The left side of the Insert dialog box, shown in Figure 15.4, has a series of drop-down fields for specifying the structural shape.

Figure 15.4. Frame Member Selection group

You use the Standard, Family, and Size fields to select the member from the Content Center. These fields are progressive, and the update behavior varies. If you select a new standard, the first family is automatically selected. If you select a new family, the size is not automatically selected.

After you have selected the placement geometry, you can change the position and orientation of the member. A thumbnail of the profile is displayed in a grid of radio buttons that control the position of the member, as shown in Figure 15.5. These positions are based on the rectangular bounds of the profile. As a result, the corner positions of a 1″ by 1″ square tube are the same as a 1″ diameter pipe.

Figure 15.5. Orientation group

If a custom profile has been authored with an alternate base point, the Custom Point control is enabled. This adds another insertion point to the nine standard ones. The custom point is not displayed in the thumbnail image, so you should confirm the preview is in the expected position relative to the selected edge.

You can fine-tune the position by entering values in the horizontal and vertical fields. You can also rotate the member. For example, food processing equipment frequently has horizontal members rotated 45 degrees so spilled food doesn't build up on top of square tubing.

The Mirror Frame Member button is used for profiles that don't have rotational symmetry, such as C-channel and angle iron.

The orientation changes affect all the members of a select set. Depending on the geometry, it might be more efficient to use a batch select tool and change the orientation of a few members afterward, or you might want to select only those members that have a similar orientation.

Since structural shapes are extruded, Frame Generator needs a method for determining the extrude direction. When an edge is selected, Frame Generator uses the closest endpoint as the start of the extrusion. Depending on where you select an edge, the same radio button can cause the member to be in a different position. The thumbnail is the view of the profile looking at the XY plane. It takes some practice to get a good feel for the relationship between how an edge is selected and the behavior of the radio buttons. Once you understand this relationship, you will be able to predict the behavior and use it to increase your productivity.

To see how this is accomplished, open the file named mi_15a_001.iam from the Chapter 15 directory of the Mastering Inventor 2010 folder. You can use this file to explore the options in the coming pages. When placing frame members, you first specify the Standard, Family, Size, and Material Style settings, as shown in the dialog box in Figure 15.6. Click the first edge near the bottom and select the corner radio button to place the member inside the surface, as in this figure.

Click the next edge near the bottom, as shown in Figure 15.7, and its relative position is the same as the first member. This places the member outside the surface.

The second member needs to be inside the surface, so deselect it by holding the Ctrl key and clicking it. Then reselect the edge near the top, as shown in Figure 15.8. This time, since the extrusion direction was reversed, the member is inside the surface.

Figure 15.6. Preview of the first member when selected near the bottom

Figure 15.7. Preview of the second member when selected near the bottom

Figure 15.8. Preview of the second member when selected near the top

When using a custom profile with an alternate insertion point defined, the Custom Point control is enabled. This point is in addition to the standard insertion points around the profile. Figure 15.9 shows a profile with an alternate insertion point.

Figure 15.9. Profile with an alternate insertion point

When you select placement geometry, you can select edges and lines, or you can select two endpoints. When you select edges and lines, you can insert multiple members. When you select two endpoints, you can place only one member at a time. The most common placement method is by selecting lines and edges. This allows the most flexibility in geometry selection and the use of batch select tools.

There are two philosophies for placing frame members. Some people like to place frame members individually, making sure each one is in the correct position and orientation. Other people like to place as many members as possible and then edit them as necessary. The method you choose will depend on the type of models you work with, how much effort you put into setting up the skeleton models, and, most important, the way you like to work.

Batch Selection Tools

Frame Generator has several tools for selecting geometry. Multi Select is the default selection mode. These are the standard tools for building a selection set: picking, using selection windows, and using the Shift and Ctrl keys to add and subtract. Two additional select modes are available in the context menu shown in Figure 15.10: Chain Select and Sketch Select.

