IN THIS CHAPTER
Using the Hole Wizard
Understanding Toolbox
Tutorial: Gaining experience with the Hole Wizard and Toolbox
The Hole Wizard and Toolbox are two applications that go together because of the information they share; they both work from a single database of matching hole and screw sizes. One of the most useful examples of combining these two applications is the ability to automatically place holes through multiple parts and put appropriately sized screws and hardware into the holes, all in one step. The hole knows which fastener or stack of fasteners needs to go together.
This tool is called a wizard because it guides you through the process step by step. The process of creating a Hole Wizard hole can be summarized as follows:
Pre-select the face to put the holes on, although this is not required. This turns out to be an important issue that is related to the type of placement sketch, and I revisit this subject later.
Select the type of hole, for example, counterbored, countersunk, drilled hole, tapped hole, pipe tap, or legacy.
Set the standard to be used, such as ANSI inch, ANSI metric, or ISO.
Select the type of screw. For example, a counterbored hole can accommodate a socket head cap screw or a hex head screw, among others.
Select the size of the screw.
Select the fit of the screw into the hole, such as normal, loose, or tight.
Select the end condition of the hole.
Select options for clearance and countersinks or edge breaks.
Alternatively, you can use or assign a Favorite. A favorite is a hole with settings that you use frequently and want to save. These are discussed later in this chapter.
You can use Custom Sizing when you need a hole with non-standard dimensions.
Locate the center of the hole or holes. You can place multiple holes in a single Hole Wizard feature, even on different faces and curved faces. I address the specifics of this step later in this chapter.
Click OK to accept the type, size, and placement of the hole.
The Hole Wizard PropertyManager interface is shown in Figure 17.1.
Hole Wizard holes are made of two sketches: a center placement sketch and a revolved cut profile. Figure 17.2 shows a simple part with an expanded Hole Wizard feature. Notice that the feature is named for the size and type of the hole.
Note
Another useful aspect of naming the hole feature is that if you change the type or size through the Hole Wizard interface, the name changes to match.
If you create a Hole Wizard feature with more than one hole, there is still just a single revolved sketch. A multiple-hole Hole Wizard feature works similar to making a revolved cut and using a Sketch Driven feature pattern to create the multiple instances.
The placement sketch is listed first under the Hole Wizard feature. It has one or more sketch points marking the hole centers. It may also contain construction geometry with relations and dimensions to fully locate the hole centers. Placement sketches are discussed in more detail in the next section, 2D versus 3D placement sketches.
The revolve profile sketch is not on an identifiable sketch plane that you can reuse for other features, although that would be useful. You can change the sketch dimension outside of the wizard interface, and if you later use the wizard to edit it, then the changes appear in the Custom Sizing panel. Figure 17.3 shows the Custom Sizing panel with the changed counterbore diameter highlighted.
If you select any of the choices from the Options panel, then the revolved sketch profile is altered to accommodate the change. For example, the sketch changes to add a line for the countersink; a separate chamfer feature is not added.
Possibly one of the most difficult aspects of the Hole Wizard for new users to grasp is the use of 2D and 3D sketches to place the centers of the holes. There is a condition that is not immediately obvious, which is that if you preselect a flat face, then the placement sketch is 2D, and if you do not pre-select a flat face (meaning that if you just start the Hole Wizard without having selected a flat face), then the placement sketch is 3D.
The main advantages of the 2D sketch method are the simplicity and completeness of the available tools. Everyone knows how to manage 2D sketches, sketch planes, dimensions, and construction geometry. I have argued for years that the 2D placement sketch should be the default sketch used, because of its universal nature.
A limitation of the 2D sketch is that the holes that you create through this method are limited to a single planar face. Sometimes this creates a great limitation, while other times it does not matter.
The obvious advantage of the 3D placement sketch is that it can put a set of holes on any set of solid faces, regardless of whether they are non-parallel or even non-planar. This function offers multiple holes, multiple faces, and multiple directions. In situations where that is what you need, then nothing else will do.
A limitation of the 3D sketch is that if you have never used 3D sketches, they can be fairly cumbersome. Also, several relation types that are familiar in 2D sketches are not available in 3D sketches.
Dimensions work very differently in 3D sketches compared to 2D sketches. For example, to create and place a hole in a specific position on a cylinder, you need to follow these steps:
Begin with a circle with a diameter of one inch, drawn on the Top plane, and extruded using the Mid-plane option one inch.
Start the Hole Wizard without any preselection, either through the Features toolbar or by selecting Insert
Set the interface to use an ANSI inch, one-quarter-inch, counterbored hole for a socket head cap screw. Use Through All for the End Condition, and a Normal fit, with a .100-inch head clearance (in the Options panel), and no custom sizing changes. These settings are shown in Figure 17.4.
Click the Positions tab, which is located at the top of the PropertyManager window. The interface automatically changes to a 3D sketch with the Point tool turned on. This means that wherever you click, you create a point.
Note
Be careful about clicking when the Point tool is turned on. For example, if you click in a blank space, then the Point tool places a point off the part. SolidWorks will try to use the point later to create a hole in empty space, which usually causes an error.
Click the cylindrical surface of the part. The surface appears red when you move the cursor over it to indicate that an OnSurface sketch relation will be created between the sketch point and the cylindrical surface.
The hole should be positioned from one end of the cylinder. Using the SmartDimension tool, click one flat end face of the cylinder and the sketch point. Place the dimension and give it a value of .300 inches, as shown in Figure 17.5.
Locating the point angularly around the cylinder is more difficult. You can use several methods to do this, but this example shows one using construction sketch geometry.
