You create presentation files by using an .ipn template and then referencing an existing assembly. To create this presentation, start with the Standard (mm) .ipn template:

The first step in creating an assembly explosion is referencing an assembly. A presentation file can reference only one assembly file at a time, but the assembly can be used to generate as many explosions as you might need to properly document your design. For example, you may create one explosion to be used as a 2D drawing view and another explosion to be used as an animation. You may also choose to explode each subassembly in its own explosion. Walk through the following steps to create an assembly explosion:

You'll now see the selected assembly in your presentation graphics area. It's time to start adding tweaks to explode the assembly. A tweak is simply a stored movement vector for a selected set of one or more components. You can define both linear and rotational tweaks. In the next steps, you'll create a linear tweak by first establishing a move direction, then choosing a component to move, and finally setting the move distance:

Once you create a tweak or tweaks based on one set of inputs, you can continue to tweak additional components with new inputs by first clicking the Clear button without dismissing the dialog box. Now that you have created a basic linear tweak, you'll explore how to create more advanced tweaks in the next section.

You can add rotational tweaks in much the same way as you created the linear tweaks, though rather than indicating the x-, y-, or z-axis for linear direction, the x-, y-, or z-axis is used as an axis of rotation, and the tweak value is entered as degrees of rotation rather than a linear distance.

If you're tweaking only one component at a time and you're comfortable with the selection, orientation, and direction behavior, you can establish direction, choose your component, and input the tweak distance all with one mouse click. You can try this with the cyan-colored gib plate.

Your presentation should look similar to Figure 12.3.

Figure 12.3. Creating tweaks

Trails are added by default. A trail is a line (or an arc in the case of a rotation tweak) that is displayed in the graphics area showing the start and endpoints of a particular tweak. By default, the start and endpoints are defined by the three-dimensional geometric center of all the components that are chosen for a tweak. However, an optional fourth step in the tweak creation process is to manually select the tweak points by selecting one or more points on each of your selected components. Here are a few more points to know about trails:

Don't forget that the browser filter controls the way tweaks are listed in the browser. When in the Assembly View, as you create tweaks, a browser node representing that tweak is generated in your browser and nested under the selected components that are part of that tweak. When in the Tweak View, tweaks are listed as line items and the components are nested below them. By selecting the tweak in the browser, you can enter a new movement value.

If your assembly is large or complex, consider making several explosions and tweaking only a few components per explosion. You can add explosions by clicking the Create View tool. Each subsequent time the Select Assembly dialog box is shown, a new assembly file cannot be specified. You can, however, choose a different view, positional, or LOD representation than your previous explosions.

If the end goal of your presentation is to simply create an explosion that looks good in one or more 2D drawing views, then you already know just about everything you need to know, and you never have to use more than two tools inside the presentation environment. Simply continue adding tweaks as needed.

Before you save your file and move on to creating your drawing, make sure to set your camera view up exactly as you'd like to see it on the page. Use Zoom, Orbit, and the ViewCube in conjunction with the Precise View Rotation feature to get a view that makes things as clear as possible. Then right-click in the graphics area and choose Save Camera. You can use this saved camera to create a view in the 2D drawing. You can also right-click and choose Restore Camera any time you have changed the camera view.

You can group and reorder tweaks for the purpose of animating components in a presentation. For instance, in the steps in the "Creating a Basic Explosion" section earlier in this chapter, you pulled the cap screws out all at once and then rotated them one at a time. You may want to have these actions separated, reordered, or grouped in order for them to behave correctly when animated. To see how this works, follow these steps:

Although the rotation of the cap screws is still not true to life, you should be able to see that you can create tweaks in any order you choose and then group and reorder them as required later.

You can create assembly instructions for a presentation animation to share with a customer, present to a group, or be used by the people on the shop floor. The animations and instructions can be published to a DWF file and viewed with the free Autodesk Design Review application. Follow these steps to explore how to create assembly instructions. You can skip the first two steps if you have the file from the previous exercise open still.

Here are a couple of other actions you can take to organize tasks:

If you need to share assembly animations and instructions with someone who does not use Inventor, such as the people on the shop floor, you can publish the presentations to a .dwf file:

The key differences between the two DWF file types is that the 2D DWFx can be read by Windows Vista and XP (with Internet Explorer 7 installed) without the need for an extra viewer such as Autodesk Design Review. 3D DWFx and DWF files still require Design Review. Note too that the DWFx file is generally on the order of twice as large.

You can invite vendors and clients as well as the shop floor to download Design Review for free from the Autodesk website.

By default, Inventor templates are stored in and accessed from Program FilesAutodeskInventor 2010Templates. The default location is set on the File tab in the Application Options dialog box under Default Templates. Click the Tools tab, and click the Application Options button to access the Application Options dialog box.

For stand-alone users, consider using this same location for your design projects. If you're part of a networked workgroup, you should create a template folder on a shared network drive and change the default templates path accordingly.

The default template location can be overridden on a per-project basis as well by setting the templates location in the project file configuration. Keep in mind that if you have a template location set in Application Options and another set in the project file, the project file always takes precedence.

Prior to Inventor 2008, the .idw file format was the only native 2D file type recognized by Inventor. DWG TrueConnect, introduced with Inventor 2008, enables you to use both .dwg and .idw as valid file formats in Inventor's Drawing Manager.

Using .dwg as your file format enables you to open Inventor DWG files in AutoCAD (or an AutoCAD vertical product such as AutoCAD Mechanical) without going through a translation process. Although the data you create natively in Inventor cannot be manipulated directly in AutoCAD, all of the Inventor data can be viewed, measured, and printed using conventional AutoCAD commands.

Choosing .dwg as your default file format allows downstream consumers of your designs to view your 2D drawing documents in AutoCAD without having to purchase or install Inventor or download the Inventor file viewer. Vendors, customers, or other internal personnel can open the native Inventor DWG file and view, measure, and plot the Inventor data, or they can even add AutoCAD data to the file to create a hybrid document that can be viewed quickly and efficiently in either application.

