USING DRAFT IN THE RIB FEATURE

When you create ribs, you almost always apply draft to them. You can apply draft as a separate feature, or you can apply draft as a part of the Rib feature. It's often easier to just do it as part of the Rib feature, but some people like to make all their drafts as separate Draft features to keep the part faces orthogonal for as long as possible, or they just like to organize all the Draft features into a folder at the end of the FeatureManager so that there's never any question about which feature controls the draft.

By default, when you apply draft as a part of the Rib feature, the draft is applied from the sketch end of the rib. This can cause rib thickness problems if you have created a skyline rib where the rib may have various heights. In this case, the top of the rib will vary in thickness, and it may cause the base of the rib to be too thick. When you work this way, sometimes you have to experiment with the proper thickness at the top of the rib in order to get a thickness at the bottom of the rib that doesn't cause sink marks on the outside face of the part. A solution to this is to use the At Wall Interface option, which appears only after you enable Draft in the PropertyManager. Then you can specify the thickness and draft so that the base of the rib maintains a specified thickness.

USING INTERSECTION CURVES AS REFERENCES

Ribs are features that typically go inside hollowed-out parts. For that reason, they're often difficult to visualize, especially when they're on a plane that is deep down inside a part. You may find it useful to use some sort of a reference that shows where the current sketch plane intersects the wall of the part. For this, I typically use intersection curves. This technique can be used in either plan view or skyline-type ribs.

The Intersection Curve tool is on the Sketch toolbar. While in a 2D sketch, activate the tool and then select faces that intersect the current sketch plane. Deactivate the tool when you're finished. You may want to select all the lines selected by the Intersection Curve tool and turn them into construction geometry. This provides a good reference for the rib sketch without interfering with the Rib feature.

Figure 38.7 shows an example of using an intersection curve as a reference for setting up a rib sketch. The construction lines at the ends and below the right end of the skyline rib sketch are intersection curves.

At the ends of the shell, the intersection curves serve to give the sketch a reference point to be fully defined. Under the right end of the rib sketch, the intersection curve gives you a reference to dimension the height of the rib in the shallower section of the part. The part shown in Figure 38.7 is in the download material, with the filename Chapter 38 – skyline.sldprt.

TERMINATING RIBS

The Rib feature automatically extends and trims ribs based on your rib sketch. This is a great ease-of-use function, but it tends to lead to sloppy sketching for Rib features. If you sketch a rib and the sketch doesn't lead all the way to the wall of the part, SolidWorks extends it. If your sketch line goes past the wall, SolidWorks trims the rib so that it only goes up to the wall of the part. Figure 38.8 shows how the two straight ribs are extended from the existing sketches on a pair of plan view ribs.

Sometimes, you don't want a rib extended to the wall of the part. You may want to terminate a rib at a specific location in the middle of the part. The way to do this is to use a skyline rib and end the skyline sketch with a vertical (plus or minus draft) line that points to the base of the part. Figure 38.9 shows how to accomplish this. Notice that on the left end of the rib, it's extended straight down to the bottom of the part, and on the right side of the rib, it's extended up to the next wall.

A final termination situation I want to mention is one that can sometimes happen at curved edges. If the extension of the rib cannot be contained by the model, the rib will fail. This situation isn't always as obvious as you might think. When a nonhorizontal rib intersects a curved edge, it usually forces you to fake something a little. Figure 38.10 shows an example of why this happens.

The reason for the error shown in Figure 38.10 is that even though the rib sketch intersects the edge of the part, the width of the top of the rib would go past the edge and not intersect anything. One way to deal with this is to make the sketch intersect the part a little closer to the center of the part from the edge.

USING THIN FEATURES

Thin Feature extrusions are sometimes used in place of ribs. Thin features don't have all the specialized options available with the Rib feature, but they do offer simplicity as the main attraction. Thin features can substitute for Rib features when the rib is a stand-alone rib that doesn't touch the side walls of the part. They can be used to sketch and extrude from the bottom of the rib or from the top. When extruding a thin feature with draft, the end (thickness) faces get drafted as well, which might cause a problem if you are trying to attach the rib to a wall. Extruding a thin feature down from the top of the rib can replace a plan-view rib, but it won't enable you to break sketch rules like the plan-view rib.

