layout. Although Large Scale Design also uses standard SolidWorks functionality such as sketching, part modeling, assembly modeling, weldments, and drawings, these latter topics don't have Large Scale Design–specific capabilities at this time.

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IN THIS CHAPTER, YOU WILL LEARN TO:

• Understand Large Scale Design
• Use Walk-through
• Export to IFC
• Create a grid structure
• Lay out a facility
• Use Large Design Review

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Using Large Design Review

Large Design Review is a view-only mode that enables you to perform design review activities with large assemblies. You have access to the following features of SolidWorks:

• FeatureManager
• Measure tool
• Section tool
• Hide/Show
• Assembly Xpert
• Walk-through
• The Large Design Review tab on the CommandManager

In Large Design Review, you don't have access to these features:

• Part features
• Assembly features
• Component patterns
• Mates
• Dynamic assembly motion
• The Assembly tab of the CommandManager
• Change component properties
• Change configurations in LDR mode

To open an assembly in Large Design Review, use the Open dialog box, and in the Mode drop-down box, select Large Design Review (LDR), as shown in Figure 22.1.

FIGURE 22.1 Using the Open dialog to open an assembly in Large Design Review mode

Figure 22.2 shows the dialog box that welcomes you to LDR on the left and the LDR FeatureManager and toolbar on the right.

FIGURE 22.2 Large Design Review enables you to review large assemblies more quickly.

One of the things that has been removed from this window is a list of some of the limitations. When working with a new tool, it is important to know how far you can expect it to go. The window does suggest that you have a look at the Help for more information on limitations. However, the linked Help page does not directly list limitations; per the typical SolidWorks method of handling such things, you are on your own to discover the boundaries of what can and cannot be done.

For example, Large Design Review is a stripped-down interface, built to help you look at a simplified data set. For this reason, it does not enable you to do everything you can do in the full SolidWorks interface, so some tools will be missing. You cannot see assembly features or mates. Some of the fancy visual effects such as RealView, shadows, reflections, and some materials will also be missing. Also, things like rebuild or forced rebuild will not have any effect.

The Large Design Review interface appears as shown in Figure 22.3.

FIGURE 22.3 The Large Design Review interface

Updating Large Design Review

Components within an assembly opened in LDR mode can become out-of-date due to changes to other components. To be notified when parts become out-of-date, you can use a system option at Tools ➢ Options ➢ Assemblies ➢ Automatic Check and update all the components. You may also need to update a component after the assembly has been opened in LDR. Options to do this are available from the RMB menu within an LDR assembly. Figure 22.4 shows some of these options.

FIGURE 22.4 An out-of-date component and how to update it

If you are working on a model that someone else has open in LDR and you make and save a change, you will get a message that warns you of the situation and gives you the option to update the LDR graphics, as shown in Figure 22.5.

FIGURE 22.5 When making a change to a model open in LDR, SolidWorks gives you the option to update the graphics.

Resolving Components

Because LDR is a lightweight mode, gaining full edit capabilities to parts within an assembly requires resolving that component. To do this, you can use one of the Selective Open or Set All options shown in Figure 22.2.

Taking Snapshots

Snapshots save a custom named view as a Snap feature in the Scene, Lights, And Cameras tab of the DisplayManager. One difference between a snapshot and a custom named view is that hidden parts remain hidden in a snapshot.

You can access the Snapshot tool from the View toolbar, through the menus at View ➢ Lights And Cameras ➢ Take Snapshot, or though the default hotkey Alt+spacebar. When you take the snapshot, SolidWorks asks you to name it, just as with a custom named view. Figure 22.6 shows snapshots saved in the DisplayManager.

FIGURE 22.6 Snapshots are saved in the DisplayManager.

The Home Snapshot is like the Default configuration. It is automatically created if you open an assembly in Large Design Review.

Creating a Walk-Through

Walk-through is a method to create an animation simulating what a person would see as he walks through a large-scale design. This chapter looks at the example of the very large dump truck. This turns out to be a good example of equipment design where a walk-through could be useful. Figure 22.7 shows the walk-through area of the DisplayManager along with the model used for this example. You can do walk-throughs using an interface to direct an avatar (virtual mannequin), or you can drive the camera along a sketched path. The sketched path method has some overlap with MotionManager animation, which is covered in Chapter 23, “Animating with the MotionManager.”

FIGURE 22.7 Using the DisplayManager to manage a walk-through

The interface for the walk-through consists of two elements. The initial setup is controlled by the Walk-through PropertyManager, shown in Figure 22.8.

