When you use CAD programs, you typically create a part once, but edit it many times. Design for change is at the core of most of the modeling work that you will do in SolidWorks, and deletion is not an editing option.
The initial stages of modeling are the most crucial. This is when you set up parametric relations between the features and sketches that form the foundation for an assembly or complex part. For this reason, editing often quickly turns into repair. Granted, some changes are simply unavoidable, but a thorough knowledge of editing — and repairing — can help you to understand the how, what, and why of modeling best practice.
This chapter starts with some very basic concepts of editing, which you may have picked up if you have been reading this book from the beginning. Because this is the last chapter in Part II, and the last that deals strictly with part modeling, it also contains a summary of part modeling best practice techniques and a set of model evaluation tools that can help you evaluate the manufacturability and aesthetic properties of parts. I have included these evaluation tools in a chapter on editing because the create-evaluate-edit-evaluate cycle is one of the most familiar in modeling and design practice.
Rolling back a model simply means looking at the results of the design tree up to a certain point in the model history. In SolidWorks, you can actually change history — that is, you can change the order in which operations are completed. The order in which you create features is recorded, and if you change this order, you get a different geometric result.
You can use several methods to put the model in this rolled-back state:
Dragging the Rollback bar with the cursor.
Right mouse button (RMB) clicking and selecting one of the Rollback options.
Editing a feature other than the last one in the design tree. (SolidWorks rolls back the model automatically.)
Choose Tools
Saving the model while editing a feature or sketch, and then exiting the model. When the part is opened again, it is rolled back to the location of the sketch that was being edited.
Pressing Esc during a long model rebuild. This method is supposed to roll you back to the last feature that was rebuilt when you pressed Esc; however, in practice, I have rarely seen it do this, and it usually rebuilds the entire model anyway.
The Rollback bar, which typically appears at the bottom of the FeatureManager in SolidWorks part documents, enables you to put the part into almost any state in the model history. This is not the same as the Undo command, but is the equivalent of going back in time to change your actions, and then replaying everything that you did after that point. Figure 11.1 shows the Rollback bar in use. Notice how the cursor changes into a hand icon when you move it over the bar.
When you use a sketch for a feature such as a Sketch Driven Pattern, the sketch is left in the design tree, in the place where it was created. However, most other features, such as extrudes, consume the sketch, meaning that the sketch disappears from its normal order in the FeatureManager and appears indented under the feature that was created from it. Consumed sketches are sometimes also referred to as absorbed sketches.
In genealogical family tree diagrams, the parent-child relationship is represented with the parent at the top, and the children branched below the parent. In SolidWorks, parent-child relationships are tracked differently. Figure 11.2 shows the difference between a genealogical family tree and the SolidWorks design tree.
You can display the parent-child relations between SolidWorks features, as shown in Figure 11.2, by right-clicking on any feature and selecting Parent/Child. This helps you determine relationships before you make any edits or deletions because you can see which features will be removed or go dangling (lose their references).
When SolidWorks puts the child feature at the top, it is, in effect, turning the relationship upside down. In the SolidWorks FeatureManager, the earlier point in history is at the top of the tree, but the children are listed before than the parents. The SolidWorks method stresses the importance of solid features over other types of sketch or curve features.
For example, you create an extrude from a sketch, and, therefore, the sketch exists before the extrude in the FeatureManager. However, when you create the extrude, SolidWorks places the sketch underneath the extrude. This restructuring can become more apparent when a sketch (for example, Sketch1) is created early in the part history, and then not used to create a feature (for example, Extrude5) until much later. If you roll down the FeatureManager feature by feature, you arrive at a point at the end of the design tree where Extrude5 appears and Sketch1 suddenly moves from its location at the top of the tree to under Extrude5 at the bottom of the tree.
This scenario may cause a situation where many sketches and other features that are created between Sketch1 and Extrude5 are dependent on Sketch1, but where Sketch1 suddenly appears after all these other features. This can be difficult to understand, but is key to effectively editing parts, especially parts that someone else created.
The main point here is that SolidWorks displays many relationships upside down. You need to understand how to navigate and manage these history-bound relationships.
One way to get around difficulties in understanding the chronological order of features when compared against the relationship order of features is to roll back a model tree item by item. This can help you sort through the issues. Also remember that from SolidWorks's point of view, the solid feature is the most important item in the tree and is what the rest of the items in the tree support. SolidWorks has made the solid features easily visible and accessible in the tree.
