CHAPTER 17

Dimensioning and Tolerancing

Dimensioning and tolerancing is an art form as much as a science. People become very passionate when discussing the right way to perform these tasks. In truth, the techniques are not so black and white, but are highly dependent on the industry, the means of manufacture, and the purpose of the drawing. Drawings might be used for quotes, manufacturing, inspection, assembly, testing, and so on; and the drawings, as well as the dimensioning and tolerancing used, for each purpose might need to be somewhat different in each circumstance.

While it is important to follow standards and use drawing conventions properly, this is not an argument that I want to reignite here. In this chapter, I will focus on how the available tools work. You will need to decide for yourself how to apply them in each situation. Refer to the SolidWorks Administration Bible (Wiley, 2009) for more information on standards and conventions.

Putting Dimensions on Drawings

The debate on how to get the dimensions from the model to the drawing is much like the “tastes great/less filling” debate. Each side of the issue has valid points, and the question is not likely to be resolved any time soon.

At the center of this debate is whether you should place the dimensions that you use to create the model directly on the drawing or whether you should use reference dimensions created on the drawing. In the following sections, I examine each method for its benefits and drawbacks.

Using Insert Model Items

Insert Model Items takes all the dimensions, symbols, annotations, and other elements that are used to create the model and puts them onto the drawing. Because these dimensions come directly from the sketches and features of the model, they are driving dimensions. This means that you can double-click and change them from the drawing the same way you can change sketch and feature dimensions, and with the same effect. As a result, changing these dimensions even from the drawing causes the parts and assemblies in which they are used to be changed.

You can insert the model items in several ways: on a per-feature basis, bringing only the items that are appropriate into the current view, or bringing items into all views. Insertion can be further broken down by type of item, and it can become as specific as pattern counts, Hole Wizard items, specific symbol types, and reference geometry types. To use Insert Model Items, you can choose Insert Model Items or can access this command from the Annotations toolbar. The Model Items PropertyManager interface is shown in Figure 17.1.

FIGURE 17.1 The Model Items PropertyManager interface

Often, the dimensions need to be rearranged to some extent, although SolidWorks does try to arrange them so that they do not overlap. Figure 17.2 shows the result of bringing dimensions into all views for the part. The part is on the DVD in the Chapter 17 materials.

Figure 17.2 contains duplicate dimensions, overlapping dimensions, unnecessarily long leaders, radius dimensions pointing to the wrong side of the arc, and a lot of awkward placement. This is what you can expect from using the automatic functions. At best, these dimensions require rearranging, and at worst, they probably require that you delete and replace some of them or move them to new views where they make more sense.

To move a dimension to another view, you can Shift+drag it from one view to the other (make sure that the dimension is appropriate in the destination view). To copy a dimension, you can Ctrl+drag it. If you cannot place the dimension in the view that you have dragged it to, then the cursor will indicate this with a special cursor symbol.

FIGURE 17.2 The default placement of dimensions into all views

If you approach this task by placing dimensions on a per-feature or per-view basis, it does not change the number of dimensions that you will have to move; it just means that you will insert fewer dimensions several times. Keep in mind that if you choose this method, there is a significant amount of cleanup and checking that you must do. The convenience of having the dimensions put into the views for you and the ability to actually change the model from the drawing are quite useful, but you may not save very much time or effort by doing things this way.

Using reference dimensions

One alternative to automatically inserting all model dimensions is to manually place reference dimensions. You create reference dimensions by using the regular Smart Dimension tool. At first, this appears to be simply re-creating work that you have already done, and this is somewhat true, but there is more to the story.

These dimensions are not duplicates of the model items. In fact, the reference dimensions that you manually place on the drawing are completely different from the dimensions that are used in the model. The dimensions serve completely different purposes in the two settings.

When modeling, I tend to dimension symmetrically, but only on one side, which would not be shown on a manufacturing or inspection drawing. I frequently use workarounds to avoid some special problem that forces a different model dimensioning scheme than I would prefer to use. Often, a feature is located from the midpoint of an edge, which involves no dimensions whatsoever. Sketch entities may have Equal relations, which also leave sketch elements undimensioned. Dimensions may lead to faces or edges that are not in the final model or to faces that are later changed by scale, draft, or fillets. Beyond that, when draft is involved, as is the case with plastic or cast parts, the dimensions of the sketch that you used to create the feature often have little to do with the geometry that is dimensioned on a print for inspection or mold building. Dimension schemes in models reflect the need for the model to react to change, while dimension schemes in drawings reflect the manufacturing or inspection methods, in order to minimize tolerance stack-up, and to reflect the usage of the actual part.

