CHAPTER 9

Patterning and Mirroring

Patterning and mirroring in SolidWorks are great tools to help you improve your efficiency. SolidWorks software provides many powerful pattern types that also help you accomplish design tasks. In addition to the different types of patterns, there are options that enable functionality that you may not have considered. A solid understanding of patterning and mirroring tools is necessary to be able to build the maximum amount of parametric intelligence into your models, and to open up the possibilities of your design objectives.

Patterning in a Sketch

You can use both pattern and mirror functions in sketch mode, although sketch patterns are not a preferred choice. The distinction between patterning and mirroring in sketch mode is important when it comes to sketch performance.

You might hear a lot of conflicting information about which features are better to use in different situations. Users coming from a 2D background often use functions such as sketch patterning because it's familiar, without questioning whether there is a better approach, and often without having any way of measuring how it performs. When in doubt, you can perform a test to determine which features work best for a given situation.

To compare the performance of various types of patterns, I made a series of 20-by-20 patterns using circles, squares, and hexagons. The patterns are both sketch patterns and feature patterns, and I created them with both Verification on Rebuild and Geometry Pattern turned on and off. Verification on Rebuild is an error-checking setting that you can access through Tools Options Performance, and Geometry Pattern is a setting that is applicable only to feature patterns that disables the intelligence in patterned features.

Table 9.1 shows the rebuild times (in seconds) of solid geometry created from various types of patterns as measured by Feature Statistics (found at Tools Feature Statistics). Sketch patterns are far slower than feature patterns, by a factor of about ten. The biggest speed reduction occurs when you use sketch patterns in conjunction with the Verification on Rebuild setting, especially as the number of sketch entities being patterned increases.

Generally, the number of faces and sketch relations being patterned has a significant effect on the speed of the pattern. The sketch pattern times are taken for the entire finished model, including the sketch pattern and a single extrude feature, using the sketch with the pattern to do an extruded cut. The sample parts are on the DVD for reference. Look for the filenames beginning with Reference1 through Reference7.

TABLE 9.1 Pattern Rebuild Times

The most shocking data here is the difference between a sketch pattern of a hex when a patterned sketch cuts into a flat plate compared to a feature pattern of a single extruded hex with each using the Verification on Rebuild option — 0.36 seconds compared to 126 seconds.

Always keep this general information about sketch patterns in mind:

• Sketch patterns are bad for rebuild speed.
• The more faces created by any pattern, the longer it takes to rebuild.
• The more sketch relations a sketch pattern has, the longer it takes to rebuild.
• Geometry pattern does not improve rebuild speed (unless a special end condition like Up to Surface has been used).
• Verification on Rebuild dramatically increases rebuild time with the number of faces but is far less affected by feature patterns than extruded sketch patterns.

Figure 9.1 shows one of the parts used for this simple test.

FIGURE 9.1 A pattern part used for the test

One interesting result of this test was that if a patterned extruded feature creates a situation where the end faces of the extruded features have to merge into a single face, the feature could take ten times the amount of time to rebuild as a pattern with unmerged end faces. This was an inadvertent discovery. I'm sure you would make your own discoveries if you were to investigate rebuild speeds for end conditions for cuts such as Through All, Up to Face, Up to Next, and so on, as well as the difference between cuts and boss features. Further, using Instant 3D can be an impediment when you're editing very large sketches simply due to the effects of the preview.

You should also note that the situation this simple test covers is very limited in scope. Because the plate is a constant thickness, the Geometry Pattern option actually works, which it wouldn't if the plate varied in thickness (with the through holes). It also only tests the Through All end condition, and the Geometry Pattern is best used to simply disable intelligent end conditions. I get the impression that many people use it as a random toggle trying to get patterns to work that SolidWorks would otherwise not allow to work.

I discuss the Geometry Pattern option in more detail later in this chapter. I wanted to start the chapter with a discussion that called attention to the misperception that some people have that sketch patterns are somehow better than feature patterns.

Debunking more sketch myths

People often say that it is best practice to define your sketches fully. I completely agree with this statement. However, I have heard people go to the extent to say that fully defined sketches solve faster, with the rationale being that SolidWorks has to figure out how to solve the under-defined sketch, but the fully defined sketch is already spelled out. Let's find out.

In this example, I created a sketch pattern of 4 × 4 rectangles and used the Fully Define Sketch tool to add dimensions. Then I copied and pasted the sketch and removed all the dimensions and relations. Figure 9.2 shows the Feature Statistic results.