Take an example such as a loft with guide curves. If you create the guide curves first, and then you create the loft profiles by referencing the guide curves, the loft automatically reorders these sketches when they display under the loft feature such that the profiles are listed in the order in which they were selected, followed by the guide curves in the order in which they were selected. This is shown in Figure 11.3. This restructuring can be confusing if you want to go back and edit any of the relationships between the sketches. You can find this example on the CD-ROM with the filename Chapter 11 Loftwgc.sldprt.
If you want to view consumed sketches in their original order — for example, the sketches in the loft feature in Figure 11.3 — you must first expand the feature by clicking the plus (+) symbol next to it so that you can see the consumed sketches, and then roll back between the feature and the first sketch. At this point, a warning message appears, stating that the sketches will be temporarily unabsorbed during editing. You can then move the Rollback bar again to show the sketches.
This maneuver can become complicated when you have two sketches absorbed by a projected curve, the projected curve absorbed by a composite curve and the composite curve absorbed by a sweep feature. To isolate the original projected sketches, you need to repeat the technique with the Rollback bar as described earlier, once for each parent/child relationship. This is shown in Figure 11.4, and the steps to accomplish it are as follows.
To view consumed sketches in their original order, follow these steps:
Expand the sweep.
Roll back between the sweep and the profile sketch.
Answer the prompt that appears.
Roll down so that you can see the unabsorbed sketches and curves.
Expand the composite curve.
Roll back to just after the composite curve.
Roll back so that you can see the contents of the composite curve.
Expand the projected curve.
Roll back to just after the projected curve.
Roll back so that you can see the contents of the projected curve.
The Rollback feature is located on the RMB menu. Simply right-click a feature and select either Rollback or Roll to Previous. If you are already rolled back and you right-click below the Rollback bar, you can access additional options to Roll Forward and Roll to End.
Editing any feature other than the last feature also serves to roll back the model while you are in Edit mode. As soon as you rebuild the feature or sketch, SolidWorks rebuilds the entire design tree.
The Tools
Warning
The one situation where this technique does not work as expected is when you are working on a part in the context of the assembly, with the design tree rolled back. The down arrow simply causes the Rollback bar to roll immediately to the end of the design tree.
The ability to reorder features is one that offers SolidWorks users control over the modeling process and its outcome. Without this capability, editing would not be one of the strengths of the software. As you already know, feature order can make a difference in the final shape of a part. For example, this order:
Extrude
Cut
Fillet
Shell
gives you a very different part from this order:
Extrude
Shell
Cut
Fillet
The results of these different orders are shown in Figure 11.5. (The part is split and partially transparent for demonstration purposes only.) You can view this part on the CD-ROM; it is filename Chapter 11 Reorder.sldprt.
On the part in the example shown in Figure 11.5, it is fairly simple to reorder the Shell feature by dragging it up the design tree. As a result, the well created by the Cut feature is not shelled around (to create a tube) if the cut comes after the shell. Also, notice the effect of applying the fillets after the shell rather than before it. The corners inside the box are sharp, while the outside corners have been filleted. When you apply the fillet before the shell, fillets that have a radius larger than the shell thickness are transferred to the inside of the shell.
If two adjacent features are to swap places, it generally does not matter whether you move one feature up the design tree or you move the other one down. However, there are isolated situations that are usually created by the nested, absorbed features discussed earlier, where one feature cannot go in one direction, but the other feature can go in the opposite direction, achieving the exact same result. If you run into a situation where you cannot reorder a feature in one direction even though it appears you should be able to, try moving another feature the other direction.
Note
While this behavior may appear to be a bug, it is more likely just a product of parent/child relationships hidden by the way SolidWorks reorders consumed parent sketches and other types of features. If you were able to stretch the FeatureManager out into a straight line from earliest to latest, the difficulties in reordering would become apparent.
There are times when, regardless of which features you choose to move and which direction you choose to move them in, you are faced with the task of moving many features. This can be time-consuming and tedious, not to mention have the potential to introduce errors. To simplify this process, you can put all the features to be moved into a single folder, and then reorder the folder. Keep in mind that the items in the folder need to be a continuous list (you cannot skip features), and you can only reorder the folder if each individual feature within the folder can be reordered.
