Wiley SolidWorks 2009 Bible Part 6 ppt

Features such as fillets, shell, and draft by design require selections from solid geometry, but other features, such as any feature created from sketches, could be made with only refere

If two adjacent features are to swap places, it generally does not matter whether you move one ture up the design tree or you move the other one down However, there are isolated situations

fea-that are usually created by the nested, absorbed features discussed earlier, where one feature

can-not go in one direction, but the other feature can go in the opposite direction, achieving the exact same result If you run into a situation where you cannot reorder a feature in one direction even

though it appears you should be able to, try moving another feature the other direction

Reordering Folders

There are times when, regardless of which features you choose to move and of which direction you choose to move them in, you are faced with the task of moving many features This can be time-

consuming and tedious, not to mention have the potential to introduce errors To simplify this

pro-cess, you can put all of the features to be moved into a single folder, and then reorder the folder

Keep in mind that the items in the folder need to be a continuous list (you cannot skip features), and you can only reorder the folder if each individual feature within the folder can be reordered

BEST PRACTICE

BEST PRACTICE Folders are frequently used for groups of features that go together and that may be suppressed or unsuppressed in groups You can also use folders in assemblies

Folders are frequently used for the mass of cosmetic fillet features that are often found at the

end of design trees for plastic parts or for groups of hole features.

To create a folder, right-click a feature or a selected group of features and select Add to New

Folder Folders should be renamed to have a name that helps identify their contents You can der folders in the same way as individual features When you delete a folder, the contents are

reor-removed from the folder; they are not deleted

You can add or remove features to or from the folders by dragging them in or out If a folder is the last item in the FeatureManager, the next feature that is created is not put into the folder; you must place it in the folder manually You cannot drag features out of a folder and place them immedi-

ately after it, because they will just go back into the folder If you want to pull a feature out of a

folder and place it after the folder, there must be another feature between the feature that you are

moving and the folder However, you can pull a feature out of the folder and place it just before the

folder

Using the Flyout FeatureManager

The Flyout FeatureManager resides at the top-left corner of the graphics window, and was

intro-duced when SolidWorks began to consolidate floating dialog boxes into the PropertyManager dow The PropertyManager goes in the same space as the FeatureManager, and is sometimes too

win-big to allow this area to accommodate both managers in a split window

You can use the Flyout FeatureManager in parts or in the assembly However, you cannot use the Flyout FeatureManager to suppress or rollback the tree.

CROSS-REF Other functionality and limitations of the Flyout FeatureManager that relate to its function in assemblies can be found in Chapters 12 to 15.

You can access the settings for the Flyout FeatureManager at Tools ➪ Options ➪ FeatureManager ➪ Use Transparent Flyout FeatureManager in Parts/Assemblies

You may prefer not to work with the flyout FeatureManager If this is the case, you can use the detachable PropertyManager instead Detaching the PropertyManager removes the need for the fly-out I often dock the detachable PropertyManager where the flyout FeatureManager would go The main advantage of using the detachable PropertyManager instead of the flyout FeatureManager is that with the detachable PropertyManager you don’t have to locate features in the FeatureManager that were already in view

Figure 11.6 shows the difference between the flyout FeatureManager on the left, and the able PropertyManager on the right My preference is clearly the detachable PropertyManager When you use this, everything is predictable, and you don’t have to go hunting for features that were listed right in front of you when you do something that opens a PropertyManager I usually decrease the overall size of the SolidWorks application window, and place the PropertyManager to the left of the SolidWorks application This works best on a wide aspect monitor If you use a small monitor or a normal aspect monitor, using the Auto Collapse option with the PropertyManager docked to the right of the FeatureManager (where the flyout FeatureManager would otherwise go)

detach-is also a good option

You may correctly ask “what’s the difference?” The difference is that when you do something like editing a sketch plane, the current state of the FeatureManager is covered over and replaced by the PropertyManager You may have had the new plane you wanted to use in view Especially with long FeatureManagers, in both parts and assemblies, when the flyout appears, you have to again scroll to find the plane that was right in view This has been a problem since SolidWorks started employing the PropertyManager many releases ago However you use the detachable

PropertyManager, I think you will find it an improvement over the flyout

FIGURE 11.6

Comparing the flyout FeatureManager with the detachable PropertyManager

Summarizing Part Modeling Best Practice

This section is a summary of best practice suggestions for modeling parts Best practice lists are

important because they lay the groundwork for conservative usage of the software, which is helpful for new users and users who are trying to experiment with the limits of the software

I believe that it is only after you respect the rules and understand why they are so important, that you know enough to break them However, best practice lists should not be taken too seriously

They are not inflexible rules, but conservative starting places; they are concepts that you can

default to, but that can be broken if you have good reason

n Learn to sketch using automatic relations.

n Use fully dimensioned sketches when possible Splines are often impractical to fully dimension

n Limit your use of the Fixed constraint

n When possible, make relations to sketches or stable reference geometry, such as the Origin or standard planes, instead of edges or faces Sketches are far more stable than faces, edges, or model vertices, which change their internal ID at the slightest change and may disappear entirely with fillets, chamfers, split lines, and so on

n Do not dimension to edges created by fillets or other cosmetic or temporary features

n Apply names to features, sketches, and dimensions that help to make their function clear

n When possible, use feature fillets and feature patterns rather than sketch fillets and sketch patterns

n Combine fillets into as few fillet features as possible; this also allows you to control fillets that need to be controlled separately, such as fillets to be removed for Finite Element Analysis (FEA), drawings, and simplified configurations; or added for rendering

n Create a simplified configuration when building very complex parts or working with large assemblies