Tip
To force a 3D dimension to have a certain orientation, dimension from a plane or planar face rather than from an edge, vertex, or sketch entity. A dimension from a plane is always measured in a direction perpendicular to the plane, but a dimension from a line or point is always measured by the shortest distance between the entities. Two-dimensional sketches can force dimensions to be horizontal or vertical, but 3D sketches cannot.
Warning
3D sketches have the ability to make planes within the sketch, without leaving the sketch environment. Planes that are made in this way cannot be referenced from outside the sketch, are not created using the same methods as regular planes, and do not follow documented techniques reliably. They have been removed from the SolidWorks Corporation training manual examples, and for this reason, I recommend finding other more reliable methods to do the same things.
With the Line tool activated while still in the 3D sketch, Ctrl-click the flat end face that the previous dimension referenced. This moves the red "space handle" origin to the selected face, and constrains any new sketch entities to that face. You are still in the 3D sketch, but are constrained to the selected plane, and still must play by all of the 3D sketch rules. The elements of 3D sketches are described in detail in Chapter 31.
Turn on the Temporary Axes view by selecting View
Place the cursor near the center of the activated end face; a small, black circle appears, indicating that the end point of the line will pick up a coincident relation to the temporary axis. Draw the line so that it picks up an AlongX sketch relation. The cursor shows the relations about to be applied, just like in a 2D sketch.
Draw a second line again from the center, but this time do not pick up any automatic relations. This line should also be on the flat end face.
Note
Although you can set these lines to display as construction lines if you like, this is not required in order for the feature to work; they also work as regular solid lines.
Put an angle dimension between the lines, and change the angle to 30 degrees. To be thorough (which is always recommended in 3D sketches, which have a tendency to handle underconstrained sketch geometry unpredictably), constrain the ends of the lines to the circular edge of the cylinder. At this point, the part looks like Figure 17.6.
Create an AlongY sketch relation between the points indicated in Figure 17.7. The hole centerpoint on the cylindrical face is one of the points, as well as the endpoint of the angled line. Change the angle dimension to ensure that it is controlling the sketch point as expected.
The finished part from this example is on the CD-ROM, and is called Chapter 17 3D Hole Placement.sldprt.
Hole Wizard Favorites store types of holes that you use frequently so that you can simply recall a favorite, rather than manually making all of the changes every time you use the same hole. Favorites are saved to a database named Default.mdb as you create them, and are immediately available from all other part documents. You can also save favorites to a special file type, with the extension *.sldhwfvt. You can then load these files and add them to other Default.mdb databases.
To create a Hole Wizard Favorite, set up a Hole Wizard hole as you normally would, and then use the Add Favorite button to add it to the Favorites database. The Hole Wizard Favorite panel contains five buttons:
You can use Hole Wizard Favorites to store custom holes. Create the hole with its custom sizes, and then add the favorite and give it a recognizable name. The custom hole will now be available to anyone who connects to the same database file.
The database file is typically found in the Data subdirectory of the SolidWorks installation directory, but an option in Tools
Further, the *.sldhwfvt files do not have an entry in the File Locations list, but seem to always default to the langenglish subdirectory of the SolidWorks installation directory. Neither this location nor the Data directory makes sharing among multiple users very convenient, but both file types can be copied to other installations.
Note
It is a best practice to create a folder for library type files that you want to save and use with a future version of SolidWorks. You can specify the locations for these files through Tools, Options, File Locations. I recommend a location such as D:Library. This moves the file off of the same drive as the operating system, in case you need to reformat, and it keeps it out of the Program Files area to prevent it from being lost or overwritten when SolidWorks is installed, uninstalled, upgraded, or changed in other ways. Even for files that need to remain in the SolidWorks installation directory (such as macros) it is best to also have these backed up in a library location.
Hole Wizard Favorites seem to have a couple of quirks that are possibly "sub-optimal," as they say. First, you can only see the favorites for a specific type of hole when that type of hole is activated in the interface. For example, if you have a number of favorites for countersunk holes, but you currently have the counterbored hole icon activated, then you will not be able to see the countersunk favorites until you switch to the countersunk icon.
If you have a lot of favorites, then this may be beneficial, but if you have only a few favorites, or you do not use favorites frequently, then it may be confusing, and can create some unnecessary steps to find all of your favorites.
A second quirk occurs when you allow SolidWorks to name the favorites and you have fractional values such as 1/4—which happens now and then in hole sizes—and then try to save the favorites. Each favorite is saved as a separate file, using the name that was automatically assigned to it by SolidWorks as the filename. Unfortunately, the character "/" is not allowed in a filename, and so it fails.
Fortunately, you can change favorites names by using the Add Or Update Favorites button on the Favorites panel of the Hole Wizard PropertyManager.
When saving Hole Wizard Favorites, SolidWorks has no way to establish a default folder for these files, although it seems to always go to the langenglish subdirectory of the SolidWorks installation directory. You need to determine a folder to put them into and load them from, and browse to that location every time, especially if you are using a shared network. Also, remember to copy any favorites files to a backup library location.
The Hole Series used to be part of the Hole Wizard, but has since been exported as a separate tool. It is now a four-step, wizard-based feature. Figure 17.8 shows the interface for the various steps.
Notice in the first panel that there is an option to add a Smart Fastener. The Toolbox feature, which I discuss in the next section, is required to be able to add Smart Fasteners.
When using the Hole Series feature, you must follow these basic steps:
Have an assembly open with two or more parts in it that need to be fastened together.