Best Practice
Folders are frequently used for groups of features that go together and that may be suppressed or unsuppressed in groups. You can also use folders in assemblies. Folders are frequently used to group cosmetic fillet features that are often found at the end of design trees for plastic parts or for groups of hole features.
To create a folder, right-click a feature, or a selected group of features, and select Add to New Folder. Folders should be renamed with a name that helps identify their contents. You can reorder folders in the same way as individual features. When you delete a folder, the contents are removed from the folder and put back into the main tree; they are not deleted.
You can add or remove features to or from the folders by dragging them in or out. If a folder is the last item in the FeatureManager, the next feature that is created is not put into the folder; you must place it in the folder manually. You cannot drag features out of a folder and place them immediately after it, because they will just go back into the folder. If you want to pull a feature out of a folder and place it after the folder, there must be another feature between the feature that you are moving and the folder. However, you can pull a feature out of the folder and place it just before the folder.
The Flyout FeatureManager resides at the top-left corner of the graphics window. The PropertyManager goes in the same space as the FeatureManager, and is sometimes too big to allow this area to accommodate both managers in a split window.
The Flyout FeatureManager enables you to select items from the design tree when the regular FeatureManager is not available because it is covered by the PropertyManager. It usually appears collapsed, so that you can only see the name of the part and the part symbol. To expand it, click the plus icon next to the name of the part in the Flyout FeatureManager.
You can use the Flyout FeatureManager in parts or assemblies. However, you cannot use the Flyout FeatureManager to suppress or roll back the tree.
Cross-Reference
Other functionality and limitations of the Flyout FeatureManager that relate to its function in assemblies can be found in Chapters 12 to 15.
You can access the settings for the Flyout FeatureManager by choosing Tools
You may prefer not to work with the flyout FeatureManager because it interrupts your workflow by covering the regular FeatureManager with a PropertyManager. If this is the case, you can use the detachable PropertyManager instead. Detaching the PropertyManager removes the need for the flyout. I often dock the detachable PropertyManager where the flyout FeatureManager would go, or even use it undocked on a second monitor. The main advantage of using the detachable PropertyManager instead of the flyout FeatureManager is that with the detachable PropertyManager you don't have to re-locate features in the FeatureManager that were already in view.
Figure 11.6 shows the difference between the flyout FeatureManager on the left, and the detachable PropertyManager on the right. My preference is clearly the detachable PropertyManager. When you use this, everything is predictable, and you don't have to go hunting for features that were listed right in front of you when you do something that opens a PropertyManager. I usually decrease the overall size of the SolidWorks application window, and place the PropertyManager to the left of the SolidWorks application. This works best on a wide aspect monitor or multiple monitors. If you use a small monitor or a normal aspect monitor, using the Auto Collapse option with the PropertyManager docked to the right of the FeatureManager (where the flyout FeatureManager would otherwise go) is also a good option.
You may correctly ask "What's the difference?" The difference is that when you do something like editing a sketch plane, the current state of the FeatureManager is covered and replaced by the PropertyManager. You may have had the new plane you wanted to use in view. Especially with long FeatureManagers, in both parts and assemblies, when the flyout appears, you have to again scroll to find the plane that was right in view. However you use the detachable PropertyManager, I think you will find it an improvement over the flyout.
This section is a summary of best practice suggestions for modeling parts. Best practice lists are important because they lay the groundwork for usage of the software, which is helpful for new users and users who are trying to experiment with the limits of the software.
I believe that it is only after you respect the rules and understand why they are so important, that you know enough to break them. However, best practice lists should not be taken too seriously. They are not inflexible rules, but conservative starting places; they are concepts that you can default to, but that can be broken if you have good reason. Following is a list of suggested best practices:
Always use unique filenames for your parts. SolidWorks assemblies and drawings may pick up incorrect references if you use parts with identical names.
Using Custom Properties is a great way to enter text-based information into your parts. Users can view this information from outside the file by using applications such as Windows Explorer, SolidWorks Explorer, and Product Data Management (PDM) applications.
Learn to sketch using automatic relations.
Use fully dimensioned sketches when possible. Splines are often impractical to fully dimension.
Limit your use of the Fixed constraint.
When possible, make relations to sketches or stable reference geometry, such as the Origin or standard planes, instead of edges or faces. Sketches are far more stable than faces, edges, or model vertices, which change their internal ID at the slightest change and may disappear entirely with fillets, chamfers, split lines, and so on.