n Model with symmetry in mind Use feature patterns when possible

n Use link values or global variables to control commonly used dimensions

n Do not be afraid of configurations Control them with design tables where there are more than a few configs, and document any custom programming or automated features in the spreadsheet

n Use display states when possible instead of configurations

n Use multi-body modeling for various techniques within parts; it is not intended as a means to create assemblies within a single part file

n Cosmetic features — fillets, in particular — should be saved for the bottom of the design tree It is also a good idea to put them all together into a folder

n Use the setting at Tools ➪ Options ➪ Performance ➪ Verification on rebuild in tion with the Ctrl+Q command to check models periodically and before calling them

combina-“done.” The more complex the model, or the more questionable some of the geometry or techniques might be, the more important it is to check the part

n Always fix errors in your part as soon as you can Errors cause rebuild time to increase, and if you wait until more errors exist, troubleshooting may become more difficult

Using the Skeleton or Wide Tree Approach

SolidWorks is not the first parametric modeler to challenge the linear logic of genealogical

analy-sis The users of software like Pro/ENGINEER are responsible for developing many of the

con-cepts and best practice techniques that SolidWorks users use today

NOTE The term Skeleton in Pro/ENGINEER has a different significance than the way it is being used here SolidWorks does not have any feature or function named

“skel-eton.” The term is just being used to refer to a set of sketches, planes, axes, and reference

points used to lay out the major faces and features of a part.

The SolidWorks Help files, tutorials, and training curricula have encouraged users in some respects

to take a “fast and loose” approach to modeling, which lends itself best to simple models that are not

changed frequently Little thought is given to the structure of the part; the focus is on the final shape

The main consideration seems to be the simplest way to do something, or how it could be done

rather than how it should be done This mentality fit well with the initial several releases of the

SolidWorks software, which at that time was marketed as being simple and fast

The software has progressed immensely since those days It is now entirely plausible to create complex

castings and plastic parts with many hundreds of features, weaving in and out of surface and solid

techniques, multi-bodies, and external references This is a far cry from the typical tutorial or training

part, which still tend to have fewer than 15 features, half of which may be fillets With the simpler

parts, you hardly give a thought to parent/child relationships, rebuild times, or the consequences of

continued

n Do not add unnecessary detail For example, it is not important to actually model a

knurled surface on a round steel part This additional detail is difficult to model in

SolidWorks, it slows down the rebuild speed of your part, and there is no advantage to

actually having it modeled (unless you are using the model for rapid prototype or to

machine a mold for a plastic part where knurling cannot be added as a secondary

pro-cess) This is better accomplished by a drawing with a note The same concept applies to thread, extruded text, very large patterns, and other features that introduce complex

details

n Do not rely heavily on niche features For example, if you find yourself creating helices

by using Flex/Twist or Wrap instead of Sweep, then you may want to rethink your

approach In fact, if you find yourself creating a lot of unnecessary helices, then you may want to rethink this approach as well, unless there is a good reason for doing so

n File size is not necessarily a measure of inefficiency

n Be cautious about accepting advice or information from Internet forums

If you are the CAD Administrator for a group of users, you may want to incorporate some best

practice tips into standard operating procedures for them The more users that you have to

man-age, the more you need to standardize your system

Building Intelligence into Your Parts

Part II

making changes that cause a feature to fail, because the whole part can be rebuilt from scratch in ten

minutes anyway This is because the people who know the software best were doing brief sales demo vignettes and small models that could be finished before the students fell asleep

SolidWorks users have traditionally been taught to build each feature linearly, on top of the one that came before This is the genealogical equivalent of each generation having a single child, and then that child having a single child, and so on The family tree, or FeatureManager, winds up looking like a long staircase, with each generation related only to the generation immediately before it In the SolidWorks world, this creates long, linear, daisy-chained relationships between consecutive features

It turns out that even though this has been hailed as the pinnacle of associative, parametric, based modeling, it is not really such a great idea, especially as the parts begin to get more complex When each feature is dependent upon the one before it, all of the features must be solved in a par-ticular order, and if one feature fails, so do all of the features that come after it This also slows down the rebuilding process Especially as we move into the age of parallel multi-threaded processing, a linear set of commands or features must be executed in order one after the other, and there is really little room for parallel processes

history-The sophistication of the documentation provided with SolidWorks software has not kept pace with the sophistication of the software itself, which I suppose is why you are reading this book rather than the help files provided with the software The documentation is still based on the simple scenarios, and the advanced user is left to figure things out on his or her own

As the software gets more sophisticated, the models created with the software can get more ticated, and the methods used to build the models must also get more sophisticated It’s time to leave the linear modeling approaches behind

sophis-Rather than using a linear daisy-chain modeling scenario, it is better practice to base features on entities that are less likely to fail or change in such a way that dependent downstream features also fail In earlier chapters, I have already suggested that you make sketch relations to other sketches when possible instead of model edges for this very reason

Taking that scenario one step further, what if a handful of sketch and plane features were used to centralize control of all of the rest of the features? What if every feature, to the extent possible, related back to these “skeleton” features? Features such as fillets, shell, and draft by design require selections from solid geometry, but other features, such as any feature created from sketches, could

be made with only reference to those original skeleton sketches and planes The parent/child tionship would look very different for a model made in this way Instead of looking like a long stair-case, this tree would look more like a tree that gets wide very quickly There would be fewer

rela-“generations,” but each generation would be more populated

The first thing to notice is that errors in features at the top of the tree do not cascade down the tree

as they do in the “stairstep” model Second, it is always much easier to find how a model is structed, because all the reference geometry used to build it is set up in the first few features This scenario also has the potential to make better use of multi-threaded processing because the logic is less linear and more parallel

con-Using Evaluation Techniques

You can use evaluation techniques to evaluate geometry errors, demonstrate the manufacturability

of a given part, or to some degree to quantify aesthetic qualities of a given part, or section of a part

I discuss evaluation techniques here because the design cycle involves iterations around the nation of evaluate-edit-evaluate functions I discuss the following techniques in this section:

The Verification on rebuild option

With the setting turned on, SolidWorks checks each face with every other face in the model This represents a better check than with the setting off, and a greatly increased workload The switch is off by default to prevent rebuild times from getting out of control For most parts, the default set-ting is sufficient; however, when parts become complex, you may need to select the more

advanced setting

If you see additional errors in the design tree that were not there before, then the combination of Verification on rebuild and Forced Rebuild has worked If not, then your problem may be else-where You still need to fix any errors found this way.

PERFORMANCE

PERFORMANCE For speed reasons, it is normal practice to turn Verification on rebuild off, and to use it selectively to check models with potential errors The type of speed

tion that you can see is in the 10-percent to 60-percent range Some of the performance tion as relates to patterns is documented in Chapter 8.

degrada-Check

Check is a tool that checks geometry for invalid faces and other similar geometry errors It is also often used to find open edges of surface bodies, short edges, and the minimum radius on a face or entity I usually apply the Check tool before turning on the Verification on rebuild option The Check tool points to specific face or edge geometry (not features or sketches) that is the cause of the problem When it finds general faults the locations that the Check tool points to may or may not have something obvious to do with a possible fix

Much of the time, the best tool for tracking down geometry errors is the combination of experience and intuition It is not very scientific, but you come to recognize where potential problems are likely to arise, such as attempting to intersect complex faces at complex edges Figure 11.8 shows the Check Entity dialog box

FIGURE 11.8

The Check Entity dialog box

Reflective techniques

Evaluating complex shapes can be difficult Subjective evaluation is typically personal, and requires

an eye for the type of work you are doing Objective evaluation requires some sort of measurable criteria for determining a pass or fail, or it enables you to assign a score somewhere in the middle.One way to subjectively evaluate complex surfaces, and in particular the transitions between

surfaces around common edges, is to use reflective techniques If you look at an automobile’s

fender, you can tell whether it has been dented or if a dent has been badly repaired by seeing how the light reflects off of the surface The same principle applies when evaluating solid or surface

models Bad transitions appear as a crease or an unwanted bulge or indentation The goal is to

turn off the edge display and not be able to identify where the edge is between surfaces for the

transition to be as smooth as if the whole area were made from a single surface

Zebra Stripes

Zebra Stripes can be activated one of two ways, through the menus at View ➪ Display ➪ Zebra

Stripes, or from a toolbar button on the View toolbar The technique that was really made for

analyzing complex shapes is Zebra Stripes This places the part in a room that is either spherical or cubic, where the walls are painted with alternating black-and-white stripes (although you can

change the colors and the spacing of the stripes) The part is made to be perfectly reflective, and

the way that the stripes transition over edges tells you something about the qualities of the faces on either side of the edge Four conditions are of particular interest:

n c0 = faces contact at edge

n c1 = faces are tangent across edge

n c2 = curvature of each face is equal at the edge and the transition is smooth

n c3 = rate of change of curvature of each face is equal at the edge

The Zebra Stripes tool can only help you identify c0, c1, and c2, and only subjectively This feature

is of most value between complex faces Figure 11.9 illustrates how the Zebra Stripes tool shows

the differences between these three conditions

Notice how on the Contact-only model, the Zebra Stripe lines do not line up across the edge On the Tangent example, the stripes line up across the edges, but the stripes themselves are not

smooth On the Curvature Continuous example, the stripes are smooth across the edges The part shown in Figure 11.16 is a surface model, and can be found on the CD-ROM with the filename

Chapter11ZebraStripes.sldprt

TIP You should rotate the model a lot when you are using the Zebra Stripes tool Changing the density of the lines can also help, as can increasing the image quality

(Tools➪Options➪Document Properties➪Image Quality) Turning off the edge display may also help.

to be tangent

Original faceswith curvature continuousblend between the faces

CROSS-REF RealView techniques and usage are covered in more depth in Chapter 5.

Lights and specularity

If the other methods are not working for you, then you can also try to use simple lights with the specularity turned up This does not work as nicely as the highly reflective Zebra Stripes and RealView techniques, but the bright spots created by the specularity settings for lights can give similar results for evaluating the quality of transitions between faces

Curvature display

Model curvature can be plotted onto the model face using colors, as shown in Figure 11.10 The

accuracy of this display leaves a bit to be desired, but it does help you identify areas of very tight

curvature on your part Areas of tight curvature can cause features such as fillets and shells to fail

FIGURE 11.10

Curvature display

Deviation Analysis

Deviation Analysis measures how far from tangent the surfaces on either side of a selected edge

actually are For example, the edges shown in Figure 11.11 are found to be fair, but not very good

I prefer deviations of less than 0.5 degrees Often with some of the advanced surface types such as Fill, Loft, and Boundary, SolidWorks can achieve edges with less than 0.05-degree maximum

deviation

FIGURE 11.11

An example of Deviation Analysis

Tangent Edges as Phantom

Using the Tangent Edges as Phantom setting is an easy way to evaluate a large number of edges all

at once This feature does not do what the Zebra Stripes tool does, but it gives you a good tion of the tangency across a large number of edges

indica-Although this is an easy method to use, it is not completely reliable I have not seen this function deliver false positives (edges displayed as tangent when in fact they were not), but I have seen many false negatives (edges that display as non-tangent when in fact they were) Figure 11.12 shows a situation where the edges are displayed with solid edges, but Deviation Analysis shows them to have a zero-degree maximum deviation