For Inventor users, there is essentially no difference between using .dwg or the traditional .idw file format. The native .dwg file includes a Layer 0 in the layer list and an AutoCAD Blocks folder in Drawing Resources. These are the only noticeable differences between the two file formats.

An .idw file can always be saved as an Inventor DWG, and vice versa, without any loss of fidelity or data. If there's a good chance of someone wanting to see a DWG version of your Inventor file, you might consider choosing .dwg as your default file format.

Inventor's Task Scheduler enables you to batch convert a set of IDW files into DWG files.

When you start a new drawing from one of the templates installed with Inventor, a border and title block are already present on the sheet, and the sheet is set to a default size. You can change the default sheet size by choosing Edit Sheet from the sheet's right-click menu in the browser. If you're using the ANSI (in) template, the default sheet size is C. If you change the sheet size to D, the border on the sheet updates automatically to accommodate the change in sheet size.

To have your templates default to a different size of sheet, follow these steps:

Now when you start a new file from the template, this new sheet size will be active.

If needed, you can add sheets to your template, which is recommended if most of your design documents require more than one sheet. It is recommended that you use caution when creating multiple sheet sets of a sizable number, because performance may suffer, depending upon the size and complexity of the models you are detailing. Be aware too of "putting all of your eggs into one basket," should a file become corrupt or lost. To insert a new sheet into your document, follow these steps:

The default border that's instanced on the Inventor templates may not meet your needs. You should first delete the default border from your sheet before creating a new border; then follow these steps:

Recall that this removes the instance of the border from the sheet. The border definition is still stored in the Borders folder of the Drawing Resources node.

To create a new, custom border in your template, follow these steps:

Customizing title blocks is done in much the same way as borders. Title blocks typically contain more text-based information than the border, so the concentration here will be on creating sketch text in this section. There are three common ways of creating a custom title block:

In this next section, you will bring in an existing AutoCAD title block and make it intelligent to Inventor. In doing so, you will explore the tools used to create a title block used in the other methods mentioned. Although not required, you should probably first delete the default title block from your sheet before creating a new title block. To do this, follow these steps:

Obviously you have not configured the entire title block at this point, but before going any further, it is important to understand where the properties you linked to the title block text fields are coming from. You can find these properties in the file iProperties. Follow these steps to change an iProperty in the file and see that change show up in the title block:

Your title block will have updated the two fields automatically based on the iProperty changes you made, demonstrating that you have linked those fields to the iProperties of this particular drawing file.

Each Inventor file has its own iProperties allowing you to pull that information into your title block. There are two distinct areas from which you can draw iProperties into your title block: from the drawing file or from the model file.

Table 12.1 lists the standard iProperties available. Each of these can be accessed from the Type drop-down in the Text Format dialog box as described in the previous steps. You'll learn more about iProperties in Chapter 13.

Follow these steps to modify a title block so that it is pulling information from the model iProperties. You'll note that this title block is calling the model filename iProperty for the drawing title. Most of the other fields are being pulled from the drawing iProperties. The field you will be modifying is static and needs to be set to pull for the model iProperties.

In addition to iProperties, you can use some other standard file properties to fill out your title block automatically. You can access them from the Type drop-down in the Text Format dialog box just as you did the iProperties. Table 12.2 lists several general properties that can be called into a text field.

Follow these steps to set up the sheet number area of the title block to call on general file properties of the drawing file to automatically fill out the title block:

You can also create fields in your title block to enter information manually using what is known as a prompted entry. However, experienced Inventor users will tell you that prompted entries should be used sparingly, for two reasons.

First, information entered into a prompted entry field is stored in the title block and nowhere else. This creates a limitation in that if you need to update the title block for your entire drawing library at some point in the future, you can do so easily with Inventor's Drawing Resource Transfer Wizard, which can swap out old title block definitions with a new one, en masse. (See Chapter 13 for more on this tool.) This works well when title blocks have been populated with iProperties, because the information resides in the file, not the title block. However, if a prompted entry was used, that information will not be carried over, because it exists only in the old title block instance.

Second, since iProperties are stored in the file, there are a couple of important tasks that can be performed on them:

Getting in the habit of using iProperties will pay large dividends in the future, once you have created many Inventor files. With these things in mind, you should use prompted entries in title blocks rarely. Here are the steps for creating a prompted entry in a title block if you determine that it is required:

You can edit a prompted entry in a title block by expanding the block instance in the browser and double-clicking the Field Text node. If no prompted entry is established, you will be able only to view the fields.

Sketched symbols are created, edited, placed, and managed much like other drawing resources, but there is no limit to the number of sketch symbol instances you can place on a sheet. Like other drawing resource definitions, sketched symbols are placed by double-clicking the definition node in the browser or using the User symbols icon found on the Symbols panel of the Annotate tab.

Sketched symbols can optionally include a leader. Using a leader, you can associate a sketch symbol with a model so that model-specific properties can be displayed in the symbol. For example, you could create a sketch symbol that calls out a component's mass:

You'll notice that symbol in Figure 12.6 has a bit more geometry than the simple symbol you just created. You can make a sketch symbol as elaborate as you like, but for the purposes of this exercise, the Mass property reference is all that is required. A finished symbol named Mass_2 has been created for you in this drawing file.

If the Mass shows up as "N/A," it indicates that the model needs to be updated. You can open the assembly model and go to the Manage tab and click the Update Mass icon to do this. Then return to the drawing to see the update.

Figure 12.6. Applying sketched symbols to a drawing view

Here are some more sketch symbol points to remember:

Sheet formats are a preset collection of a drawing sheet, border, title block, sketched symbols, and/or base and projected views. They essentially give you the ability to quickly generate multiview drawings just by referencing a single model file. To create a multiview drawing, follow these steps:

You will note that a new sheet has been created to the specifications of the sheet format and set active. This technique is ideal if you find yourself detailing similar designs of common size and complexity.