I personally prefer to use Rib features, except for freestanding ribs where you don't want the sides extended up to the next wall.

NEUTRAL PLANE DRAFT

The workflow for Neutral Plane draft is as follows:

1. Select Neutral Plane (the plane or planar face at which the intersection of the drafted face doesn't move). The direction of pull is always normal to the neutral plane.
2. Set the draft angle (how many degrees from the direction of pull vector the selected faces should be tilted). This is not a cumulative angle, so applying 3 degrees of draft to a face that is already drafted 5 degrees results in 3 degrees rather than 8 degrees.
3. Select the Direction (one side or the other side of the neutral plane). The arrow points in the direction of decreasing material. If you're drafting a surface body, the “decreasing material” concept doesn't apply, so you just have to experiment to see which direction is the one you intend. The Draft feature doesn't have a preview option.
4. Select the faces to draft using Face Propagation options. Inner/Outer faces refer to inside or outside loops around the Neutral Plane face. All means that all faces that have an edge on the Neutral Plane face.

PARTING LINE DRAFT

The workflow for Parting Line draft is as follows:

1. Select a direction of pull. This can be an edge, axis, sketch line, plane, or planar face. You also have to set the direction to positive or negative along the selected direction.
2. Select the parting lines. These are edges of the faces you want to draft. The parting line edges remain stationary while the rest of the face tilts. Along with the parting line selection, you may also need to use the Other Face option. Every edge is adjacent to two different faces. The Draft feature automatically selects the face it thinks you want to draft, but it doesn't always get it right. The Other Face option enables you to intervene when the automatic selection is incorrect.
3. Set the draft angle. Remember that you can use the Allow Reduced Angle option if necessary.

STEP DRAFT

The most complex type of draft that SolidWorks creates is the Step draft. Step draft is used on nonplanar parting lines when Parting Line draft would cause the drafted faces to be split into multiple faces.

The word “step” can be said to refer to two different aspects of this feature. First, the parting line can be said to be a “stepped” parting line because it's nonplanar and at two different levels. Second, the draft actually steps out the drafted face at one level of the parting line. Step draft keeps the face intact and introduces an intentional mismatch ledge (step) at the parting line.

Figure 38.12 shows the difference between Parting Line draft and Step draft on a simplified part. The image on the left is the Parting Line draft. The middle image is Step draft, where a ledge is created only on one side of the parting line. The image to the right is essentially double Step draft, where the total step size is minimized by distributing it across both sides of the stepped parting line. The draft in these images is slightly exaggerated to make it easier to see.

The workflow for Step draft is as follows:

1. Start with a part that has a stepped split line, where the angled line makes angles of more than 90 degrees rather than less than 90 degrees.
2. Create a plane that defines the direction of pull and is located at the level of one of the split lines (for single Step draft) or at the midpoint of the angled line (for double Step draft). The location of the plane will determine the “pivot” point for the drafted faces. Essentially, the line of intersection between this plane and the drafted face will remain stationary and the rest of face will pivot around it.
3. Initiate the Draft feature and set the option to Step Draft. Consult your tooling people about whether to use tapered or perpendicular steps. Perpendicular steps are probably the easiest to tool.
4. Select the edges of the parting line. Make sure that the yellow arrows indicate the faces to which you want to apply draft.

The Step Draft feature can draft faces only on one side of the parting line at a time. Drafting the faces on the other side of the parting line doesn't require another Step Draft feature. You can use a Neutral Plane feature, using the plane created in step 2 as the neutral plane. It maintains the steps created by the Step Draft feature.

SOME DRAFT LIMITATIONS

One important limitation of draft in SolidWorks is that it cannot draft faces in both directions in the same feature. For example, if you have a parting line on a part, you must first draft the faces on one side of the parting line and then the faces on the other side of the parting line. This results in two separate Draft features rather than one and is simply an inconvenience.