(for-You can start SimulationXpress through the Tools menu The interface guides you through a very simple wizard If you have any familiarity with FEA applications, you will find SimulationXpress easy to understand and use

The first step in running a simple analysis is to assign a material Once you have made your tion, click Apply Figure 11.13 shows some of the materials selection

FIGURE 11.13

Assigning a material in SimulationXpress

The material assigned through the SimulationXpress interface is applied as a SolidWorks material, complete with RealView, if applicable

Restraint

You can apply restraints to the part The restraints are limited to Fixed for the faces that are

selected Figure 11.14 shows the interface and the restraint symbols on the part

FIGURE 11.14

Applying restraints

good ways to export the results, including as eDrawings, AVI, and HTML (Hypertext Markup

Language)

FIGURE 11.17

A Stress plot for the analysis

Optimization

Optimization takes a single dimension and varies it to try to achieve the best stress-to-weight ratio

As shown in Figure 11.18, the gussets have been made smaller to reduce weight and to keep the

Factor Of Safety above 4

FIGURE 11.18

Optimization results

1 Open the existing part with the filename Chapter11TutorialStart.sldprt

Roll the part back and step through it feature by feature to see how it was made Edit the loft feature to see which sketches were used to create it This can help you to understand how the part was built Exit the loft command and move the rollback bar back to the bot-tom of the tree

2 Start the Deviation Analysis tool (Tools ➪ Deviation Analysis) Select the edges, as

shown in Figure 11.19

FIGURE 11.19

Deviation analysis of an existing part

SelectRMB then select tangency

The maximum deviation is about ten degrees, which is far too much This part needs to

be smoothed out, which you can do using splines in place of lines and arcs

3 The first step is to make the outlet all one piece with the spiral You can do this with

a Fit Spline You need to create the Fit Spline before the loft profiles and after the spiral Expand the loft, and rollback between the loft feature and the first sketch Answer OK to the prompt, and then rollback to just after the spiral, as shown in Figure 11.20

FIGURE 11.20

Rolling back to just after the spiral

4 Right-click the spiral in the FeatureManager and show it Open a new sketch on the

Top plane

5 Try to draw a horizontal line from the outer end of the spiral You will notice that

you cannot reference the end of the spiral

TIP Curves that are absorbed into other features are notoriously difficult to work with Generally, you need to select them from the FeatureManager to do anything at all

with them Also, if you need to reference an end of an absorbed curve, you are better off using Convert Entities to make it into a sketch entity.

6 Notice that you cannot select the spiral from the graphics window Even when

selected from the FeatureManager, it appears not to be selected in the graphics window Ensure that it is selected in the FeatureManager, and then click the Convert Entities but-ton on the sketch toolbar

7 Draw a horizontal line from the outer end of the spiral and dimension it to be three

inches long, as shown in Figure 11.21.

8 Select both the converted spiral and the line, and click Tools ➪ Spline Tools ➪ Fit

Spline Set the Tolerance to 1 and make sure that only the Constrained option is

selected Click OK to accept the Fit Spline Test to make sure that a single spline is ated by moving your cursor over the sketch to see if the whole length is highlighted

cre-NOTE The Fit Spline feature fits a spline to a set of sketch entities within the specified tol- erance It can be a useful tool for smoothing out sketch geometry.

CAUTION

CAUTION Do not exit the Fit Spline by pressing the Enter key as you do with other commands, because it simply exits you out of the command without creating a spline.

9 Exit the sketch, and create a new plane Click Insert ➪ Reference Geometry ➪ plane

Select the Parallel Plane at Point option Select the Right plane from the Flyout FeatureManager and the outer end of the Fit Spline that you have just created Click OK

to accept the new plane This is illustrated in Figure 11.22

Creating a new plane

10 Drag the Rollback bar down between Sketch3 and Loft1 If it goes beyond Loft1, then

you need to navigate back to this position again

11 Right-click Sketch3 and select Edit Sketch Plane Select the newly created Plane1 from

the Flyout FeatureManager, and click OK to accept the change

12 Notice that the loft profile has moved to a place where it does not belong This is

because the sketch has a Pierce constraint to the spiral, and there are multiple places where the spiral pierces the sketch plane

Edit Sketch3 and delete the Pierce constraint on the sketch point in the middle of the

construction line Create a Coincident relation between the sketch point and the outer end of the Fit Spline, as shown in Figure 11.23 Do not exit the sketch

FIGURE 11.23

Sketch3 in its new location

13 One of the goals of these edits is to smooth out the part Remember that the Deviation

Analysis told you that the edges created between the lines and arcs in Sketch3 were not very tangent For this reason, it would be a good idea to replace the lines and arcs in Sketch3 with another Fit Spline

Right-click one of the solid sketch entities in Sketch3, and click Select Chain

14 Create another Fit Spline using the same technique as in Step 8 Exit the sketch.

15 Drag the Rollback bar down one feature so that it is below the Loft Notice that the

Loft feature has failed If you hold the cursor over the feature icon, the tooltip confirms this by displaying the message, “The Loft Feature Failed to Complete.”

16 Edit the Loft feature Expand the Centerline Parameters panel if it is not already

expanded, and delete the Spiral from the selection box In its place, select the Spiral Fit Spline

Building Intelligence into Your Parts

Part II

17 If the loft does not preview, check to ensure that the Show Preview option is

selected in the Options panel, at the bottom.

18 If it still does not preview, right-click in the graphics window and select Show All

Connectors Position the blue dots on the connector so that it looks like Figure 11.24.

19 Click OK to accept the loft The loft should be much smoother now than it was before

In addition, the spiral feature should no longer be under the loft, and should now be the first item in the design tree

20 Drag the Rollback bar down to just before the Shell feature Notice that Fillet5 has

failed Move the mouse over Fillet5 The tooltip tells you that it is missing some ences Edit Fillet5 and select edges in order to create fillets, as shown in Figure 11.25

FIGURE 11.24

Positioning the connectors

Position connector dots

in approximately correspondinglocations on the two loft profiles

FIGURE 11.25

Repairing Fillet5

Make selections to fillet edges

21 Right-click in the design tree and select Roll To End This causes the FeatureManager

to become unrolled all the way to the end

22 The outlet of the involute is now longer than it should be This is because the original

extrude was never deleted from the end Right-click the Extrude1 feature and select Parent/Child The feature needs to be deleted, but you need to know what is going to be deleted with it

23 The Shell is listed as a child of the extrude because the end face of the extrude was

chosen to be removed by the Shell Edit the Shell feature and remove the reference to

the face (A Shell feature with no faces to remove is still hollowed out.)

24 If you right-click Extrude1 and select Parent/Child again, the Shell feature is no

lon-ger listed as a child.

25 Delete Extrude1, and when the dialog box appears, press Alt+F to select Also

Delete Absorbed Features.

26 Edit the Shell feature and select the large end of the loft Exit the Shell feature The

results up to this step are shown in Figure 11.26

27 Drag a window in the design tree to select the four fillet features Then right-click

and select Add to New Folder Rename the new folder Fillet Folder

28 Click the Section View tool, and create a section view using the Front plane.

29 Reorder the Fillet folder to after the Shell feature.

30 At this point, you should notice that something does not look right This is because

creating the fillets after the Shell causes the outside fillets to break through some of the inside corners The fillets should have failed, but have not, as shown in Figure 11.27

Fillets that should have failed

31 Go to Tools ➪ Options ➪ Performance, and turn on Verification on rebuild Then

click OK to exit the Tools, Options, and press Ctrl+Q The fillets should now fail

32 Click Undo to return the feature order to the way it was.

33 Save the part.

Working effectively with feature history, even in complex models, is a requirement for working

with parts that others have created When I get a part from someone else, the first thing that I ally do is to look at the FeatureManager, and roll it back if possible to get an idea of how the part was modeled Looking at sketches, relations, feature order, symmetry, redundancy, sketch reuse, and so on are important steps in being able to repair or edit any part Using modeling best practice techniques helps to ensure that when edits have to be done, they are easy to accomplish, even if

usu-they are done by someone who did not build the part

Evaluation techniques are really the heart of editing, as you should not make too many changes

without a basic evaluation of the strengths and weaknesses of the current model

The chapters of Part III detail the tools you need to be

familiar with in order to get the most from your

assem-blies Of these, Chapters 12 and 16 are my favorites

These are loaded with best practice suggestions and tips for

effi-cient workflow Chapter 16, the in-context chapter, is

particu-larly important for SolidWorks users from many different fields

who need or want to make parametric relations between parts

A lot of erroneous information floats around the SolidWorks

community on this topic, and this chapter helps you separate

the helpful information

Working with Assemblies

IN THIS PARTChapter 12

Building Efficient Assemblies Chapter 13

Getting More from Mates Chapter 14

Assembly Configurations and Display States Chapter 15 Component Patterns Chapter 16

Modeling in Context

Chapter 4 provides a brief introduction to the basics of assemblies,

how to put parts together, the basics of mating, and so on The

basic process for putting assemblies together remains the same for

assemblies of any size, but once the assembly passes a certain point — and

this point is likely different for each user or application — the assembly will

benefit from some sort of organization or management techniques This

chapter introduces you to the tools and techniques that are available to help

you manage performance issues as well as general-use issues, efficiency,

browse-worthiness, or searchability

Identifying the Elements

of an Assembly

From Chapter 4, you know that an assembly can contain parts and mates

However, the simple tutorial in Chapter 4 does not go beyond this low level

of detail While the tutorial may have gotten you started, it does not provide

enough information to make you competent with the broad range of decisions

that you must make to create efficient real-word assemblies Real-world

assemblies can become very complex

As the assembly grows in the number of parts and design requirements,

you may need to add some of the following types of assembly elements

(You may already be familiar with some of these parts from having worked

with part documents.) The assembly elements are listed here with brief

explanations, and detailed either later in this chapter or in other chapters

IN THIS CHAPTERIdentifying the elements of an assembly

Using SpeedPaks Using subassemblies Using folders Working with tree display options Finding useful assembly tools Tutorial: Managing the FeatureManager

Working with Assemblies

Part III

n Assembly equations

n Assembly Layout feature

n Assembly layout technique

n Assembly reference geometry (plane, axis, point, coordinate system)

n Parts

n Subassemblies

n Folders for parts

n Folders for mates

n Assembly Design Table

n Assembly Bill of Materials (BOMs)

Standard reference geometry items

The three standard planes and the Origin are all familiar to you in the assembly FeatureManager design tree, as are the other standard items, such as the Annotations, Design Binder, Sensors, and Lights and Cameras folders These items offer the same standard functionality of their part document counterparts

FIGURE 12.1

Elements of an assembly

NOTE Remember that you can use the Tools permanently turn on or off various folders in the header of the FeatureManager ➪Options➪FeatureManager page to

Also be aware that some folders when set to Automatic do not automatically turn on when they should In cases like this, you should manually go to Tools➪Options➪FeatureManager to set

them to Show.