Initiate the Hole Series tool by selecting Insert
If the Hole Series is to be started from an existing hole, then select it in the Hole Position panel. If not, then use sketch points, construction geometry, dimensions, and sketch relations to locate the hole centerpoints.
Use the blue arrow at the top of the PropertyManager to advance from one panel to the next.
The Start Hole Specification is referring to the part where the series of holes starts.
The Middle Hole Specification is for all parts between the first part and the last part.
The End Hole Specification is the last part and is either a through clearance hole or a threaded hole.
The finished feature leaves an in-context feature in each part, with the Hole Series part in the assembly, as shown in Figure 17.9.
Warning
Improper installation, maintenance, or management of Toolbox can cause the loss of all useful information about fasteners and hardware in your assemblies.
Toolbox is an add-in that requires SolidWorks Office or higher, although you can also purchase it separately. In this book, I typically avoid talking about add-ins because the amount of material simply becomes overwhelming at a certain point; however, Toolbox is the cause of much consternation among users and CAD Administrators, and so it deserves some attention.
Toolbox is an application that creates fasteners and other hardware components, on the fly or reuses existing parts when possible. Technically, Toolbox is not a library, but a configurator. Libraries store existing components, while configurators build them on the fly from information supplied by the user.
One advantage of configurators is that the parts start out very compact because there is only the default size, and the sizes are efficiently stored in a database, and created as needed.
The advantage of a library is that it allows you to simply plug in the parts and they work. No mess, no fuss. This is not how Toolbox works, but it is good to remember the fact that what Toolbox really needs to do for users is provide a library of parts. Anything more than that is only beneficial if it offers some improvement over a simple library of existing parts without introducing any risks or setbacks.
Because Toolbox is not a library, and is not passive the way a library is, there is a component of it that is active. To make an analogy, no one asks how a staircase works, because it does not work, it simply exists, and people use it. An escalator, however, is a different issue. With an escalator, there is a complex installation, and then to operate it, you have to know how to get on and get off, and what to do if it stops working. The end results of using the staircase and using the escalator are the same (you start at the bottom and arrive at the top), but the complex automation is supposed to save you some effort.
That is one of the ways in which you can look at Toolbox. The end product is supposed to be the same as using a static library of parts, but there is some mechanism behind the scenes that has to be set up and maintained properly in order for it to work in the way you expect. Most SolidWorks books, tutorials, or training materials are going to ask you to accept what happens inside Toolbox as a "black box" and just assume that the end results are exactly what you need and intend. Here, I supply you with information about how it works, because it is important.
When Toolbox is installed, it starts as a set of SolidWorks parts with named features and dimensions, some suppressed features (depending on settings), some dlls (executable programs), and a database. The parts have a single Default configuration, which is typically one of the size extremities, either the largest or smallest. The database starts out about 65MB, and includes all of the size information for all of the parts, as well as all of the standards information.
If you create a custom standard in Toolbox, it actually replicates a section of the database. By doing this, the database file can easily double in size.
Later, you will see that a network installation of Toolbox requires the database to be on the network, and every time you create a new fastener, it has to open the database. As a result, simply placing a screw in an assembly can mean that even if your assembly is located on your local hard drive, you still have to open a very large database file across the network. The first rule about performance with SolidWorks is to work locally rather than across a network.
By default, the database is located at C:Program FilesCommon FilesSolidWorks DataBrowserlangEnglishSWBrowser.mdb. You can open this file with Microsoft Access or Excel.
Note
When specifying network paths, it is best to specify a universal naming convention, or UNC, path rather than a mapped address. A UNC address follows the format, \ServerShared Folder. The advantage of the UNC over the mapped drive is that mapped drives do not always connect immediately, but the UNC should be able to find its link as long as the network is working. Also, mapped drives can vary from one computer to another, but the UNC is always the same.
If you have just installed Toolbox the way that most, if not all, new users do, then you will accept all defaults, and trust the software that you just purchased to not give you bad advice. In this situation, the database is installed locally and Toolbox is set to use configurations for sizes.
When you put a Toolbox part into an assembly, you do not even notice anything other than the part going into the assembly, although it may hesitate while the large database is opened. If you check the part configurations, you may notice that there is a Default config and a new one that represents the size that you just created. Every new size that you create makes another new configuration. Figure 17.10 shows a Toolbox part with the FeatureManager and ConfigurationManager open.
Next, you may receive an assembly from a client. Often, because Toolbox parts are located in an area where you would not necessarily look for parts, users send assemblies and parts, but do not send Toolbox parts. You may think that this is okay; after all, you have Toolbox on your system, and so it should pick up your toolbox parts. The truth is that when receiving an assembly from someone else, you are better off if one of the parties does not have Toolbox on their system. Here's why:
If both you and the client who sent the assembly have Toolbox, then you should be okay, right? Well, yes and no. Yes, your client's assembly will pick up your Toolbox parts, but no, it will not work properly because you do not have all of the same configurations and sizes that your client has. In cases like this, you will experience what I have come to refer to as the Huge Screws syndrome. When SolidWorks finds the right file but cannot find the right configuration, it uses another configuration, usually the Default, which is generally the biggest size. This is where the Huge Screws name came from.
Part of the really bad news is that if you save your assembly with the Huge Screws, SolidWorks has no way of knowing that the huge screws are not the correct screws, and the problem can be solved only by manually going through the assembly and reassigning sizes to the huge screws.