Do not dimension to edges created by fillets or other cosmetic or temporary features.
Apply names to features, sketches, and dimensions that help to make their function clear.
When possible, use feature fillets and feature patterns rather than sketch fillets and sketch patterns.
Combine fillets into as few fillet features as possible; this also enables you to control fillets that need to be controlled separately — such as fillets to be removed for Finite Element Analysis (FEA), drawings, and simplified configurations — or added for rendering.
Create a simplified configuration when building very complex parts or working with large assemblies.
Model with symmetry in mind. Use feature patterns and mirroring when possible.
Use link values or global variables to control commonly used dimensions.
Do not be afraid of configurations. Control them with design tables where there are more than a few configs, and document any custom programming or automated features in the spreadsheet for other users.
Use display states when possible instead of configurations.
Use multi-body modeling for various techniques within parts; it is not intended as a means to create assemblies within a single part file.
Cosmetic features — fillets, in particular — should be saved for the bottom of the design tree. It is also a good idea to put them all together into a folder.
Use the Tools
Always fix errors in your part as soon as you can. Errors cause rebuild time to increase, and if you wait until more errors exist, troubleshooting may become more difficult.
Troubleshoot feature and sketch errors from the top of the tree down.
Do not add unnecessary detail. For example, it is not important to actually model a knurled surface on a round steel part. This additional detail is difficult to model in SolidWorks, it slows down the rebuild speed of your part, and there is no advantage to actually having it modeled (unless you are using the model for rapid prototype or to machine a mold for a plastic part where knurling cannot be added as a secondary process). This is better accomplished by a drawing with a note. The same concept applies to thread, extruded text, very large patterns, and other features that introduce complex details.
Do not rely heavily on niche features. For example, if you find yourself creating helices by using Flex/Twist or Wrap instead of Sweep, then you may want to rethink your approach. In fact, if you find yourself creating a lot of unnecessary helices, then you may want to rethink this approach as well, unless there is a good reason for doing so.
File size is not necessarily a measure of inefficiency.
Be cautious about accepting advice or information from Internet forums. You can get both great and terrible advice from people you don't know, along with everything in-between. Sometimes even groups of people can be dead wrong. Get someone you trust to verify ideas, and as always, test them on copied data to determine if they're effective.
If you are the CAD Administrator for a group of users, you may want to incorporate some best practice tips into standard operating procedures for them. The more users that you manage, the more you need to standardize your system.
Cross-Reference
Best practice development is covered at length in the SolidWorks Administration Bible (Wiley, 2009).
You can use evaluation techniques to evaluate geometry errors, demonstrate the manufacturability of a given part, or to some degree quantify aesthetic qualities of a given part, or section of a part. I discuss evaluation techniques here because the design cycle involves iterations around the combination of create-evaluate-edit-evaluate functions. I discuss the following techniques in this section:
Verification on rebuild
Check
Zebra Stripes/RealView/Lights and specularity
Curvature display
Deviation analysis
Tangent Edges as Phantom
Geometry Analysis
Feature statistics
Curvature comb
SimulationXpress
Many of these techniques apply specifically to plastic parts and complex shapes, but even if you do not become involved in these areas of design or modeling, these tools may help you to find answers on other types of models as well.
In SolidWorks 2010, a new tab, Evaluate, appears on the default Command Manager. You can use the commands on this tab to evaluate parts in several ways. Some focus on plastic parts or thin walled parts or symmetric parts, and so on. Most of these tools are from the Tools toolbar, but are found on the Evaluate tab in the Command Manager.
Verification on rebuild is an option that you can access by choosing Tools
With the setting selected, SolidWorks checks each face with every other face in the model. This is a better check than with the setting off but greatly increases the workload. The switch is deselected by default to prevent rebuild times from getting out of control. For most parts, the default setting is sufficient; however, when parts become complex, you may need to select the more advanced setting.
If you are having geometry or rebuild error problems with a part and cannot understand why, then try turning Verification on rebuild on and pressing Ctrl+Q. Ctrl+Q applies the Forced Rebuild command, and rebuilds the entire design tree. Ctrl+B, or the Rebuild command, only rebuilds what SolidWorks determines needs to be rebuilt.
If you see additional errors in the design tree that were not there before, then the combination of Verification on rebuild and Forced Rebuild has identified problem areas of the model and the features that caused the errors failed. If not, then your problem may be elsewhere. You still need to fix any errors found this way.
Performance
For speed reasons, it is normal practice to turn Verification on rebuild off, and to use it selectively to check models with potential errors. The type of speed degradation that you can see is dependent on the number of faces in the model. Some of the performance degradation as relates to patterns is documented in Chapter 8.
Much of the time, the best tool for tracking down geometry errors is the combination of experience and intuition. It is not very scientific, but you come to recognize where potential problems are likely to arise, such those that occur when you attempt to intersect complex faces at complex edges. Figure 11.8 shows the Check Entity dialog box.
Evaluating complex shapes can be difficult. A subjective evaluation requires an eye for the type of work you are doing. An objective evaluation requires some sort of measurable criteria for determining a pass or fail, or a way for you to assign a score somewhere in the middle.
One way to subjectively evaluate complex surfaces, and in particular the transitions between surfaces around common edges, is to use reflective techniques. If you look at an automobile's fender, you can tell whether it has been dented or if a dent has been badly repaired by seeing how the light reflects off of the surface. The same principle applies when evaluating solid or surface models. Bad transitions appear as a crease or an unwanted bulge or indentation. The goal is to turn off the edge display and not be able to identify where the edge is between surfaces for the transition to be as smooth as if the whole area were made from a single surface.
c0 = faces contact at edge
c1 = faces are tangent at edge
c2 = curvature of each face is equal at the edge and the transition is smooth
c3 = rate of change of curvature of each face is equal at the edge
The Zebra Stripes tool can only help you identify c0, c1, and c2, and only subjectively. This feature is of most value between complex faces. Figure 11.9 illustrates how the Zebra Stripes tool shows the differences between these three conditions.
Notice how on the Contact-only model, the Zebra Stripe lines do not line up across the edge. On the Tangent example, the stripes line up across the edges, but the stripes themselves are not smooth. On the Curvature Continuous example, the stripes are smooth across the edges. The part shown in Figure 11.9 is a surface model, and can be found on the CD-ROM with the filename Chapter 11 Zebra Stripes.sldprt.
Tip
You should rotate the model a lot when you are using the Zebra Stripes tool. Changing the density of the lines can also help, as can increasing the image quality (Tools
RealView causes reflections that can be used in a way similar to the reflections in Zebra Stripes. Rotate the part slowly and watch how the reflections flow across edges. Instead of black and white stripes, it uses the reflective background that is applied as part of the RealView Scene.
Cross-Reference
RealView techniques and usage are covered in more depth in Chapter 5.
While Deviation Analysis helps to quantitatively measure how close to tangent the faces on either side of the selected edge are, it does not tell you anything about curvature, so you must still run Zebra Stripes to get the complete picture of the flow between faces. Both tests have to return good results to have an acceptable face transition.
Using the Tangent Edges as Phantom setting is an easy way to evaluate a large number of edges all at once. This function does not do what the Zebra Stripes tool does, but it gives you a good indication of the tangency across a large number of edges very quickly. Again it only represents tangency, and tells you nothing about curvature continuity.
Although this is an easy method to use, it is not completely reliable. I have not seen this function deliver false positives (edges displayed as tangent when in fact they were not), but I have seen many false negatives (edges that display as non-tangent when in fact they were). Figure 11.12 shows a situation where the edges are displayed with solid edges, but Deviation Analysis shows them to have a zero-degree maximum deviation.
The measure of tangency has some tolerance. Users cannot control the tolerance, nor does the documentation say what it is. If SolidWorks says two faces are not tangent at an edge, you can believe that, but if SolidWorks says that the faces are tangent, you still have to ask how tangent. That is the question that Deviation Analysis can answer.
Short edges
Small faces
Sliver faces
Knife edges/vertices
Discontinuous faces or edges
These specific types of geometry typically cause problems with other features, such as shells or fillets. If you are having difficulty with a feature failing for a reason that you can't explain, use the Geometry Analysis tool to point out potential problem spots. This is not a tool that will do your job for you, but it is a tool that gives you useful information to help you do your job better and faster.
Feature Statistics lists the rebuild times of each individual feature in a part. This is useful for researching features, benchmarking hardware or versions of SolidWorks, and developing best practice recommendations for different tools and techniques. Figure 11.14 shows the Feature Statistics interface.
Overall, I do not recommend relying too heavily on the data the Feature Statistics tool provides; this is not because it is inaccurate, but because rebuild time is not always the best way to evaluate a model. You can certainly use the information, but you also need to keep it in perspective. A feature that takes a long time to rebuild but gives the correct result is always better than any feature that does not give the correct result, regardless of rebuild time.
Figure 11.15 shows a curvature comb applied to a spline. Notice that the spline continuously changes curvature. An arc has constant curvature.
When the comb crosses the spline, it means that the direction of curvature has changed. When the comb intersects the spline, it means that the spline at that point has no curvature (it is straight).
Cross-Reference
The Curvature Comb is discussed in depth in the SolidWorks Surfacing and Complex Shape Modeling Bible (Wiley, 2008).
SimulationXpress (formerly COSMOSXpress) is a limited version of SolidWorks Simulation (formerly COSMOS Works) that is bundled with SolidWorks to acquaint users with FEA. The full version of SolidWorks Simulation does a wide range of analysis, from vibrations to large deformations. SimulationXpress is a very quick and easy wizard for simple stress analysis on stand-alone parts with simple constraints. It does simple linear stress analysis on a single part with a single material using only fixed constraints and a load. You can also use SimulationXpress to do a simple stress/weight optimization based on dimensions that you select to be altered.
You can start SimulationXpress through the Tools menu, or from the Evaluate tab of the CommandManager. The interface guides you through a very simple wizard. If you have any familiarity with FEA applications, you will find SimulationXpress easy to understand and use, but possibly lacking in flexibility or capability.
Starting in SolidWorks 2010, SimulationXpress uses a combination of the Task Pane on the right of the graphics window and the PropertyManager on the left side of the graphics window. In this book, I am using the detached PropertyManager, so I can position it for more compact screen shots.
SimulationXpress is intended as a quick and dirty analysis run to see whether you are even close to having a part that will stand up to the loads you apply to it. As with any type of analysis, the results are only of value if the setup was correct and if you are able to interpret the results.
In this chapter I do not aim to teach analysis theory or best practice, this is simply a quick overview of how to use the tool. FEA is a field of study unto itself, and you should learn it from a dedicated resource. Analysis is a field that depends on approximations and simplifying assumptions. Knowing how and when to make the correct approximations and assumptions along with being able to interpret approximated results are some of the keys to success not provided by this book.
As you step through the process, the notes in the Task Pane seem to continually prompt you that various conditions will require the next level higher (not free) in order to correctly solve the model. SimulationXpress is clearly a sales and marketing tool, but if your needs are simple, and you understand the process, you may be able to get useful information from it.
When you start SimulationXpress, an image welcomes you to the tool and lets you know what to expect from the process. It also issues a disclaimer that seems to downplay the value of this tool. There is also a link here for some valuable web-based training if you are new to analysis or simulation. Figure 11.16 shows the new Welcome screen.
If you are a veteran SimulationXpress user, starting with SolidWorks 2010, most of what you see here is new, including the order of the steps and some of the terminology.
Every analysis must have at least one face that is held stationary in order for the analysis to work. These are usually faces on the bottom of the part.
In SolidWorks 2010, Fixtures are what was formerly referred to as Restraints. You must apply Fixtures to the part to be analyzed as the first step in the process. A PropertyManager appears to collect the faces you select. Fixtures are fixed, meaning they are the faces in the analysis that remain perfectly stationary. These are usually some sort of mounting location, or a welded area.
On this part, I have used the Split Line feature to split out areas of the bottom face around the bolt holes to represent sections of the part that will not move regardless of how much force is applied to the part.
The dark blue underlined text in the Task Pane are links to simple animations showing some possibilities for assigning Fixtures. Clicking the Add a fixture link in the Task Pane brings up the Fixture PropertyManager, shown in Figure 11.17.
With early versions of SolidWorks 2010, the display of the Fixture symbols seems erratic and incorrect depending on the rotation angle of the part.
You can apply forces or pressures to model faces. Forces are normal to selected faces by default, but you can select an axis, edge or sketch element to specify a selected direction for the force. Again links in the Task Pane enable you to see small video hints or tool tips. Figure 11.18 shows the Loads interfaces.