Another inconvenience that affects many features in addition to draft is that you can only draft faces from a single body at a time—an understandable limitation, but annoying and inconvenient.

The biggest limitation is that you can't draft a face if it has a fillet on one of its edges that runs perpendicular to the direction of pull. To get around this, you usually have to tinker with the feature order, or use the DraftXpert to place the draft where it should be. On imported parts, you might have to use FeatureWorks to remove the fillet or Delete Face to reintroduce the sharp corner.

You may sometimes find that draft doesn't work if you don't draft all faces that are tangent to one another. This is the situation where the fillet is on an edge that is roughly parallel to the direction of pull.

WHAT TO DO WHEN DRAFT FAILS

Part of the key to success with the Draft feature is that you have your expectations aligned with the actual capabilities of the software. If you recognize a situation where the draft cannot work, you may be able to correct the situation by changing feature order, combining Draft features into a single feature, breaking the draft into multiple features, or changing the geometry to be more “draft friendly.”

Sometimes, the Allow Reduced Angle option can be used for Parting Line draft. If you use this, follow it up with a draft analysis to make sure that you have sufficient draft in all areas of the model. This option enables the software to cheat somewhat in order to make the Draft feature work. The SolidWorks Help documentation actually has a more detailed explanation of when to use this option. I tend to just select it if a draft fails, particularly if the parting line used becomes parallel or nearly parallel to the direction of pull.

Draft can fail for a number of reasons, including tangent faces, small sliver faces, complex adjacent faces that cannot be extended, or faces with geometry errors. When modeling, it's best to minimize the number of breaks between faces. This is especially true if the faces will be drafted later. Generally, the faces you apply draft to are either flat faces or faces with single-direction curvature. You can't expect SolidWorks to draft anything you throw at it; you should try to give it good, clean geometry.

When Draft does fail for a reason that doesn't seem obvious to you, you should use the Check utility under the Tools menu and also try a forced rebuild (Ctrl+Q) with Verification On Rebuild turned on. The Check utility checks the model for geometry errors. Verification On Rebuild checks more rigorously for features intersecting the model incorrectly. Some features may fail with the option on that would not fail with it off. When this happens, there's something wrong with that feature that the simplified default error checking didn't catch.

DRAFTXPERT

DraftXpert is a tool used to create multiple Neutral Plane Draft features quickly. You can also use it to edit multiple drafted faces without regard for which features go to which faces.

USING MULTI-THICKNESS SHELL

Figure 38.14 shows the PropertyManager set up for a multi-thickness shell. In this case, the bottom of the bottle is 0.150-inches thick, while the rest of the bottle is 0.050-inches thick. The top of the bottle is selected so that it's open. If you don't select a face to be open, the bottle will simply be hollow with no openings. The image on the right in Figure 38.14 shows half of the bottle in Wireframe display to help you visualize the thickness differences. To get a better view of this model, you can find it in the download materials, with the filename Chapter 38 – creased bottle.SLDPRT.

An important part of using the Multi-Thickness settings is to remember that SolidWorks can't assign different thicknesses to faces that are connected by tangency. All the adjacent tangent faces must have the same thickness. Another way to say this is that adjacent faces that are to have different thicknesses must not be tangent to one another. The reason for this is that SolidWorks cannot transition between two thicknesses when the two faces are tangent.

USING SHELL OUTWARD

Shell Outward is another option, and it is especially useful for bottles. You may be more interested in modeling the contents of a container than the actual container. To help you visualize this idea, think of modeling a liter of frozen water—not the bottle, just water frozen in the shape of the inside of the bottle. Now that you have the contents, you want to create the bottle. This is what the Shell Outward option is meant to do. Figure 38.15 shows the result, where the inside is the original modeled shape and the bottle shown on the outside was “grown” by the Shell Outward option.

Figure 38.16 shows one of the trickier usages of the Shell feature. This figure shows a planter tray that's manufactured by thermoforming. It may be difficult to tell how to model a part like this, because it could be shelled from either side—the top or the bottom.