Figure 15.10. Select mode context menu

Chain Select automatically selects all lines and edges that are tangentially connected to the selection. Chain Select will not follow past a point that has multiple lines or edges, even if one of them is tangential.

Sketch Select selects all the lines in a sketch. You can select the sketch in the browser or click a line in the graphics window.

Placement by Selecting Lines and Edges

The default selection mode is Insert Members On Edges. You can select any combination of sketch lines and model edges and surface edges. Figure 15.11 shows conveyor model mi_15a_001.iam. The frame skeleton is constructed of surfaces and sketch lines. The power roller is in the correct position, but it needs support members.

Figure 15.11. Belt conveyor skeleton model

Figure 15.12 shows the conveyor frame populated with ANSI AISC HSS (square) tubing. The legs are 3 × 3 × ¼ square tubing positioned inside the surface. On one side, the legs have a removable section for installing the belt. The legs can be inserted in pairs by using the edge selection technique demonstrated in the "Changing the Orientation" section earlier in this chapter.

Use Chain Select

Use Chain Select to select the four vertical legs as single lines and to place frame members by edge.

The horizontal members are 2 × 2 × ¼ square tubing inserted at 45 degrees. Switch to Sketch Select to select all of the geometry in a sketch at once (see Figure 15.13). After these tubes are inserted, you can turn off the visibility of the conveyor frame skeleton part to reduce clutter by right-clicking it in the browser.

Rename Your Files When Prompted

Frame Generator uses an algorithm to create filenames, and it is unlikely they will match your corporate standards. It is tempting to dismiss this dialog box when you are creating a frame, but it is better practice renaming the files now rather than go back and rename them later.

Figure 15.12. Conveyor frame with all frame members inserted

Figure 15.13. Inserting the horizontal members

The power roller supports are 1½ × 1½ × 3⅙ square tube. The lower support is flush with the flat, and there is a small gap between the upper support and flat. Select the edge of the lower flat, and offset the tube horizontally to align it with the leg. Select the edge of the upper flat and offset it horizontally to align with the lower support and 0.125″ vertically, as shown in Figure 15.14.

Figure 15.14. Inserting the upper power roller support

Where Are the Other Common Sizes?

You might note that there are several common sizes you might use daily that are not listed in the size drop-down. The sizes included are only the sizes listed in that particular standard. Of course, most mills produce other sizes commonly used in general design. You can add these sizes using the Structural Shape authoring tools.

Placement by Two Points

In some cases, it can be more productive to select the endpoints rather than create the geometry. The select set is limited to two points, but you can speed up the insertion process by selecting Apply from the context menu and then picking the next pair of points.

In this example, the conveyor frame needs horizontal members in the center. The conveyor frame skeleton is turned back on. Change the placement method to Insert Members Between Points in the Insert dialog box. Pick the endpoints of the side lines in each sketch, as shown in Figure 15.15, to place the 2 × 2 × ¼ square tube.

Figure 15.15. Inserting the cross members

Real World Scenario: Plan Ahead

Frame Generator is flexible when it comes to creating a frame. You can select different types of geometry, and there are different selection modes. Although this makes it easy to dynamically create frames, you will be more productive and have a more stable model if you plan ahead.

When I create a frame, I initially look at the key parts of the frame—the overall size, mounting points from components, leg location, and so forth. I place key components in the assembly ahead of time, whether or not I am going to reference component edges during frame creation. Some people like to sketch the full model before adding frame members while others prefer to only sketch the main members and use point-to-point to insert cross braces. The second method is usually faster, but you are less likely to miss a member using the first method.

As with most tools in Inventor, there are many right and wrong ways to accomplish the task. The correct method for you is the one that allows you to reliably get your work done on time.

Frame Generator follows two rules to give a frame member its initial orientation. If it is the first member in a select set, the member is aligned to adjacent geometry or the coordinate system. For the rest of the select set, Frame Generator tries to align the members to the first selection. These rules work well for most rectangular machine frames. If part of the frame is at an angle and there isn't a good reference, Frame Generator can select an orientation that doesn't match the design intent.