To save your own sheet format, set up your sheet the way you like it, select Create Sheet Format from the active sheet's right-click menu in the browser, and name the sheet format as you'd like.

Here are some more sheet format points to remember:

You can copy drawing resource definitions from drawing to drawing by following these steps:

You can use this technique to add both new drawing resources and update existing resources with an updated change. You can also select the entire Drawing Recourses folder in one drawing and paste it into the Drawing Recourses folder of another drawing. You will be prompted to replace or make a new instance of any duplicate resources.

The copy-and-paste technique is efficient for single changes or transfers between two drawings, but to push one or more new or updated design resource definitions to multiple drawings, use the Drawing Resources Transfer Wizard discussed in Chapter 13.

The true key to understanding how styles are used to determine the formatting of everything you can create on a drawing sheet is the notion of object defaults.

In the previous example, it was clear that the majority of a designer's day-to-day drawing work is focused on creating prints for manufacturing. Therefore, the styles used for that type of drawing would be the styles set up as the object defaults. Object defaults are automatically set as the current styles in the template drawings. In that example, the object defaults would likely be configured as shown in Table 12.3.

Now that you understand the overall concept of object defaults, follow these steps to see how they are managed:

When setting object defaults, you typically want to use the most common style. Of course, you can always use another style by manually selecting the style from the Style drop-down as you place the object or by selecting an existing object on the page and then choosing the style from the list. You'll note that when you select an existing object, the Style and Layer drop-downs display that object's style and layer.

Objects that have been set to a specific style, rather than following the By Standard, will not update if you make any modifications to the object defaults. However, the objects will update if the specific style is updated. A quick way to get a set of objects (like our balloons, for example) to return to their object default is to window or Ctrl-select the objects on the screen and then select By Standard from the style drop-down. All the objects will update to use the newly selected standard.

As evident in the balloon example, you can have multiple styles for the same object type. Or you can have a single style that you always use. It's up to you to choose how many styles you have for each type, which will be dictated largely by need. Although this section will not go through all the settings for all the styles, you will explore how to create and configure a new style as a foundation to creating all style types.

Although the settings for each style type vary, the concepts for creating them remain consistent throughout all styles. These concepts are as follows:

A basic example of a substyle in the modeling environment is the color style, which is a substyle of the material style. Once you apply a new material to a part, not only are you changing its physical parameters but you're potentially changing its color so that it shows the material's color substyle.

The use of substyles in the Drawing Manager is extensive. Almost every kind of annotation you create in a drawing contains some kind of text (dimensions, weld symbols, and parts lists), and many make use of leaders. The text style and leader style, therefore, are frequently used as substyles of other styles. This basically provides one-stop shopping if you wanted to quickly change all the text on your document. If you wanted to change the font for all text, for example, you wouldn't have to go to the parts list style and change the font, then to the dimension style and change the font, and so on; instead, you would simply change just one or two text styles that are being called into those other styles.

Substyles are coupled with their parent styles, which means a substyle cannot be purged if it's in use by another style. If you cache a high-level style into your document from the library or if you save a high-level style into the library from your file, all substyles participate in those operations.

Styles are an extremely powerful formatting tool that enables you to quickly change the entire face of a document. This also serves as a warning that modifying styles without understanding how they work can quickly generate unexpected results.

Each drawing template that comes with Inventor has a full set of styles saved (cached) in the drawing document. Although you can use the style library as a sharing and update tool, there is no direct link between objects on your sheet and styles in your library. Any in-use style is loaded into your document either automatically or manually.

If your project is set to use the style library (the Use Style Library setting is Yes or Read Only), then it's important to keep your style definitions in sync between your template file and the library. If your project is using the style library and you have a style in the library that has the same name as a style in your template and those styles have different settings, the definition in the library automatically overwrites the definition in the template each time it's used to start a new drawing (a warning dialog box is shown when this condition is detected).

The best way to ensure synchronization is to open your template file and run either the Update Styles tool (which pulls updates from the library) or the Save Styles To Style Library tool, depending on which way you want to transfer the styles. You can find both of these options and the Purge tool on the Manage tab.

Creating views in an Inventor drawing is a very intuitive process. You'll start by creating some basic views of a part file, while exploring the procedure and options along the way. Before you create any views, first open the part to become familiar with it.

Here are some tips for working with base views:

Once a base view is created, you can quickly create other views based on it without having to specify the model again:

Figure 12.8. Drawing views in the browser

Here are some tips for working with projected views:

You can move drawing views between sheets by dragging and dropping the browser nodes. When a projected view is moved to a different sheet than its parent, a view arrow is generated automatically on the parent view.

To move a view, follow these steps:

To copy a view, follow these steps:

Section views are created by "sketching" a line across an existing view, to define the section cut. The sketch is created automatically for you as you define the section line.

To create a section view, follow these steps:

Look at the browser to see how the section view was added as a child view of the base. Also, notice the sketch that was created on the base view listed just above the section view node (Figure 12.9). This sketch is the section line itself and can be edited like any other sketch. You can add or remove constraints (including sketch dimensions) as needed to precisely position the section line around your base view. You do this by right-clicking the sketch in the browser and choosing Edit Sketch, just as you would any other sketch.

Figure 12.9. Part section view

Here are some tips for working with section views:

You defined the section line on the fly during the previous exercise. Now you will bring in a sketch created in the part model and use it to create a section view. Figure 12.10 shows the sketched line in the model.

Figure 12.10. Section line sketch on model

To create a section from a model sketch, proceed with these steps. If you still have mi_12a_051.idw open, you can skip to step 3.

Your section should look similar to Figure 12.11.

