Shaft Component Generator

Use the Shaft Component Generator to design the shape of a shaft, add and calculate loads and supports, and other calculation parameters. Perform a strength check and generate the shaft into the Autodesk Inventor. The shaft is assembled from single sections (cylinder, cone and polygon) including features (chamfers, fillets, neck-downs, and so on).

Use the Shaft Component Generator to:

For certain features, Shaft Generator uses data from Content Center.

Note: You must be connected to Content Center server and Content Center must be configured on your computers to insert components using Shaft Generator.

Select the following features from Content Center:

When designing shafts, use 3D grips in the graphics window to modify section dimensions to speed up your design.

 

Edge Features

dacc_shaft_edge.png

Features which can be placed only on the shaft edge, for example: chamfers, fillets, lock nuts, threads. You can place only one feature on the shaft edge.

 

Middle Features

dacc_shaft_middle.png

Features which can be placed on the shaft section, for example: keyways, retaining rings, notches, and so on. You can place an unlimited number of these features on a shaft section.

Position markers

dacc_shaft_hotspots.png

Defining points on a section to which the loads and supports are positioned. Use Alt + drag to move a force or support and assign it to another position marker.

 

Graphical Previews

dacc_shaft_preview.png

When designing shaft using Shaft Generator, the 3D graphical preview (with all sections, features, and 3D Grips) is available in the Autodesk Inventor window and 2D preview is available in the Design tab. 2D preview is optional.

When you switch to the Calculation tab, the graphical previews in the Autodesk Inventor window and in the Calculation tab changes to preview of loads and supports.

Tip: See the Engineer's Handbook for used calculation formulas for designing shafts.

 

Procedures:

Design shafts

Design a shaft

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design tab:
    • In the Placement box area, specify the shaft placement within the assembly, if needed.

      Note: Placement is not required to design shaft using Shaft Generator.

    • In the Sections box area, use the pull-down list to design a shape of the shaft. Depending on your selection, the commands within the toolbar display.
      • Select Sections to insert shaft features and sections.
      • Select Bore on the right/Bore on the left to design a hollow shaft shape.
    • Select commands from the menu (Insert Cone, Insert Cylinder, Insert Polygon) to insert shaft sections. Selected section displays in the tree control. Based on the section type (cone, cylinder, and so on) and based on the section position (first, in the middle, and so on) the list of available features is available for each section. You can insert unlimited number of sections.
    • Select the shaft feature or section and click icon_custom_prop.gif to edit the dimensions.
    • Select the shaft feature or section and click icon_delete.gif to delete the feature or section.
    • (Optional) Click icon_dacc_shaft_toolbar_14.png Options from the toolbar (which is always available) to set options for 3D graphical preview and 2D preview.
    • (Optional) Click icon_more_options.gif More in the right lower corner of the Design tab to add a designed shaft to the Templates Library.
  3. Click OK to insert a shaft to the Autodesk Inventor assembly.

Note: You can switch to the Calculation tab to set the shaft material and add loads and supports.

Click icon_toolbtn_createreport.gif Results to display the HTML report.

Design a hollow shaft shape

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design tab:
    • In the Placement box area, specify the shaft placement within the assembly.

      Note: Placement is not required to design shaft using Shaft Generator.

    • Select Sections from the pull-down list in the Sections box area, and insert shaft sections.
    • Select Bore on the right/Bore on the left from the pull-down list in the Sections box area. Insert Cylindrical Bore and Insert Conical Bore options display on the toolbar. Click to insert a hollow shaft of an appropriate shape.
    • Select the bore in the tree control and click icon_custom_prop.gif to edit the dimensions.
    • Select the bore in the tree control and click icon_delete.gif to delete the bore.
    • (Optional) Click icon_dacc_shaft_toolbar_14.png Options from the toolbar (which is always available) to set options for 3D graphical preview and 2D preview.
    • (Optional) Click icon_more_options.gif More in the right lower corner of the Design tab to add a designed shaft to the Templates Library.
  3. Click OK to insert a shaft to the Autodesk Inventor assembly.

Split selected shaft cylinder

When designing shaft with cylinder you can split the selected cylinder into two parts. The length of the cylinder remains the same.