The frame in Figure 15.16 is the roof for a sunroom. The members for the base and back have already been inserted, and the two angled rafters need to be inserted. When you insert a member on the left line, the orientation is skewed, as shown in Figure 15.17.

Figure 15.16. The sunroom roof has angled rafters.

Figure 15.17. The left rafter is skewed.

On the right side, a reference line was added to the base. If that line is selected before the left line, as shown in Figure 15.18, Frame Generator can align the angled member. Since a frame member isn't needed on the bottom line, it can be deselected, and the angled member is inserted correctly, as shown in Figure 15.19.

Figure 15.18. Selecting a reference line to align the rafter

Figure 15.19. The right rafter is aligned correctly.

Using reference geometry for angled frame members is an art. If you regularly create these types of frames, you will develop a feeling for the ways that Frame Generator aligns members, and you will learn when and how you need to add references.

The Miter end treatment makes angle cuts on two members. Figure 15.20 shows the Miter dialog box. You can miter multiple members by applying the end treatment to each pair of members.

Figure 15.20. Miter dialog box

The default selections cut along an angle resulting in full-face contact between the members as shown in Figure 15.21. Bi-sect Miter splits the angle between the members. Figure 15.22 shows the cut is located where the centers of the two members intersect.

Figure 15.21. The standard miter joint has full-face contact.

Figure 15.22. The optional bi-sect miter cuts both members at the same angle.

You can add a gap between the members. The default gap is split between the two members. If you want to have the end gap on one member, as shown in Figure 15.23, it will be removed from the first selection.

Figure 15.23. Miter gap on one member

The sunroom frame, named mi_15a_007.iam, has a miter end treatment between the two angled members on the back, and the vertical member needs to be mitered to fit, with a small gap to allow for manufacturing tolerances.

Figure 15.24 shows the first step to create the miter. The gap should be cut only on the vertical member, so it needs to be the first selection.

The vertical member still needs a miter to trim the other side, so the miter is repeated with the same settings, as shown in Figure 15.25.

The resulting miter shown in Figure 15.26 requires two cuts on each member. An alternate method that produces a more cost-effective joint will be shown in a later section.

This end treatment trims or extends both members so they are flush. The first selection is made flush to the second selection, and the second selection butts up to the first. Figure 15.27 shows the selections, and Figure 15.28 shows the results.

Figure 15.24. First miter cut

Figure 15.25. Second miter cut

Figure 15.26. Resulting miter joint between the three members

This end treatment is the only one that can trim multiple members at once. You select the members you want to trim, and then you select the cutting face. A separate end treatment feature is created for each frame member. If you edit or delete the end treatment for a particular member, it does not affect the other members.

Returning to the conveyor example, the conveyor frame is a typical machine frame. All of the members are perpendicular with simple butt joints. Since you can select multiple members, as shown in Figure 15.29, using Trim and Extend is an efficient way to add details. Since the frame is symmetrical, you can trim the members on both sides at once. If a design change requires an offset leg, it is pretty straightforward to edit the end treatments on the members and change the face selection.

Figure 15.27. Trim To Frame selections

Figure 15.28. Trim To Frame results

Figure 15.29. Trim the horizontal members to a leg.

This end treatment can also be used to create miters. Applying miter end treatments to the sunroom frame resulted in a complex joint. Trimming the vertical member to fit the angled members results in the less expensive detail shown in Figure 15.30.

Figure 15.30. Creating a miter using Trim

Notch cuts one frame member to match the other. It uses the profile to create a cutting surface. You can't create an offset, so the cut is an exact match. This is simply a cut operation, so the frame member is not shortened or extended before the cut. If you notch the short I-beam shown in Figure 15.31, which extends past the tall I-beam, the extra lump will be left as shown in Figure 15.32. If the members don't intersect, the notch will have little or no effect.