Although there are strictly technical reasons for dimensioning drawings independently from the way the model was dimensioned, there are other factors such as time, and the neat and orderly placement of dimensions. Time is an issue because by the time you finish rearranging dimensions that were inserted automatically from the model — checking and eliminating duplicates and then manually adding dimensions that were left out or that had to be eliminated because they were inappropriate for some reason, as well as ensuring that all the necessary dimensions are on the drawing — it would have been much quicker to manually dimension the drawing correctly the first time using reference dimensions.

In most cases, inserting model dimensions into the drawing is impractical for manufacturing or inspection drawings unless you have simple plates with machined holes. This is because of the amount of time required to rearrange and check the dimensions, the need to ensure that you have placed the necessary dimensions and taken geometric tolerancing into account, and the simple fact that the dimensioning and sketch relations needed for efficient modeling are usually very different from the dimensioning needed for manufacturing or inspection.

I recommend that you use the manual dimension placement option, which works much in the same way as when dimensions are added to sketches. Dimensions that you place in the drawing in this way are called driven, or reference, dimensions. In drafting lingo, reference dimensions are usually shown with parentheses around them. In SolidWorks, reference dimensions are simply driven rather than driving dimensions. To find the setting that controls the parentheses around reference dimensions, choose Tools Options Document Properties Dimensions Add Parentheses By Default.

Rapid Dimension

Rapid Dimension offers a manipulator wheel that shows the possible locations of a dimension you are trying to place. Rapid Dimension works for dimensions inside drawing views, not on dimensions on the sheet. It enables you to choose from either two or four options, and you can move between the options with the Tab key, making your selection with the Spacebar. You can also left-click on the manipulator to select an option The Rapid Dimension manipulator wheel is shown in Figure 17.3 in the placement of diameter and linear dimensions.

The tool does have some limitations, however. It does not seem to be capable of handling combined aligned dimensions and horizontal and vertical dimensions. For example, if you dimension an angled line, Rapid Dimension would only allow a dimension that is aligned to the angled line. If you dimension between the diagonal corners of a rectangle, it would not allow you to place the diagonal dimension, only the horizontal and vertical dims.

You can disable the Rapid Dimension manipulator and control some of the other dimensioning assistance tools in the Dimension PropertyManager. This might lead to some confusion, because it seems that there are three separate Dimension PropertyManagers. The one I am talking about here is the PropertyManager that appears when the Dimension tool is active in the drawing. You see a different PropertyManager when the Dimension tool is active in the part, and another one when you select an existing dimension on the drawing.

FIGURE 17.3 Placing dimensions with the Rapid Dimension manipulator wheel

Figure 17.4 shows the Dimension PropertyManager that gives you some control over automatic dimension tools (on the right).

FIGURE 17.4 The Dimension PropertyManager for choosing DimXpert or Reference dimensions

Reference dimensions and the DimXpert

You can apply reference dimensions to the 3D model or to the drawing. In this chapter, I talk mainly about adding them to the 2D drawing, but I do want to take a moment to talk about how reference dimensions in the model relate to the DimXpert functionality, which you will find later in this chapter.

Reference dimensions on the solid model

By default, when you go to add new reference dimensions to a solid model, you may see some error messages you aren't accustomed to seeing and some odd toolbars. If you are not expecting it, the DimXpert can interfere with reference dimension functionality.

When you activate the Smart Dimension tool in the part environment, a PropertyManager appears, giving you the option to use dimensions to drive the DimXpert (the default) or use it to place reference dimensions. Figure 17.4 shows this Smart Dimension PropertyManager for parts on the left and for drawings on the right.

Reference dimensions on the drawing

I've already made the case for why I think it is better to use reference dimensions on the drawing than model dimensions. This is opinion, of course, and I realize that for many simple parts, you actually can model them the way you would detail them, so the model items make more sense in that case. Many respectable power users use model items on drawings. I mostly model complex plastic parts, which are often only annotated with a handful of critical inspection dimensions that you can measure with available instruments.

