Manipulating Curves

Curves cannot be mirrored, moved, patterned, or manipulated in any way. (A workaround for this may be to use Convert Entities to create a sketch from the curve, or to create a surface using the curve, and pattern or mirror the surface, using the edge of the surface in place of the curve feature.)

Working with Helix Curve Features

The Helix curve types are all created from a sketch circle. The circle represents the starting plane, center, and diameter of the helix. Figure 8.1 shows the PropertyManagers of the Constant Pitch and Variable Pitch helix types.

You can create all the helical curve types by specifying some combination of total height, pitch, and the number of revolutions. The start angle depends on the relation of the sketch plane to the origin. The start angle can be controlled outside of the PropertyManager through dimensions, design tables, equations, and so forth. The term pitch refers to the straight-line distance along the axis between the rings of the helix. Pitch for the spiral is different and is described later.

USING THE TAPER HELIX PANEL

The Taper Helix panel in the Helix PropertyManager enables you to specify a taper angle for the helix. The taper angle does not affect the pitch. If you need to affect both the taper and the pitch, you can use a Variable Pitch helix. Figure 8.2 shows how the taper angle relates to the resulting geometry.

USING THE VARIABLE PITCH HELIX

You can specify a Variable Pitch helix either in the chart or in the callouts that are shown in Figure 8.3. Both the pitch and the diameter are variable. The diameter number in the first row cannot be changed but is driven by the sketch. In the chart shown, the transition between 4 and 4.5 revolutions is where the pitch and diameter both change.

When you double-click a helix feature, SolidWorks displays the dimensions on the screen, which you can then double-click and change. The dimensions displayed this way aren't as organized as when using the PropertyManager, but it may be more convenient.

USING THE SPIRAL

A spiral is a flattened (planar) tapered helix. The pitch value on a spiral is the radial distance between revolutions of the curve. (See Figure 8.4.)

Creating Projected Curves

There are two types of projected curves:

• Sketch On Faces
• Sketch On Sketch

These names can be misleading if you do not already know what they mean. In both cases, the word sketch is used as a noun, not a verb, so you are not actively sketching on a surface; instead, you are creating a curve by projecting a sketch onto a face.

USING SKETCH ON FACES

With this option set, the projected curve is created by projecting a 2D sketch onto a face. The sketch is projected normal (perpendicular) to the sketch plane. The sketch can be an open loop or a closed loop, but it may not be multiple open or closed loops, nor can it be self-intersecting. Figure 8.5 shows an example of projecting a sketch onto a face to create a projected curve.

USING SKETCH ON SKETCH

The easiest method to use for visualizing Sketch On Sketch projected curves is the Intersecting Surfaces method. In this method, you can see the curve being created at the intersection of two surfaces that are created by extruding each of the sketches. This method is shown in Figure 8.6.

Using the Curve Through XYZ Points Feature

The Curve Through XYZ Points feature enables you to either type or import a text file with coordinates for points on a curve. The text file can be generated by any program that makes lists of numbers, including Excel. The curve reacts like a default spline, so the teeter-tottering effect may be noticeable, especially because you cannot set end conditions or tangency. To avoid this effect, it may be a good idea to overbuild the curve by a few points on each end or to have a higher density of points.

If you import a text file, the file can have an extension of either *.txt or *.sldcrv. The sample data file Chapter 8 - Curve File.sldcrv is in the download material. The data that it contains must be formatted as three columns of X-, Y-, and Z-coordinates using the document units (inch, mm, and so on), and the coordinates must be separated by a comma, space, or tab. Figure 8.7 shows both the Curve File dialog box displaying a table of the curve through X, Y, and Z points, and the *.sldcrv Notepad file. You can read the file from the Curve File dialog box by clicking the Browse button; but if you manually type the points, then you can also save the data out directly from the dialog box. Just like any type of sketch, this type of curve cannot intersect itself.

Using the Curve Through Reference Points Feature

The Curve Through Reference Points feature creates a curve entity from selected sketch points or vertices. The curve can be an open loop or a closed loop, but a closed loop requires that you select at least three points. You cannot set end conditions of the curve, so this feature works like a default spline in the same way as the XYZ curve.

The most common application of this feature is to create a wire from selected points along a wire path. Another common application is a simple two-point curve to close the opening of a surface feature such as Fill, Boundary, or Loft. One drawback in that regard is that the end tangency directions cannot be controlled on curve features. If a 3D sketch spline is used, end tangency direction is controlled easily through the use of spline handles and tangency to construction geometry. Curve Through Reference Points is largely unused, probably because 3D sketch splines are so much more powerful.