Figure 15.31. Frame members before notch

Figure 15.32. The result of removing the intersecting material

A notch is frequently a secondary end treatment. For example, if you add a Trim/Extend To Face end treatment first, the notch will remove any intersecting material.

Sometimes, there isn't another frame member you can use as a reference for an end treatment. For example, the power roller supports on the conveyor are stubs that were placed by selecting the part edges. The power roller is moved to adjust the belt tension, so the tubes need to be extended away from the frame.

The tubes were already extended to the frame. Since the total length of the tube should be a nominal value, measure the length of the tube before starting the command. In this case, the tube is 9.088″ long. The tube needs to be about 3″ longer, so the overall length should be 12″. Copy the length from the Measure Distance dialog box, and paste it into the Lengthen–Shorten dialog box to build an expression.

Frame Generator modifies the end closest to the pick point, as shown in Figure 15.33. If the pick is closer to the frame, an error will display because there is already an end treatment at that end. Although it isn't obvious at first, this is an intuitive way to select the member, since you are likely to pick the member close to the end you will modify.

Figure 15.33. Lengthening the power roller supports

The Remove End Treatments tool removes all end treatments from a frame member. You can also select multiple members for the batch removal of end treatments. This is handy if you need to change the end treatments on a few members or if you have to rebuild a frame.

The Frame Member Information tool is used to query frame members. It displays the family and size information, mass properties, and material. This is a useful tool because it quickly gives you information about a member. For example, it can tell you the wall thickness of a tube. Since the tool filters for frame members, you can use it at any level of the assembly.

The Refresh tool is a Content Center tool. It checks the Content Center for the latest revision of the members in the frame. If a newer version is available, it will prompt you to replace it. End treatments are retained during refresh, but other features, such as holes, are not carried over to the new member.

Referring to the conveyor assembly again, the Beam And Column Calculator might be used to calculate the loading on the power roller supports. When the tube is selected the calculator automatically loads the section properties from the Content Center, as shown in Figure 15.34. Although the Content Center has most of the section properties, be aware that some data is missing. You can use several methods for determining the properties.

Figure 15.34. The section properties for the power roller support are loaded from the Content Center.

Inventor has a tool to calculate the properties of a closed sketch profile. If you want to use this tool for the section properties of a frame member, you can open the frame member, place a sketch on one end, and project the face. Once you have the profile, select Tools

The regional properties are calculated with respect to the sketch origin. Depending on the profile, you may have to edit the sketch coordinate system to locate the sketch origin at the center of the profile.

Another option for calculating section properties is to use the Section button in the Beam And Column Calculator. When you click the button, a list of geometric shapes displays. When you select a shape, a dialog box like Figure 15.35 displays for entering dimensions. The calculated properties assume sharp corners and constant thickness, so the results won't be accurate for profiles with tapered flanges.

Figure 15.35. Rectangle section properties calculation dialog box

Flip Section is used to change the orientation of the x- and y-axes. The z-axis is always in the direction of the extrusion. Gravity is always in the negative y-axis direction, so it is important to make sure the calculation coordinates match the assembly coordinates. If the beam is at an angle, you have a couple of options for handling gravity. You can place a copy of the beam horizontally in the assembly. If you want to ignore the effect of gravity, there is an option on the Beam Calculation tab to turn the gravity load off.

Both beam and column calculations are available. The beam calculations focus on deflection based on loads and supports. The Column calculation checks for buckling. You can select Beam, Column, or both calculation types. The Calculation tabs are turned on and off based on the selections.

The default material properties do not correspond to an actual material. They give you an example of the required properties. You can enter properties for a particular material, or you can select a generic material. When you check the box, a dialog box displays with materials such as gray cast iron, steel, and aluminum. These properties can be used for initial calculations, but for more accurate results, you should enter the properties for the particular alloy you are using.

The following steps use the power roller supports found in the file named mi_15a_014.iam. Follow these steps to enter the member data into the dialog box:

The coordinate system alignment is correct for this example. In this case, gravity could be ignored, but having the correct orientation simplifies adding the loads and interpreting the results.