The third step in setting up SolidWorks SimulationXpress is to assign a material. Once you have made your selection, click Apply. Figure 11.19 shows some of the materials selection. Materials can be created or customized in the same way that you would create or customize standard SolidWorks materials.
Tip
My experience with the early versions of SimulationXpress in SolidWorks 2010 sp0.0 has been that much of the tool did not work properly the first time. It took several tries to get a material to apply, the loads appeared to be applied incorrectly, and the initial screen did not appear when I first started the software.
Analyzing simple parts on modern computers usually takes a matter of seconds. Because SimulationXpress is limited to single parts, most analyses you run will not take very long. You need to make sure that you have green check marks to the right of Fixtures, Loads, and Material before you can run the analysis. Figure 11.20 shows the analysis of this part in the process of running.
SimulationXpress makes three different types of results available to you:
vonMises stress plot
Displacement plot
Factor of Safety (FOS) plot
Each of these can be animated. The deformation shown by the model is exaggerated by a deformation scale factor, which is shown as part of the legend on the screen. It is typically around 1000x. Deformation is exaggerated to make it easier to visualize how the structure flexes under load.
Figure 11.21 shows a deformed vonMises stress plot.
All the values that you enter and faces that you select are stored in the SimulationXpress Study panel, which shows up by default on the bottom in a split PropertyManager, as shown in Figure 11.22. This is saved with the part, and is displayed any time you have the SolidWorks SimulationXpress panel open in the Task Pane.
The final step in the Simulation process, if you choose to use it, is the Optimization. Optimization enables you to vary a dimension of the part and run multiple studies to determine what value for that dimension produces the best result.
Optimization displays another panel at the bottom of the graphics window that enables you to establish a range for the dimension that will be varied during the optimization. This panel is shown in Figure 11.23.
When you run the optimization, SolidWorks will change the model dimension within the range that you specified, and run an analysis for each dimension value. For this to be most successful, you must have a robust model where all the features can adapt to the range of dimensions for the feature being changed.
Using this tutorial, you make some major edits to an existing part. You use some simple loft and spline commands, and work with the rollback states and feature order, as well as some evaluation techniques. Please follow these steps:
Open the existing part with the filename Chapter 11
Tutorial Start.sldprt. Roll the part back and step through it feature by feature to see how it was made. Edit the loft feature to see which sketches were used to create it. This can help you to understand how the part was built. Exit the loft command and move the rollback bar back to the bottom of the tree.Open the Deviation Analysis tool (Tools
Deviation Analysis). Select the edges, as shown in Figure 11.24.The maximum deviation is about ten degrees, which is far too much. This part needs to be smoothed out, which you can do using splines in place of lines and arcs.
The first step is to make the outlet all one piece with the spiral. You can do this with a Fit Spline. You need to create the Fit Spline before the loft profiles and after the spiral.
Expand the loft, and roll back between the loft feature and the first sketch. Click OK in response to the prompt, and then roll back to just after the spiral, as shown in Figure 11.25.
Right-click the spiral in the FeatureManager and show it. Open a new sketch on the Top plane.
Try to draw a horizontal line from the outer end of the spiral. You will notice that you cannot reference the end of the spiral.
Tip
Curves that are absorbed into other features are notoriously difficult to work with. Generally, you need to select them from the FeatureManager to do anything at all with them. Also, if you need to reference an end of an absorbed curve, you are better off using Convert Entities to make it into a sketch entity.
Notice that you cannot select the spiral from the graphics window. Even when selected from the FeatureManager, it appears not to be selected in the graphics window. Ensure that it is selected in the FeatureManager, and then click the Convert Entities button on the sketch toolbar.
Draw a horizontal line from the outer end of the spiral and dimension it to be three inches long, as shown in Figure 11.26.
Select both the converted spiral and the line, and click Tools
Spline ToolsFit Spline. Set the Tolerance to .1 and make sure that only the Constrained option is selected. Click OK to accept the Fit Spline. Test to make sure that a single spline is created by moving your cursor over the sketch to see whether the whole length is highlighted.
Note
The Fit Spline feature fits a spline to a set of sketch entities within the specified tolerance. It can be a useful tool for smoothing out sketch geometry.
Warning
Do not exit the Fit Spline by pressing the Enter key as you do with other commands, because it simply exits you out of the command without creating a spline.
Right-click on spline and select the Curvature Comb. Notice how the comb is affected by the transition from the spiral to the straight line.
Exit the sketch, and create a new plane. Choose Insert
Drag the Rollback bar down between Sketch3 and Loft1. If it goes beyond Loft1, then you need to navigate back to this position again.
Right-click Sketch3 and select Edit Sketch Plane. Select the newly created Plane1 from the Flyout FeatureManager, and click OK to accept the change.
Notice that the loft profile has moved to a place where it does not belong. This is because the sketch has a Pierce constraint to the spiral, and there are multiple places where the spiral pierces the sketch plane.
Edit Sketch3 and delete the Pierce constraint on the sketch point in the middle of the construction line. Create a Coincident relation between the sketch point and the outer end of the Fit Spline, as shown in Figure 11.28. Do not exit the sketch.
One of the goals of these edits is to smooth out the part. Remember that the Deviation Analysis told you that the edges created between the lines and arcs in Sketch3 were not very tangent. For this reason, it would be a good idea to replace the lines and arcs in Sketch3 with another Fit Spline.
Right-click one of the solid sketch entities in Sketch3, and click Select Chain.
Create another Fit Spline using the same technique as in Step 8. Exit the sketch.
Drag the Rollback bar down one feature so that it is below the Loft. Notice that the Loft feature has failed. If you hold the cursor over the feature icon, the tooltip confirms this by displaying the message, "The Loft Feature Failed to Complete."
Edit the Loft feature. Expand the Centerline Parameters panel if it is not already expanded, and delete the Spiral from the selection box. In its place, select the Spiral Fit Spline.
If the loft does not preview, check to ensure that the Show Preview option is selected in the Options panel, at the bottom.
If it still does not preview, right-click in the graphics window and select Show All Connectors. Position the blue dots on the connector so that it looks like Figure 11.29.
Click OK to accept the loft. The loft should be much smoother now than it was before. In addition, the spiral feature should no longer be under the loft; it should now be the first item in the design tree.
Drag the Rollback bar down to just before the Shell feature. Notice that Fillet5 has failed. Move the mouse over Fillet5. The tooltip tells you that it is missing some references. Edit Fillet5 and select edges in order to create fillets, as shown in Figure 11.30.
Right-click in the design tree and select Roll To End. This causes the FeatureManager to become unrolled all the way to the end.
The outlet of the involute is now longer than it should be. This is because the original extrude was never deleted from the end. Right-click the Extrude1 feature and select Parent/Child. The feature needs to be deleted, but you need to know what is going to be deleted with it.
The Shell is listed as a child of the extrude because the end face of the extrude was chosen to be removed by the Shell. Edit the Shell feature and remove the reference to the face. (A Shell feature with no faces to remove is still hollowed out.)
If you right-click Extrude1 and select Parent/Child again, the Shell feature is no longer listed as a child.
Delete Extrude1, and when the dialog box appears, press Alt+F to select Also Delete Absorbed Features.
Edit the Shell feature and select the large end of the loft. Exit the Shell feature. The results up to this step are shown in Figure 11.31.
Drag a window in the design tree to select the four fillet features. Then right-click and select Add to New Folder. Rename the new folder Fillet Folder.
Click the Section View tool, and create a section view using the Front plane.
Reorder the Fillet folder to after the Shell feature.
At this point, you should notice that something does not look right. This is because creating the fillets after the Shell causes the outside fillets to break through some of the inside corners. The fillets should have failed, but have not, as shown in Figure 11.32.
Choose Tools
OptionsPerformance, and select Verification on rebuild. Then click OK to exit the Performance menu and press Ctrl+Q. The fillets should now fail.Click Undo to return the feature order to the way it was.
Save the part.
Working effectively with feature history, even in complex models, is a requirement for working with parts that others have created. When I get a part from someone else, the first thing that I usually do is look at the FeatureManager and roll it back if possible to get an idea of how the part was modeled. Looking at sketches, relations, feature order, symmetry, redundancy, sketch reuse, and so on are important steps in being able to repair or edit any part. Using modeling best practice techniques helps ensure that when edits have to be done, they are easy to accomplish, even if they are done by someone who did not build the part.
Evaluation techniques are really the heart of editing, as you should not make too many changes without a basic evaluation of the strengths and weaknesses of the current model. SolidWorks provides a wide array of evaluation tools. Time spent learning how to use the tools and interpret the results is time well spent.