In this part, several faces were removed in the Shell feature, which you may not think of doing with the conventional examples used to show this function, but it works very well for cases like this, especially thermoformed type parts.

Open the file called Chapter 38 – potting tray.SLDPRT from the download materials. The final feature is used to allow you to better visualize the effects of the shell.

UNDERSTANDING THE SHELL WORKFLOW

The workflow for using the Shell feature to produce the potting tray part goes like this:

1. Create a solid part where one side of the solid represents the faces of the finished model. The other side may be a simple block. Figure 38.17 shows the model before applying the Shell feature.

   

2. Initiate the Shell command. In the Faces To Remove selection box, select all the faces that should be removed or that will become thickness faces. This should amount to the six faces of the block sitting on top of the tray.
3. Use the Show Preview option if you are having difficulty visualizing the result. Be aware that this option may slow down the operation of the software while the Shell PropertyManager is open, but it will help you see the result based on your current selection.

BASIC

The Basic draft analysis (with no options selected) simply colors faces red, green, or yellow. Colors may display transitioning if the draft shifts between two classifications. This transition type is shown in Figure 38.21 in the image to the right. For a clearer view of this method, look at the Chapter 38 Draft Analysis.sldprt part in the download materials.

You can perform all types of draft analysis in SolidWorks by selecting a reference flat face or plane and setting a minimum allowable angle. In Figure 38.21, all walls have at least a 1-degree draft, except for the rounded edge shown in the image to the right and the dome. Both of these shapes transition from an angle less than 1 degree to an angle greater than 1 degree.

This basic analysis is good for visualizing changes in draft angle, but it also has some less desirable properties, which become apparent as you study the other types of draft.

GRADUAL TRANSITION

Although the Basic draft analysis can show a transitioning draft, the Gradual Transition draft analysis takes it a step further. With the Gradual Transition draft, you can specify the colors. It's also useful because it can distinguish drafts of different amounts by color. It may be difficult to tell in the grayscale image in Figure 38.22, but the ribs, which were created at 1 degree, have a slightly different color than the floor of the part, and the walls also have a different color. Notice that cavity and core directions have different colors as well (called Positive and Negative draft in the draft analysis). You may want to open this part in SolidWorks, re-create the settings, and run the analysis so you can see the actual colors.

Some problems arise when you use this Display mode, the first being the flat, non-OpenGL face shading that's used to achieve the transitioning colors. This often makes it difficult to distinguish curved faces and faces that face different directions. The second problem is that you cannot tell that the boss on top of the dome has absolutely no draft. In fact, there's no way to distinguish between faces that lean slightly toward the cavity and faces that lean slightly toward the core. The third problem is the strange effect that appears on the filleted corners. The corners were filleted after you applied the draft and before the shell, so the filleted corners should have exactly the same draft as the sides; however, from the color plot, it looks to be a few degrees more.

FACE CLASSIFICATION

Face Classification draft analysis groups the faces into classifications using solid, nontransitioning colors. You'll notice a big difference between the coloration of the Face Classification draft analysis faces and of the Basic or Gradual Transition faces. Face Classification uses OpenGL face shading, which is the same as that used by SolidWorks by default. This allows for better shading and differentiation between faces that face different directions. The Basic Analysis coloration looks like all the faces are painted the same flat hue, regardless of which direction they are facing, which makes shapes more difficult to identify. The non-OpenGL alternative shading method makes it possible to display a transition in color. SolidWorks OpenGL shading cannot do this.

Another advantage of using the OpenGL shading is that the face colors can remain on the part after you have closed the Draft Analysis PropertyManager.

Face Classification draft analysis also adds a classification that isn't used by the Basic draft analysis. The term straddle faces refers to faces that straddle the parting line, or faces that, due to their curvature, pull from both directions of the mold. These are faces that need to be split. On this part, a straddle face is shown in Figure 38.23.