You can work around this by opening an assembly that has not yet been saved with the Huge Screws, by using the Advanced option in the Open dialog box, and selecting the New Configuration Showing Assembly Structure Only option. With this option, all components are suppressed. You can unsuppress any non-Toolbox parts and continue working. Ask your client to send you his Toolbox parts and then unsuppress those parts in the assembly, making sure that it finds the right parts, which is probably best done by having the correct parts already open before you open the assembly. These options are shown in Figure 17.11.
If you replace your Toolbox parts with the Toolbox parts from the client, then you may experience the same problem in reverse if you had configs that your client did not. In the end, it would be great to be able to merge the two parts to combine all of the available sizes into a single file. There is a way of doing that, which I will describe later. Files that have the same names and different content are at the top of the list of things you shouldn't do in file management, and yet the SolidWorks Toolbox system frequently creates this very situation.
To be fair, SolidWorks has fixed the Huge Screws problem in the 2007 version, by coming up with a clever method for figuring out which size is missing and building it on the fly when the assembly is opened. Additional information about the Toolbox parts is now stored in the assembly, which helps identify the missing parts. Unfortunately, the fix only works for assemblies that use the parts from the new 2007 library and assemblies that have been built in SolidWorks 2007. To sum up, if you have assemblies built in an older version of SolidWorks, and your Toolbox library becomes corrupted or lost, or you are sent an assembly that uses a different Toolbox library, even if you are working in SolidWorks 2007, you cannot benefit from this fix.
This is disappointing in many respects because anyone who has existing Huge Screws problems will continue to have them until they rebuild the assembly or manually repair the configurations. It is doubly disappointing because the information needed to recreate the correct configuration has always been stored in the assembly—the filename and the configuration name are enough—but SolidWorks has missed an opportunity to really fix this problem.
Before the Summary at the end of this chapter, I have some recommendations if you are still interested in using Toolbox.
Toolbox parts can be organized in a number of ways. The raw parts are organized as follows:
Standard and Units (for example, ANSI Inch or ANSI Metric; most standards do not include multiple units, they assume metric).
Hardware Type (such as bearings, bolts, and bushings).
Each type is organized differently, but bolts and screws are organized by drive or head type (for example, you have socket head screws, hex head, and thumb screws).
Filenames look like Socket Button Head Cap Screw_AI.SLDPRT, where the "AI" represents ANSI Inch.
Figure 17.12 shows this organization in part.
By now you are probably unsure about the use of configurations in general. If so, that is not the impression I am trying to convey. Configurations in themselves are not the problem; the problem here is in the file management practice of having files with the same names but different content. Mixing that with the practice of trying to treat "configurator" software like a "library" exacerbates the problem.
That said, you have two options regarding how you create different sizes. The default option is that sizes are created as configurations within a single part. The other option is that sizes are created as individual files.
The best time to make this choice is before you install SolidWorks. Unfortunately, before you install SolidWorks, you probably do not have any idea that these issues exist. The reason for making this decision not just early, but immediately, is that if you start using the default setting (configurations), and make a few configurations for some parts, and then switch to using the Save Parts setting, the parts that are saved out will all have the pre-existing configurations, and thus different sizes.
If you find yourself in this situation, it is better to reinstall Toolbox, or simply to copy over a new default library with no configurations.
You can access the option to either Create Configurations or Create Parts by selecting Toolbox
The following list contains some pros and cons of each option.
Configurations are better for:
Controlling data across several sizes. For example, a design table can drive custom properties that are added to all configurations. Doing this with many individual parts would be very messy.
The interface to select configurations from a list is easier to work with than the interface to select a part from a list.
File management organization is somewhat easier for configured parts.
Separate parts are better for:
Keeping the file size small.
Replacing all of one size part with another.
A guarantee that you will never have the Huge Screws problem.
Maybe your company uses screws of different materials or finishes in your products. Toolbox, in its default arrangement, does not have an option to deal with this directly. If you ask a tech support person whether materials and custom part numbers can be used in SolidWorks, they will tell you "of course, simply enter in the desired quantity when making the part." The implication here is that you do them one at a time, and that whoever creates the part uses the same syntax as everyone else.
Figure 17.14 shows the PropertyManager interface for adding a Toolbox part to an assembly. You can access this interface by dragging a Toolbox part from the Design Library window into the assembly graphics window. The materials assignment is usually intended to be done as part of the Description. You can access this interface and the Part Number fields through the Add Favorite button in the upper-left corner of the Favorites panel.
The way that SolidWorks expects you to work with materials and custom part numbers is simply not practical unless you have one person doing all of the work, and you do not have many parts to create. SolidWorks does not provide any direct way to mass-populate data of this type.
One method to work around the lack of a mass-population tool is to first create all of the sizes for a part using configurations. Then auto-create a design table and you can use Excel techniques to build descriptions, custom part numbers, materials, and whatever custom property you want to have.
Another method to do this is to create a custom standard for materials. A custom standard essentially copies a high level in the database such as ANSI Inch. You can specify a name such as Company X Stainless Hardware, or Company X Black Oxide Hardware.
I have already mentioned that adding custom standards greatly increases the size of the database, and contributes to the delay in adding the Toolbox parts to an assembly. If this is not a handicap for you—and you should at least try it—then it may be a more viable way to incorporate materials and finishes.
There are a few ways in which you can make Toolbox work the way it is intended to. The most reliable way is to remove your computer from the network, and to not bring in any assemblies from external sources that were created referencing Toolbox parts. That sounds like an extreme measure, but it is necessary, as Toolbox's weaknesses come from sharing Toolbox data.