The dialog box should look like Figure 15.36. Note that all the section properties except Shear Displacement Ratio are calculated. This property is optional for the calculations. Comparing the calculated values with the original ones, Section Area and Moments Of Inertia are close but higher.

Figure 15.36. Model data entered into the Beam And Column Calculator

The Beam Calculation tab, shown in Figure 15.37, has the controls for defining the loads and supports for beams and columns, as well as calculation options. The Engineer's Handbook (available from the Design Accelerator panel bar or the Help system) contains the equations used in the calculations. You should review those equations before you use this calculator.

The Calculation Properties Group

The Calculation Properties group, as shown in Figure 15.39, has four controls. The controls adjust how the calculations are made.

The Use Density check box adds gravity as a load. This is selected by default.

Figure 15.37. The Beam Calculation tab

Table 15.2. Loads Buttons

Button	Description
	Adds a force.
	Adds an axial force.
	Adds a distributed force.
	Adds a bending moment—a single twisting force perpendicular to the z-axis.
	Adds a torque load—a twisting force around the z-axis. Two equal and opposite torque loads are required.
	Adds a combined load—any of the forces added at the same point on the beam.

Table 15.3. Supports Buttons

Button	Description
	Displays the Options dialog box.
	Adds a fixed support.
	Adds a free support.
	Fixes one end of the beam.

Figure 15.38. Loads & Supports Options dialog box

Figure 15.39. The Calculation Properties group

The Shear Displacement Ratio check box is used when calculating the twist angle caused by torsional loads. The value is determined by the profile shape. It is also called the form factor of shear. Textbooks contain formulas for calculating this number. This check box is selected by default.

The default setting for Number Of Beam Divisions is 1000. Increasing the number of divisions can result in improved accuracy for longer beams. You should experiment with different values to see whether the number of divisions causes a significant change in the results.

Mode Of Reduced Stress has two options for modeling the stress distribution. The Huber-Mises-Hencky (HMH) method is based on the maximum-energy-distortion criterion, and the Tresca-Guest method is based on the maximum-shearing-stress criterion. The HMH method is the default selection.

Results

The result pane on the right side updates when you click the Calculate button. Warnings will display in the lower plane if the calculation indicates that stresses are too high.

For the conveyor example, the support is welded to the frame at one end and unsupported at the other. The power roller weighs 150 pounds, and the torque is 40 pound-feet. The torque causes the power roller to twist between the supports. The edge of the flat is 1.5″ from the center of the power roller. This means the reaction force at that point is 320 pounds. Both the weight and the reaction force are split between the two sides.

1. For the power roller weight, add a 75-pound radial force at 10″ (the maximum distance for the power roller).

2. For the torque reaction, add a 160-pound radial force at 11.12″.

3. Switch to the Supports browser.

4. Delete the Free support.

5. Click the drop-down arrow for the Fixed support, and select Restraint.

6. Leave Use Density checked.

7. Deselect Use Shear Displacement Ratio since you don't have a value for that property.

8. Click Calculate; the reduced stress is 4126 psi, which is 9.4 percent of the 44000psi yield stress.

The dialog box should look like Figure 15.40. Note that the forces are displayed in the graphics window. If you hover over a force, a tool tip displays the information. You can drag the force to a different position, or you can double-click the force to display the properties dialog box.

Figure 15.40. Loads & Supports data entered into the calculator

The Graph Selection pane allows you to select the results you want to display. The selected graph displays in the bottom of the Graph group. At the top of the Graph group is a schematic of the beam, supports, and loads. You can drag the supports and loads to different positions. If you double-click a support or load, the properties dialog box displays so you can directly edit the data. The Calculate button is not available on the Beam Graphs tab, so you have to switch back to the Beam Calculation tab to update the results.

The Beam Graphs tab is primarily intended for reviewing results. Twenty-two graphs are available on the tab. This example is a pretty simple analysis. You should experiment with other loads (torques and bending moments) and support types and then view the results on the graphs.