Using the DimXpert

The DimXpert is a tool to apply reference (driven) dimensions with tolerances to models and drawings. DimXpert employs feature and topology recognition so it can work on either native data or imported data. Use the DimXpert tab at the top of the part Feature manager, and click the Autodimension Scheme button (the first button on the left) to apply dimensions to the entire model based on selected datums. The goal of DimXpert is to comply with ANSI Y14.41, which deals with 3D annotated models. The general consensus on this is that neither the standard nor the DimXpert tools are up to the rigors of daily production use at this time. The concept seems compelling, but the implementation is not yet practical.

When you use the dimensions and tolerances created with the DimXpert in conjunction with the TolAnalyst, you are able to do simple stack-up analysis. TolAnalyst is outside the scope of this book, because it is part of the Premium package and I confined this book to SolidWorks Standard. A limitation of this system is that you can only apply location or size dimensions; you cannot apply non-dimensional geometric form tolerancing such as parallelism, cylindricity, or flatness. All controls must drive size or location, and have associated dimensions.

When you use the DimXpert on a drawing, it first places a datum at a vertex or centerpoint. After that, it automatically dimensions the entire feature in the view that is the parent of the edge you select. Figure 17.5 shows the Dimension PropertyManager when DimXpert is activated. The image on the right shows a few dimensions applied by the DimXpert, along with the datum used for the dimensions in the view.

You can choose to place the DimXpert dimensions on the drawing when placing the views either through the second page of the Model View PropertyManager or on the Import Options panel (which is closed by default). No, it's not your imagination, this is about as obscure as SolidWorks could possibly make this functionality. Apparently they didn't really expect anyone to use it. Both pages of the Model View (Insert Drawing View Model, or click Model View from the View Layout tab on the Command Manager) are shown in Figure 17.6. The Import Options panel is shown at the bottom of the second page, although I have cut the second page off about halfway down.

You can find this functionality in one other place: when you drag views from the View Palette in the Task Pane. This interface appears in the image on the right in Figure 17.6.

FIGURE 17.5 Dimension PropertyManager for DimXpert in drawing

FIGURE 17.6 The setting to import DimXpert annotations is buried well.

Consensus on this functionality is that it is a work in progress, and while it may offer some interesting functionality, you may not find that it is ready to save you a lot of time when you are dimensioning and tolerancing parts on a drawing. It seems that it has particular difficulty with molded or cast parts, which typically don't have parallel faces.

Annotation views

Annotation views are views in the model in which annotations have been added. You can access annotation views from the Annotations folder in the model FeatureManager. They are created automatically when you add dimensions or notes to the part. You can use the annotation view in the model to show the note or dimension in the view in which it was created or on the drawing to help parse the dimensions into views where they are easily read.

Annotation views can be inserted manually or automatically. You can access the settings for annotation views through the right mouse button (RMB) menu of the Annotations folder of the model, shown in Figure 17.7. The image on the right shows part of the PropertyManager you get when inserting a named view on a drawing. It shows that the Front and Top views of the model have annotations associated with them (indicated by the A on the view symbol).

FIGURE 17.7 The Annotations folder RMB menu and the Model View orientation panel

Driven dimension color

Driven dimensions on the drawing display in gray, and this can be a problem when the drawing is printed out. There are two methods that you can use to deal with this printing problem. The first method is to set the Page Properties of the drawing to force it to print in black and white rather than color or grayscale. To find the Page Properties, choose File Page Setup. The Page Setup dialog box is shown in Figure 17.8.

The second method is to set the color for driven dimensions to black rather than gray. You find this color setting by choosing Tools Options Color Dimensions Non-Imported (Driven).

FIGURE 17.8 The Page Setup dialog box

Ordinate and baseline dimensions

Ordinate and baseline dimensions are appropriate for collections of linear dimensions when you have a number of items that can all be dimensioned from the same reference. Flat patterns of sheet metal parts often fall into this category. When you apply ordinate dimensions, a zero location is selected first, followed by each entity for which you want a dimension. When dimensions become too tightly packed, SolidWorks automatically jogs the witness lines to space out the dimensions adequately. You can create jogs manually by using the RMB menu. Once you create a set of ordinate dimensions, you can add to the set by selecting Add To Ordinate from the RMB menu.