Unfortunately, most SolidWorks users do not have this luxury. They generally share files with other users across a network, in a PDM system, or across the Internet through FTP, e-mail, or VPN. If each user has their own Toolbox installation locally, as happens with the default installation, then you could run into the same problems as described above when receiving an outside client's files. As a result, you must somehow share Toolbox.
Keep thinking to yourself "Toolbox is just a library, Toolbox is just a library . . ."
You can share Toolbox by redirecting the Common Files part of the SolidWorks installation to a shared network location. This part of the installation is shown in Figure 17.15.
This is fine for the first installation, but for any installation where a version of the software already exists on your computer, the shared files also already exist. There is no installation option to accommodate this situation, and so you have to either install over the shared documents or install to a dummy location and redirect SolidWorks to the shared files manually. You have to go through this installation, even the dummy installation, because it is installing the application part of Toolbox. Remember that a Toolbox installation has three components: the empty default library part files, the database with all of the information in it that is used to populate the library, and the application dlls that make everything work.
This is particularly important to pay attention to if the library has been changed. If you overwrite the database, that is not really important unless, for example, standards have been changed, or custom properties added. However, if the library has been changed (for example, by adding configurations) and a later installation overwrites it, then you can cause yourself or someone else a lot of difficulties.
For this reason, you need to know how to manually redirect Toolbox to a different location. A file called Toolbox.ini is located in the Toolbox subdirectory of the SolidWorks installation directory, as shown in Figure 17.16.
When you edit this file with a text editor such as Notepad, the file contains the path of the SolidWorks Data folder. The database that controls both Toolbox and the Hole Wizard is located in the langEnglish (or appropriate language) folder, and is called SWBrowser.mdb. The Toolbox library parts are in the rowser folder, under the appropriate folders, as displayed in the Design Library. Figure 17.17 shows the Toolbox.ini file open in Notepad.
If you have only one user, you can do what you like—even use the default installation—and Toolbox should work for you. If, however, you are administering an installation with more than one user, you need to be informed of the issues involving setting up and using Toolbox mentioned above, and a few more mentioned below.
If a Toolbox is shared, is it possible that multiple people can access the same files at the same time? This is one of the most frequently asked questions about Toolbox administration. If two people need to write to a file at the same time, then that can cause problems. In order to remedy this, SolidWorks plays referee between multiple users who are accessing the same Toolbox files.
You need to apply the following settings to share Toolbox files on a network:
Toolbox
The Windows users should have full permissions to access the SolidWorks Data directory, and the SolidWorks DataBrowser directory should be set to Read-only for all users.
It is time to upgrade. You have your SolidWorks 2007 disks, and SolidWorks 2006 is installed. You can now go ahead and install SolidWorks 2007, but when it comes to the part in the installation shown in Figure 17.15, take notice again of what you are doing. The installation may default to the SolidWorks 2006 Toolbox location. If you overwrite this location, then you will not be able to use Toolbox with SolidWorks 2006 (because the library will be a future version). If you intend to use multiple versions, then you also need to maintain multiple Toolbox installations.
You should also consider what would happen if you make a mistake and completely overwrite the SolidWorks 2006 library that contains all of the configuration data that you have worked hard to create. When upgrading, you do not want to overwrite your existing library. The following is a set of steps to help you upgrade safely and effectively:
Install the new version with Toolbox in a new location, for example SolidWorks 2007 Data or a directory name that helps to distinguish this library from another.
Copy the old SolidWorks 2006 data (containing the correct configurations) over the top of the new SolidWorks 2007 data.
Browse to the Toolboxdata utilities subdirectory of the SolidWorks installation directory and run UpdateBrowserData.exe. The interface for this program is shown in Figure 17.18.
Select the Updating Database field and use the ellipsis button to browse to Toolboxdata utilitieslangEnglishupdatedb.mdb in the SolidWorks installation directory.
Select the Database To Update field and browse to SWBrowser.mdb. You can find this file by following the ToolboxPartFolder path in the Toolbox.ini file, and looking in the langenglish subdirectory.
Click Update.
This prevents you from overwriting your old version, while still copying the old version to the new installation and avoiding the Huge Screws syndrome.
If you have been using SolidWorks and Toolbox for a few releases, then you may recall that Toolbox had a function called the Add My Parts Wizard, which added user-created parts to the Toolbox libraries. The parts were limited in that you could not use them with Smart Fasteners, but the interface would work if the part had configurations.
In SolidWorks 2007, the Add My Parts Wizard has been removed. However, you can still add your own parts to Toolbox by simply dragging-and-dropping them. Drag-and-drop is available in third-level folders. Levels are counted from the Standard folder, which is level 1.
You can add folders to Toolbox through the RMB menu. Just RMB click a first- or second-level folder, and select New Folder. You can create a new level-1 folder by RMB clicking the Toolbox icon, as shown in Figure 17.19.
You can merge Toolbox libraries by simply copying or moving one folder in with the existing library folders. Another type of merging may be less successful. If you have two Toolbox parts from different sources and they have different sets of size configurations, these are things you may want to merge to get the benefits of both sets of sizes.
Unfortunately, there is no direct way of doing this in Toolbox. The best way would be to auto-create design tables in both parts, and then to copy the configurations from one design table to the other design table. This should effectively copy configurations between parts, although you may need to remove any duplicate configuration rows.
This topic could be a chapter on its own, but I will not delve too deeply into it here because it goes beyond the intended scope of this book. A discussion of Toolbox requires some mention of how it may be used in conjunction with a PDM product.