Assembly equations

Assembly equations work mainly like part equations, but with some additional complications

and considerations For example, one of the additional features of assembly equations is the ability

to drive the dimensions of one part from another part The syntax is slightly different for this

application, as shown in Figure 12.2 Overall, issues with equation order and using driven sions on the right side of the equation are the same between parts and assemblies

dimen-CROSS-REF Equations are discussed in detail in Chapter 9.

by an assembly So in this case, the in-context external reference can only be solved if the original part, the referenced part, and the assembly where the relationship was created are all open at the same time.

CROSS-REF In-context references are discussed in depth in Chapter 16.

When one part drives another part in this way, the assembly must also be open to drive the relationship If just the two parts are open individually, then changing the driving part does not update the driven part; because the relationship was created in the context of the assembly, the assembly must also be open to facilitate the change

Link values and global variables

Link values and global variables also work in assemblies, but they do not work between parts Local assembly sketches can use these functions, and the parts can use them when edited in the context of the assembly, but they cannot cross any document barriers (links must remain within a single document)

Renaming

Equations update with new part names regardless of how the part is renamed Names of

subassemblies also update when assembly files are renamed This includes renaming a document using the Save As command, using SolidWorks Explorer, or using Windows Explorer It also includes redirecting the assembly to the new part name, as well as renaming the assembly using each of these techniques If the assembly can find the part and recognizes the part as the one that it

is looking for, then the equation will work

Some of the methods named previously for renaming parts are not recommended; for testing purposes I specifically tried to break the relationships in the equations in using them SolidWorks Explorer and the Save As methods can be effective when used properly References between files are a different issue altogether from an equation’s references to local file names

CAUTION You may have unexpected results if a single dimension is controlled from more than one location For example, if you have a part-level equation and an

assembly-level equation, then one of the equations will be automatically set to Read Only and will not be used.

Assembly layout sketch

In SolidWorks 2008, a new assembly level feature was added to the software called a Layout Prior to

2008, the word layout referred to any assembly level sketch that you used to position or size parts or

features within parts The distinction between the technique and the formal assembly feature is bound

to be confusing, especially because they accomplish mostly the same things with a few differences

SolidWorks’ new Layout feature only works in assemblies, but layout techniques have been used in

parts as well as assemblies for many years In this chapter I will describe the old technique, and leave

the new Layout feature for Chapter 16 When you look at the two functionalities, the new feature is

definitely intended to be used as an in-context tool, while the existing technique can be used most easily

as a reference for controlling part position (through mating) rather than a way to directly control the

sizes and shapes of the parts

CROSS-REF The new Layout feature is described in more detail in Chapter 16, while the technique using assembly sketches to lay out an assembly is described here The material in this

chapter is written as if the Layout feature does not exist, mainly to give you a straightforward view

of how it works without worrying about two different functions at the same time.

The layout sketch is a very useful tool for constructing complex assemblies or for laying out a

mechanism in an assembly Sketches in the assembly have the same characteristics as they do in

the part environment In Figure 12.3, the assembly layout sketch is indicated with a heavy, dashed line for emphasis

When combined with in-context techniques, assembly layout sketches can help to determine the shape of parts You can also use layout sketches to mate assembly components to far more robust and dependable mates, rather than mating part to part The sketch shown in Figure 12.3 is used

for both of these techniques The shape of the frame and the major pivot points are established in the 2D sketch The wheels are also mated to the sketch

When you use an assembly layout sketch for either the in-context part building or simply part

positioning, the main advantage that it offers is having a single driving sketch that enables you to change the size, shape, and position of the parts You can use as many layout sketches as you want, and you can make them on different sketch planes This enables you to control parts in all directions

Working with Assemblies

Part III

FIGURE 12.3

An assembly layout sketch

One of the drawbacks of this technique is that you give up dynamic assembly motion To move the parts, you have to move the sketch The part does not move until the sketch is updated If you need to combine layout functionality with dynamic assembly motion, see the Layout feature in Chapter 16

Virtual components

Virtual components are covered in more depth in Chapter 16 Virtual components are parts that are created in the context of the assembly, and are at least temporarily stored in the assembly You can save them out so that they are external to the assembly and can be reused in other assemblies

BEST PRACTICE

BEST PRACTICE Virtual components are a technique that is useful for concept work in assemblies, but you will not see them show up on any best practice list The main limitation of

this technique shows up in the form of data management and reuse.

Assembly reference geometry

Planes and axes are frequently created within assemblies to drive symmetry or placement of parts You can use assembly layout sketches to create the reference geometry entities When you create reference geometry within the assembly in this way, be aware that the normal history-based parent/child relationships are still followed The familiar icons for reference geometry entities are also used in the assembly tree

History-based and non-history-based portions

of the assembly tree

Because features such as sketches and reference geometry are history-based and found in the

assembly tree, at least a portion of the assembly FeatureManager is history-based However, not all

of it is For example, the list of parts and subassemblies is not history-based

Sketches and reference geometry may appear before or after the list of parts, subassemblies, and

mates All of the remaining entity types that can be found in the assembly FeatureManager are

also history-based features, and you can reorder them in the tree However, several situations can disrupt the process Under normal circumstances, sketches and reference geometry at the top of

the assembly FeatureManager are solved, then the parts are rebuilt if required, and then the mates are solved This ensures that the sketches and reference geometry are in the correct locations so

that if parts are mated to them, then all of the components end up being the correct size and in the right position

Assembly-level reference geometry can be created that references component geometry instead of layout sketches This creates a dependency that changes the usual order For example, the planes

are usually solved before the part locations, but when the plane is dependent on the part location, the plane has to be solved after the part If a part is then mated to the plane, you are beginning to

create a dependency loop, such that the plane is solved, followed by the part, then the plane again because the part has moved, and then the mate that goes to the plane has to resolve the part

BEST PRACTICE

BEST PRACTICE If you are a bit confused by all of this, don’t worry You can simply follow this rule: Do not mate to anything that comes after the mates in the assembly FeatureManager

tree This includes assembly planes or sketches that are dependent on part geometry, assembly features such as cuts, in-context features, component pattern instances, Series Holes, or Smart Fasteners.

This is probably a lot of information if you are a new user, but if you remember this rule, then

you can avoid creating models with circular references, where A is dependent on B, which is

dependent on A — a never-ending loop that causes major problems for large assembly rebuild

times.

Parts and subassemblies

Parts and subassemblies are shown with their familiar icons in the design tree You can reorder and group them in folders, which is covered in the next section

Parts are sometimes shown with a feather, which indicates a lightweight part, and assemblies can have an icon that indicates a flexible subassembly

Special icons also exist for hidden and suppressed components

You should not confuse assembly features with in-context features In-context features are created

in the assembly with a reference between parts, but the sketch and feature definition are in the part itself

Starting with SolidWorks 2009, features created in the assembly can be propagated to reside in the affected parts

Component patterns

Component patterns can pattern either parts or assemblies by creating either a pattern defined in the assembly, or a pattern that follows a pat-tern feature created in a part The pattern is listed as a feature in the assembly FeatureManager, and all the instance parts appear indented from the pattern feature in the design tree You can hide or suppress each instance, change its configuration, and in most ways control it as if it were a regular part in the design tree

Because the options for locally defined patterns are comparatively limited, users generally like to use part feature patterns to drive the component patterns when possible

PERFORMANCE

PERFORMANCE To improve performance, it is best to pattern subassemblies if possible If it is not possible, then patterning a group of parts is the next best option Making multiple

patterns, one for each part, is an inefficient way to accomplish the same thing.

In-context reference update holders

It is difficult to get a good picture of assemblies in general without including a discussion about

in-context references, but to treat the subject properly, it also requires its own section, and in fact, this book gives in-context modeling its own chapter (Chapter 16) When you create a reference

between parts in an assembly, the assembly needs to remember which parts are involved in the

reference, and what the spatial relationship between them is The parts also need to remember

which assembly was used to create the relation because the parts are positioned in the assembly,

and the reference has meaning only with regard to a particular relative position between the parts.When you create the relation, a placeholder has to be left behind in the assembly to hold this

information This placeholder is called an Update Holder The Update Holders do not display by default To see them, you must right-click the top level in the FeatureManager and select Show

Update Holders They only exist when in-context references exist in the assembly, and there is one Update Holder for each in-context reference (one holder per sketch or feature) You cannot do very much with the Update Holders, other than query them for parent/child relations and to list the

external relations, but they serve as a reminder that you have in-context references to maintain

Several years ago, they were displayed by default, but they were later hidden by default, presumably because users were confused by the presence of something that you could not do anything with

In-context modeling methods are often scorned by some users, and if you have a list of 50 or 60

Update Holders, then you may be perceived as an overzealous novice For more information on

this feature, see Chapter 16

Popular perceptions of in-context techniques aside, in-context modeling is powerful If you follow the best practice suggestions outlined in Chapter 16, you will soon gain confidence and master this technique rather than being frightened by it The functionality works, and if you do not abuse it, it will serve you well

Smart Fasteners

Smart Fasteners are assembly features that automatically select Toolbox parts for use in standard-sized holes, and you can use them in many different ways The Smart Fastener feature in the assembly FeatureManager is used to edit the definition of the

Smart Fastener, which can include adding items such as nuts and washers You can also use Smart Fasteners in conjunction with the Hole Wizard to place appropriate holes and matched fasteners, all in a single step

CROSS-REF Smart Fasteners, Toolbox, and the Hole Wizard are discussed in detail in Chapter 17.

Hole Series

The Hole Series is a Hole Wizard–type feature that you apply in an assembly This wizard leaves

the feature icon in the assembly, but also adds features directly to the individual parts It also adds in-context Update Holders to the assembly FeatureManager, as shown in Figure 12.4 The Series

Hole is designed to go through a series of parts, placing the appropriate hole type in each part,

be used to replace an entire subassembly within an upper-level assembly SpeedPaks are intended

to increase performance with very large assemblies and drawings

Figure 12.5 shows first the SpeedPak PropertyManager, which is accessed by right-clicking an active configuration, and selecting Add SpeedPak Each configuration can have only one SpeedPak.Figure 12.5 also shows the configuration list with the SpeedPak listed indented under the Default config, and the entire assembly The final image shows the SpeedPak inserted into an assembly document, consisting of a single face and two solid bodies Notice the special icon associated with SpeedPaks You can change a part in an assembly from or to a SpeedPak in the same way that you would change a configuration, using Component Properties

FIGURE 12.5

Managing SpeedPaks

Model of Garmin assembly from the SolidWorks demo sets

Remember this is a tool for increasing assembly speed, and to increase speed, there is always

something that you have to give up If your expectations of the tool are in line with the actual

functionality, you will be very satisfied with the functionality SpeedPaks offer

it displays, but cannot be selected When the cursor gets near ghost geometry, the ghost fades away, revealing only selectable geometry Notice at the bottom of the SpeedPak PropertyManager that you can also choose to remove the ghost data and further increase the memory savings.

Sharing Self-contained Data

The SpeedPak is self-contained All the selected face and body geometry is saved inside the assembly

If you want to send someone a visual representation of an assembly, make a SpeedPak configuration and send only the assembly file — no parts are required This is the equivalent of being able to put

an eDrawing file into an assembly This is one of the better performance ideas to come out of SolidWorks in some time

Using SpeedPak with drawings

You can even use SpeedPaks with drawings Just remember that only the faces or bodies in the Include lists can be dimensioned to Some functionality exists for the ghost data, such as BOM inclusion and numbered balloons Ghost data displays as gray on the drawing, while geometry in the Include list is black

Using Subassemblies

The first tool for organizing assemblies is the subassembly A subassembly is just a regular assembly that is used as a component in another assembly

BEST PRACTICE

BEST PRACTICE The number of levels of subassemblies is not limited to a specific number, although for different sizes and types of assemblies, I encourage you to establish a best practice for

your company For example, establish a guideline that suggests that subassemblies of 100 parts or less go no deeper than three levels.

You can use several criteria to determine how subassemblies are assigned:

n Performance

n BOM

n Relative motion

n Pre-fabricated, off-the-shelf considerations

n According to assembly steps for a process drawing

n To simplify patterning

The underlying question here is based on the multiple functions of your SolidWorks assembly

model Is it primarily a design tool? A visualization tool? A documentation tool? A process tool? As

a design tool, the assembly is used to determine fits, tolerances, mechanisms, complex shapes that span parts, and many other things As a visualization tool, it simply has to look good and possibly move properly if that is part of the design As a documentation tool, it is important how the model relates to the BOM, and the order in which subassemblies are added As a process tool, you need

to be able to show the assembly in various intermediate states of being assembled

I have seen companies create multiple assembly models for different purposes Sometimes the

requirements between the different methods are contradictory and cannot all be met at the same

time with a single set of data Again, depending on what information you need to be able to extract from your SolidWorks models, you may want to approach assembly modeling and organization

differently

Creating subassemblies from existing parts

You can create subassemblies from parts that already exist in an assembly To do this, select the

parts that you want to add to the subassembly using shift+, Ctrl+, or box select techniques, and

then select Form New Subassembly Here from the right-mouse button menu You are then

prompted to assign a name or possibly select a template for the new subassembly

CAUTION

CAUTION When creating a new subassembly from existing parts or when moving parts into or out of a subassembly from the upper-level assembly, some things may be lost

For example, mates are moved from the upper level to the subassembly If you have in-context

relationships, they may be removed Operations that create subassemblies cannot be undone

Working with Assemblies

Part III

NOTE When you are dragging a part out of an assembly and into another one, you may again see the cursor symbol that appears in Figure 12.5 If you do not want this to

happen, then hold down the Alt key while dragging The cursor symbol changes to the Reorder cursor (a reversed, L-shaped arrow), and the part is placed after the subassembly rather than within it.

Insert a new subassembly

Along with the right-mouse button menu option Form New Subassembly Here, which takes existing parts and puts them into a newly created subassembly, you can use another option called Insert New Subassembly The names of these functions do not adequately describe the difference

in what they do Insert New Subassembly inserts a blank subassembly at the point in the design tree that you indicate by right-clicking it You can place components into the subassembly by dragging and dropping them from the main assembly, or you can open the assembly in its own window, and insert parts by using the usual methods

Dissolving subassemblies

If you would like to get rid of a subassembly but want to keep its parts, then you can use the Dissolve Subassembly option through the right-mouse button menu This option has some of the same consequences of the Form New Subassembly Here option in that mates are moved from the subassembly to the upper-level assembly, and you may lose in-context relations and assembly features

Organizing for performance

Performance in SolidWorks is a euphemism for speed Subassemblies can contribute to speed-saving modeling techniques by segmenting the work that the software needs to do at any one time

Solving mates

The mates that contribute to putting the pieces of an assembly together are solved at the level of the top assembly Under normal circumstances, subassemblies are treated as static selections of parts that are welded together, and their mates are not solved at the same time that the top-level assemblies’ mates are solved This segmenting of the mates leads to improved performance by only solving one set of mates at a time

Mates are usually solved as a single group unless there is a special situation, such as mates to in-context features, component pattern instances, or an assembly feature, all of which have already been described in this chapter When one of these situations occurs, the mates have to be divided into separate groups or solved multiple times This is done transparently behind the scenes so that the user does not have to worry about it

Flexible subassemblies

When you create subassemblies, the mates for these parts are not solved in the upper-level assembly This means that if a subassembly is a mechanism, the mechanism does not allow Dynamic Assembly Motion in the upper-level assembly For example, in Figure 12.7, the front fork is a linkage

mechanism, but it is also a subassembly Without reassembling the parts of the fork in the

upper-level assembly, you can allow the mates from the fork subassembly to be solved in the upper-upper-level

assembly by using an option in the Component Properties dialog box, which is also shown in Figure 12.7 When you select the Flexible option in the Solve As section, you enable the mates of this

subassembly to be solved in the upper-level assembly

FIGURE 12.7

Creating a flexible subassembly

Solve as flexible or rigid

To access the Component Properties dialog box, right-click the subassembly and select Component Properties from the menu

Flexible subassemblies are another source of great superstition in SolidWorks software, particularly with users that have used the software for several years In releases past, flexible subassemblies

required all instances to be flexible, and required a different configuration for each flexible instance This was very inconvenient, and a lot of users remember trying to get flexible subassemblies to work with a painful expression