Baseline dimensions are normal linear dimensions that all come from the same reference and are stacked together at a defined spacing. To find the default settings for baseline dimensions, choose Tools Options Dimensions Offset Distances.

You can access ordinate and baseline dimensions from the Dimensions/Relations toolbar or by right-clicking in a blank space, selecting More Dimensions, and then selecting the type of dimension that you want to use.

Autodimensioning

If the Insert Model Items feature is not likely to produce dimensions that are usable in a manufacturing drawing, then the Autodimension feature is even less likely to do so. However, if you use autodimensioning in a controlled way, in the right situations, it can be a valid way to create selected dimensions. The Autodimension PropertyManager is shown in Figure 17.10. Autodimension is only available in the drawing environment. In the part environment, similar functionality for sketches is part of the Fully Define Sketch tool. To access Autodimension, click the Smart Dimension toolbar icon and click the Autodimension tab in the PropertyManager.

FIGURE 17.9 Ordinate and baseline dimensions in the same view

FIGURE 17.10 The Autodimension PropertyManager interface

The Autodimension function can fully dimension the geometry in a drawing view. This is best for ordinate or baseline dimensioning where many dimensions are derived from a common reference, as is often the case with sheet metal parts or a plate with many holes drilled in it. You should limit the use of this option to cases where that type of dimensioning is what you would choose, having the choice of all available types of dimensions — do not allow the software to dictate the dimensioning scheme for your drawing.

Reference sketches

For some types of dimensions, you may need to create additional reference sketch entities. For example, with angle dimensions, it may be desirable to add construction lines to help define the angle. You can add centerlines as separate axis-like entities, as discussed in Chapter 16, but you can also sketch in centerlines manually if needed. This type of sketch is most often attached to the view rather than the drawing sheet.

Understanding dimension options

The Dimension PropertyManager contains settings, default overrides, tolerances, styles, and several other important settings for use with dimensions. The PropertyManager for driven dimensions is shown in Figure 17.11. I cover styles and tolerances specifically later in this chapter; the other tabs of the Dimension PropertyManager are as follows.

FIGURE 17.11 The Dimension PropertyManager interface

Dimension Text

The Dimension Text panel enables you to add text to the dimension. You can add lines of text both above and below the dimension value itself, and you can also add text before and after the DIM value on the same line. The DIM field is what places the actual value; if this syntax is somehow deleted, you can type it back in and the dimension will still work.

The Dimension Text panel includes some formatting tools, such as justification settings and a setting for the position of the dimension line. The last two rows of buttons include the more commonly used symbols, with access to the complete library, such as any custom symbols that you may have made for the library.

Primary Value Override

The most famous bad habit former AutoCAD users use is overriding dimension values. Apparently due to popular demand, the Primary Value Override is now available in SolidWorks, in the Dimension PropertyManager, as shown in Figure 17.11. This option was added to the software mainly to enable the creation of dimensions with words instead of numbers, as shown in Figure 17.12.

FIGURE 17.12 Using the Override Dimension value

Display Options

You can control the default setting for parentheses around driven (reference) dimensions in the Add Parenthesis By Default dialog box by selecting the choosing Tools Options Document Properties Dimensions Add Parentheses By Default.

Although you can also control dual dimension defaults in the Options dialog box by choosing Tools Options, you can turn them on and off from this interface for individual dimensions. When you enable the Dual Dimension option, SolidWorks uses the settings from the Tools Options menu.

The foreshortened radius is only valid for individual radial dimensions. A foreshortened radius is shown in Figure 17.13. Foreshortened radius dimensions are typically used for large radii when dimensions to the centerpoint are not important. The Foreshortened radius function does not work on diameter dimensions. The inspection dimension is shown in Figure 17.13 with an oval around the dimension.

You cannot foreshorten a diameter; however, you can dimension a diameter and then hide the extension line and dimension line in one direction. This option is found by right-clicking on boththe extension line and dimension line, and there is an option in the RMB menu for hide extension line and hide dimension line. This is useful if you have a diameter dimension in a detail view where the opposite side of the diameter is outside the detail view. This can also be used for linear dimensions that terminate to a known end outside the drawing view.