Putting Together a Composite Curve

A composite curve joins multiple curves, edges, or sketches into a single curve entity. The spring shown in Figure 8.8 was created by using a composite curve to join a 3D sketch, Variable Pitch helix, and projected curve. You can also use model edges with a composite curve. The curve is shown on half of the part; the rest of the part is mirrored. Curves cannot be mirrored, but solid/surface geometry can.

Composite curves overlap in functionality with the Selection Manager to some extent. In some ways, the composite curve is nicer because you can save a selection in case the creation of the feature that uses the Selection Manager fails. (If you can't create the feature, you can't save the selection.) On the other hand, composite curves don't function the same way as a selection of model edges for settings like tangency and curvature.

Using Split Lines

Split lines are not exactly curves; they are just edges that split faces into multiple faces. Split lines are used for several purposes, but they are primarily intended to split faces so that draft can be added. They are also used for creating a broken-out face for a color break or to create an edge for a hold-line fillet, as discussed in Chapter 7, “Modeling with Primary Features.”

There are some limitations to using split lines. First, they must split a face into at least two fully enclosed areas. You cannot have a split line with an open-loop sketch where the ends of the loop are on the face that is to be split; they must either hang off the face to be split or be coincident with the edges. If you think you need a split line from an open loop, try using a projected curve instead.

Using the Equation-Driven Curve

An equation-driven curve is not really a curve feature; it is a sketch entity. It specifies a spline inside a 2D sketch with an actual equation. Even though this is a spline-based sketch entity, it can be controlled only through the equation and not by using spline controls. This feature is covered in more detail in Chapter 3, “Working with Sketches and Reference Geometry,” with other sketch entities.

Using Scale

The Scale feature, found at Insert ➢ Feature ➢ Scale, is mainly used for preparing models of plastic parts to make mold cavity geometry; however, it can be used for any purpose on solid or surface geometry. Scale does not act by scaling up dimensions for individual sketches and features; rather, it scales the entire body at the point in the FeatureManager history at which it is applied. The Scale PropertyManager is shown in Figure 8.9.

The Scale feature becomes available only when the part contains at least one solid or surface body. You can scale multiple bodies at once and select from one of three options for the Scale About setting or fixed reference: the part origin, the geometry centroid, or a custom coordinate system. Of these, it is generally preferable to select the part origin because you most often want the standard planes moving with respect to the rest of the part as little as possible. If you needed to scale about a specific point on the geometry, you would need to create a custom coordinate system at that point and use that as the reference.

The Scale Factor works like a multiplier, so if you want to double the length, you would enter the Scale Factor 2. This does not work like the Scale function in the Cavity feature, which is less commonly used. Scale within Cavity uses a scale factor that is shown as a percentage increase, so to double the linear dimensions of a part would require a scale factor of 100 percent. The Cavity feature is available only in the context of an assembly and has fallen out of favor with most mold designers.

Scale is also configurable, meaning that different configurations can use different scale factors. Configurations are covered in Chapter 11, “Working with Part Configurations.”

An interesting aspect of the Scale feature is that you can disable the Uniform Scaling option. This allows you to apply separate scale factors for the X, Y, and Z directions. In mold making, this can be used if you have a fiber-filled material and the mold requires differential shrink compensation based on the direction of plastic flow, and thus of fiber alignment (the part will shrink less in the direction of fiber alignment). But you could also use it to size any general part. Just remember that if you apply differential scale, circles may be distorted. To get around this, you may be able to reorder the features to apply the Scale feature before the circular features are added.

Because Scale is simply applied to the body rather than to features and sketches, it can be applied to imported parts as well as SolidWorks native parts. Sometimes, people use the Scale feature to compensate for improper imported units. For example, if a part was originally built in inches and translated in millimeters, you might want to scale the part by a factor of 25.4. You can also enter an expression in the Scale Factor box so that if the import units error went the other way, you could scale a part down by 1/25.4. The limitation to the Scale feature is that the SolidWorks modeling space for a single part is a box that’s approximately 500 to 700 meters centered about the origin. There appears to be some difference between sketching limits and 3D solid limits.

An implication of the Scale feature that is not stated outright is that it does not scale features, sketches, or dimensions. It is a history-based feature, so the size difference only applies after the Scale feature in the tree.

Using the Dome Feature

The Dome feature in SolidWorks is generally applied to give some shape to flat faces or an area of a flat face. A great example of where a dome fits well is the cupped bottom of a plastic bottle or a slight arch on top of buttons for electronic devices. Domes can add or remove material.

Until SolidWorks 2010, another very similar feature existed, which was called Shape. You can no longer make Shape features, but you may run into one from time to time in old parts. If you find a Shape feature on an old part, it will continue to function unless any of its parent geometry changes. Shape features do not update in SolidWorks 2010 or later. SolidWorks recommends you re-create the geometry as another feature, possibly a Dome or Freeform feature. Included in the sample parts for Chapter 8 is a part called Chapter 8 Domes.sldprt; this part is shown in Figure 8.10. Opening this part will allow you to see the error that appears when you open a part with a Shape feature. The part also demonstrates several ways in which Dome features can be used.

