IN THIS CHAPTER
Patterning in a sketch
Mirroring in a sketch
Geometry pattern
Patterning bodies
Patterning faces
Patterning fillets
Understanding pattern types
Mirroring in 3D
Tutorial: Creating a circular pattern
Tutorial: Mirroring features
Patterning and mirroring in SolidWorks are great tools to help you improve your efficiency. The software provides many pattern types that also help you accomplish design tasks easily. In addition to the different types of patterns, there are many more detailed 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.
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.
Note
Although there are many metrics for how software performs, in SolidWorks, the word performance means the same thing as speed. Sketch patterns have a very adverse effect on speed.
You can hear a lot of conflicting information about which features are better to use in different situations. Users coming from a 2D background often prefer to use functions such as sketch patterning because it looks familiar, without questioning whether there is a better way. When in doubt, you can perform a test to determine for yourself which is better.
In this test, I made a series of 20-by-20 patterns using circles, squares, and hexagons. The patterns were both sketch patterns and feature patterns, and were created with both Verification On Rebuild and Geometry Pattern turned on and off. Verification On Rebuild is a setting that you can access through Tools
Table 8.1 shows the rebuild times (in seconds) of certain types of patterns as measured by Feature Statistics (found at Tools
Generally, the number of faces 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 CD-ROM for reference. Look for the filenames beginning "Reference1" through "Reference7."
Table 8.1. Pattern Rebuild Times
Pattern Type | Default | Geometry Pattern | Verification on Rebuild |
|---|---|---|---|
20×20 sketch circle | 1.75 | n/a | 10.5 |
20×20 sketch square | 10.8 | n/a | 143 |
20×20 sketch hex | 19.4 | n/a | 294 |
20×20 feature circle | .19 | .28 | .19 |
20×20 feature square | .34 | .55 | .33 |
20×20 feature hex | .48 | .70 | .48 |
Figure 8.1 shows one of the parts used for this simple test.
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.
Tip
When creating a linear sketch pattern, be sure to select the Add Dimension check boxes. If these dimensions are not added, then editing the pattern becomes more difficult.
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.
Direction 2 works a little differently. You must first specify how many instances you want, and then the other information becomes available.
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.
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 when the mirror and the original would form a single line or a single arc. SolidWorks may delete certain relations and dimensions in these situations.
When you activate this function, the centerline displays with hatch marks on the ends, and remains active until you turn it off or exit the sketch. Figure 8.4 shows the centerline with hatch marks.
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 8.5 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 is to avoid the effect of patterning the end-condition parametrics.
Under some conditions, Geometry Pattern will not work. One example is any time a patterned face would merge with an unpatterned face. These situations can be difficult to identify. Figure 8.6 shows a pattern that cannot be created using the Geometry Pattern option. The boss merges with the side face of the block, which generates the error message shown in the figure. The circular part shown in the image is an exception where the partial cylindrical bosses merge with the side of the cylinder, but Geometry Pattern works.
The topic of multiple bodies is covered in depth in Chapter 26, but it must be dealt with briefly here. Any discussion of patterning is not complete without a discussion of bodies because using bodies is an available option with all of the pattern and mirror types.
SolidWorks parts can contain multiple solid bodies. A body is a solid that comprises a single contiguous volume. Surface bodies are defined differently, but they can also be patterned and mirrored as bodies.
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 130 seconds with or without Verification On Rebuild. It is the function that 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, I believe 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. Also, the Merge Bodies option does not work as you would want it to. 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 (for solid bodies) or knit (for surface bodies) to put the final results together.
Note
Bodies are discussed in more detail in Chapter 26. Surface modeling is covered in Chapter 27.
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 8.7 shows an example of the Pattern Faces option working with a Circular Pattern feature.
To get around this limitation, you can knit and pattern the surface body, as shown in Figure 8.8.
Note
Working with surface bodies is covered in Chapter 27.
You may hear people argue that you cannot pattern fillets. This is partially true and partially untrue. 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 cannot be done. 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 of the fillets affecting a feature, but it certainly does work.
Up to now, I have discussed patterns in general, differentiated sketch patterns from feature 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.
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 8.9 shows the difference between a default two-direction pattern and one using 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. Pink dots are the instances that remain, and the red dots are the ones that have been removed. Figure 8.10 shows the interface for skipping instances. You may have difficulty distinguishing the red and pink colors on the screen.
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 if you ever need to use it.
Vary Sketch allows the sketch of the patterned feature to maintain its parametric relations in each instance of the pattern. It is analogous to the 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 8.11 shows the sketch relations and the resulting pattern. The preview function for this feature does not work.
To adequately understand how this feature works, open the sample file from the CD-ROM called Chapter 8 Vary Sketch.sldprt, and edit Sketch2.
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 do this, then it cannot be used with the Vary Sketch option. In this case, the .40-inch dimension was used as the direction. 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.
To make the sketch react this way to changes in the dimension, the slot was created using the bi-directional 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. 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.
The Circular Pattern feature requires a straight edge, an axis, or a temporary axis to act as the center of the pattern. All of 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 8.12 was created using this technique.
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. An interesting thing about the Curve Driven Pattern is that it can have a Direction 2, and Direction 2 can also be a curve. This pattern type is one of the most interesting, with many options available.
For an entire sketch to be used as a curve, the sketch must not have any sharp corners—all of the entities must be tangent. This could mean using sketch fillets or a fit spline. The example shown in Figure 8.13 is 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 of the pattern instances aligned in the same direction.
Figure 8.14 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 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 8.15. 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 CD-ROM with the filename Reference 3d Curve Driven.sldprt.
Using a Direction 2 for a curve-driven pattern will create a result similar to that in Figure 8.16. 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.
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 8.17 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.
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 8.18.
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 through the menus at Insert, Reference Geometry, Coordinate System. 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 8.19.
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 pre-set 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 8.20.
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.
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 design 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.
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. 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 8.21 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.
In future version of SolidWorks, these features will hopefully be outfitted with more complete merge and feature scope functionality, such as Extrude features.
Note
Mirroring bodies is the fastest and simplest method when a part has complete symmetry. However, this may not be an option if the part is not completely symmetrical. Also, the decision to mirror must often be made when you are creating the first feature. If the first feature is modeled as a sketch that is built symmetrically around the Origin, then you may need to cut the part in half in order to mirror it. This is an adequate modeling technique, although it is not as clean as it could be.
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. If possible, it is better to mirror bodies than features, but you should not go too far out of your way or model in an unnatural, contrived manner in order to make this happen.
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 of 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, which have not been covered yet in this book.
Note
Configurations are covered in detail in Chapter 10.
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 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, cosmetic threads, and surface bodies. Sketches and features are two commonly requested items to be brought forward by the Mirror Part command, but this is not possible in the current version of the software.
Follow these steps to get practice with creating circular pattern features:
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.
Pre-select the top face of the block and start the Hole Wizard. (Pre-selection avoids a 3D placement sketch.) Select a counterbored hole for a 10-32 socket head cap screw, and place it as shown in Figure 8.22.
Create an axis using the Front and Right planes. Click Insert
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.
In the Features To Pattern panel, select the counterbored hole. Make sure that Geometry Pattern is turned off.
Click OK to finish the part, as shown in Figure 8.23.
Follow these steps to get some practice with creating mirror features:
Open the file from the CD-ROM called Chapter8 Tutorial2.sldprt.
Open a sketch on the side of the part, as shown in Figure 8.24. The straight line on top is 1.00 inch long, and the angled line ends 2.70 inches from the edge, as shown.
Click the Rib tool on the Features toolbar or select it from the menu at Insert
Create a linear pattern using the rib, making it go 2 inches into the part.
Create a chamfer on the same side of the part as the original rib, as shown in Figure 8.26. The chamfer is an Angle-Distance using 60° and .5 inches.
Create a round hole, sized and positioned as shown.
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 8.27.
Feature patterns and mirrors are powerful tools, but they require 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.