FIGURE 17.13 A foreshortened radius

Witness/Leader Display

This panel enables you to set the arrows and dimension lines to be placed inside the witness lines. You can perform this function more easily by using the handles on the arrowheads. From this panel, you can also change the display type of individual arrowheads.

Break Lines

When you select the Use document gap option in this panel, the witness, or extension, lines of the selected dimension are broken by other crossing dimension lines, witness lines, or arrows. This is shown in Figure 17.14.

FIGURE 17.14 Broken witness lines

Formatting dimensions with the Dimension Palette

When you select a dimension on a drawing (the dimension can be a model item or a reference dimension), a small symbol appears above and to the right of the dimension. If you click the symbol, the Dimension Palette expands. The Dimension Palette enables you to:

• Add tolerances
• Specify dimension precision
• Assign styles (favorites)
• Apply parentheses
• Center the dimension between the witness lines
• Apply inspection dimension
• Offset the text with a leader
• Establish horizontal and vertical justification
• Add text on top, before, after, and below the dimension value

The Dimension Palette appears when you select a dimension and disappears when you move the cursor away from it. The Dimension PropertyManager still appears, but the Dimension Palette pops up right next to the dimension, making it very easy to use. Figure 17.15 shows the Dimension Palette.

FIGURE 17.15 Adding text and tolerances to dimensions using the Dimension Palette

The Dimension Palette seems to be the most convenient place to make these alterations to the basic dimension itself.

Adding Tolerances

You can add dimension tolerances in the Dimension PropertyManager, which you can activate by selecting the dimension that you want to modify. Available tolerance types include:

• Basic
• Bilateral
• Limit
• Symmetric
• MIN
• MAX
• Fit
• Fit with tolerance
• Fit (tolerance only)

Refer to the Tolerance/Precision panel shown in Figure 17.11. The appropriate number entry fields are activated when you assign the corresponding tolerance type to the dimension. The tolerance types that are available in SolidWorks are shown in Figure 17.16.

FIGURE 17.16 The available tolerance types in SolidWorks

Changing precision values

In SolidWorks, precision means the number of decimal places with which dimensions are displayed. Typically, SolidWorks works to eight places with meters as the default units. You can create templates that use up to eight places as the default setting, and then change the number of places for individual dimensions as necessary. The first of the two boxes under Precision is used for the dimension precision, and the second is used for tolerance precision.

You can change Precision values for individual dimensions in the PropertyManager for the dimension as well as the entire document by choosing Tools Options Document Properties Units.

Using Geometric Tolerancing symbols

The full range of Geometric Tolerancing symbols is available for control frames, datums, datum targets, and so on. You can use the Geometric Tolerance dialog box to build control frames. This dialog box is shown in Figure 17.17. For commonly used Geometric Tolerance symbols, you may want to create and use styles.

FIGURE 17.17 The Geometric Tolerance settings

Using Dimension Styles

You can use dimension styles to apply many items to dimensions. Styles were formerly known as favorites in SolidWorks. Unlike notes, this is not limited to fonts and formatting. Some of the most common uses of dimension styles are

• To add standard tolerances to dimensions
• To set precision values for dimensions
• To add text, such as TYP, to a dimension
• To add a commonly used GD&T (geometric dimensioning and tolerancing) reference

You can save styles from one document and load them into another document, even between document types. For example, you can load part dimension styles into a drawing.

When a style is updated from an external file, any document that it is linked to also updates. In addition, you can break links to external styles (with the appropriate button on the Styles panel). Otherwise, dimension styles have very similar functions to the other types of styles; the functions of all the buttons on the Styles panel are the same.

Aligning Dimensions and Annotations

When you place dimensions and annotations on a drawing, it is nice to have them lined up in an orderly way. Drawings contain a lot of information, and that information needs to be easy to read. Keeping items lined up in horizontal and vertical alignment is one of the keys to making the information on a drawing easily accessible.

SolidWorks has a toolbar just for the alignment of dimensions and annotations. The toolbar is shown with labels for individual icons in Figure 17.18. To add the Align toolbar to the CommandManager, right-click one of the CommandManager tabs, and select Customize CommandManager. Then click the new tab that appears and select the Align toolbar from the list.