FIGURE 22.8 Using the Walk-through PropertyManager for the initial setup

In the PropertyManager, you select a base plane, which acts as a floor, and then you establish a camera height to simulate the height of your eyes off the floor. If you intend to drive the walk-through using a sketch, you can select the sketch elements in the Motion Constraints selection box. For the most fluid motion, use splines. You can use 2D or 3D sketches.

To start the walk-though, click the Start Walk-through button on the PropertyManager, and the interface shown in Figure 22.9 will appear.

FIGURE 22.9 The Walk-through interface helps you manipulate the view and the motion of the camera.

Capturing the walk-through requires an interface that's significantly different from other SolidWorks tools, shown in Figure 22.9. Although the interface and documentation refer to an “avatar,” you won't notice any sort of virtual manikin walking through the model, except in SolidWorks sales demonstrations.

When you're in this mode, the scroll wheel on your mouse works backward from standard SolidWorks functionality for zooming. You also cannot turn and walk at the same time. The feel is very much like an early 1990s primitive video game.

The workflow to create a walk-through goes like this:

1. Select a suitable model, preferably something with an interior that you want to virtually wander around inside. It works best with models on the scale of buildings.
2. Click the DisplayManager tab in the FeatureManager area.
3. Click the Scene, Lights, And Cameras button.
4. Right-click the Walk-through entry in the list and select Add Walk-through.
5. Establish a floor or vertical direction and tell it which end is up (literally). Also establish the height of your eyes above the floor.
6. If you are using a sketch path, select the sketch segments in the Motion Constraints selection box.
7. Begin the capture of your walk-through. If you are using sketches to drive the motion, just press the Forward button on the interface, and the camera will walk along the path. If you are not using sketches, use the arrows on the interface to make the camera (called an “avatar” in this interface) move.
8. Generate and save the video.

The Dump Truck files I used for this example are in the download materials from the Wiley website. This is a good model to use for practice.

Creating a GridSystem

In SolidWorks, a GridSystem is a 3D sketch that repeats a 2D sketch on every level of a structure. You start by creating a 2D sketch where lines represent structural members for that level. SolidWorks uses derived sketches on planes. The 3D sketch itself contains only columns. The structure could be bolted together from fabricated I-beams, a welded tubing structure, or an assembled scaffolding, for example.

The GridSystem can help you identify interior and exterior walls, structural columns, and beams.

Figure 22.10 shows a complete GridSystem.

FIGURE 22.10 Building a GridSystem in SolidWorks

Here is the basic workflow for creating a GridSystem:

1. Click the GridSystem button on the Feature toolbar or in the Insert ➢ Reference Geometry menu selection.
2. Draw a sketch that represents the outer shape of the structure, as well as inner structural members.
3. Use the GridSystem PropertyManager to establish the number of levels (floors), the default height for levels, and the specific height for each level.
4. Click OK in the PropertyManager, and watch SolidWorks build the GridSystem.

Each step includes some detail and requires more explanation to make it work.

Starting the GridSystem Feature

The GridSystem toolbar icon is listed as part of the Feature toolbar, although it's not there by default. If you want to add the GridSystem icon to any toolbar, use Tools ➢ Customize ➢ Commands, and select it from the end of the list of icons for the Feature toolbar.

You can access GridSystem through the menus by default, but it's in a different location. Through the menus, click Insert ➢ Reference Geometry ➢ GridSystem.

Creating the Sketch

When you start the GridSystem feature, SolidWorks puts you into a 2D sketch on the Top (XZ) plane, but it provides no other explanation. The software is waiting for you to create a sketch with some specific properties. This sketch essentially represents the layout of the structural members forming one level of the structure. Figure 22.11 shows a sample sketch.

FIGURE 22.11 Sketching a sample structural layout

The sketch is dimensioned in inches, but you also can use more appropriate units, such as feet or meters.

Notice also that annotations label the intersections of the lines with letters for the X direction and numbers for the Z direction. Structural engineers use this method to identify the columns in the structure. The column in the center of the sketch shown in Figure 22.11 would be called 1B. These column line labels are automatically generated by SolidWorks when the Autonumber Balloons option at the bottom of the GridSystem PropertyManager is turned on.

Several rules for the sketch are not obvious. First, all the lines are planar and either horizontal or vertical within the sketch. You cannot make a circular structure or use the sketch to lay out something like a power line tower. You might be able to add diagonal members later, but you cannot use them as part of the initial layout for the GridSystem.