It is safe to say that fully defined sketches are best practice, but it is not due to rebuild speed. Sketch relations are costly from a rebuild time point of view. Patterning sketch relations are even more costly. The rebuild time does not even come close to the time that it takes the Fully Define Sketch tool to create all the dimensions and relations in the first place. This combination of geometry, software, and hardware took about 30 seconds of CPU time to add the relations and dimensions.

FIGURE 9.2 Comparing rebuild times of a fully defined sketch to a completely undefined sketch

For most models that have fewer than 50 features, you may never notice this rebuild time, and the price you pay is certainly worth the peace of mind you get from having the stability of a fully defined sketch. For large models where you have hundreds of features, or features that use a lot of very busy sketches, you should pay attention to how much information you put into the sketch, and try to limit sketch patterns and even elements such as sketch fillets, using feature fillets instead where possible.

Patterning a sketch

I used the first part of this chapter to debunk some SolidWorks myths about sketches and sketch patterns. In this section, I will discuss how to use sketch patterns. Sketch patterns are an available tool, they are valid, and in a few cases, they are truly necessary.

It is best to pre-select the sketch entities that you want to pattern before using the Sketch Pattern tool. If you do not pre-select, then after the PropertyManager is open, you can only select entities to pattern one by one, because the window select is not available for this function. The right mouse button selection options, such as Select Chain, are also not available in this interface, reinforcing the need to treat sketch patterns as a pre-selection feature.

Using the Linear Sketch Pattern

The Linear Pattern PropertyManager is shown in Figure 9.3.

Unlike other PropertyManagers, the selected entities for the sketch pattern functions are found at the bottom of the PropertyManager instead of at the top. This is a little confusing. Sketch tool PropertyManagers, such as Convert Entities and Mirror, place the selection box at the top.

The Direction 1 panel works predictably by establishing the direction and spacing, and then the number. The Angle setting enables you to specify a direction that does not rely on anything outside of the sketch.

FIGURE 9.3 The Linear Pattern PropertyManager

The Direction 2 panel works a little differently. You must first specify how many instances you want, and then the other information becomes available. The spacing is grayed out until you tell it you want more than one instance in Direction 2.

Using the Circular Sketch Pattern

The Circular Sketch Pattern defaults to the sketch Origin as the center of the pattern. You can move and position this point using the numbers in the PropertyManager, but you cannot dimension it until after the pattern is created. Again, this is another feature where you need to pre-select because window selection is not available (patterned sketch entities must be selected one by one to go into the Entities to Pattern panel). Figure 9.4 shows the Circular Pattern PropertyManager.

FIGURE 9.4 The Circular Pattern PropertyManager

Mirroring in a Sketch

Mirroring in a sketch is a completely different matter from patterning in a sketch. It offers superior performance, and the interface is better developed. Mirrored entities in a sketch are an instrumental part of establishing design intent.

Two methods of mirroring items in a sketch are discussed here, along with a method to make entities work as if they have been mirrored when in fact they were manually drawn.

Using Mirror Entities

Mirror Entities works by selecting the entities that you want to mirror along with a single centerline, and clicking the Mirror Entities button on the Sketch toolbar. You can use this simple and effective tool on existing geometry. This method is the fastest way to use the tool, but there are other methods. You can pre-select or post-select, using a dialog box to select the mirror line, which does not need to be a centerline.

One feature of Mirror Entities may sometimes cause unexpected results. For example, in some situations, Mirror Entities will mirror a line or an arc and merge the new element with the old one across the centerline. This happens in situations where the mirror and the original form a single line or a single arc. SolidWorks may delete certain relations and dimensions in these situations.

Figure 9.5 shows the Mirror Entities PropertyManager.

If you are a longtime user, you should note that there are some relatively new ways to use functions such as Mirror Entities, which can now involve a selection box in a PropertyManager window. Longtime users are used to operating tools such as Mirror, Offset, and Convert Entities without an interface. In more recent versions of SolidWorks, these functions have had PropertyManagers that enable a selection list window.