In the graphics window or the 2D Preview area of the Design tab, select the cylinder and click icon_static_dacc_shaft_toolbar_05.png Split Selected Section in the toolbar.

Specify supports

Drag supports along the whole shaft length, if appropriate. Only one support carries the axial load, and its diagrammatic display is different from others.

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design tab, design a shaft shape.
  3. Switch to the Calculation tab:
    • In the Loads & Supports area, select Supports from the pull-down listicon_dacc_shaft_load_09.png. Add Fixed Support and icon_dacc_shaft_load_10.png Add Free Support commands display in the toolbar.
    • Add free or fixed support.
    • Select the support in the tree control and click icon_custom_prop.gif to edit the support dimensions.
    • Select the support in the tree control and click icon_delete.gif to delete the support.

Specify loads

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design tab, design a shaft shape.
  3. Switch to the Calculation tab:
    • In the Loads & Supports area, select Loads from the pull-down list. Available commands display in the toolbar.
    • Click icon_static_dacc_shaft_load_07.png or icon_dacc_shaft_load_04.png to add common or continuous load.
    • Select the load in the tree control and click icon_custom_prop.gif to edit the load dimensions.
    • Select the load in the tree control and click icon_delete.gif to delete the load.

Specify forces

Forces are specified in all directions. Fx (axial), Fy (XY plane) and Fz (XZ plane). Positive force actuates in the opposite direction than the positive coordinate axis.

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design tab, design a shaft shape.
  3. Switch to the Calculation tab:
    • In the Loads & Supports area, select Loads from the pull-down list. Available commands display in the toolbar.
    • Click icon_dacc_shaft_load_02.png or icon_dacc_shaft_load_03.png to add radial or axial force.
    • Select the force in the tree control and click icon_custom_prop.gif to edit the force dimensions.
    • Select the force in the tree control and click icon_delete.gif to delete the force.

Specify moments

Specify moments in all directions. Mx (torque), My (bending - XZ plane) and Mz (bending - XY plane). Positive moment actuates in the counterclockwise direction.

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design tab, design a shaft shape.
  3. Switch to the Calculation tab:
    • In the Loads & Supports area, select Loads from the pull-down list. Available commands display in the toolbar.
    • Click icon_dacc_shaft_load_05.png to add bending moment.
    • Select the bending moment in the tree control and click icon_custom_prop.gif to edit the bending moment dimensions.
    • Select the bending moment in the tree control and click icon_delete.gif to delete the bending moment.

Specify torque

Torque is entered using two forces which are mutually opposite. One force represents the actual torque, and the other force must be negative (for example, 150 Nm and -150 Nm). The sum of all torques (Max) must be equal to 0.

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design tab, design a shaft shape.
  3. Switch to the Calculation tab:
    • In the Loads & Supports area, select Loads from the pull-down list. Available commands display in the toolbar.
    • Click icon_dacc_shaft_load_06.png to add torque.
    • Select the torque in the tree control and click icon_custom_prop.gif to edit the torque dimensions.
    • Select the torque in the tree control and click icon_delete.gif to delete the torque.

Edit shafts using Shaft Generator

icon_cmd_editcmd_32x32.png

  1. Open the Autodesk Inventor assembly with the already inserted Design Accelerator shaft.
  2. Select the shaft, right-click to display the context menu and select the Edit Using Design Accelerator command.
  3. Edit the shaft. You can add, delete features and sections, edit the calculation parameters. If you changed calculation values, click Calculate to see the strength check. Calculation results are displayed in the Results area. The inputs that fail the calculation are displayed in red (their value does not correspond with other inserted values or calculation criteria). Reports of the calculation are displayed in the Summary of Messages area.
  4. Click OK.

Add shafts to Templates Library

You can save shafts to Templates Library.

To display the Templates Library, on the Design tab, click icon_more_options.gif More in the lower right corner.

  • Click Add to add the shaft to templates.
  • Click Set to open the selected shaft template.
  • Click Delete to delete selected template.

In the Templates Description dialog box, set the template name, and click OK.

On Microsoft Windows XP, the shaft templates are saved to the following location: ...Documents and Settings\%USERNAME%\Application Data\Autodesk\Inventor [ver]\DesignAccelerator\Templates.

On Microsoft Windows Vista, the bolted connection templates are saved to the following location: AppData\%USERNAME%\Autodesk\Inventor [ver]\DesignAccelerator.

Set shaft options

Within the Shaft Generator, you can set options for features and inner sections visibility in 3D graphical preview and 2D preview.

The availability of options depends on which tab you used to open the Options dialog box. The options vary for Design and Calculation tabs. Selections made in the Design tab apply to that particular tab..

icon_cmd_design_shaft_32x32.png

  1. On the ribbon, click Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft .
  2. On the Design or Calculation tab, select icon_dacc_shaft_toolbar_14.png Options.

    Note: Options command is always available.

  3. On the Options dialog box you can:
    • On the 3D Preview box area, set options for 3D visibility of features, display of the shaft coordinate system.
    • On the 2D Preview box area, set options for 2D preview within the Design tab.
  4. Click OK.

Use padlocks to specify if the variable is independent

Lock the particular dimension to stick to the dimensions of shaft sections next to them. Use padlocks to make certain dimensions dependent and independent.

When dimensions are unlock, they can be freely changed.

Lock particular dimension - cone diameter, for example. Cone has no grips available. The dimensions change according to the dimension of section next to the cone. When you change the dimension of such section - cylinder, for example, the diameter of cone changes also. Changes in the cylinder dimensions affect the cone.

Padlocks are available for hollow sections too.

icon_tutorial.pngShaft Tutorial

 

References

Shaft Component Generator - Design tab

Use the Design tab to design a shaft of a shape. The designed shaft can contain unlimited number of sections. Each section can have two edge features and unlimited number of middle features. The preview of the shaft displays in the Autodesk Inventor window. On the Design tab (which is optional) as you design, its shape changes according to the specification made in the Design tab (number of sections, shape of sections, hollow shaft shape, and so on).

In the Autodesk Inventor window, use the 3D grips to change and define parameters of the shaft. Click the shaft element to enable it and when the grips are shown, you can:

  • Browse the selected section to see the tooltip with displayed dimension values.
  • Double-click the section to open the Edit dialog box where you can set values such as length or diameter. A preview of the section is also shown.
  • Double-click the grip to open the Edit dialog box where you can set the appropriate value (length or diameter).

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft icon_cmd_design_shaft_32x32.png

Placement

Defines the placement of the shaft. Within the Autodesk Inventor window, select cylindrical face or work axis, start plane and shaft orientation, as needed.

When you define placement, the shaft is previewed in that location in the Autodesk Inventor window. Click OK to create and constrain the shaft in the assembly.

Note: By default, the shaft is previewed in an origin - X is an axis, YZ is a start plane and XY is an orientation plane.

Axis

Select the cylindrical face or axis.

Start

Select the work plane or face that can mate with the start of the shaft.

Orientation

Select the work plane to rotate shaft or its features.

Flip

Reverses direction of the shaft.

Mate

Check the box to mate the shaft onto the selected geometry.

Sections

Use this area to design a shape of the shaft. Use the graphical toolbar and the section tree control. Select Sections or Bore on the right/Bore on the left from the drop-down list. Your selection displays the appropriate commands on the toolbar. The Options command is always available.

Click the button to add appropriate shaft section (cone, cylinder, or polygon) and feature (keyway for example). For edge features, a dialog box displays where you can set the appropriate values. Click the middle feature icon to open the edit dialog box.

Selected section and feature displays in the list where you can edit or delete it.

The graphical representation of features and sections is displayed in Autodesk Inventor window as 3D preview and in the Design tab as 2D preview (which is optional). Work with the preview as with 3D Grips. You can drag the preview to the appropriate position. Double-click to display the Edit dialog box. Move the mouse cursor above the graphical representations to display a description of a section/feature.

Tip: Enable the Always Show option in the 2D Preview area of the Options dialog box to display the 2D preview in Design tab.

Use hotkeys to perform following actions:

On the shaft toolbar:

Click a section icon

Adds the section behind the selected one.

CTRL + Click a section icon

Inserts the section before the selected one.

On the tree control:

Double-click

Opens an edit dialog box.

Right-click

Displays the context menu.

Hover mouse over the tree item

Displays a tooltip with the tree item (section/feature) information (size, for example).

Drag (for sections only)

Moves section.

Sections

icon_dacc_shaft_toolbar_02.png

Insert Cylinder inserts the cylinder section after the selected shaft section.

icon_static_dacc_shaft_toolbar_05.png

Split Selected Section splits the selected shaft cylinder while keeping the same length of the shaft.

icon_static_dacc_shaft_toolbar_03.png

Insert Cone inserts cone section after the selected shaft section.

icon_static_dacc_shaft_toolbar_04.png

Insert Polygon inserts polygon section after the selected shaft section.

icon_static_dacc_shaft_toolbar_08.png

Specify shaft by picking geometry in assembly measures the shaft geometry from selected cylindrical face, planar face, work planes or sketches from the assembly.

icon_dacc_shaft_toolbar_11.png

Collapse All Children collapses the section tree.

icon_dacc_shaft_toolbar_12.png

Expand All Children expands the section tree.

icon_dacc_shaft_toolbar_14.png

Options opens the Options dialog box where you specify your preferences for shaft 2D and 3D previews.

Bore on the left

icon_static_dacc_shaft_toolbar_06.png

Insert Cylindrical Bore inserts inside cylinder section on the left after the selected shaft section.

icon_static_dacc_shaft_toolbar_07.png

Insert Conical Bore inserts inside cone section on the left after the selected shaft section.

Bore on the right

icon_static_dacc_shaft_toolbar_09.png

Insert Cylindrical Bore inserts inside cylinder section on the right after the selected shaft section.

icon_static_dacc_shaft_toolbar_10.png

Insert Conical Bore inserts inside cone section on the right after the selected shaft section.

The sections and features are editable:

icon_custom_prop.gif

Opens the appropriate dialog box to edit dimensions.

icon_delete.gif

Deletes the selected feature or section or bore.

shaft_toolbar_features.png

Section tree control

Section tree control contains controls for shaft sections and features. Middle features display as children of the sections. Edge features display as a part of sections. Section tree control displays sections or bores at one time only.

Left edge features

The list of available features in the menu is filtered based on the section type (cone, cylinder, and so on) and based on the section position (first, in the middle, on so on).

Click the arrow to display list of available left edge features.

Click to add a feature.

Following left edge features are available:

  • icon_dacc_shaft_feature_left_02.png Chamfer
  • icon_dacc_shaft_feature_left_03.png Fillet
  • icon_static_dacc_shaft_feature_left_04.png Lock Nut Groove
  • icon_static_dacc_shaft_feature_left_05.png Relief
  • icon_static_dacc_shaft_feature_left_06.pngThread
  • icon_static_dacc_shaft_feature_left_07.png Plain Keyway Groove
  • icon_static_dacc_shaft_feature_left_08.png Keyway Groove with one rounded end

Section types

Three shaft section types are available within the Shaft generator. According to your section selection, the features are available. For Cone, no middle features are available. For polygon, no edge features are available, only Through Hole is available.

  • icon_dacc_shaft_elememt_type_01.png Cylinder
  • icon_static_dacc_shaft_elememt_type_02.png Cone
  • icon_static_dacc_shaft_elememt_type_03.png Polygon

Right edge features

The list of available features in the menu is filtered based on the section type (cone, cylinder, and so on) and based on the section position (first, in the middle, and so on).

Click the arrow to display list of available left edge features.

Click to add a feature.

Following right edge features are available:

  • icon_dacc_shaft_feature_right_02.png Chamfer
  • icon_dacc_shaft_feature_right_03.png Fillet
  • icon_static_dacc_shaft_feature_right_04.png Lock Nut Groove
  • icon_static_dacc_shaft_feature_left_05.png Relief

Section features

List of available features in the menu is filtered based on the section type (cone, cylinder, and so on) .

Click the arrow next to the icon_dacc_shaft_el_feature_01.png icon to display list of available section features.

Click to add a feature.