Toolbox and PDMWorks Workgroup, or any other PDM product for that matter, can be a challenge to combine. Generally, it is useful to be able to see the fasteners in PDM because of the BOM capabilities, quantities, Where Used options, and complete searches. Some users choose not to put library parts in the vault because they are not revision-managed documents. All the same, revision management is not the only reason to put items in the vault.
Looking at it from the Toolbox point of view, Toolbox cannot work with its parts in the vault, and if changes were allowed to the parts (sizes add configurations), then you would need to check in the part every time you added a size. This is not necessarily a problem, but it does become awkward.
Some PDM products allow files to exist outside the vault, while pointers to the files exist within the vault. This is one very good option for using Toolbox with a PDM product.
Another good option is to simply use the Create Parts setting. This creates individual files that are easier to manage. It may also be important for a different reason: some PDM products, such as PDMWorks Workgroup, do not distinguish configurations as separate controllable or separately identifiable documents.
You can find Toolbox settings in the Toolbox menu, by selecting the Configure option. The Configure Data dialog box has four tabs: Content, Settings, Properties, and Smart Fasteners.
The Content tab shows all of the standards. If you are not using certain standards, then you can turn them off by deselecting their check mark. You can do the same for folders and even specific parts within the standard. If you have added folders or custom parts in the Design Library window, they appear here.
As you expand the standard, and then the fastener type and the specific head types, you can select individual parts. The Countersunk Bolt is selected in the list shown in Figure 17.20.
Several tabs contain different types of information for Toolbox parts:
You can use the General tab to offer alternate filenames.
You can use the Size tab to disable specific sizes.
The Finish tab is not available for all fasteners, but you can use it to remove parts of the description.
You can use the Length tab to limit the available lengths.
You can use the Thread Display tab to limit the available thread types. Available thread types are shown in Figure 17.21.
The All Configurations tab enables you to create all of the configurations that are available for a particular Toolbox part. It will also export the database data to an Excel spreadsheet, and import a spreadsheet that is created in this way.
Creating all of the configurations for a single part can take a couple of hours, and in the few times I have done it, I have never seen the SolidWorks interface recover from starting the command, although it seems to finish. Having all of the configurations is very useful, especially if you are being plagued by the Huge Screws.
The Settings tab is where you can set the config and part options. If you choose to create parts, then you also need to specify a location for the parts to be kept. If you choose a network location, it is best to use the UNC path, rather than a mapped drive because mapped drives may not reconnect on start up and may be mapped to different letters from computer to computer, but the UNC always points to the same location from any point on the network.
The Settings tab also enables the Administrator to establish a password for Toolbox data configuration changes. The Settings tab is shown in Figure 17.22.
The Properties tab enables you to set up properties that appear in the PropertyManager. For example, you can enable fill-in or drop-down lists for values. Properties can be enabled for specific items, as shown in Figure 17.23.
The Smart Fasteners tab controls Smart Fasteners, which are discussed later in this chapter. The tab is shown in Figure 17.24. As an example of the types of settings you can use here, you can control which screw types are used with which types of Hole Wizard or non-Hole Wizard holes.
Up to now in this chapter, we have looked at Toolbox mainly from the administrative point of view; now, we will look at it from the user's point of view. Toolbox has two components: Toolbox and Toolbox Browser. In practice, the Toolbox component is actually ignored, and the Toolbox Browser component is generally referred to as Toolbox.
The Toolbox Browser is the Task pane interface, and is found on the Design Library tab, as shown in the image to the left in Figure 17.25. The Toolbox component is found in the Toolbox drop-down menu. It includes structural steel shapes, grooves, cams, and beam and bearing calculators.
You can turn on Toolbox and the Toolbox Browser through the Tools, Add-Ins dialog box. The column of check boxes on the left indicates that the add-in will be active for the current session of SolidWorks only. The column of check boxes on the right indicates that the add-in will be active every time the software starts up, as shown in Figure 17.26.
Once the Toolbox Browser is turned on, you can use it by expanding the Task pane at the right of the SolidWorks graphics window and clicking the Design Library, which looks like a stack of books. In this panel, you will see the Toolbox screw symbol. Expand icons until you find the fastener or other hardware that you are looking for, and then drag the part into the assembly.
Holes can be populated in several ways, such as dragging-and-dropping, populating multiple holes at once, and using feature-driven component patterns. I discuss manual and patterning options here, and Smart Fasteners in the next section.
The simplest way to bring Toolbox parts into an assembly is to drag-and-drop them. Position the part that the fastener goes into so that you can see the edge of the hole where the screw head will go. Then browse to the correct fastener, and drop the fastener onto the edge, as shown in Figure 17.27.
Because of the use of Mate References in Toolbox parts, they know that they are supposed to snap into holes on flat faces. When dropping the fastener into the hole, the Smart Mate icon momentarily appears. A Smart Mate of this sort applies two mates, one that is concentric between cylindrical faces, and one that is coincident between two flat faces.
Figure 17.28 shows the progression from a plate with holes in an assembly. In this example, you would select the edges of the holes, then select a fastener, and then choose Insert Into Assembly from the RMB menu, to fully populate the part.
Chapter 15 discussed Feature Driven component patterns (also known as derived patterns), where a pattern of parts in an assembly is driven by a feature pattern in a part. You can find this assembly feature in the assembly menus under Insert
One way to use Smart Fasteners is in conjunction with Hole Wizard Hole Series. Hole Series creates the holes through multiple parts at once, creating the appropriate type of hole through each part, and then Smart Fasteners automatically places fasteners in the holes, even including nuts and washers. To do this, you can select the option on the first panel of the Hole Series PropertyManager interface, as shown in Figure 17.29. If you are planning on using Smart Fasteners, using them in conjunction with the Hole Series is your best bet, using them in conjunction with the Hole Series holes.