The Column Calculator tab checks for column buckling. In the Loads group, you enter the axial load and the factor of safety, and you select a coefficient for the end loading conditions. When you click the ... button, a dialog box displays with four end conditions. If you have different end conditions, you should enter the proper coefficient from a reference book.

You shouldn't have to enter any data in the Column group. The length, section area, and least moment of inertia are carried over from the Model tab. The reduced length value is calculated by multiplying the length by the end coefficient.

For example, let's say that during transport, the frame shifts and the power roller supports slam into the trailer wall. The power roller was removed during shipping, so the supports take all the force from the impact, estimated at 4,000 pounds evenly distributed across the four supports. Set the axial load to 1,000-pound force, and click Calculate to determine whether the supports will buckle. Figure 15.41 shows the results.

Figure 15.41. Column calculator results

When you click the Results button in the upper-right corner of the dialog box, an HTML page displays with all the data, calculation results, and graphs.

The authoring process for a frame member is similar to component authoring. The Structural Shape Authoring tool, located on the part-modeling panel bar, is used to prepare the part for publishing. The tool identifies the geometry used for placement, sets the parameters, and modifies the part so Frame Generator can use it.

Creating a Rubber Bumper

This example uses the file named mi_15a_020.ipt found in the Chapter 15 folder on the book's accompanying DVD. This iPart is a rubber bumper that is attached to frames. There are parameters to control the dimensions, but the engineering properties (moments of inertia and so on) were never calculated. Since this isn't a load-bearing part, these properties aren't required.

Once the part is open, you can access the Structural Shape Authoring tool by clicking the drop-down on the Manage tab's Author panel. When the authoring tool starts, everything is blank. Once a category is selected, the dialog box will update with the appropriate controls. Since this is an unusual part, select the Other category, as shown in Figure 15.42. Frame Generator looks in the Structural Shapes category only, so you have to select one of the standard categories or create a new one in the Content Center editor. You can't add a category through the authoring tool, so you have to add the category to the Content Center before authoring. See Chapter 7 for more information on Content Center.

Figure 15.42. Selecting the category

Since there is only one extrusion in the part, the base feature is automatically selected. The default base point is indicated at the center of the profile. For this part, the inside corner of the flanges is the natural insertion point. Click Select Geometry, and select that point in the model, as shown in Figure 15.43.

Figure 15.43. Selecting the default base point

The Parameter Mapping tab has one required field: Base Length. This is the parameter for the extrusion distance. Since this is an iPart, when you click in the field, the iPart properties are listed as shown in Figure 15.44. If this were a regular part, the Part Template Parameters dialog box would display a browser tree, as shown in Figure 15.45. The rest of the parameters are optional. They are mechanical properties of the profile necessary for calculating loads with the Beam And Column Calculator.

Figure 15.44. Specifying the length parameter for an iPart

When the geometry and Base Length parameter are mapped, the Publish Now and OK buttons are enabled. Clicking either button will update the part and close the dialog box. Publish Now will also launch the Content Center publishing wizard. When the part is updated, a dialog box displays with information about the changes. A log file, as shown in Figure 15.46, is created in the project directory that lists the changes to the part.

If you inspect the part after authoring, you will see that the browser and parameters have been updated. The details of the model and parameters are discussed in the section "Exploring the Anatomy of a Frame Member," earlier in this chapter.

Figure 15.45. Specifying parameters for a regular part

Figure 15.46. Log file for an authored part

Test Before You Publish

Before you publish the member for use by all your team members, be sure to test it in every conceivable situation. Even a seemingly well-constructed frame member can cause issues after applying end treatments.

The publishing process uses the Publish Guide wizard. Since the part was authored, most of the publishing information has already been added to the file. If you aren't familiar with publishing to the Content Center, you should spend some time learning how to work with libraries before you publish a part.

These publishing steps are important for Frame Generator: