CHAPTER 23

Using Imported Geometry and Direct Editing Techniques

The direct editing set of tools in SolidWorks enables you to change a part without having access to the history of features that created the part. Direct editing works on both native and imported geometry either by simply moving faces or by editing the geometry directly rather than indirectly through feature definitions or sketches.

This chapter looks at recent direct editing developments in the CAD world and also describes the tools on the Direct Editing tab, which is shown in Figure 23.1.

The new tab has the following tools on it, listed from left to right from Figure 23.1:

• Move Face
• Move/Copy Bodies
• Fillet
• Chamfer
• Linear Pattern
• Delete Solid/Surface
• Delete Face
• Split
• Combine

Additional direct edit tools exist in SolidWorks that should possibly be added to the Direct Edit tab:

• Flex
• Deform
• Freeform

FIGURE 23.1 SolidWorks has a Direct Editing tab on the CommandManager.

Combining these tools with some of the new Instant 3D functionality gives direct editing tools in SolidWorks many of the advantages of the direct edit–only CAD software. Before a discussion of direct editing will make sense, you need to know a little bit about imported geometry.

Understanding the Basics of Imported Geometry

Geometry that is transferred between CAD packages is called imported geometry. The transfer usually happens through IGES (Integrated Geometry Exchange Standard; pronounced eye-jess), STEP (Standard for the Exchange of Product), Parasolid, or ACIS (named for the initials of three people and one company who created the standard: Alan, Charles, Ian, and Spatial) formats. SolidWorks also reads some native CAD data directly. For example, SolidWorks can read data directly from versions of Pro/ENGINEER, Unigraphics/SDRC (NX), Inventor, Solid Edge, CADKEY, and Rhino, as Figure 23.2 shows. In almost all cases, features are not transferred between CAD packages. The geometry that you wind up with is called “dumb” geometry because the smart parametrics and design intent (meaning the list of features) that the model had in its parent software is no longer there.

FIGURE 23.2 SolidWorks opens neutral format files as well as several native formats.

You can bring in imported data in one of two ways. The most common way is to use the Open dialog box and switch the Files Of Type to an imported file format. The other way is to use the Imported Geometry feature by choosing Insert Features Imported Geometry from the menus. The Open dialog box creates a new part with the imported feature at the top of the FeatureManager, as shown in Figure 23.3. Using the Imported Geometry feature enables you to insert imported geometry anywhere you like within the FeatureManager, even after other features have been added.

FIGURE 23.3 Imported geometry comes in without any feature history.

You can use the new Data Migration tab in the CommandManager to find tasks that support imported geometry. The tools on this tab are shown in Figure 23.4.

FIGURE 23.4 SolidWorks Data Migration tab on the CommandManager helps you find import tools.

The tools on the tab, listed in order from left to right, are

• Open
• Imported Geometry
• Import Diagnosis
• Check
• Draft Analysis
• Recognize Features (FeatureWorks)
• Heal Edges
• Knit Surface
• Move/Copy Bodies
• Move Face
• Delete Face
• Replace Face
• Split
• Combine
• Covert to Sheet Metal
• Insert Bends (sheet metal)

Many of these tools are not directly related to imports but may be frequently used with imports. FeatureWorks is a part of the SolidWorks Professional bundle, and as such is beyond the scope of this book; however, it is mentioned as part of one possible workflow for editing imported geometry toward the end of this chapter.

Gaining experience with imports

When SolidWorks imports data from another CAD program, the result is an Imported feature in the FeatureManager. The example shown in Figure 23.3 is the situation you are typically looking for: the result as a single solid body. Frequently, imports do not come in this clean. When imports start giving you trouble, you will see errors on a single body, or possibly multiple bodies, or even surface bodies. SolidWorks can address some types of errors automatically, and you can address some manually. From time to time and for various reasons, you might get a part that is such a mess that you just want to try a different method for importing it (for example, different import or export settings, or a different file type).

The best way to start to feel comfortable with imported data is to be exposed to a wide range of files, some that work and some that don't. This chapter is not intended to be a short course on import repair, but repair is certainly part of the reality of working with imported data. When imports fail, it is not often because of SolidWorks; it is often because the parent software fails. SolidWorks import tools are very good and have improved over time.

Understanding the results of imports

When you import geometrical data into SolidWorks, you can get a number of different types of results:

• Single solid body in a part file
• Assembly of multiple parts
• Multiple solid bodies in a part file
• Surface bodies in a part file
• Combination of solid and surface bodies in a part file

When you get an assembly of parts, SolidWorks uses the default template that you have designated in Tools Options Default Templates, creates new parts, and saves them to your hard drive automatically.

Some imports also create a report file with the extension *.rpt or *.err. This file includes statistics about the entities and precision of the data, filename, units, the originating system, and also some information about errors that occurred during the import.

Figure 23.5 shows the first section of a report written for the import of an IGES file.

FIGURE 23.5 Report files can help you understand the contents of the imported file.

Demonstrating some data import

I am going to import a few parts that don't come in perfectly and ask you to follow along with the files on your DVD. This is not so much a click-by-click tutorial as a “watch over my shoulder” demonstration with commentary.

Starting with a Parasolid import because these are the fastest and easiest, open the part called Chapter 23 Robot Arm.x_t from the material on the DVD for Chapter 23. You can open translated format files in a couple of different ways. Many people look for an Import or Translate option in the File menu, but it's not there. You can use the Open command, and select Parasolid from the Files Of Type drop-down list. That is one way to do it, but it is slow. I prefer to open a translated file using Windows Explorer, and drag-and-drop the file onto the SolidWorks window.

After you open the file, you will notice a couple of things. The first thing that stands out to me is that the model displays in Shaded mode, regardless of how you have the display set. For example, I like to use Shaded With Edges, but imports always set it back to Shaded.

The next thing to notice is the Imported1 feature in the FeatureManager. In this case, the import was clean, so there are no warnings (yellow triangles) or errors (red circles). This is not always a good indication of the state of the part, though, because some errors that SolidWorks knows about are not displayed on the Imported feature icon. To investigate closer, right-click the Imported1 feature and select Import Diagnosis, or click Import Diagnosis from the Evaluate tab of the CommandManager.

In this case, the model really is clean. Running Import Diagnosis is the only way you can really know this. Figure 23.6 shows the FeatureManager, the Import Diagnosis, and the part itself.

Next, open the Parasolid file called bad face.x_t. This one also imports without an error or warning on the Import feature, but there is clearly a missing face. It is easier to visualize the separate faces of the part if you change the display mode to Shaded With Edges. If you examine the part closely, you can see that several faces are not lined up square with the rest of the part. Notice also that there are small sliver faces. This may be intentional, or it may be part of the problem. Triangular faces and sliver faces (with very sharp corners, usually long and narrow) are often the source of errors in translated parts.

FIGURE 23.6 Clean imports from Parasolid have the tendency to be fast and trouble-free.

Right-click the Import feature and run the Import Diagnosis; you will see the faulty face listed. Click the Attempt to Heal All button to fix the faulty face. Figure 23.7 shows the part with the faulty face.

FIGURE 23.7 Three-sided and sliver faces are often the source of errors with imported parts.

Now open the Pro/ENGINEER file called bad face 2.prt.29. Pro/ENGINEER files often end with version numbers as the extension of the file. You need to be careful if you see a file that looks like a Pro/ENGINEER file with no version extension. SolidWorks used the *.prt extension for the first couple of years and still opens this type of file as a native file. You may still find some of those parts in circulation.

Open the file using the Import Geometry Directly option, and switch the display to Shaded With Edges, and run an Import Diagnosis. The part has a bad face. If you click on the face in the Faulty Faces list, you can see that the face is next to a small, pointy triangular face, shown in Figure 23.8. The Attempt to Heal All option takes care of it.

FIGURE 23.8 Importing the same data in different ways can give you different results.

Import the same file, but this time choose the Analyze the Model Completely option. It should tell you that it recognizes 13 out of 13 features. Click the Features button and watch the part rebuild. Notice that this time the part comes up with a feature error. The error is on a fillet. It is not an accident that the previous error was on a face next to a fillet face.

Notice that the Parasolid parts came up almost immediately, but the Pro/ENGINEER parts take several seconds to process the data. As the imported files become larger and larger and branch into assemblies, this difference becomes more and more pronounced.

Next is a sheet metal part. Open sheet metal.x_t. Change the display to Shaded With Edges. The part looks good, and Import Diagnosis says that it is okay. Because this is a sheet metal part, and it appears to have a consistent thickness, you will try to flatten it. Click the Sheet Metal CommandManager tab, and click the Insert Bends icon (on the far right side). Select the big flat face as the face to remain stationary (the top selection box), and click the green check mark button to accept the result.

The sheet metal features are added to the part, but notice in Figure 23.9 that they have failed. A close inspection of the part reveals that there is a small ledge between the big flat face and the inside bend on both ends. This was probably a modeling error rather than a translation error. You might be able to fix this to make it usable as a sheet metal part, but for imported geometry editing, you'll need to go to the end of this chapter. Here I cover the results of attempting to repair this model.

The last part I want to show in this “watch over the shoulder” demonstration is a part that I consider to be a complete loss. This is an IGES file that came from an Autodesk Mechanical product. In the DVD, open the file called valve body.igs. This part takes several seconds to import. When it does import, it has 11 surface bodies, 2 of those with errors, and some obvious problems with a couple of faces that somehow became out of control. This is one of the reasons so many users do not recommend using IGES files. This type of error is more prevalent with IGES files than other formats. Figure 23.10 shows the FeatureManager and the part on the screen. Again notice that the locations where the huge problem faces come off the model are pointy triangular faces.

FIGURE 23.9 Very small errors can cause special functionality in SolidWorks not to work, and repairing it is not always straightforward.

FIGURE 23.10 Some parts are simply beyond repair.

If you get a part that is this bad, your first move should be to try to get better data from the source. If that isn't available, you are going to have an uphill battle trying to make this part work. Automatic healing with the Import Diagnosis isn't going to touch this part. Repair is going to be an exercise in manual surface modeling. If you don't have the patience for that, you could try solid modeling from the reference faces on the part. If you look closely at the interaction of some of the fillets, it is no surprise that the translation failed so badly. Many of the fillets are badly hacked together. In addition, if this is a casting, someone is going to need to apply draft to the part, and with all the fillets on it, this part is not going to lend itself to that very well.

Using direct converters

SolidWorks contains some direct converters that either extract the kernel data (Parasolid information) or read the actual feature data and rebuild feature-based parts. The direct converter for Pro/ENGINEER data is probably the most widely used. Figure 23.11 shows the dialog box for the Pro/ENGINEER to SolidWorks Converter.

FIGURE 23.11 Converting Pro/ENGINEER files to SolidWorks gives you some options.

If you use the Import geometry directly option, you just get the dumb solid. Pro/ENGINEER uses its own “kernel,” or underlying geometry engine, called Granite. SolidWorks shares its kernel with NX and Solid Edge (Parasolid). To read the geometry directly, SolidWorks has to read the Granite data stored inside the Pro/ENGINEER file and translate it to Parasolid geometry.

If you choose the Analyze Model Completely option, you get a dialog box similar to the one shown in Figure 23.12. In this case, the Pro/ENGINEER part had 42 features, and the SolidWorks converter can read them all. Here too, you are given the option to take the features or the body. It is not clear that the Body option is the same as the Import geometry directly option, but they both result in the import of the dumb solid.

You would want to click the Body option if the percentage of recognized features was low, or if you didn't really need the parametric features that much. Sometimes, even if it doesn't recognize all the features, you might still get all the sketches you need to re-create the part.

If you choose the Features option, SolidWorks rebuilds each sketch and feature to build a history-based model. This is not usually what people mean when they talk about imported geometry. Many CAD neophytes assume that features just automatically transfer from one CAD system to another, but this is by far the exception rather than the norm.

Figure 23.12 shows the Pro/ENGINEER to SolidWorks Converter dialog box and the finished imported model.

FIGURE 23.12 A Pro/ENGINEER part can be translated with a complete feature tree.

This translation depends on the version of the Pro/ENGINEER file. Check the SolidWorks documentation to see what versions of Pro/ENGINEER are supported.

Handling import errors

Import errors are usually caused by differences between the exporting and importing CAD software vendors. Some imports are more prone to errors than others. For example, the IGES format is interpreted different ways by different software vendors, and is, therefore, very prone to errors.

Another type of error is the error due to tolerance or accuracy issues. Catia is notorious for having very large tolerances on exported data. This is to enable Catia to work with large data sets more easily, but it means that when the geometry is read into SolidWorks, which typically requires more accurate data, you can see a lot of errors. The fact that the Catia to SolidWorks translation is one of the most problematic in the CAD industry seems odd because SolidWorks and Catia are both owned by Dassault Systemmes, but the difficulties have persisted for more than a decade, so it is not a technological difficulty, it is a business decision.

Repairing import errors automatically

SolidWorks has a tool called Import Diagnostics. Import Diagnostics can run automatically or manually to find the errors in imported data and to make repairs if possible. You can access Import Diagnostics by right-clicking an imported feature in the FeatureManager, as long as there are no native SolidWorks features that follow the imported feature. Figure 23.13 shows typical results from a faulty import.

FIGURE 23.13 Import Diagnostics helps you find and repair errors in imported data.

Sometimes the errors Import Diagnostics finds are things you can see, like missing faces, and sometimes they are things you can't see, like the edges of a face that don't intersect or inconsistent face normals. When errors can be found and repaired by Import Diagnostics, it is the best way to go. In fact, whenever I import a model, I always run Import Diagnostics on it to make sure everything is good.

Repairing import errors manually

Some errors are so big that the Import Diagnostics cannot fix them. An example of this type of error would be when a face is missing altogether from the imported data. When something like this happens, the only thing you can do is resort to surface modeling. If the import leaves you with surface bodies, and it cannot repair them automatically, you have to be able to remove the bad faces and replace them with new faces that you construct. This is all about using surface tools to create the new face, extending and possibly trimming the new face to fit into the gap caused by the bad face or faces, and then knitting everything together back into a solid. This may be an oversimplification of the workflow for manual import repair, but it is essentially the big-picture steps that you have to go through to get the task done.

There is such a thing as models that are so bad that you can't fix them, or that would not be worth your time to fix. If automatic repairs don't work, and simple manual repairs don't work, the next thing to do would be to go back to the source of the file and ask for better data.

If you get bad data and you do not have access to the source, and automatic and manual errors prevent you from using the data, then the next best thing is to rebuild the part using the error-filled data as a reference. This is never a pretty thing, but if you really need the data to be clean, and there is no other way, this is what you need to do.

You can take measurements in one file and build a new part in another file, build one file in the context of an assembly directly over the problem file, or even rebuild it as a multi-body part.

Tricking data into working

Occasionally you can employ tricks to heal problem imports. Simply saving out of SolidWorks as Parasolid and reading back in repeatedly can sometimes heal troublesome imported geometry. I frequently use Rhino to import problem files, then export from Rhino as a Parasolid. Rhino is an inexpensive surfacing application. You can read more about it at www.rhino3d.com. You can download and install a trial version that allows you to save 25 times. Rhino works great as a translator because it reads and writes many file types that SolidWorks does not read. Sometimes when I get a very bad IGES file, I read it into Rhino, and save it out as Parasolid, then read the Parasolid into SolidWorks. Sometimes this will repair the data to the point that SolidWorks can deal with it more effectively.

This is not to say that Rhino is a better file translator than SolidWorks, because this workaround does not always improve things. It is sometimes effective, and because it is free, the only thing it will cost you to try it is time.

You can use the same trick with other CAD packages. For example, if you know that you have an IGES file from VX, and you are having difficulty reading it into SolidWorks, it might pay to download a trial version of VX (www.vx.com) and see if it can import the data and re-export. It is best to use the source program to read and re-export when possible.

Ensuring that you get good data

If you can't get a SolidWorks file from someone who needs to send you data, the type of translation file that you get has a huge influence on the likelihood that your translation will be successful. Ask for data in this order:

1. Parasolid (including native formats that use Parasolid, such as NX, Unigraphics, and Solid Edge). Parasolid can come in text format (*.x_t) or binary format (*.x_b). You may also see file extensions such as .xmttxt from older versions of Unigraphics. Of these, the binaries are smaller, but the text files have WordPad readable and editable headers that can be useful in various situations, such as correcting units or part scaling, as well as telling what the parent CAD program was.
2. STEP (AP 214 or AP 203; Standard for the Exchange of Product model data). The AP stands for application protocol. Most mechanical CAD programs use these two protocols, which were developed for automotive and configuration controlled design (read more at www.steptools.com/library/standard/step_2.html).
3. ACIS (named for the initials of the three people and one company who created the standard: Alan, Charles, Ian, and Spatial). ACIS creates *.sat files.
4. *.VDAFS, *.VDA (Verband der Automobilindustrie Flächenschnittstelle) A German automotive geometry transfer format.
5. IGES (Integrated Geometry Exchange Standard; pronounced eye-jess). Because of the age and lack of clear definition in the IGES format, there is little that is truly standard about it any more, and many geometry creation software packages export data that SolidWorks cannot read correctly. While this format is an old standby for old-timers, it is one you probably want to avoid unless you are getting data from someone you know will give you something usable.

Another advantage of the Parasolid data is that SolidWorks reads it so quickly. A large IGES or STEP file can take minutes to read in, where SolidWorks can read equivalent Parasolid data in a couple of seconds. Once the data is read into SolidWorks, it should all be the same, with no difference between data from Parasolid and any other source, because it is all converted to Parasolid to be stored inside the SolidWorks file; but because it's now all Parasolid you save time on the initial read.

Whether or not the data you receive is of value to you depends in part on what you want to do with it. If your data only has to be a visual representation, and not a CAD-accurate NURBS (Non Uniform Rational B Spline) model, you may be able to accept a wider range of data types. If you are looking for manufacturing quality data, some formats are simply not worth your time to deal with. These file types are mesh data that SolidWorks can read and are useful for visual data, but useless for clean NURBS data:

• *.stl. Stereolithography, typically used for rapid prototypes
• *.vrml. Virtual reality markup language, typically used for games, an old format that allowed color to be transmitted with the mesh geometry
• *.cgr. Catia graphics

Converting point cloud data

One of the most common import questions is how to import data from file formats such as *.obj or *.3ds, among others. These file types are mesh files, which means they are simply point cloud data. SolidWorks and most other CAD programs create geometry that is based on NURBS data, where the surfaces are represented by very accurate mathematics. Mesh data is represented by points in space, which is much faster to work with because it is similar to the data used by graphics cards and drivers to display curvy shapes. Mesh data is used by Hollywood, video game developers, and computer graphics studios, and NURBS data is used in engineering and manufacturing. It is easy to convert NURBS to mesh, but more difficult to convert mesh to NURBS. The mesh to NURBS conversion can be done, but complex software and specialized expertise is needed for it to happen correctly.

Understanding the IFC file format

The *.ifc (Industry Foundation Classes) file format is from the AEC (Architecture, Engineering, and Construction) industry, which means it is for buildings. IFC is related to the BIM (Building Information Modeling) initiative that enables the transfer of more than just geometrical information about a building. Much of the AEC discussion is well beyond the scope of this book. If you want more information on IFC, BIM, and AEC modeling, a good place to start is at www.aecbytes.com/feature/2004/IFCmodel.html.

SolidWorks appears to be reaching into this market with a couple of enhancements in the 2011 release, including the large-scale design options with 3D sketches and weldments.

Understanding the Traditional Role of Direct Edit Tools

What I call “direct editing” is also known by other names. You may hear it referred to as direct modeling, explicit modeling, history-free modeling, or even synchronous technology. I call it direct editing because the way the geometry is created is all approximately the same and the difference is in the way edits are made. In fact, one of the claims to fame of direct editing software tools is that it is the only system that deals effectively with imported geometry, because “geometry is geometry,” regardless of its source — native or imported. This is the reason why I cover imported geometry and direct edit tools together in this chapter.

Traditionally, direct editing CAD software has lived by the rule that how you create geometry should not affect how you edit the geometry. Therefore, direct edit CAD packages still use functions like extrude and revolve to build parts, but they would not return to those functions to edit the part; they would instead directly manipulate faces of the part by moving, offsetting, and rotating.

CAD software that depends on direct editing tools has existed for a long time: it has been around longer than history-based CAD software. In the last several years, some new direct edit CAD products (Sketchup and Spaceclaim) have appeared on the scene and have renewed an interest in direct edit techniques. Until this recent resurgence, the direct edit programs were seen as old-fashioned and inferior to parametric history-based programs.

Part of the charm of the direct edit scheme was that the software didn't add any information to the model. The model could be transferred between direct edit CAD packages without losing any information. This is clearly not the case with parametric history-based CAD software, where you basically lose the ability to edit the existing model when you transfer it from one parametric history-based program to another. You can add new features, but you can't change what originally appears.

Defining the role of direct edit tools

But direct edit CAD software has not taken over the market, even with all of the recent hype. History-based modelers are still popular with users who design things. There must be more to this story: the direct edit scheme does have some weaknesses. While making individual changes is easy and intuitive, making conceptual changes (changes to the design intent) can be just like starting over again with direct edit. There are also situations in which certain edits cannot be made, or reversing a set of edits does not result in the original configuration. People who are used to the control and power of history-based systems will be less likely to relinquish that control for simple ease of use.

It turns out that the simplified capabilities of direct edit tools are more suited to non-CAD specialists who still need to work with geometrical data either upstream or downstream from the main production modeling. This means that a non-specialist can do the equivalent of a 3D napkin sketch in Sketchup and hand it off to a specialist to create the detailed production model. It means that an FEA (Finite Element Analysis) analyst can make simple edits to a model given to her by a specialist. A machinist can add stock to a finished detail model without being highly CAD proficient. I don't see CAD power users or production modelers giving up history-based CAD software and changing over to direct edit-only tools any time soon.

As a part of the direct edit resurgence, CAD companies have figured out how to apply the concept of parametrics (driving dimensions and geometrical relationships) directly to the solid model, without using sketches or feature definitions as an intermediate step. Also, the history-based modelers are adding some direct-editing functionality. This cross-pollination helps bridge the gap that is now becoming mainly a discussion about how to combine direct edit and history-based modeling techniques. In this chapter, I do not cover the details of how each CAD program has implemented the direct editing scheme; I just want to help you understand where SolidWorks is today in the direct edit spectrum, and what you might have to look forward to as the comparison between the history-based and history-free worlds continues to take shape.

This background information is important as a part of the overall discussion of the place of these tools within the SolidWorks software. Adding direct edit tools to SolidWorks is not an earth-shattering change, but of secondary importance. Notice that the topic of direct edit does not dominate this book, just 1 chapter out of 24. SolidWorks includes the tools because they are useful, not because they are necessary.

Understanding the strengths and limitations of direct edit tools in SolidWorks

Some of the selling points for the direct edit CAD tools are that you don't have to worry about how a part was made (you just make the changes you want to make), and that feature trees with “history” always include feature rebuilds (which users tend to complain about taking a long time, especially for large parts and assemblies).

Without a doubt, grappling with feature order and feature rebuild times are problems that SolidWorks users face daily and often complain about.

Direct edit strengths include:

• Avoid feature order problems
• Avoid rebuild time
• Changes are more intuitive
• Concept of moving faces directly is very intuitive

Probably the most serious limitation of direct edit tools is that once a face has been eliminated from the model, you cannot bring it back using more direct edit tools. For example, take the part in Figure 23.14.

FIGURE 23.14 Editing limitations with direct editing

If you change the bottom square area such that the flat face between the bottom square and the arc disappears, you cannot get it back by just moving the face back to where it was; you would have to move the face and then make a cut to reinstate the flat face. This limitation is less serious when the direct edit tool is just another tool within a history-based modeler, because you can resort to the more powerful history-based tools to compensate, but with a dedicated direct edit–only tool you will be up against a more difficult task.

Other limitations of direct edit–only CAD software are going to center around features that themselves are some sort of process, such as fillets or shells. While fillets and shells are two of the most problematic features for history-based modeling, they are also two features that create the biggest limitations for direct edit software.

Using SolidWorks Direct Edit Tools

So how does SolidWorks, a history-based system, incorporate the advantages of direct editing techniques, which are not typically thought of as history-based? What does it look like when contradictory regimes collide and start sharing ideas? SolidWorks has taken ideas from a history-free scheme and incorporated them into a history-based scheme.

First, I will show you how this works in a simple example. Using the part from Figure 23.14, Figure 23.15 shows the FeatureManager and the original sketch. Notice that the original sketch has not changed, but the part itself has. Rolling back eliminates the Move Face features, and making changes to the original sketch changes the starting points for the Move Face features when they are unrolled.

FIGURE 23.15 Direct edits in a history-based part

You may be able to imagine that in a part with a much longer feature tree, where the relationships between the faces and the features are more complex, overriding that complexity by editing a face directly could have some appeal.

Combining direct edit with history

SolidWorks has several features that do not create new geometry, but edit existing geometry only, whether it is native or imported. These include the following:

• Move Face
• Delete Face
• Freeform
• Flex
• Deform
• Draft
• Scale

I'll show you a slightly more complex example. In traditional SolidWorks usage, if you wanted to move the face indicated in Figure 23.16, you would go back and edit the sketch or feature that was used to create it. That would be easy enough, and the fillets would update to match the new geometry.

The direct edit salesmen would say that first finding the feature you need to change is difficult, then waiting for the change to rebuild all the features, and last dealing with the downstream features like fillets that might fail due to the changes is frustrating, and he would be right. (You can find a feature in the tree by right-clicking geometry in the graphics window and selecting Go To Feature In Tree.) The problem is that the part, as shown in Figure 23.16, cannot be changed at all in the traditional direct edit scheme. In the direct edit scheme, the fillets are just faces; they are not intelligent features. If you move faces they are attached to, you have to also explicitly tell the fillet faces what to do.

FIGURE 23.16 Fillets greatly complicate direct editing schemes.

While the direct edit implementation in software such as Solid Edge ST3 is smart enough to make changes to models with fillets on them, the direct edit tools in SolidWorks are less sophisticated and cannot deal with the fillets at all.

Here's how to simplify the part by suppressing fillets and using the Move Face feature to change the part (see Figure 23.17). Here, I've moved the ring around the top of the barrel as well as the mounting boss.