Following section features are available:

  • icon_static_dacc_shaft_el_feature_02.png Keyway groove
  • icon_dacc_shaft_el_feature_03.png Retaining Ring
  • icon_static_dacc_shaft_el_feature_04.png Wrench Opening
  • icon_static_dacc_shaft_el_feature_05.png Relief D
  • icon_static_dacc_shaft_el_feature_06.png Through Hole
  • icon_static_dacc_shaft_el_feature_07.pngicon_static_dacc_shaft_el_feature_08.png Groove - A, Groove -B

2D Preview

When you design shaft, you have an option to display a 2D preview of the designed shaft within the Design tab. To display 2D Preview, select the Always Show option within the 2D Preview box of the Options dialog box, and click OK.

2D Preview area is resizable.

When you select a section, appropriate section is also selected in the tree control in the Design tab, and in the Autodesk Inventor window.

Right-click to display a context menu with available features.

Place the mouse cursor above a shaft section or feature to display a tooltip informing about section or feature dimensions.

Tips:

  • Double-click the section to display the dialog box where you can edit section dimensions.
  • Press CTRL + Drag to reposition the section.
  • Hover mouse over the tree section/feature to display a tooltip with the tree item (section/feature) information (size, for example).

Results

To display the Results area on the right side of the Design, Calculation, and Graphs tabs, double-click the double line on the right or click the chevron.

Displays the calculated dimensions values such as main diameter. Click Calculate to display the values. The units of the calculated results values can be changed. Double-click the specified value you want to change.

The following output parameters are displayed in the Results pane:

  • Dimensions
    • Shaft Length (L)
  • Cylinder
    • Main Diameter (D)
    • Length (L)
  • Cone
    • First Diameter (D1)
    • Second Diameter (D2)
    • Length (L)
  • n-Side
    • Diameter Circumscribed (Dout)
    • Diameter Inscribed (Din)
    • Length (L)
    • Number of Edges (N)
    • Main Diameter (D)

Graphical Preview

A graphical preview of the selected geometry is displayed in Autodesk Inventor. You can use grips to specify section and feature dimensions. 3D Grips are available for selected section or middle feature.

Double-click or drag the 3D grip to change the dimension.

You can use 3D grips to edit following dimensions:

  • Cylinder:
    • diameter of the section
    • length of the section
  • Cone:
    • first diameter of the section
    • second diameter of the section
    • length of the section
  • Polygon
    • diameter of the section
    • length of the section
    • rotation of section
  • Keyway
    • distance of feature from section start
    • rotation of feature
    • length of the feature - available only if there is a list of available data - from Content Center, for example
  • Retaining Ring
    • distance of feature from section start
  • Wrench
    • feature width
    • feature length
    • distance of feature from section start
    • rotation of feature
  • Relief D
    • distance of feature from section start
  • Through Hole
    • feature diameter
    • distance of feature from section start
    • rotation of feature
  • Groove - A
    • distance of feature from section start
  • Groove - B
    • distance of feature from section start
    • rotation of feature

Tips:

  • Double-click a 3D grip to open the dimension edit dialog box.
  • Double-click a section/feature to open the feature edit dialog box.
  • Hover mouse over the tree section/feature to display a tooltip with the tree item (section/feature) information (size, for example).

Toolbar commands

Template Description

 

Shaft Component Generator - Calculation tab

Set material, loads, and supports to calculate the shaft.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft icon_cmd_design_shaft_32x32.png and click the Calculation tab.

Material

Specify material or select it from Material Database. Check the box to open the Material Database where you can select the appropriate material.

If a material is selected from the Material Database, its values are inserted automatically into the following edit fields, and the edit fields are locked. To unlock the fields clear the box.

Warning: Strength parameters of material are determined empirically and reflect minimum values applicable for a group of materials. Although these values are close to the values obtained using measurement of particular materials, we recommend that in cases of final calculations, to use the parameters of material according to the material sheet or specifications of the producer.

Modulus of Elasticity

(also called Young's module) is the ratio of unit stress to unit strain within the proportional limit of a material in tension or compression.

Modulus of Rigidity

Enter the modulus of rigidity of the shaft material.

Density

Enter the density of the shaft material.

Calculation Properties

Use this group box to specify the calculation properties.

Use density

Check the box to include the mass in the calculation. If you clear the Density checkbox, the Density is not included in the calculation. Mass is calculated as if the density is used.

Use shear displacement ratio

Determines if the value is used in the deflection calculation.