Figure 12.11. Section using model sketch

You can also use a breakout to show a cutaway. Unlike the Section View tool that creates a new view, a breakout is a cut operation you perform on an existing view, such as our right-side projected view.

Breakouts start with a closed loop profile drawn on a view sketch, so you'll begin there as well. It is important to note that in order to use a sketch for a breakout, it must be associated to the drawing view. To create an associated sketch, first select the view, and then click the Create Sketch button. Clicking the Create Sketch button without selecting the view first will result in a sketch that is not associated with any view.

To create a breakout view, follow these steps:

Your result should look similar to Figure 12.13. Note the Break Out view node in the browser. You may be able to see some portions of the internal parts, because they have been cut away as well. You'll explore how to control this in the coming pages.

Figure 12.13. Break Out view node

Next you'll open a file and modify a breakout view to explore the other depth options:

Figure 12.15. Break out through part option

It should be pointed out that the preceding steps have created a situation that may yield inconsistent results by excluding some of the parts from the section participation settings and then setting the depth of the breakout to Through Part. Typically you would use the section participation settings only with the first three depth options and not with the Through Part option.

You will have noticed that, as you modified the breakout, the isometric view was linked to those changes. This was because isometric projected views created for views with a breakout inherit the breakout by default. Orthographic projected views, such as the top view, do not inherit the breakout.

To switch the inheritance setting of the isometric view, right-click it and select Edit View. Go to the Display Options in the Drawing View dialog box, and deselect the Break Out check box in the Cut Inheritance area, as shown in Figure 12.16. You can also turn on hatching from this tab.

Figure 12.16. Cut inheritance for isometric views

You can use the detail view to enlarge and segregate a particular portion of a drawing view as a new view. Follow these steps to explore the options of the detail views:

Here are more options for detail views:

There are four standard centerline and center mark tools as well as an automated centerline tool. These tools are called Centerline, Centerline Bisector, Center Mark, and Centered Pattern, and you can access them from the Symbols panel of the Annotate tab (look for the four buttons next to the Create Sketch button). Recall that hovering your mouse pointer over the tool buttons provides a tool tip with the button name and that hovering a second longer allows a dynamic tool tip to appear showing an illustrated example of each. The automated centerline tool is accessed differently.

Centerline

Use Centerline to draw a centerline style line, arc, or circle by specifying points. When arcs are selected as centerline endpoints, a center mark is drawn on the arc along with the centerline.

1. On the Get Started tab, click the Open button.

2. Browse for the file named mi_12a_082.idw located in the Chapter 12 directory of the Mastering Inventor 2010 folder, and click Open.

3. On the Annotate tab, click the Centerline tool.

4. On VIEW 1, click the hole at the 12 o'clock position and then the hole at 2 o'clock. Notice the tool is drawing a straight line at this point.

5. Click the hole at 4 o'clock, and notice the centerline becomes an arc.

6. Continue on around clicking each hole and then close the centerline by clicking 12 o'clock once again; then right-click and choose Create.

7. You should still be in the centerline tool at this point. On VIEW 4, click the center of hole A1, then B1, then B2, and finally A4.

8. Right-click and choose Create; then right-click and choose Done. Your centerline should resemble the one on the left of Figure 12.18.

Figure 12.18. Centerlines

As you can see, the Centerline tool will triangulate the first three points and attempt to establish a centered pattern. In this way, you can use it to draw centerline arcs, circles, and lines. However, if you just need to draw a series of lines, this functionality can get in the way.

To draw just centerlines, click the first two points, then click any blank space on the sheet, then click the next two points and click a blank area again, and so on. The blank clicks are the same as right-clicking and choosing Create. Try this on VIEW 5 to draw centerlines between each of the corner holes.

Watch Your Mouse Clicks During Centerline Creation

The Centerline tool is a bit specific in the order it wants to see mouse clicks. After you have selected the final features on which to place the center mark, right-click and select Create. If you do not select Create and continue to select the next hole, you may end up with undesirable results. Also, do not be confused by the Done option. This exits you from the Centerline tool without creating any of the centerlines that have not yet been created. It takes a little getting used to, but you'll quickly figure it out.

Centerline Bisector

Use Centerline Bisector to create a centerline halfway between two edges or two points. Note that the edges do not have to be parallel or the same length. You can even select two circles, and you will get a centerline halfway between them.

1. Still in mi_12a_082.idw, select the Centerline Bisector tool on the Annotate tab.

2. Zoom in on the center shaft area of view Section A-A.

3. Click the top and bottom lines on the shaft.

4. Notice that the distance between the two lines is bisected with a centerline.

5. Place bisector centerlines in two holes in Section A-A by clicking the opposing lines for each.

6. Right-click, and choose Done.

7. Click the centerline you placed in the center shaft and drag out the left end so that it extends past the shaft. Bisector centerlines are created based on the size of the lines you choose and may need to be adjusted. Your section view should resemble Figure 12.19.

Figure 12.19. Bisecting centerlines

A significant portion of any detailing job is placing and modifying dimensions, so it's important to become familiar with the various dimension tools and formatting options available in Inventor's Drawing Manager. Here is a quick reference of the dimension types available:

Most of these dimensions can be created with just one tool, the General Dimension tool.

General Dimensions

You can find the General Dimension tool by clicking the Dimension button on the Annotate tab. This will be your primary dimensioning tool. It works very much like the Sketch Dimension tool discussed earlier in this book in that this single tool can generate several different types of dimensions depending on the geometry you select.

Once geometry is selected, you can right-click to choose the options that are applicable to placing the type of geometry you've selected. You can also control snap options, arrowhead options, and leader options from the right-click menu specific to each dimension type.

A few more types of dimensions are available in drawings than can be generated in sketches using the General Dimension tool. For instance, once an arc is selected (not a full circle), a radius dimension is created by default, but prior to placement, you can right-click and choose Diameter, Angle, Arc Length, or Chord Length from the Dimension Type flyout, as shown in Figure 12.20.

Figure 12.20. Arc dimension options

Prior to placing a linear dimension between two points or two parallel lines, you can create Linear Diameter or Linear Symmetric dimensions from the dimension's right-click menu, that is, the Dimension Type flyout. These types of dimensions are used commonly with symmetrical parts, especially turned cylindrical parts. Figure 12.21 shows the Linear dimension options available when two points or two parallel lines have been selected.

Figure 12.21. Linear dimension options

Prior to placing diameter dimensions, you can right-click and switch to a radius or change the leader options, as shown in Figure 12.22.

Figure 12.22. Diameter dimension options

You can create and access selection filters by holding your Shift key down and right-clicking. Selection filters specify the elements that can be selected when in drawings. For instance, if you choose the Detail selection filter, only common objects common to detailing tasks are selectable, and items such as view boundaries, view labels, section view lines, and so on, are filtered out and cannot be selected. You can create a custom filter also by Shift+right-clicking and choosing Edit Select Filters.

Baseline Dimensions

Baseline dimensions are a series of linear dimensions that each terminate to a common point (or baseline). The Baseline Dimension and Baseline Dimension Set tools offer a mechanism to quickly add dimensions to a drawing view in an orderly way.

When you execute the Baseline Dimension tool, you're left with a series of conventional linear dimensions. This tool simply automates what you could do on your own with the General Dimension tool. The Baseline Dimension Set tool, however, generates a collected group of linear dimensions that are moved (through dragging and editing) and edited as a single group.

To understand this more fully, open the file named mi_12a_085.idw located in the Chapter 12 directory of the Mastering Inventor 2010 folder, and compare the two dimensioned views. The one on the left was done with the Baseline Dimension tool, and the one on the right was done with the Baseline Dimension Set tool. Use the views on the bottom to create baseline dimensions. Start either tool, click the left vertical part edge (this will be the baseline), and then manually or multiselect additional features (these can be model edges or hole centers). When you've selected all the geometry you want to dimension, right-click and click to place the dimensions (shown in Figure 12.23). After you place the dimensions, you can continue to select points on the view (points on geometry rather than explicit geometry), or you can right-click and select Create.

Figure 12.23. Baseline dimensions

Ordinate dimensions and ordinate dimension sets are created much the same way. Again, a dimension set is managed and formatted as a single, selectable object (with some exceptions), while the Ordinate Dimension tool results in independently controlled dimensions.

Another key difference between ordinate dimensions and an ordinate dimension set is that you can have multiple ordinate sets on a single view with different origin points. Once you specify an origin for ordinate dimensions on a view, all ordinate dimensions placed on that view will reference that origin as well as any hole tables referencing that view. The reverse is true as well: once an origin is specified for a hole table, ordinate dimensions on that view share the origin.

To understand this more fully, open the file named mi_12a_099.idw located in the Chapter 12 directory of the Mastering Inventor 2010 folder, and compare the two dimensioned views. The one on the left was done with the Ordinate Dimension tool, and the one on the right was done with the Ordinate Dimension Set tool. Use the views on the bottom to create ordinate dimensions and ordinate dimensions sets.

Dimensions in Isometric Views

Although you may have been taught at some point that dimensions should never be placed on isometric views because traditional detailing techniques do not allow an accurate dimension to be pulled from an isometric, Inventor can overcome this by pulling the intelligence from the physical model. When you use the General Dimension tool to add dimensions to an isometric view, the resulting dimensions are fundamentally different from those you place in orthographic views.

This is immediately noticeable when you see how the resulting dimensions are drawn on the sheet: all of the dimension geometry (text, arrowheads, extension lines, and dimension lines) are drawn in 3D space and not in sheet space (like orthographic views). Dimensions generated on isometric views are called true (meaning they reflect the true model space dimensional value). Dimensions added to orthographic views are known as projected because the dimension value represents the calculated distance or angle between endpoints or geometry projected onto the sheet.

When placing an isometric dimension, Inventor tries to determine an appropriate annotation plane based on your geometry selection. In many cases, particularly with linear dimensions, multiple inferred annotation planes are available. Prior to placing the dimension, you can toggle through these inferred annotation planes by clicking the spacebar.

If none of the inferred work planes meets your needs, you can project the dimension either onto the sheet plane or onto a model work plane. For instance, oftentimes you will find that hole notes and leader dimensions such as radii and diameters look better placed on the sheet plane rather than in the isometric plane; therefore, you can right-click and choose Use Sheet Plane when placing them.

The change in dimension behavior (true vs. projected) happens automatically depending on the view orientation. Any projected isometric or base isometric view results in True dimensions. As a rule, newly added dimensions to a view are treated as true if none of the model's origin planes is parallel to the sheet (with the exception of auxiliary views).

You can override this rule on a view-by-view basis by right-clicking a view and changing the dimension type (True or Projected).

Isometric dimensions are functionally identical to orthographic dimensions; however, they cannot be "moved." That is, they cannot be detached and reattached to different geometry, and they can't be moved using the dimension Move option on the dimension's right-click menu. All formatting options and behavior are otherwise identical.

Although placing isometric dimensions may seem unconventional, you can, in fact, oftentimes eliminate the number of views required to concisely communicate the design by placing dimensions on an isometric view. Try adding dimensions to the isometric view in mi_12a_105.idw, as shown in Figure 12.24.

Figure 12.24. Isometric view dimensions

Hole and Thread Notes

A hole note differentiates itself from a traditional diameter dimension by calling out feature information beyond just the hole diameter.

The Hole/Thread Note command (in the View Annotation panel) generates a leadered note that displays all pertinent hole feature information derived from the hole edge that is selected.

For example, a hole note pointing to a simple blind hole might appear as 10 × 20. A hole note pointing to a through partial-tapped hole might appear as 10-32 UNF-2B × 20.00. Inventor provides you with the ability to tailor the exact contents of the hole note through your dimension style.

Use the Hole/Thread Note tool to add a single note for the mounting hole and tapped hole in the faceplate front view. You can configure hole notes to display whatever string of description text you prefer as well as set the various hole parameter values' Precision and Tolerance settings. These preferences are set and stored in the dimension style.

You can configure more than 50 types of holes in this interface; they generally correspond to the different kinds of holes you can create using the Hole feature tool in part and assembly modeling ("holes" as a result of circular-extruded cuts, voids, or circular sheet-metal cut features are also supported by hole notes).

You can configure hole notes to display the hole quantity as part of the note. You can add a quantity note either directly on an individual note through the Edit Hole Note dialog box (right-click a hole note and choose Edit Hole Note) or at the style level (right-click a hole note and choose Edit Dimension style) so they appear for all holes of the same type. You can use the hole note in mi_12a_107.idw to explore this.

To add a quantity note at the style level, make sure you're editing the dimension style associated with the hole notes on your drawing (the best way to ensure this is to right-click on the hole note and choose Edit Dimension Style). Select Thru – Full Thread in the Note Format drop-down, and then click in the text field so that the cursor is in front of the note text; finally, click the button with the # sign on it. This inserts the <QTYNOTE> variable token in front of the note, as shown in Figure 12.26.

Figure 12.26. Hole note settings in dimension style

You can customize the quantity note by clicking the Edit Quantity Note button on the dimension style's Notes And Leaders tab, as shown at the bottom left of Figure 12.26. By default, the quantity note is set up as a prefix to the full hole note (2 ×). This dialog box also lets you determine how the hole quantity is determined (either the number of holes in a feature or pattern or a complete evaluation of identical holes in a view where all the hole axes are normal to the view).

As soon as you save the changes to your dimension style, you should see the hole note for the tapped holes update to include the quantity of holes (2 ×).

The Notes And Leaders tab on the Dimension style also enables you to preconfigure other kinds of feature notes including chamfer notes (which are actually calculated notes and not feature-dependent), punch notes, and bend notes (both of which are available only for views of sheet-metal parts).

Leadered Symbols

Many of the annotations you can apply to a drawing belong to a common class of annotations we'll refer to as leadered symbols. These are all grouped together in the Drawing Annotation panel: Surface Texture Symbol, Welding Symbol, Feature Control Frame, Feature ID Symbol, Datum ID Symbol, and five different Datum Target tools. Each of these are created the same way, and each is formatted by their own dedicated style.

In the following steps, you will walk through an exercise that involves adding geometric dimensioning and tolerancing symbols to a drawing of a faceplate:

1. On the Get Started tab, click the Open button.

2. Browse for the file named mi_12a_109.idw located in the Chapter 12 directory of the Mastering Inventor 2010 folder, and click Open.

3. On the Annotate tab, use the drop-down on the Symbols panel, and choose the Datum Identifier Symbol button.

4. Click the far-right edge of the part, and drag the leader to the desired length.

5. Click the screen to set the leader, and then right-click and choose Continue.

6. Accept the default A value in the text editor, and hit OK.

7. Click the bottom edge to add a second datum ID (B), but rather than placing a leader, right-click, and choose Continue immediately after clicking the initial part edge point. You can do this with most Inventor leader features.

8. Next, on the Annotate tab, use the drop-down on the Symbols panel, and choose the Feature Control Frame button.

9. Rather than attaching the frame to the part, instead hover your mouse pointer near the bottom middle of the hole note, until you see a green dot indicating the snap point (just below the N in UNF), and then click it.

10. Then right-click and choose Continue to place the frame without a leader.

11. Fill out the appropriate fields for a positional tolerance relative to the A and B datums, as shown in Figure 12.27; then hit OK.

12. To see that the frame is attached, select the hole note, and then drag the leader landing to move the note. Notice how the frame remains constrained to the hole note.

Figure 12.27. Feature control frame attached to hole note

Hole Tables

You can document hole descriptions, quantities, and locations on a view by using a hole table rather than using hole notes. Indeed, you can use the hole table to document not only hole features but sheet-metal punches as well. You can even use a hole table to call out locations of recovered work points in your model. You can use this technique to detail specialized features such as slots and bosses.

Hole tables, like most types of annotation in Inventor, are initially formatted by an associative style—a Hole Table style in this case. The Hole Table style enables you to select which columns you want displayed in your table, format precision and units for the X and Y location columns, change line formatting, filter on different hole types, and configure various grouping mechanisms depending on your needs.

Everything about the hole table is formatted by the Hole Table style except for the description string for the hole. The description string uses the same configuration as your hole notes and receives this particular formatting by the hole tag's dimension style (hole tags are created with the hole table and are formatted by a dimension style).

In the following steps, you'll walk through setting up a Hole Table style and creating a hole table for the faceplate:

1. On the Get Started tab, click the Open button.

2. Browse for the file named mi_12a_111.idw located in the Chapter 12 directory of the Mastering Inventor 2010 folder, and click Open.

3. On the Manage tab, click the Styles Editor button.

4. In the left pane of the Styles Editor, expand the hole table node, and click the style named Hole Table – mm (ANSI). The right pane will update to show the settings for this style, as shown in Figure 12.28.

   

   Figure 12.28. Hole Table Style interface

5. At the top of the right pane, click the New button, and set the name of the new hole table style to HT_02.

6. Click the Column Chooser button, and select the Quantity property on the left of the resulting property list.

7. Click the >> button to add it to the included list of columns on the right.

8. Use the Move Up button to move the Quantity column up in the list as you like; then hit OK.

9. Right-click the XDIM Property in the Default Column Settings frame, and select Format Column.

10. In the Format Column dialog box, change the precision to three places, and change the column heading to X LOCATION. Note that you can format columns in this manner in almost all of Inventor's annotation tables, such as parts lists and so on.