FIGURE 23.17 Using Move Face to extend the length of the barrel of the cast part after the fillets have been removed

In order to make this move, I had to select seven faces:

1. Top of ring
2. Bottom of ring on left
3. Bottom of ring on right
4. Top of boss
5. Bottom of boss
6. Full round on end of boss
7. Hole in the mounting boss

Notice how the Web now extends up the side of the barrel. This is the type of edit that would be clumsy in SolidWorks if it were what you wanted to do. In direct edit, it is the kind of edit that would be clumsy if it were not what you wanted to do.

This is one of the limitations of direct edit techniques in general — not a limitation of SolidWorks, but a limitation of the concept as implemented in SolidWorks. Direct edit cannot make new faces without adding another feature and has problems with the intelligent type of face creation that you find in history-based systems. Direct edit programs are certainly not more powerful than SolidWorks or any other history-based CAD program. They have weaknesses in different areas, and the weaknesses are more limiting than SolidWorks history-based weaknesses.

Figure 23.18 shows where the weakness of using the direct edit tools within SolidWorks begins to show up. The first feature in the part is a revolve that uses a sketch. The last feature in the part is a Move Face feature that moves the faces created by the revolve. So if you want to change the geometry of the barrel, it is controlled by two different features. If you make the sketch a specific size, the Move Face feature will change it. Move Face can only change relative to a starting point; it cannot make something a specific dimension, so it will always either add or subtract a given amount from the geometry created by the original feature.

FIGURE 23.18 Move Face features put some geometry in double jeopardy — it can be changed from two different places.

Some SolidWorks power users consider this double-jeopardy condition sloppy design or bad practice. You can make a strong case that the direct edit tools should not be used on native SolidWorks parts, and that you should edit the feature the way it was created. There is certainly a place for that argument. But I know from my own modeling work that sometimes changing a feature way back in the tree can have unintended repercussions later in the tree, so using a Move Face feature late in the tree avoids fixing a lot of propagated errors. Is that a cheap, sleazy cheat? You will have to decide that for yourself.

Combining direct editing with imported geometry

Regardless of any argument against using direct edit tools on native SolidWorks data, there can be no such argument against using them on imported data. Direct edit tools may have their limitations, but when dealing with imported geometry in SolidWorks, your choices are limited, as you see from the following:

• Direct edit tools
• Cut and add modeling
• Manual surfacing tools
• FeatureWorks deconstruction

When faced with these options, direct edit tools look like the safe choice. The big problem will be that if the part is covered with fillets, you may not be able to change much. In cases like that, you might use a combination of tools, such as FeatureWorks to remove fillets, and then direct edit to make changes.

Handling imported data with FeatureWorks

FeatureWorks is not part of the scope of this book because it is a part of SolidWorks Professional, and the book is limited to SolidWorks Standard. FeatureWorks is an add-in that rebuilds imported solid models as feature-based models. It can recognize and rebuild features automatically, or semi-automatically with you guiding it through the process.

FeatureWorks works by deconstructing, or “unbuilding,” the part, removing faces of features that would be applied last. For example, first it will try to recognize fillets, and removes them from the model. Then it recognizes other types of features, including holes, and then finally it recognizes the base extrude or revolve feature.

You can use this as part of your process, but only deconstructing the part partially, leaving the portion of the part that is not assigned to a feature as an imported body. If you remove the fillets and the holes, you might be able to do the edits that remain using direct edit tools. This will leave you with a partially imported part with some parametric features and some direct edit features. Some folks might consider this a sloppy mess, but getting work done on schedule does count for something; if that is what it takes, then it removes the sting to some extent. The FeatureWorks PropertyManager is shown in Figure 23.19.

FIGURE 23.19 Use FeatureWorks to fully or partially deconstruct models to allow direct edit tools to work.

Tutorial: Importing and Repairing Solid Geometry

This tutorial walks you through the button-clicks to import CAD data from IGES and make some edits.

1. From the DVD, open the file called cover.igs. You can open this file by selecting it in the Open dialog box (File Open) or dragging and dropping it from Windows Explorer.
2. Right-click the Imported1 feature and run Import Diagnosis. Notice that Import Diagnosis finds no errors on the part.
3. Look at the inside of the part, in the area near the part origin. Notice on one end of the tab, all the fillets come to a point, as shown in Figure 23.20. This is clearly not right, although Import Diagnosis did not identify it as a problem.
4. Open a sketch on the flat face from which the tab protrudes. Right-click any edge where the tab intersects the sketch face, and select Select Tangency. Then click the Convert Entities toolbar button, and click the green check mark icon to accept the result, and exit the sketch.