FIGURE 9.5 Selecting items in the Mirror Entities PropertyManager

Some longtime users find the PropertyManager disruptive to their workflow. Other people may appreciate the benefit of the selection list window. Here are three workflows for this function that allow you to use a range of techniques:

• Traditional method. To continue to work with the Mirror Entities tool using the traditional method without an interface, click the Mirror Entities button on the Sketch toolbar and disable the pushpin. The pushpin is shown disabled (pointing to the left instead of into the screen) in Figure 9.5. Now when you use the function, pre-select your sketch geometry, including the centerline you want to mirror about. You do not see the interface; your sketch geometry is just mirrored for you. This is actually the fastest way to work.
• New method. To always make sure that you see the new Mirror Entities PropertyManager with the selection list box, make sure the pushpin is enabled (where the pin is pointing into the screen). This allows you to always see the list of selected entities and to make sure that the line you want to mirror about is selected. One of the hidden benefits of using the Mirror Entities PropertyManager is that you can select a non-centerline to mirror about — a convenient and useful option. Overall, this method is slower and more deliberate, but it offers more control, and it's there if you need or want it. If you pre-select sketch entities before activating the tool, you are still presented with the PropertyManager.
• Hybrid method. To some extent, you can have it both ways. If you unpin the Mirror Entities PropertyManager, you can pre-select your geometry, as in the traditional method, and the PropertyManager never appears, or you can select the geometry afterwards using the new method, and you are presented with the PropertyManager to be more deliberate about the selections. To me, this is the method that makes the most sense because you can determine what you need as you perform the operation. Both the fast and the more deliberate methods are available to you on the fly.

Notice also that the Mirror Entities PropertyManager has a Copy check box. This option is activated by default, and in this configuration, it works as you usually intend the Mirror function to work. If you disable this option, then the entities you want to mirror are simply flipped to the other side of the mirror line, and the entities in the original location are removed.

I have heard many people complain about these new PropertyManagers. It is possible that people are just reacting to the interruption of the old workflow without stopping to see what benefits it offers. In my opinion, the new options add functionality, and if you understand how to use them, they will not interrupt your fast workflow.

Using Dynamic Mirror

As the name suggests, Dynamic Mirror mirrors sketch entities as they are created. You can activate it by selecting a centerline and clicking the Dynamic Mirror button on the Sketch toolbar. Dynamic Mirror is not on the toolbar by default; you need to choose Tools Customize Commands to add it to the toolbar. You can also access Dynamic Mirror by choosing Tools Sketch Tools Dynamic Mirror from the menu.

When you activate this function, the centerline displays with hatch marks on the ends and remains active until you turn off or exit the sketch. Figure 9.6 shows the centerline with hatch marks. Dynamic Mirror has no other interface.

The Dynamic Mirror function remains active until you turn it off. You can use the same toolbar icon you used to turn it on. The icon remains depressed until you release it or exit the sketch.

FIGURE 9.6 The Dynamic Mirror centerline with hatch marks

Using Symmetry sketch relation

I have covered the Symmetry sketch relation in previous chapters on sketching, but I mention it again here because it offers you a manual way to mirror sketch entities. There are editing situations when you may not want to create new geometry, but instead use existing entities with new relations driving them. To create the Symmetry sketch relation, you must have two similar items (such as lines or endpoints) and a centerline selected.

To add the symmetry relation after you have made the proper selection, use the popup toolbar interface, the Sketch PropertyManager, or the Add Relation toolbar button. These three options are shown in Figure 9.7.

You can find more information on manipulating sketch relations in Chapter 3.

FIGURE 9.7 Three ways to add a symmetric sketch constraint

Using Mirroring in 3D sketches

Chapter 8 deals with 3D sketches in more detail, but I discuss the mirror functionality here to connect it with the rest of the mirroring and patterning topics. Three-dimensional sketches can contain planes, and if you are sketching on a plane in a 3D sketch, you can mirror items on it. You cannot mirror general 3D sketch entities.

Sketch patterns are also unavailable in the 3D sketch, but you can use the Move, Rotate, and Copy sketch tools on planes in 3D sketches. Combining one questionable functionality (planes in 3D sketches) with another (sketch patterns) does not usually improve either one.

Exploring the Geometry Pattern Option

The SolidWorks Help file says that the Geometry Pattern option in feature patterns results in a faster pattern because it does not pattern the parametric relations. This claim is valid only when there is an end condition on the patterned feature such that the feature will actually pattern the end condition's parametric behavior. The part shown in Figure 9.8 falls into this category. The improved rebuild time goes from .30 to .11 seconds. Although a 60 percent reduction is significant, the most compelling argument for the use of the Geometry Pattern has nothing to do with rebuild time. It is to avoid the effect of patterning the end-condition parametrics.