The Dome feature has several attributes that either help it qualify for a given task or disqualify it. These attributes can help you decide if it will be useful in situations you encounter:

• The Dome feature can create multiple domes on multiple selected faces in a single feature, although it creates only a single dome for each face.
• Using the Elliptical Dome setting, Dome can create a feature that is tangent to the vertical.
• Dome can use a constraint sketch to limit its shape.
• Dome works on nonplanar faces.
• Dome cannot establish a tangent relationship to faces bordering the selected face.
• Dome cannot span multiple faces.
• Dome displays a temporary untrimmed four-sided patch that extends beyond the selected face when you use it on a non-four-sided face.
• Dome functions only on solids, not on surfaces.

The Dome feature has two notable settings: Elliptical Dome and Continuous Dome.

The Elliptical Dome is available only on flat faces where the boundary is either a complete circle or an ellipse. The cross section of the dome is elliptical and does not account for draft, which means that it is always tangent to the perpendicular from the selected flat face.

Continuous Dome is a setting for any noncircular or elliptical face, including polygons and closed-loop splines. The setting results in a single unbroken face. If you deselect the Continuous Dome setting, it functions like the Elliptical Dome setting. Figure 8.10 shows the most useful settings for the Dome feature.

The workflow for the Dome feature is as follows:

1. Select an area to be domed, or use a split line to create an area to be domed on an existing face.
2. Initiate the Dome feature, set a height, tell it to add or remove material, and set the other settings including the constraint sketch.
3. Accept the feature with the green checkmark icon.

Using the Wrap Feature

The Wrap feature enables you to wrap 2D sketches around analytical or complex faces. Trying to wrap around 360 degrees can cause some difficulties, so you might try that sort of thing in two steps, either with two wraps or a combination of features.

The Wrap feature works by flattening the face, relating the sketch to the flat pattern of the face, and then mapping the face boundaries and sketching back onto the 3D face. It is not a simple projection; it actually does wrap the sketch onto curved faces. Figure 8.11 shows the Wrap PropertyManager interface along with a Wrap onto a cylinder and a Wrap onto a complex shape. The complex wrap is available in the download materials for this chapter (see Complex Wrap.sldprt).

The Wrap feature has three main options:

• Emboss
• Deboss
• Scribe

Wrap can be placed on analytical (cylindrical, conical, and the like) or complex spline surfaces (lofts, sweeps, etc.).

USING SCRIBE

Scribe is the simplest of the options to explain, and understanding it can help you understand the other options. Scribe creates a split line–like an edge on the face.

Several requirements must be met in order to make a wrap feature work:

• The face must be a cylindrical or conical face.
• The loop must be a closed-loop or nested-closed-loop 2D sketch.
• The sketch must be on a plane that is either tangent to or parallel to another plane that is tangent to the face.
• Wrap supports wrapping onto multiple faces.
• The wrap should not be self-intersecting when it wraps around the part. (Self-intersection will not cause the feature to fail, but on the other types, Emboss and Deboss, it may produce unexpected results.)

Scribes can be created on solid or surface faces. Scribed surfaces are frequently thickened to create a boss or a cut. Figure 8.12 shows a scribed wrap.

Using the Flex Feature

The Flex feature is different from most of the other features in SolidWorks. Most of them create new geometry, but Flex (and Deform, which follows) takes existing geometry and changes its shape. Flex can affect the entire part or just a portion of it. Flex works on both solid and surface bodies, as well as imported and native geometry as shown in Figure 8.13.

Flex has four main options and many settings. The four main options are as follows:

• Bending: This option establishes two trim planes to denote the ends of the bent area and specifies an angle or radius for the bend.
• Twisting: This option establishes two trim planes to limit the area of the twist and enters the number of degrees through which to twist.
• Tapering: This option establishes two trim planes to limit the area of the taper. The body is larger toward one end and smaller toward the other end.
• Stretching: This option establishes two trim planes to limit the area to be stretched. You can stretch the entire body by moving the trim planes outside of the body.

The part shown in the figure can be found in the download material under the filename Chapter 8 Flex.sldprt.

In some cases, the Triad and trim planes are slightly disoriented. The best thing to do in situations like this is to simply reorient the Triad using the angle numbers in the Triad panel of the PropertyManager. This is also a solution if the planes are turned in such a way that the axis of bending is not oriented to the bend that the part requires.

The Flex feature is very conscious of separate bodies. In some cases this can be helpful, but in default situations when there is only one body in the part, it can be annoying. Remember to select the body to be affected in the very first selection box at the top of the PropertyManager.