11. Click OK, and repeat for the YDIM column.

12. Click the Save button to save the changes, and exit the Style Editor dialog box with the Done button.

You will now need to place a hole table on the drawing. Three hole table variations are available on the Table panel of the Annotate tab:

Selection

This allows you to select the holes you want to include in the table, and then only those holes are included.

View

This documents all holes in a view, although you can use filters to exclude certain hole types. As holes are added to the part, the hole table updates to include them.

Features

This allows you to select an instance of the types of holes you want to include in the table, and then all holes of that type are included.

To continue this exercise, you'll choose to place a hole table using the View method.

1. On the Annotate tab, select the Hole drop-down on the Table panel, and choose Hole View.

2. Select the view on the sheet.

3. Next you need to place the origin on the view. You can click any edge or vertex of the part, or you can project the edges to find the apparent intersection of the lower-left corner.

4. To place a table using the table style you created, go to the Style drop-down at the top right of the screen, and choose HT_02 from the list.

   Finding a Corner Intersection

   To find an apparent intersection for placement of an origin marker, zoom into the lower-left corner of the part. Then scrub your mouse pointer over the vertical and horizontal edges of the part, and bring your mouse pointer to the apparent intersection; you should see the edge projected down and over and a yellow dot at the intersection. When you do, click it to set the origin at that point. Be sure you run over the edges (lines) and not just the endpoints of the edges.

5. Next, click the screen to set the hole table on the sheet.

For each individual hole in the view, a hole tag is placed next to the hole edge, and a corresponding row is generated in the hole table. Also notice that because each hole is called out individually in this table, each row has a quantity of 1 (shown in Figure 12.29). You can edit the hole table by right-clicking it and choosing Edit Hole table. From there, you can set the table to roll up all A-type holes and all B-type holes from the Options tab by selecting the Rollup radio button.

Figure 12.29. Hole table

You can also edit the Tag, Note, or Description text by right-clicking the text in the table. You can make direct overrides to hole descriptions by double-clicking the description text, and you can override X and Y location precision by right-clicking an individual cell. You can access several other options by right-clicking the text in the table as well, so be certain to explore them all.

Hole Tables Save Time on Large Parts

For large plates with many different holes, hole tables are wonderful. A large plate could take a half hour or more to fully dimension. Furthermore, it's often difficult for a machinist to tell where all five of the same holes are located if they are not all called out individually. The hole table gives the machinist X and Y locations of the holes that they can use to program their CNC milling machine extraordinarily quickly. Don't be surprised if the machinist asks you to dimension all your parts using hole tables.

One of the most significant differences between part and assembly model views are the view options available for assembly views. When an assembly file is referenced in the Base View, representation options become available on the Component tab of the Drawing View dialog box. These controls allow you to specify which assembly view, positional, or LOD representation is displayed in the resulting drawing view.

View representations can optionally be made associative to the view (using the check box at the top of the View Representation control). Specifically, an associative view representation means that as a component's visibility is changed from the assembly, the change is witnessed in the drawing view as well. If the associative option is deselected, you can toggle component visibility from the drawing itself.

Recall the general definitions of each assembly representation type:

In the next several steps, you will edit a view of an assembly to see how to use assembly representations in drawing views:

You'll see that now just the handle, shaft, and ram parts are shown (because the LOD representation), and the positional representation is controlling the positions of these parts.

Assembly components can be designated as Reference. You can apply this attribute as a document setting on the part or assembly file itself or on a per-instance basis when placed in a higher-level assembly.

In addition to being omitted from the assembly mass property calculations, BOM, and subsequent drawing parts lists, reference components are drawn and calculated differently in assembly drawing views.

By default, all reference component edges are mapped to a unique layer with a broken line style (double-dash chain). Hidden line calculation, by default, is run separately for reference components than nonreference components. Finally, reference components do not affect the calculation of the drawing boundary. This means that if you have a reference component well apart from nonreference parts in an assembly, it may not be visible in a drawing view until you increase the reference margin.

To explore these settings, you can open the file named mi_12a_117.idw located in the Chapter 12 directory of the Mastering Inventor 2010 folder and compare the two views. The view on the left shows the reference part at the default settings. The view on the right has been adjusted to show the reference part as a standard part. Right-click the view and choose Edit to adjust all the reference data view behaviors on the Model State tab of the Drawing View dialog box. Figure 12.31 shows the default settings.

Figure 12.31. Reference data settings

As you place and constrain components in an assembly file, it may be necessary to create an interference condition between parts. This is common for press-fit conditions such as pins in undersized holes. This condition is common in Inventor even when you have a threaded fastener being inserted into an equal-diameter threaded hole. These edges are designated as interference edges and can be turned on or off as needed.

Although not specific to assemblies, you can also control the display of tangent edges for cylindrical faces, filleted edges, and so on, in your drawing views. Both tangent and interference edges can be enabled by editing the view and selecting the Interference Edge check box on the Display Options tab.

Figure 12.32 shows the difference between two views with these edges turned off and turned on. The interference edge in this case is the small set screw in the middle of the plate. All other differences are tangent edges.

Figure 12.32. Tangent and Interference edges

Parts lists are a formatted report of the assembly bill of materials placed on the drawing in a table. Most of the data you see in a parts list comes ultimately from the assembly BOM, but the BOM and the parts list are managed separately inside Inventor, providing control and flexibility for managing both.

Parts lists have a dedicated formatting style that provides dozens of formatting variations. We'll walk through a typical parts list editing and creation workflow to demonstrate what kind of capabilities can be levered in the parts lists.