Shear displacement ratio: The radial forces acting on the profile cause it both to bend, and to slide. If the profile is expected to bend a lot (long or thin profiles), the sliding effect does not appear and the shear displacement ratio may be disregarded - switched off. For thick or rigid profiles this effect is more significant. Value 1.18 is used as a default for cylindrical profiles.

Number of Shaft divisions

Specify the number of the shaft divisions used for calculation.

Mode of reduced stress

Select either HMH or Tresca-Guest mode of reduced stress calculation. The selected mode affects calculated value of reduced stress. See the Engineer's Handbook for the formula used.

Loads & Supports

Use this area to specify loads and supports. Select Loads or Supports from the drop-down list. Your selection displays the appropriate commands on the toolbar. The Options command is always available.

Click the button to add appropriate force, load, or support. A dialog box displays where you can edit the values.

Selected force or support displays in the list where you can edit or delete it.

The graphical representation of loads and supports is displayed in Autodesk Inventor window. Work with the preview as with 3D Grips. You can drag the preview to the appropriate position. Double-click to display the edit dialog box. Move the mouse cursor above the graphical representations to display a description of a force or support. When you select load or support in the list in the Beam Calculation tab, its graphical representation is selected within the Autodesk Inventor window, and vice versa.

Only one support carries the axial load, and its diagrammatic display is different from others.

Tips:

  • Double-click a force/support to open an edit dialog box.
  • Hover mouse over the tree item to display a tooltip with the tree item (force/support) information (size, for example).

Loads

 

icon_dacc_shaft_load_02.png

Add Force Opens the Radial Force dialog box where you can set the radial force properties, such as distance or angle.

icon_dacc_shaft_load_03.png

Add Axial Force Click to open the Axial Force dialog window where you can set the radial force properties, such as distance or axial force value.

icon_dacc_shaft_load_04.png

Add Continuous Load Click to open the Continuous Load dialog box and set the continuous load properties, such as length or angle.

icon_dacc_shaft_load_05.png

Add Bending Moment Specifies moments in all directions. Mx (torque), My (bending - XZ plane) and Mz (bending - XY plane). Positive moment actuates in the counterclockwise direction.

Click to open the Bending Moment dialog box and set the bending moment properties.

icon_dacc_shaft_load_06.png

Add Torque Torque is entered using two forces which are mutually opposite. One of the forces represents the actual torque, the second force must be negative (for example, 150 Nm and -150 Nm). The sum of all torques (Max) must equal 0.

Click to open the Torquedialog box and set the torque properties, such as distance or torque value.

icon_static_dacc_shaft_load_07.png

Add Common Load Click to open the Common Load dialog box and set the common load properties, such as force or length.

Supports

icon_dacc_shaft_load_09.png

Add Fixed Support Click to open the Fixed Support dialog box and set the fixed support properties.

icon_dacc_shaft_load_10.png

Add Free Support Click to open the Free Support dialog box and set the free support properties.

icon_dacc_shaft_toolbar_14.png

Options Click to open the Options dialog box for 3D and 2D graphical preview.

Loads and supports are editable:

icon_custom_prop.gif

Opens the appropriate dialog box to edit loads or supports.

icon_delete.gif

Deletes the selected load or support.

2D Preview

2D preview is displayed in the lower part of the Calculation tab, by default. To hide the 2D Preview, select the Always Hide option within the 2D Preview box of the Options dialog box, and click OK.

When you select a load or support, appropriate load or support is also selected in the tree control in the Calculation tab, and in the Autodesk Inventor window.

Place the mouse cursor above a load or support to display a tooltip informing about load or support dimensions.

Green and blue position markers are displayed in the 2D preview just as in a preview in Autodesk Inventor window. For each section, three position markers are displayed, one at each end of a section, and one position marker in the middle of each section. Blue position marker means that load or support is positioned to such position marker.

Tips:

  • Double-click the load or support to display an edit dialog box.
  • Hold CTRL + double-click to open dialog box to edit force or support dimension.
  • Hold SHIFT + double-click force to open edit dialog box for force size.
  • Drag to move force or support,
  • Hover mouse over the tree item to display a tooltip with the tree item (force/support) information (size, for example).

Results

To display the Results area on the right side of the Design, Calculation and Graphs tabs, double-click the double line on the right or click the chevron.