The light bulb icons to the left of the color swatches enable you to hide faces by classification. This is useful when you're trying to isolate certain faces or visualize a group of faces in a certain way. This can be an extremely useful feature, especially when you have a very complex part with a large number of faces, some of which may be small and easily lost in the mix with other larger faces.

The face counts that appear in the color swatches are very helpful features that are absent from the Basic draft analysis. Consider using DraftXpress for situations where you have to add draft to models, as it has built-in draft analysis.

FIND STEEP FACES

A steep face is defined as a face that transitions from less than the minimum angle to more than the minimum angle. Steep faces are different from straddle faces in that straddle faces are actually positive and negative, while steep faces are either entirely positive or entirely negative. On this part, the dome inside the part is classified as a steep face, as shown in Figure 38.24.

UNDERSTANDING THE DRAFT ANALYSIS WORKFLOW

The workflow for the Draft Analysis tool is as follows:

1. Open a part for which you want to analyze the draft.
2. Select View ➢ Display ➢ Draft Analysis, or select it from the Evaluate tab of the CommandManager.
3. Select a plane or planar face for the direction of pull, and then set the options you want to use to visualize the draft on your part. The draft colors display immediately after you select the direction of pull.
4. If you want to keep the colors on while you work, click the green checkmark icon. The Draft Analysis icon on the toolbar and menu will display as selected. If you don't want to see the colors anymore, click the red X icon. If you click the green checkmark icon and then later want to turn off the Draft Analysis display colors, you must deselect the Draft Analysis icon in the toolbar or menu.

USING THE SHOW THIN REGIONS OPTION

The Show Thin Regions option, or the Thinness Analysis, requires you to input a minimum acceptable thickness. Every face with a thickness above this value is turned a neutral gray, and every face with a thickness below this value is displayed on a graduated scale.

Figure 38.25 shows the PropertyManager for this analysis and its result on the same part used for the draft work in the preceding sections.

One of the things to watch out for here is that some anomalies occur when you apply this analysis to filleted faces. The faces shown as colored were created by the Shell feature and should be exactly 0.100 inches thick. However, it does correctly represent the undercut on the end of the part and the thickness of the ribs. A nice addition to this tool would be the identification of minimum thickness faces. Perhaps you can submit an enhancement request.

USING THE SHOW THICK REGIONS OPTION

The Show Thick Regions option works a little differently from Show Thin Regions. You need to specify an upper-thickness limit value, beyond which everything is identified as too thick. In these examples, the nominal wall thickness of the part is shown as .100 inches, and the thick region limit is set to .120 inches. For this type of analysis, the color gradient represents the thicknesses between .100 inches and .120 inches, while in the Thinness Analysis, the color gradient represents the values between .100 inches and 0 inches.

The analysis can produce some anomalous results, especially at the corners and also in the middle. Again, this is a useful tool, if not completely accurate. You can use it to find problem areas that you may not have considered, but you should certainly examine the results critically.

This feature can generate a report, which to some extent answers questions about how or why it classifies faces in the way it does. To get a complete picture of the situation, it may be useful to look at the report when you are using the results to make design or manufacturing decisions. A sample of the report is shown in Figure 38.26.

UNDERSTANDING THE THICKNESS ANALYSIS WORKFLOW

The workflow for the Thickness Analysis tool is as follows:

1. Open a thin-walled part with some variations in thickness.
2. Start the Thickness Analysis tool by selecting Tools ➢ Thickness Analysis or by clicking the icon on the Evaluate tab of the CommandManager.
3. Select the Thin or Thick Regions option, depending on what you are most concerned about.
4. For a Thin Region analysis, enter the lowest acceptable thickness. For a Thick Region analysis, enter the low and the high acceptable thickness values.
5. (Optional) Select individual faces for local analysis in the Performance/Accuracy panel. This will also give you the option to get a more accurate display. The default is the least accurate option. Accuracy comes at the cost of longer analysis time.
6. Click Calculate. This calculation may take a few seconds or longer, depending on the complexity of your part. It isn't an instantaneous display.
7. Observe the color gradient on the faces. Blue indicates that the wall is too thin, and red indicates that it's too thick.