In fact, the Geometry Pattern option's main intent is to pattern existing geometry without the parametric intelligence. The main mission of Geometry Pattern has nothing to do with rebuild speed.

Under some conditions, Geometry Pattern will not work. One example is any time a patterned face merges with a face that cannot be patterned. Figure 9.9 shows two patterns, one that can use Geometry Pattern and one that cannot.

FIGURE 9.8 A geometry pattern test

The pattern of the rectangular bosses cannot use Geometry Pattern because the face that is merged is not merged in all pattern instances. The pattern of truncated cylinders shown on the same part as the pattern of rectangular bosses can use Geometry Pattern because the flat face is merged in every pattern instance. The circular pattern in the image to the right in Figure 9.9 also allows Geometry Pattern for the same reason.

FIGURE 9.9 Merged faces

In some situations, SolidWorks error messages may send you in a loop. One message may tell you that the pattern cannot be created with the Geometry Pattern turned on, so you should try to turn it off. When you do that, you may get another message that says the pattern will not work, and that you should try to use the Geometry Pattern setting. In cases like this, you may try to use a different end condition for the feature that you want to pattern, or change the selection of features patterned along with the feature, such as fillets. You may also try to pattern bodies or even faces rather than features. These last two options are covered in the following sections.

Patterning Bodies

I cover multi-bodies in depth in Chapter 20, but I will briefly discuss the topic here. Any discussion of patterning is not complete without a discussion of bodies because using bodies is an available and highly useful option with all the pattern and mirror types.

SolidWorks parts can contain multiple solid or surface bodies. A solid body is a solid that comprises a single contiguous volume. A surface body is different — think of it as a sheet knitted together from several faces — but it can also be patterned and mirrored as a body.

There are both advantages and disadvantages to mirroring and patterning bodies instead of features. The advantages can include the simplicity of selecting a single body for mirroring or patterning. In cases where the geometry to be patterned is complex or there is a large number of features, patterning bodies also can be much faster. However, in the example used earlier with patterning features in a 20-by-20 grid of holes, when done by patterning a single body of 1“ × 1” × .5“ with a .5” diameter hole, patterning bodies gives a rebuild time of about 60 seconds with or without Verification on Rebuild. The function combines the resulting bodies into a single body that takes most of the time. This says that for large patterns of simple features, patterning bodies is not an efficient technique. Although I do not have an experiment in this chapter to prove it, it seems intuitive that creating a pattern of a smaller number of complex bodies using a large number of features in the patterned body would show a performance improvement over patterning the features.

Another disadvantage of patterning or mirroring bodies is that it does not allow you to be selective. You cannot mirror the body minus a couple of features without doing some shuffling of feature order in the FeatureManager. Another disadvantage is that if the base of the part has already been mirrored by a symmetrical sketch technique, then body mirroring is not going to help you mirror the subsequent features. In addition, the Merge Bodies option within the mirror feature does not work in the same way that it works for other features. It merges only those bodies that are part of the mirror to bodies that are part of the mirror. Pattern Bodies does not even have an option to merge bodies. Both of these functions are often going to require an additional combine feature (for solid bodies) or knit (for surface bodies) to put the final results together.

Some of these details may seem obscure when you're reading about them, but when you begin to work patterning bodies and begin trying to merge them into a single body, read over this section again. The inconsistency between the Merge option existing in Mirror but not in Pattern, as well as the functional discrepancy between the Merge in Mirror and the Merge Result in, say, Extrude is unexplainable, and a possible opportunity for an enhancement request.

Patterning Faces

Most of the pattern types have an option for Pattern Faces. This option has a few restrictions, the main limitation being that all instances of the pattern must be created within the boundaries of the same face as the original. Figure 9.10 shows an example of the Pattern Faces option working with a Circular Pattern feature.

To get around the same face limitation, you can knit faces together and pattern the resulting surface body, as shown in Figure 9.11.

FIGURE 9.10 A circular pattern using the Pattern Faces option

Patterning faces is another way of patterning geometry within SolidWorks without patterning the feature intelligence that was built into the original. It is also a way to make patterns on imported parts from existing geometry. Chapter 23 addresses this topic briefly in the discussion on imported geometry and direct edit techniques.

Patterning faces is not a widely used technique; however, it should be somewhere in your toolbox of tricks. Although it may be lurking near the bottom of the pile, it is still useful in special circumstances.

FIGURE 9.11 Patterning a surface body

Patterning Fillets

You may hear people argue that you cannot pattern fillets. This is only partially true. It is true that fillets as individual features cannot be patterned. For example, if you have a symmetrical box and a fillet on one edge and want to pattern only the fillet to other edges, this does not work. However, when fillets are patterned with their parent geometry, they are a perfectly acceptable candidate for patterning. This is also true for the more complex fillet types, such as variable radius and full radius fillets. You may need to use the Geometry Pattern option, and you may need to select all the fillets affecting a feature, but it certainly does work.

Understanding Pattern Types

Up to now, I have discussed patterns in general; differentiated sketch patterns from feature patterns, face patterns, and body patterns; and looked at some other factors that affect patterning and mirroring. I will now discuss each individual type of pattern to give you an idea of what options are available.

Using the Linear Pattern

The Linear Pattern feature has several available options:

• Single direction or two directions. Directions can be established by edge, sketch entity, axis, or linear dimension. If two directions are used, the directions do not need to be perpendicular to one another.
• Spacing. The spacing represents the center-to-center distance between pattern instances, and can be driven by an equation.
• Number of Instances. This number represents the total number of features in a pattern, which includes the original seed feature. It can also be driven by an equation. Equations are covered in detail in Chapter 9.
• Direction 2. The second direction works just like the first, with the one exception of the Pattern Seed Only option. Figure 9.12 shows the difference between a default two-direction pattern and one using the Pattern Seed Only option.

  FIGURE 9.12 Using the default two-direction pattern and the Pattern Seed Only option

  

• Instances to Skip. This option enables you to select instances that you would like to leave out of the final pattern. The pink dots are the instances that remain, and the red dots are the ones that have been removed. Figure 9.13 shows the interface for skipping instances. You may have difficulty distinguishing the red and pink colors on the screen.

  FIGURE 9.13 Using the Instances to Skip option

  

• Propagate visual properties. This option patterns the color, texture, or cosmetic thread display, along with the feature to which it is attached.
• Vary Sketch. This option in patterns is often overlooked and not widely used or understood. While it may have a niche application, it is a powerful option that can save you a lot of time and open up design possibilities you may not have considered before.

Vary Sketch allows the sketch of the patterned feature to maintain its parametric relations in each instance of the pattern. It is analogous to Geometry Pattern. Where Geometry Pattern disables the parametric end condition for a feature, Vary Sketch enables the parametric sketch relations for a pattern.

To activate the Vary Sketch option, the Linear Pattern must use a linear dimension for its Pattern Direction. The dimension must measure in the direction of the pattern, and adding the spacing for the pattern to the direction dimension must result in a valid feature.

The sketch relations must hold for the entire length of the pattern. Figure 9.14 shows the sketch relations and the resulting pattern. This feature does not have a preview function.

Edit the .40-inch dimension. Double-click it and use the scroll arrow to increase the dimension; watch the effect on the sketch. If a sketch does not react to changes properly, then it cannot be used with the Vary Sketch option. In this case, the .40-inch dimension is used as the direction, because that is the dimension that will drive the sketch down the pattern. When using this option, the feature sketch must be driven by a single dimension. If the .48-inch dimension were anchored to the origin or the edge of the part like the .40-inch dimension, the pattern would not work properly. The direction dimension has to be able to drive the sketch in the same way that this one does. These dimensions cannot pass through the Zero value and cannot flip directions or move into negative values.

FIGURE 9.14 Using the Vary Sketch option

To make the sketch react this way to changes in the dimension, the slot was created using the bidirectional offset that was demonstrated in an earlier chapter, which means that the whole operation is being driven by the construction lines and arcs at the centerline of the slot. Sketch points along the model edges are kept at a certain distance from the ends of the slots using the .50-inch dimensions. The arcs are controlled by an Equal Radius relation and a single .58-inch radius dimension. The straight lines at the ends of the slots are controlled by an Equal Length relation.

This type of dimensioning and relation creation is really what parametric design is all about. The Vary Sketch option takes what is otherwise a static linear pattern and makes it react parametrically in a way that would otherwise require a lot of setup to create individual features. If you model everything with the level of care that you need to put into a Vary Sketch pattern feature sketch, then your models will react very well to change.

Using the Circular Pattern

The Circular Pattern feature requires a circular edge or sketch, a cylindrical face, a revolved face, a straight edge, an axis, or a temporary axis to act as the Pattern Axis of the pattern. All the other options are the same as the Linear Pattern — except that the Circular Pattern does not have a Direction 2 option and the Equal Spacing option works differently.