   FIGURE 23.20 A corner where three fillets come together is not correct.

   

5. Right-click one of the long faces of the tab and select Select Tangency. This selects all but two faces of the tab. There are 16 faces altogether. Activate the Delete Face feature, and select the Delete and Patch option, select the two remaining faces of the tab, then accept the result. The model should remain a solid model, and the tab should be replaced by a smooth face.
6. Select the sketch created in Step 4 and extrude it to blind depth of 0.050 inch. Apply a fillet around the end face with a radius of 0.010 inch.
7. Activate the Move Face feature, and select all the faces of the two side tabs and the snap feature on the end. Use the Translate option, and the Right (YZ) plane as the direction, and use a distance of 0.25 inch. You should have no less than 21 faces selected. Faces that are parallel to the translate direction do not need to be selected, because they are automatically extended or trimmed to fit. If you are having trouble selecting the right faces, refer to Figure 23.21, and open the finished part on the DVD called Tutorial1finished.sldprt.

   FIGURE 23.21 Moving tabs and snap in a single Move Face feature

   

8. Save the part under a different name and exit.

Tutorial: Editing with Flex and Freeform Features

This tutorial steps you through importing and editing geometry using the Move Face, Flex, and Freeform features in SolidWorks.

1. Open the Parasolid file from the DVD called ellipse.x_t.
2. Increase the size of the part by using the Move Face feature with the Offset option. You can use the axis of the triad handle to drag the offset distance or key it in in the PropertyManager. Use an offset distance of about 0.08 inch. Make sure only the elliptical face of the model is selected.
3. Activate the Flex feature, and use the settings shown in Figure 23.22:
   • Select the body in the graphics window in the top selection box.
   • Select Bending option in the Flex Input section.
   • Select Hard edges in the Flex Input section.
   • Select 190deg for the angle.
   • In Trim Plane 1, set the distance to 1.9 inch.
   • In Trim Plane 2, set the distance to 4.5 inches.

     Accept the feature when you are done.

     FIGURE 23.22 Using Flex Bending to bend an imported part

     

4. Open a sketch on the Front (XY) plane, orient the view normal to it, and then sketch an ellipse with one end of the major axis at the origin and the rest dimensioned, as shown in Figure 23.23.

   FIGURE 23.23 Sketching an ellipse

   

5. Initiate a Split Line (Insert Curves Split Line) and select the bent face of the part. Accept the feature when you are done.

   Note

   The Split Line will split the outside and the inside of the curved face. If you select Shaded With Edges, you will be able to see the split on both sides.

6. Initiate a Freeform feature, and select the elliptical split face on the outside of the bend created by the Flex feature.

   Click the Direction 1 Symmetry option, and a gray plane should appear along the Right (YZ) plane.

7. Click the Add Curves button, and then snap the cursor to the symmetry plane and click to add a curve. The symmetry plane will highlight orange when it is selected. Add a second curve parallel to the first one about one-third of the way from the symmetry plane to the edge of the split.
8. Click the Add Points button, and place a point approximately, as shown in Figure 23.24.

   Place a point on the second curve in approximately the same location as the first point. Figure 23.24 shows one point on each curve.

   Click the Add Points button to deselect it when you are done.

9. Change the Continuity flag pointing to the edge of the split from Contact to Curvature.
10. Click on the curve on the symmetry plane, then click on the point on that curve. Drag the arrow handle to pull the point away from the part approximately, as shown in Figure 23.25.

    FIGURE 23.24 Locating a point

    

    FIGURE 23.25 Pulling the point to create a freeform shape from the existing face

    

11. Click on the second curve, and then click and move the second point in a way similar to the first point. When you are done, the part should look similar to Figure 23.26.

    FIGURE 23.26 The finished freeform surface

    

12. Save the file as a different name.

Summary

In recent years direct edit tools have received a lot of hyped press and marketing attention. However, CAD tools dedicated to working primarily as direct edit tools are not going to overtake the tools used by professionals who design and model for production. If anything, they will be used primarily by non-CAD specialists for simple editing and simple concept development, and possibly by downstream data consumers like FEA analysts or CNC (Computer Numerical Control) machinists.

The direct edit tools available within SolidWorks are powerful and are becoming more powerful with each release. While they might be best applied to imported data, they can also be applied to native SolidWorks data. This brings up questions of best practice and duplication of effort. Sometimes the changes involved in editing a feature that is near the top of a long feature tree can be time-consuming compared to simply moving a couple of faces.