The Smart Fasteners with Hole Series is a function that you should be careful when using. It is very effective, but it may cost you some performance (speed). The Hole Series is an Assembly Feature (sketch) that drives several in-context features (holes), and then parts are mated to those in-context features (fasteners).
Smart Fasteners functionality also has an automatic component. Once an assembly has parts mated into place, you can place fasteners into parts with appropriate holes by face, by part, or for the entire assembly at once.
Warning
You may not want to spend a lot of time trying to use this type of the Smart Fasteners functionality. I have tried to find examples where Smart Fasteners works well and predictably, but to no avail. I have searched through training examples, tutorial files from SolidWorks, and I have even made some of my own example files. I have looked for presentations from user groups and SolidWorks World that use Smart Fasteners, but no one appears to be talking about this functionality. Although in theory, it offers interesting functionality, in reality, it receives very little attention—definitely a warning sign.
The one assembly that I did find where Smart Fasteners worked surprisingly well (in fact, almost perfectly) was from the sample files that installed with SolidWorks. Upon closer examination, the reason this worked well was because it used assembly features for the holes, and so the holes did not appear in the individual parts. If that is the price that you have to pay just to get fasteners to populate automatically, then I would rather put them all in manually.
Smart Fasteners have some documented limitations where you should not expect them to work:
Holes in single parts
Holes created by extruding a nested loop
A mirrored hole or cut features
Holes in mirrored, imported, or derived parts
Misaligned holes
Holes with a large difference in diameter
Holes with large gaps between them (a large gap in the axial direction)
Holes made using different techniques (such as sketch pattern versus feature pattern)
If you would like to try out Smart Fasteners, then you can use the assembly included on the CD-ROM called Chapter 17 Smart Fasteners.sldasm. In this assembly, half of the holes are done correctly, and in the other half, the screws are put in either backwards or head-first. The documented method for flipping the fasteners is to expand the Smart Fastener, RMB click the series, and select Flip. In this case, my attempts resulted in success about half of time, which was somewhat higher than my attempts with other assemblies. In some cases, screws were put in the ends of shafts without holes, on filleted edges, and unfortunately missed most of the places that I did want the screws to go.
Assembly FeatureManagers are hard enough to manage when they become full of parts; they become even more unmanageable when they also need to include the many types of fastener parts. As a result, I recommend that fasteners, as well as any other type of part that is found in large quantity in the assembly, be organized into folders, as shown in Figure 17.30. You should also group parts of the same size or function together.
After spending almost an entire chapter saying what you should not do, it is finally time to say what you should do. Toolbox can be downright dangerous if you install and use it improperly; however, the following recommendations work in most situations.
If you are a single user who does not share files over a network with other users, then installing SolidWorks and Toolbox with the default settings should work for you. This appears to be the arrangement that the developers had in mind when they programmed the tool, because it is the only scenario in which it works as expected.
Be careful if you ever receive an assembly from another Toolbox user, because this is the one situation that can cause immediate trouble. If they also send their Toolbox parts, then I recommend that you open all of their Toolbox parts before you open their assembly, so that the assembly is certain to access their Toolbox parts instead of yours.
If you need to include materials and mass-populate custom properties, then I recommend that you go through the exercise of building all of the configurations of all of the parts, and then use an auto-created design table to drive the properties.
If you have more than one user, then this technique will not work for you, unless both users work independently from one another.
If you have multiple users that share assemblies, then you need to also share the Toolbox library. If you share assemblies only among yourselves, meaning only with other users who are also sharing Toolbox, then sharing Toolbox should be good enough. However, if you share assemblies with Toolbox users who do not share your Toolbox library, then you should probably go through the exercise of populating all of your parts with all of the available configurations. Setting your library to use the Create Parts setting cannot help you to avoid the Huge Screws problem when you receive an assembly from outside your group. If the originator has used parts with configurations, then you must also use configurations.
If you do not receive assemblies from outside of your group with Toolbox parts in the assembly and you have network performance problems, then it may be a good idea to install Toolbox locally, but to set it to use the Create Parts setting, where the parts are on a shared network location.
If you use a PDM system, then I would definitely install Toolbox locally, and use the Create Parts setting. The sharing occurs through the PDM system.
The least problematic technique is to turn Toolbox off altogether and either buy or make your own library of static parts. You can then distribute these files internally in your organization, as well as to any other people upstream or downstream from you who also share files with you. You can build this type of library by using Toolbox's config population tool; materials or other custom properties are then dealt with the way you want, probably using auto-created design tables.
Figure 17.31 shows a section view of the assembly used for this tutorial. Notice that there is a gasket under the Sensor part.
This tutorial assumes that you have a working copy of Toolbox running on your computer. If you do not have Toolbox, then you can proceed to the next chapter. This tutorial also assumes that your Toolbox is using the default Create Configurations setting, although it can also work with the Create Parts setting. To get some experience using this tool, follow these steps:
Open the assembly from the CD-ROM called Chapter 17 Tutorial.sldasm.
Make sure that the Toolbox Browser is turned on by selecting Tools
Expand the Task pane, found on the right side of the graphics window, and display the Design Library panel, which contains the Toolbox icon. Expand the ANSI Inch standard, and the Bolts and Screws folder, and finally click the Hex Head bolt, as shown in Figure 17.32 on the left. Drag-and-drop the hex head bolt into the indicated hole. It snaps into place because of the Mate Reference that is used on the Toolbox part. Use the settings shown in the PropertyManager to size the bolt.