Equal Spacing takes the total angle and evenly divides the number of instances into that angle. The name equal spacing is a bit misleading because all Circular Patterns create equal spacing between the instances, but somehow everyone knows what they mean.

Without using the Equal Spacing option, the Angle setting represents the angular spacing between instances.

The Vary Sketch option is available in Circular Pattern as well. The principles for setup are the same, but you must select an angular dimension for the direction. The part shown in Figure 9.15 was created using this technique.

FIGURE 9.15 A Circular Pattern vary sketch

If you are creative with the sketch relations you apply to a sketch, you can get some pretty exotic results from patterns using the Vary Sketch option.

Using the Curve Driven Pattern

A Curve Driven Pattern does just what it sounds like: it drives a pattern along a curve. The curve could be a line, an arc, or a spline. It can be an edge, a 2D or 3D sketch, or even a real curve feature. An interesting thing about the Curve Driven Pattern is that it can have a Direction 2, and Direction 2 can be a curve. This pattern type is one of the most interesting and has many options.

For an entire sketch to be used as a curve, the sketch must not have any sharp corners — all the entities must be tangent. This could mean using sketch fillets or a fit spline. The example shown in Figure 9.16 was created using sketch fillets. This pattern uses the Equal Spacing option, which spaces the number of instances evenly around the curve. It also uses the Offset Curve option, which maintains the patterned feature's relationship to the curve throughout the pattern, as if an offset of the curve goes through the centroids of each patterned instance. The Align to Seed option is also used, which keeps all the pattern instances aligned in the same direction.

FIGURE 9.16 The Curve Driven Pattern using sketch fillets

Figure 9.17 shows the same part using the Transform Curve positioning option and Tangent to Curve alignment option.

Instead of an offset of the curve going through the centroids of each patterned feature instance, in the Transform Curve, the entire curve is moved rather than offset. On this particular part, this causes a messy pattern. The Tangent to Curve option gives every patterned instance the same orientation relative to the curve as the original.

The Face Normal option is used for a 3D pattern, as shown in Figure 9.18. Although this functionality seems a little obscure, it is useful if you need a 3D curve-driven pattern on a complex surface. If you are curious about this example, it is on the DVD with the filename Reference 3d Curve Driven.sldprt.

FIGURE 9.17 Using the Transform Curve and Tangent to Curve options

Using a Direction 2 for a Curve Driven Pattern creates a result similar to that in Figure 9.19. This is another situation that, although rare, is good to know about.

The rest of the Curve Driven Pattern works like the other pattern features that have already been demonstrated.

FIGURE 9.18 Using a 3D Curve Driven Pattern

FIGURE 9.19 Using Direction 2 with a Curve Driven Pattern

Using the Sketch Driven Pattern

Sketch Driven Patterns use a set of sketch points to drive the locations of features. The Hole Wizard drives the locations of multiple holes using sketch points in a similar way. However, the Sketch Driven Pattern does not create a 3D pattern in the same way that the Hole Wizard does. Figure 9.20 shows a pattern of several features that has been patterned using a Sketch Driven Pattern. A reference point is not necessary for the first feature.

FIGURE 9.20 Using a Sketch Driven Pattern

The Centroid option in the Reference Point section is fine for symmetrical and other easily definable shapes such as circles and rectangles, where you can find the centroid just by looking at it, but on more complex shapes, you may want to use the Selected Point option. The Selected Point option is shown in Figure 9.21.

FIGURE 9.21 Using the Selected Point option in a Sketch Driven Pattern

Using the Table Driven Pattern

A Table Driven Pattern drives a set of feature locations, most commonly holes, from a table. The table may be imported from any source with two columns of data (X and Y) that are separated by a space, tab, or comma. Extraneous data will cause the import to fail.

The X, Y Origin for the table is determined by a Coordinate System reference geometry feature. The XY plane of the Coordinate System is the plane to which the XY data in the table refers.

You can access the Coordinate System command by choosing Insert Reference Geometry Coordinate System from the menu. You can create the Coordinate System by selecting a combination of a vertex for the Origin and edges to align the axes. Like the Sketch Driven Pattern, this feature can use either the centroid or a selected point on the feature to act as the reference point.