You can place the trim planes by selecting a model vertex, by dragging the arrow on the plane, or by typing in a number. Be careful when dragging the plane arrows because dragging the border of the plane drags the flex value for the feature. (Dragging the plane in a bending operation is like changing the angle or radius for the bend.)

Using the Triad can be very tricky. Moving the Triad in the Bending option moves the axis of the bend, so it determines whether the bend compresses or stretches the material. The position of the Triad also determines which side of the bent body moves or stays stationary, or if both sides move. Placing the Triad directly on a trim plane causes the material outside the bend on that side of the trim plane to remain stationary.

I highly recommend looking at the models provided with this chapter to examine the various functions of the Flex feature more carefully. The model uses configurations, which are covered in Chapter 11, “Working with Part Configurations.”

Applying the Deform Feature

Like the Flex feature, the Deform feature changes the shape of the entire model without regard to parametrics, features, history, or dimensions. Some software packages call this technique global shape modeling. Also like Flex, Deform works on surface bodies as well as solids. Deform can also handle imported geometry as well as SolidWorks native parts. Model complexity is not an issue unless the part runs into itself during deformation.

The Deform feature is another feature type that you may not use to actually design anything, but you may use to show a model in a deformed state.

Deform has three types:

• Point: This type deforms a portion of the model by pushing a point and the geometry around it.
• Curve To Curve: The most precise and useful deform type. This type selects an existing edge and forces the edge to match a curve.
• Surface Push: This type of deform, while conceptually a very interesting function, is nearly unusable in practice. The part is deformed into a shape vaguely resembling an intermediate shape between the existing state of the part and a “tool” body.

Figure 8.14 shows the PropertyManager interface for the Deform feature. The interface is different for each of the three main types, and it changes depending on selections within the individual types. The interface shown is for the Curve To Curve type because I believe this to be the most useful type.

LOOKING AT CURVE TO CURVE DEFORM

Because the Curve To Curve deform uses curve, sketch, or edge data, it is a more precise method than the other deform types. The main concept here is to transform a curve on the original model to a new curve, thereby deforming the body to achieve the new geometry.

The model shown in Figure 8.15 has been created using the Curve To Curve deform. The part starts as a simple sweep (sweep an arc along an arc), and then a split line is created to limit the deform to a specific area of the model. The model is in the downloaded files under the filename Chapter 8 Deform Curve to Curve.sldprt.

Using the Indent Feature

Indent uses the same ingredients as the Surface Push, but it produces a result that is more useful. For example, if you are building a plastic housing around a small electric motor, the Indent feature shapes the housing and creates a gap between the housing and the motor. Figure 8.16 shows the PropertyManager interface for the Indent feature, as well as what the indent looks like before and after using the feature.

In this case, the small motor is placed where it needs to be, but there is a wall in the way. Indent is used to create an indentation in the wall by using the same wall thickness and placing a gap of 0.010 inches around the motor. The motor is brought into the wall part using the Insert ➢ Part command. This is a multibody technique. Multibodies are examined in detail in Chapter 31, “Modeling Multibodies.”

It is possible to use Indent in mold applications; however, most mold designers will prefer to use the shrink percentage that you can get with the Scale/Cavity/Boolean operations rather than the discreet offset that Indent provides.

Using Intersect

Intersect combines the functionality of general solids Boolean operations, Trim Surface, Knit Surface, Split, Replace Face, and Cut With Surface. The tool does not appear to have any exclusive functionality, but it reduces the work to complete some tasks that used to take many steps with a combination of different tools. It is useful for determining the volume of “open” cavities. For example, the part file shown in Figure 8.17 is a multibody with solids and surfaces. The small part in the center is a knob. The big block around it is a mold block, currently a single piece. The four cylinders are surfaces representing alignment pins, and the cylinder in the center is an ejector sleeve. The Top plane goes through the center and represents the parting line of the mold. You can find this part file in the download material for Chapter 8 under the filename Chapter 8 - Intersect Example.sldprt.

The first step is to select all the entities involved. This is much like the Mutual Trim feature. In the Selections panel of the Intersect PropertyManager, select every solid, surface, and plane that will take part in the operation.

You have the option to cap open surfaces while doing this, but this example does not require it. If one of the holes was a blind hole, but the surface body was open inside the solid, that situation would require a capped surface.

In this example, the only thing about the feature that is not very elegant is that the Merge result is not selective. Perhaps you can think of it as being the split function that is not selective. Notice that the final feature in the tree is a Combine. This was necessary because the original part was split into pieces. You may argue that the original part should be consumed—in which case, I wouldn't have allowed the pieces to remain—but this kind of decision should be up to the individual user, not the programmer.

The Consume Surfaces option simply removes any surface bodies used in the operation.