FIGURE 17.18 Using the tools from the Align toolbar

Using the alignment tools

The alignment tools are all pre-select tools, and so it is best to box-select (or Ctrl+select) the dimensions and annotations you want to align first, and then click the toolbar icon. For example, to align a set of balloons to the right, you would drag a box around the balloons, Ctrl+select any balloons you could not select with the box, and then click the Align Right button. These tools work best with larger selections of dimensions or annotations. For aligning individual dimensions or pairs of dimensions, it might be better to use the drag methods discussed in the section “Inferencing alignment and grid snapping.”

Using the alignment tools Align Collinear/Radial and Align Parallel/Concentric creates persistent relationships, so those dimensions aligned with the tools will maintain that alignment. The other tools on the Align toolbar do not work this way. To break an alignment created by these tools, select Break Alignment from the RMB menu.

Using the Group tool allows a set of dimensions and annotations within a single view to maintain the spatial relationships for dimensions that were not aligned with the alignment tools, until they are ungrouped.

Inferencing alignment and grid snapping

When you drag individual dimensions on a drawing, they are snapping to a grid. (Annotations do not snap to the grid.) This is one way that SolidWorks helps you to align them. If you drag one dimension level with another, either horizontally or vertically, a line appears and the dimension inferences the position of the other dimension, just like lines snapping in model sketches.

Annotations will inference other annotations, but they won't inference dimensions, and they won't snap to the grid.

If you want to disable both kinds of snap (grid and inference) on the fly, just hold down the Alt key while dragging, and the dimension or annotation will slide freely. To permanently disable the snapping, go to Tools Options Drawings Disable Note/Dimension Inference. To disable the snap, make sure this option is selected. You should be aware that this option controls both the snap to the grid and the inferencing of one dimension or annotation to another. You cannot separate the grid from the inferencing.

If you like the snaps and want to change the spacing, you can do that by selecting Tools Options Document Properties Dimensions Offset Distances and changing the appropriate numbers for the distance of the dimension from the edge of the part and the distance between dimensions.

If you are used to older versions of SolidWorks, you will remember that the snapping used to depend on where you selected the dimension — from the top, middle, or bottom — and it would line up with other dimensions using the same references. Newer versions of SolidWorks are more simplified, and I think they work better.

If you want a group of dimensions or annotations that you have aligned to maintain their current alignment, box-select them and use the Group function from the Align toolbar. All of the selected dimensions and annotations must belong to the same view.

Using Dimension Palette alignment options

The Dimension Palette, mentioned earlier in this chapter, enables you to surround a dimension with all of the necessary information, such as additional text, tolerances, symbols, justification, leader control, dual dimension display, and other useful information. It can also perform some alignment functions. If you multi-select dimensions, and activate the Dimension Palette, you see what is shown in Figure 17.19. In this case, the Dimension Palette is used to apply the Align Stagger function to a set of vertical dimensions to pack them in close to one another. This function is not found on the Align toolbar. However, notice that it also has some of the Align toolbar functionality, including bottom, top, left, and right justification. The functions have different names and symbols in the Dimension Palette than in the Align toolbar, but they appear to do the same thing.

FIGURE 17.19 Selecting alignment options from the Dimension Palette

The Dimension Palette is one of my favorite tools in SolidWorks drawings because it consolidates a lot of functionality into a small space that is available right where you need it. When it was originally released, many users thought that it got in the way, but the small activation icon solved that problem, and the functionality has only improved.

Arranging dimensions automatically

Every few releases, SolidWorks improves the automatic dimension-arranging tools. But to me, they have a long way to go before I will trust them to arrange dimensions on a large drawing, where they would offer the most benefit. Sometimes they do a good job on simple rectangular parts, but they don't save much time on the complex parts.

When you put Model Items onto a drawing, SolidWorks automatically arranges the dimensions. The alignment option on the left side of the Dimension Palette is called Auto Arrange Dimensions. Also, when you use the Autodimension function mentioned earlier in this chapter, SolidWorks automatically arranges the dimensions for you.