The fact that this feature is still in a floating dialog box points to its relatively low usage and priority on the SolidWorks upgrade schedule. The interface for the feature is rather crude in comparison to some of the more high-usage features. This interface is shown in Figure 9.22.

FIGURE 9.22 The Table Driven Pattern dialog box

Using the Fill Pattern

The Fill Pattern feature fills a face or area enclosed by a sketch with a pattern of a selected feature. The type of pattern used to fill the area is limited to one of four preset patterns that are commonly used in gratings and electronics ventilation in plastics and sheet metal. These patterns and other options for the Fill Pattern are shown in Figure 9.23.

The Pattern Layout panel enables you to control spacing and other geometrical aspects of the selected pattern layout, as well as the minimum gap from the fill boundary. This is most useful for patterns of regularly spaced features with an irregular boundary.

FIGURE 9.23 Using the Fill Pattern feature

Using Cosmetic Patterns to Create an Appearance

Cosmetic Patterns are not patterns in the same sense as all the other pattern types in SolidWorks. Cosmetic Patterns do not actually create any geometry, just the appearance of geometry. They are applied using RealView functionality, which may or may not be available to you depending on your hardware, in particular your video card.

Cosmetic Patterns are appropriate if your manufacturing method does not require actual geometry. For example, rapid prototyping requires explicit geometry in order to build a part, but a perforated sheet metal panel or a knurled cylindrical handle may require only a note on a drawing for the shop to set up a manufacturing process to create the geometry.

To apply a Cosmetic Pattern to a face, feature, body, or entire part, click the Appearances, Scenes, and Decals tab from the Task pane, and choose Appearances Miscellaneous Pattern or Appearances Miscellaneous RealView Only Appearances. Drag and drop the desired pattern onto the model, and use the popup menu to apply it to a face, feature, body, or the entire part. Figure 9.24 shows the Appearances, Scenes, and Decals tab of the Task Manager with some of the Cosmetic Pattern options.

FIGURE 9.24 Cosmetic Pattern options in the Appearances, Scenes, and Decals tab of the Task Manager

Mirroring 3D Solids

Because symmetry is an important aspect of modeling parts in SolidWorks, mirror functions are a commonly used feature. This is true whether you work on machine parts, sheet metal, injection-molded, cast, or forged parts. I discussed sketch-mirroring techniques earlier in this chapter, and now I will discuss 3D mirroring techniques.

Mirroring bodies

Earlier in this chapter, I discussed patterning bodies. I mentioned that the patterning and mirroring tools in SolidWorks do not have adequate functionality when it comes to body management (specifically the merge options). Neither tool allows the patterned or mirrored bodies to be merged with the main body if the main body is not being patterned or mirrored. Figure 9.25 shows the Options panels for both the Linear Pattern (on the left) and the Mirror (on the right) features. Here you can see that the pattern function has no provision whatsoever for merging bodies. The Mirror appears to have the functionality, but it applies only to bodies that are used or created by the Mirror feature and ignores any other bodies that may exist in the part.

FIGURE 9.25 Options panels from the Linear Pattern and Mirror PropertyManagers

Mirroring features

Features can be mirrored across planes or flat faces used as the plane of symmetry. If you are mirroring many features, then it is best to mirror them all with a single mirror feature rather than to make several mirror features. You may have to do this by moving the mirror feature down the tree as you add new features. Depending on your part and what you are trying to accomplish, it may be better to mirror bodies than features, but you should not go too far out of your way or model in a contrived manner to make this happen.

Mirroring entire parts

Often when modeling, you are required to have a left- and a right-handed part. For this, you need to use a method other than body or feature mirroring. The Mirror Part command creates a brand-new part by mirroring an existing part. The new part does not inherit all the features of the original, and so any changes must be created in the original part. If you want different versions of the two parts, you need to use Configurations.

You can use the Mirror Part command by pre-selecting a plane or planar face. You should be careful when choosing the plane because the new part will have a relationship to the part Origin, based on the plane on which it was mirrored. The Mirror Part command is one of the few remaining features without a PropertyManager that relies completely on pre-selection techniques.

The Mirror Part command is found in the Insert menu. When mirroring a part, you can bring several entity types from the original file to the mirrored part. These include axes, planes, sketches, cosmetic threads, and surface bodies. You can also bring over features and even break the link to the original file.

Mirror Part invokes the Insert Part feature, which is covered in more detail in Chapters 19, on multi-bodies and Master Model techniques, respectively.