The new item numbers appear blue and bold in the Parts List dialog box to indicate that they do not match the BOM. Any change you make to any of the cells in the Parts List dialog box (except for custom rows or custom columns) are treated as overrides to the BOM data. However, only Item number overrides can be written back to the BOM. All other overrides are preserved at the parts list level, allowing for greater flexibility of parts list edits at the drawing level without worries that they will be discarded if updated in the BOM. Item number changes can be saved to the assembly BOM cell by cell from the right-click menu or for the entire parts list in one of three ways:

If you intend for the overrides of prosperities other than the item numbers to match in both the BOM and parts list, you should make those edits in the BOM, where they will push through to the parts list. You can access the BOM quickly by right-clicking the parts list and choosing Bill Of Materials. Edits made in the BOM editor are written back to component iProperties and therefore push through to the parts list, provided no parts list overrides have already been made.

The parts list is not directly associated with any drawing view (if you choose a view when you create the parts list, it acts only as a pointer to the assembly file itself). Assembly drawing views are related to parts lists by ballooning the components in the assembly drawing view.

Balloons are perhaps the only type of annotation that are relevant for assembly views only. By default, balloons are set to display just a component's assigned item number, but through changes to the balloon style, a balloon can be configured to display any component iProperty or BOM property. Review the creation and editing of balloon styles in "Editing Styles and Standards" section earlier in this chapter.

You should know that only items visible in a view can be ballooned; however, you can string multiple balloons together on a single leader, including parts that are not visible, virtual parts, and even line items added to the parts list that do not exist in the BOM. This is also a common technique when ballooning a collection of hardware such as a screw, lock washer, and split washer.

Follow these steps to explore methods and options for balloon placement:

Here are some tips for working with balloons:

If you've defined multiple positional representations in your assembly, you can use these different positional representations to create overlay views showing the mechanism in different positional states. To create an overlay view, follow these steps:

The result is a view of the alternative position shown in a phantom line—type overlaid on the original. You can dimension to the overlay lines as you would any others, in order to capture a mechanism's extension length, rotation angle, and so on. The key to overlay views is really in setting up the positional representations in the assembly beforehand.

When you create the overlay, you are given the opportunity to specify a view representation for the overlay view. It's recommended that before you create an overlay view, you create a view representation that visibly isolates only the components that move as a result of the positional representation. Otherwise (as is the case in this example), all the nonmoving components are redrawn over the same components in the base view.

You can display the center of gravity (COG) of a part or assembly in a drawing view as a center mark. Only one COG can be shown per view with the exception of overlay views. Continuing from the last step in the previous exercise on overlay views, you will now take a look at displaying the COG marker in a drawing. If you did not complete the previous section, just open the file named mi_12a_123.idw located in the Chapter 12 directory of the Mastering Inventor 2010 folder, and activate Sheet 2 to follow these steps:

Figure 12.34. Overlay view with recovered COG

When a sheet-metal part file has a flat pattern definition, you can create a drawing view of the folded model or the flat pattern. You can include both as well but need to separate base views to do so. To take a look at these options, follow these steps to create a flat pattern drawing view to start off:

Bend centerlines are drawn on sheet-metal flat pattern views where the center of the bend is located on the material face. Inventor tracks negative and positive bend centerlines independently of one another to enable users to apply different line formatting for these two conditions. This has already been done in file mi_12a_130.idw, but it should be noted that the default behavior is to have both positive and negative bend lines placed on the same layer. If you want to separate them, simply create a new layer called Bend Centerline (negative), and then go to the Object Defaults in the Styles And Standards Editor and assign the Sheet Metal Bend Centerline (+) and (-) to the appropriate layers.

Lines representing bend extents can be enabled by right-clicking the flat pattern view, choosing Edit View, going to the Display Options tab, and selecting the Bend Extents option.

You'll find two sheet-metal-specific annotation tools on the Annotate tab: Bend Notes and Punch Notes.

Bend notes are placed on bend centerlines in sheet-metal flat pattern views and can convey information about the bending operation including the bend radius, direction, angle, and K-factor. To place bend and punch notes, continue working with file mi_12a_130.idw, or open this file and activate Sheet2 to pick up from this point.

By default, the bend notes are drawn adjacent to the bend centerlines, but where the note may be obscured in the view, you can drag individual bend notes to flip them to the opposite side of the bend centerline, or you can drag away from the bend centerline, and a leader is generated back to the bend centerline. Try this with the two outermost bend notes on the electrical box flat pattern view (shown in Figure 12.35).

The style formatting and direct editing of bend notes is identical to hole notes. You can preconfigure the contents of the note with the note's dimension style by adding one or more variable tokens for the bend note attributes. Punch notes are used to convey information about sheet-metal punch features (a special kind of iFeature). Punch notes can be applied only to flat pattern views of sheet-metal parts. They can be attached to recovered punch centers (shown as center marks in the flat pattern drawing) or on any model edge generated by the punch.

Figure 12.35. Bend notes in flat pattern view

Punch notes can be configured to display the punch identifier (defined as part of the iFeature definition), the punch angle, the depth, and the direction. Punch notes are likewise formatted through dimension styles and have a similar editing interface to hole notes.

Bend information can alternatively be displayed in a table rather than a note. A bend table is generated using the General button on the Table panel on the Annotate tab. The Table tool basically morphs into several different kinds of tables depending on what you specify as a data source. If a flat pattern view is selected, then a bend table will be generated.

To create a bend table for file mi_12a_130.idw, activate Sheet3, and then follow these steps:

A bend table is edited and maintained like a parts list. The Table dialog box is essentially identical, and any changes to the cell data are treated as overrides to the data source (in this case, the bend data stored in the sheet-metal file). Figure 12.36 shows a simple bend table and bend ID tags.

Figure 12.36. Bend table

Punch information can likewise be displayed in a table, but because punches closely resemble holes with respect to the kind of information required to be displayed, a hole table is used to generate tabulated punch data. The only difference in creating a hole table and creating a punch table is that you use a predefined hole table style that is set to pick up only sheet-metal punch features.

Figure 12.37 shows a simple Punch table.

Figure 12.37. Punch table