The best auto-arrange functionality probably comes with balloons. The Auto Balloon functionality is shown in Figure 17.20. Balloons are part of assembly drawings, and as such, they are covered in more detail in the SolidWorks 2011 Assemblies Bible (Wiley, 2011).

FIGURE 17.20 Using options for automatic ballooning in an assembly drawing

The best way to use these tools with dimensions and general annotations is probably in small, controlled situations until you learn how they react to the type of work you tend to do frequently. Selecting items in groups that are close to where they need to go may help the automatic tools do a better job.

Tutorial: Working with Dimensions and Tolerances

In this tutorial, you can use a single part in several different ways to demonstrate different dimensioning and tolerance functions. Follow these steps to learn more about these topics:

1. Open the part from the DVD called Chapter 17 Tutorial.sldprt.
2. Open the drawing from the DVD called Chapter 17 Drawing.slddrw.
3. Tile the windows by choosing Window Tile Vertically, and drag the part from the top level of the FeatureManager into the drawing window. This automatically populates the four drawing views.
4. Delete the Top view, leaving the views as shown in Figure 17.21.

   FIGURE 17.21 The drawing after Step 4

   

5. Choose Insert Model Items, and ensure that the Select All option is selected for Annotations and the Marked for drawing option is selected for Dimensions. Also make sure that the Source/Destination drop-down list is set to Entire Model. Click the green check mark icon and watch the drawing populate.
6. The resultant drawing is quite cluttered. Delete and move dimensions so that the drawing looks like Figure 17.22.

   FIGURE 17.22 The drawing after dimensions have been deleted and moved

   

7. Shift+drag the surface finish symbol to the Right view, and do the same with the 1.900-inch dimension. You may have to first Shift+drag it into the other view, and then drag it again to correctly attach or position it.
8. Create a set of horizontal ordinate dimensions from the left end of the part, and dimension the X position of each column of holes. Do the same for rows of holes, using the bottom edge of the Front view as the zero reference. Remember that you can create ordinate dimensions by starting a normal Smart Dimension, right-clicking to display the More Dimensions list, and then selecting your choice.
9. If necessary, add center marks and centerlines to the view for clarity.
10. Select the.188 diameter dimension, and in the Dimension Text box, type TYP after the <DIM> text, and add a bilateral tolerance of +.003, –.005. Save this as a style by clicking the Add Style icon.
11. Apply the newly created dimension style to the R.100 dimension. The results up to this step are shown in Figure 17.23.

    FIGURE 17.23 Dimensions and tolerances after Step 11

    

12. Make one of the dimension leaders for either the.188 or the R.100 dimensions cross the extension lines of the 4.500 dimension. Then select the 4.500 dimension, and in its PropertyManager select the Use Document Gap option in the Break Lines panel, on the Leaders tab.
13. Place a B datum marker on the circumference of the smaller arc on the left end of the part. Create a Geometric Tolerance control frame, as shown in Figure 17.24.

    FIGURE 17.24 Creating a Geometric Tolerance control frame

    

14. In the Right view that shows the thickness, select the.100 dimension, and add a tolerance and a note below the text using the Dimension Palette, as shown in Figure 17.25.

    FIGURE 17.25 Using the Dimension Palette

    

15. Delete the last two dimensions of the horizontal ordinate group (3.837 and 4.076). Start a new Detail view that includes the holes those dimensions called out, as shown in Figure 17.26. Place the detail view above the main view.
16. Right-click the zero for the horizontal ordinates and select Add To Ordinate. Place the two ordinate dimensions in the detail view.
17. Use the Geometric Tolerance tool to make a Flatness call out of .002. Add a leader to the control using the PropertyManager, and attach the leader to the .100 thickness dimension in the Right view.

FIGURE 17.26 Adding more dimensions and annotations

Summary

The argument about how to set up and use dimensions on drawings is as old as the process of creating geometrical plans from which objects are built. It is often difficult to separate fact and best practice from opinion. Although I leave it up to you to decide these issues for yourself, this chapter is intended to help you understand how to create the type of drawing that you want.

The biggest conflict in this subject arises over whether to place live model dimensions on the drawing or to allow the requirements of the drawing to specify which dimensions are placed where. I am by no means impartial when it comes to this question, but again, you must make the choice for yourself.