One of the options available when you make a mirrored part is to break the link to the original part. This option brings forward all the sketches and features of the original part, and then adds a Move/Copy Body feature at the end of the tree that simply mirrors the body. Figure 9.26 shows the PropertyManager for the Insert Part feature.

FIGURE 9.26 Selecting items to bring into the mirrored part

Tutorial: Creating a Circular Pattern

Follow these steps to get practice with creating circular pattern features:

1. Draw a square block on the Top plane centered on the Origin, 4 inches on each side, .5-inch-thick extruded Mid Plane with .5-inch chamfers on the four corners.
2. Pre-select the top face of the block and start the Hole Wizard. Select a counterbored hole for a 10-32 socket head cap screw, and place it as shown in Figure 9.27.

   FIGURE 9.27 Start drawing a plate with holes.

   

3. Create an axis using the Front and Right planes. Choose Insert Reference Geometry Axis. Select the Two Planes option, and select Front and Right planes from the flyout FeatureManager. (Click the bar that says Axis at the top of the PropertyManager to access the flyout FeatureManager.) This creates an axis in the center of the rectangular part.
4. Click the Circular Pattern tool on the Features toolbar. Select the new Axis in the top Pattern Axis selection box in the Circular Pattern PropertyManager. Select the Equal Spacing option and make sure that the angle is set to 360°. Set the number of instances to 8.
5. In the Features to Pattern panel, select the counterbored hole. Make sure that Geometry Pattern is turned off.
6. Click OK to finish the part, as shown in Figure 9.28.

FIGURE 9.28 The finished circular pattern

Tutorial: Mirroring Features

Follow these steps to get some practice with creating mirror features:

1. Open the file from the DVD called Chapter9 Tutorial2.sldprt.
2. Open a sketch on the side of the part, as shown in Figure 9.29. The straight line on top is 1.00 inch long, and the angled line ends 2.70 inches from the edge, as shown.

   FIGURE 9.29 The sketch for the Rib feature

   

3. Click the Rib tool on the Features toolbar or select it from the menu at Insert Features Rib. Set the material arrow to go down toward the block, and the thickness setting to go to the inside by .375 inches. The PropertyManager and the preview should look like Figure 9.30.

   FIGURE 9.30 Applying the Rib feature

   

4. Create a linear pattern using the rib, making the pattern reaches 2 inches into the part.
5. Create a chamfer on the same side of the part as the original rib, as shown in Figure 9.31. The chamfer is an Angle-Distance using 60° and .5 inches.
6. Create a round hole, sized and positioned as shown.
7. Mirror the hole and the chamfer about the Right plane. The parametrics of the chamfer will have difficulty patterning, and so you need to use the Geometry Pattern option. The finished part is shown in Figure 9.32.

FIGURE 9.31 Additional features on the part

FIGURE 9.32 The finished part

Tutorial: Applying a Cosmetic Pattern

Follow these steps to practice creating a cosmetic pattern:

1. Open the file from the DVD for Chapter 9 called Chapter 9 – tutorial – cosmetic pattern.sldprt.
2. Click the Appearances tab in the Task Pane. These steps will work whether or not you have RealView actually selected.
3. Expand the Appearances heading, then the Metal heading, then Steel, and then drag the Sandblasted Steel icon from the lower panel onto the part. When the popup menu appears, select the Part icon to apply the appearance to the entire part. Figure 9.33 shows the Task Pane and the popup menu.

   FIGURE 9.33 Applying an appearance to a part

   

4. Expand the Miscellaneous listing (under Appearances) and the Pattern heading. Drag the Waffle Pattern onto the large cylindrical face of the part, and then Alt-click the Face icon in the popup toolbar. Using the Alt key while dragging or to select face, feature, body, or part automatically activates the PropertyManager to edit the appearance. Figure 9.34 shows the Appearances PropertyManager.
5. In the Mapping tab of the Appearances PropertyManager, select the cylindrical mapping under the Mapping Style section of the Mapping Controls panel.
6. Change the Rotation to 45 degrees, and choose the smallest Mapping Size.

FIGURE 9.34 The Appearances PropertyManager

Summary

Feature patterns and mirrors are powerful tools, but you need to have some discipline to benefit from their usefulness. Patterns in particular are extremely flexible, with many types of functions and options available. You should avoid sketch patterns if possible, not only because of performance considerations but also because complex sketches (sketches with a lot of entities and relations) tend to fail more often than simple sketches.