Using the GridSystem PropertyManager

When you are finished creating the sketch, exit the sketch using the Sketch icon in the Confirmation Corner (in the upper-right of the graphics window). This brings up the GridSystem PropertyManager, shown in Figure 22.11.

Everything in the GridSystem PropertyManager seems self-explanatory. The default level height of 118.11023622 inches is a conversion of the default 3-meter height that SolidWorks uses.

Notice that you can customize the height of each level. For example, if Level 3 has some specialized equipment that needs more room than the standard-level height, you can easily specify this as part of the design.

The setting for 3DSketch Split Lines controls whether the columns that extend through all levels of the grid will be continuous from top to bottom or whether they will be split at each level. Which option you select mainly depends on what you plan to do with the GridSystem. If you plan to use it to create a weldment, you may want to split the lines. If you plan to simply extrude shapes the entire height of the structure, you may prefer to not split them.

Understanding the GridSystem Output

The GridSystem creates a single feature in the FeatureManager with a number of derived sketches and planes, as shown in Figure 22.12.

FIGURE 22.12 Listing the GridSystem output

The additional features are listed as parents of the GridSystem, indented below it in the FeatureManager.

I already noted the derived sketches and planes, one each per level, created at the appropriate heights. A derived sketch is simply a parametric copy of the original sketch, placed on a different plane. If the original sketch changes, the derived copies also are updated. Derived sketches can be moved or rotated only. They cannot be edited; all changes must be performed at the parent sketch.

The 3D sketch in the FeatureManager contains lines forming the columns (Y-direction lines between the levels). This sketch is hidden by default.

You also may notice that the GridSystem uses transparent surfaces to represent interior and exterior walls. These are hidden by default. Depending on your structure, you may or may not have any use for information about walls, or you may care only about the exterior walls.

When you’re using the GridSystem, your interaction with surfaces is limited to showing and hiding them. You can use the Display pane or RMB menus to do this.

Viewing the Grid Components

If you right-click the GridSystem feature in the FeatureManager, you'll see a selection named View Grid Components. This is useful if you create a weldment from the grid and want to see a list of the features that comprise the grid itself, rather than all the weldment features. The View Grid Components dialog box is shown in Figure 22.13.

FIGURE 22.13 Isolating the grid components in a separate window

Transferring Data with the IFC File Type

IFC stands for Industry Foundation Classes, which was developed by the IAI (International Alliance for Interoperability) as an open data-exchange format. It's meant to be used to transfer data on building models between BIM (building information model) software packages. ArchiCAD and Revit are two examples of BIM modelers that might use this type of information.

The IFC file type includes geometry, but it also includes nongeometrical information about the function and occupant spaces within the building. You could think of this as the ability to transfer SolidWorks custom property information along with a STEP file transfer.

Although the use of SolidWorks in the AEC realm is limited, SolidWorks is firmly established in equipment design, which is closely related to the design of plants and industrial steel-framed structures.

To save a GridSystem as an IFC file, go to File ➢ Save As, and in the drop-down list, select the *.IFC file type.

You can also select the Options button in the Save As dialog box to set the units and OmniClass, as shown in Figure 22.14.

FIGURE 22.14 Saving data as an IFC file

The OmniClass classifications give you a detailed structure for classifying the data prior to importing it into a building model. Software such as SolidWorks would be useful for small components in buildings rather than for the building itself, but the equipment produced in SolidWorks could still be used in the BIM model. Air conditioning equipment, windows, plumbing, and other component hardware would be commonly created in SolidWorks.

If you want to learn more about the IFC standard, refer to the following website, which has a detailed description of the structure, purpose, and history of the file type:

http://www.aecbytes.com/feature/2004/IFC.html

The Bottom Line

SolidWorks has long been used for the design of equipment and components that go into buildings. With Large Scale Design, the software also works for the design of small plants and gridded structures. Walk-through capabilities give Large Scale Design users some animation capabilities, and the *.IFC export options allow users to share SolidWorks Large Scale Designs with other BIM software users.

• Master It Use Large Design Review to examine the dump truck.sldasm model that is included with the download materials for this chapter. Also open the same model in standard SolidWorks and familiarize yourself with the differences between the two.
• Master It Again, use the dump truck model to make a walk-through. Use either the manual controls or the 3D sketch path to direct the walk-through.
• Master It Start a new part and open a new GridSystem feature. Lay out a three-story structure to hold processing equipment, where the spacing between the first two floors is 10 feet and the spacing between Floors 2 and 3 is 12 feet.