Note
The Vendor text box that displays in the PropertyManager above will not be available to you unless you have customized the Properties tab in the Configure Data Settings dialog box.
Add a flat washer and nut to the bolt, as shown below in Figure 17.33. The washer is Plain Washer Type A, Preferred - Wide Flat Washer.
The nut used is Hex Nut, Heavy Hex Nut.
Notice that the bolt is too short, as shown in Figure 17.34. RMB click the bolt, either in the graphics window or in the FeatureManager, and select Edit Toolbox Definition, toward the bottom of the menu. Change the length of the fastener to 1.625 inches.
Tip
Use the Dynamic Preview option at the bottom of the Toolbox PropertyManager. After you select a new size, the bolt in the graphics window immediately updates to reflect the new size.
Tip
The selection of which hole the first fastener was positioned in could be arbitrary on this assembly because it uses a circular pattern, but if it had been a rectangular pattern, then the order would have mattered. When preparing to use a Feature Driven component pattern, it is important to put the components in the seed feature (the original feature that the pattern was created from).
Note
If you try to apply Smart Fasteners to the hole, then you will notice that the fastener is placed incorrectly. This is another situation where Smart Fasteners are a problem.
Create a Feature Driven component pattern (Insert
Zoom in on the sensor on the top of the assembly. There is a gray gasket between the orange sensor and the blue top parts. Click one of the flat ends of the sensor part and then click the Hole Series toolbar button, or select Insert
Tip
Remember that the pre-selection of a flat face is important so that you can use a 2D placement sketch, rather than a 3D placement sketch.
Make sure that you select the Add Smart Fastener option, as well as the Create New Hole option.
Make three sketch points and use construction geometry and dimensions to locate the holes, as shown in Figure 17.35. The size and types of holes are determined in a later step. (This is from the reverse of the normal Hole Wizard, where you first determine the type and size of hole, and then you establish the positions.)
Click the Next button (the blue arrow pointing right) to move to the First Part hole specification. Set it to a counterbored hole, for a #10 binding head screw, with a head clearance of .025 inches, as shown in Figure 17.36 in the image to the left. Click the Next button to advance to the Middle Parts hole sizing.
In the Middle Parts PropertyManager, make sure that the Auto Size Based On Start Hole option is on, as shown in Figure 17.36 in the middle image. This creates a normal fit clearance hole for the gasket part. Click Next to advance to the hole definition for the Last Part.
In the End Hole Specification panel, make sure that you select the Hole rather than the Tap option, as well as the Auto Size Based on Start Hole option. This is shown to the right in Figure 17.36. When this step is complete, click the OK button (the green check mark icon).
Note
The interface here looks unfinished. Notice that the Fit text box is available for the End Hole, even if you use the Auto Size Based on Start Hole option, but it was not available for the Middle Part. Also notice the lack of drop-down arrows for the Fit and Size text boxes.
The Smart Fasteners PropertyManager appears. Expand the Binding Head Screw header in the Fasteners panel, and notice the warning icon on Series1, as shown in Figure 17.37. When you click this warning icon, a message displays in the Information panel at the top of the PropertyManager window. This particular flag suggests that there may be an interference; however, there is no interference. This warning disappears when the feature is finished.
Add a washer and a nut to the bottom stack of the binding head screws. This is easy to do, and almost makes up for the rest of the Smart Fasteners shortcomings. To do this, RMB click the Bottom Stack entry at the bottom of the Fasteners panel and select the Bottom Stack option that pops up.
A dialog box appears, enabling you to add a washer and a nut, as shown in Figure 17.38. You may want to roll the model over so that you can see the components being added to the underside of the screw. You can add other properties to the parts using the Properties button. Notice that the screw has been lengthened to accommodate the added components.
Note
If you add a washer to the top stack, the hole does not automatically become larger, and it may cause an interference. Be careful about your choice of top-stack washers.
Note
You may have noticed that this time, Smart Fasteners worked almost flawlessly and certainly saved you some time. Although this tool is not applicable to other purposes, when used with the Hole Series, it is quite useful.
You may want to group the fasteners and even the fasteners' mates into folders, as shown in Figure 17.39.
Warning
The version of the assembly labeled Finished on the CD-ROM may open up on your computer with Huge Screws if you open it before completing the tutorial. This is because the configurations used in the assembly are on my computer. Although you have the same parts, before doing this tutorial, you may not have the same configurations, and so they cannot be found and come in Huge instead. This was intentional; it is a practical reminder of this problem and how easily it can happen to you. If you are using SolidWorks 2007, you should be able to tell Toolbox to simply recreate the sizes and continue on. If the assembly provided on the CD-ROM had been made prior to SolidWorks 2007, that option would not exist.
The Hole Wizard can make holes based on 2D or 3D sketches. The type of hole that you create depends on whether or not you have pre-selected a flat face before clicking the Hole Wizard tool. Two-dimensional sketches are far easier to use than 3D sketches.
I have met people who claim to have had good success with Toolbox even in a shared environment, but since the problems with the tool are so easy to demonstrate, these people are either extremely disciplined or extremely lucky. For all users except those who work alone and do not share files with other Toolbox users, Toolbox can cause a number of major problems. You can develop techniques to prevent you from experiencing Huge Screws, for example, either not sharing assemblies with other Toolbox users or pre-populating all of your configurable parts with all possible configurations. Further, Smart Fasteners that you use in conjunction with Hole Series violate any best practice guidelines that you could name when it comes to assembly performance and circular references; however, if you can work with that, then it is a really sophisticated technique.