The area displays calculated values such as the size of resistance in supports, deflection, and rotation in the place of the supports and loads, maximum bending and torsion stress, angel of twist, and mass of the shaft. Values are calculated when Calculate is pressed.

The following items are displayed in the Results pane:

Note: For more information on the calculated parameters, see Engineer's Handbook.

The Load and Support lists include some of the important values at the position of every load and support. For a continuous load, the values are listed both for the beginning and for the end of the load.

  • Results
    • Length (L)
    • Mass (Mass)
    • Maximal Bending Stress (smax)
    • Maximal Shear Stress (ts)
    • Maximal Torsional Stress (t)
    • Maximal Tension Stress (sT)
    • Maximal Deflection (fmax)
    • Angle of Twist (j)
  • Load
    • Deflection in Y Axis (fy)
    • Deflection in Y Axis (fx)
  • Support
    • Support Force in X axis (FX)
    • Support Force in Y axis (FY)
    • Support Force in Z axis (FZ)
    • Yielding in Y axis (YY)
    • Deflection in X axis (fX)
    • Deflection in Y axis (fY)

Summary of Messages

Displays the reports about calculation. To open the Summary of Messages area at the bottom of the Calculation and Design tabs, double-click the double line at the bottom of tabs or click the chevron at the bottom of the tabs.

Graphical Preview

A graphical preview of the loads and supports is displayed in Autodesk Inventor. Drag the preview of load and support to place it to the appropriate position.

Double-click the graphical representation of load and support to display a dialog box where you can change the appropriate properties.

Green and blue position markers are displayed in the preview. For each section, three position markers are displayed, one at each end of a section, and one position marker in the middle of each section. Blue position marker means that load or support is positioned to such position marker. Use Alt + drag to move a force or support and assign it to another position marker.

Tips:

  • Drag to move load or support.
  • Hold CTRL + Drag to rotate a force.
  • Hold ALT + Drag to move a force/support and assign it to another position marker.
  • Hold Shift + Drag (for continuous load only) to change the length of the continuous load.
  • Double-click force or support to open the Edit dialog box.
  • Hold Ctrl + double-click to open the Dimension Edit dialog box for force/support of position.
  • Hold Shift + double-click a force to open the Edit dialog box for force size.
  • Pause mouse over the tree section or feature to display a tooltip with the tree item (force or support) information ( for example, size).

Toolbar commands

 

Graphs tab

The Graphs tab displays diagrams of individual calculated characteristics. Some of the graphs are available for the YZ and XZ planes, as well as for the sum value.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft and click the Graphs tab.
  • Ribbon: Design tab ac.menuaro.gif Frame panel ac.menuaro.gif Beam/Column Calculator and click the Beam Graphs tab.

Graph Selection

Shear Force

Shear forces sum.

   

YZ Plane

shear force in the YZ plane
   

XZ Plane

shear force in the XZ plane

Bending Moment

Bending moment sum.

   

YZ Plane

bending moment in the YZ plane
   

XZ Plane

bending moment in the XZ plane

Deflection Angle

Deflection angle sum (between the Z axis and the shaft).

   

YZ Plane

deflection angle in the YZ plane
   

XZ Plane

deflection angle in the XZ plane

Deflection

Shaft deflection sum.

   

YZ Plane

shaft deflection the YZ plane
   

XZ Plane

shaft deflection in the XZ plane

Bending Stress

Bending stress sum.

   

YZ Plane

bending stress in the YZ plane
   

XZ Plane

bending stress in the XZ plane

Shear Stress

Shear stress sum.

   

YZ Plane

shear stress in the YZ plane
   

XZ Plane

shear stress in the XZ plane

Torsion Stress

Torsion stress.

Tension Stress

Tension stress.

Reduced Stress

Reduced stress.

Ideal Diameter

The graph shows an ideal shape of the shaft is based on the bending moment and calculates a diameter of a circular section which results in a 50MPa stress in every given coordinate of the shaft. This graph is independent on the selected shaft material. It shows the overall relations of the shape based on some constant stress.

Depending on the settings, the relevant graphs in the YZ plane (and the sum graphs as well) may include the effect of gravity and material density.

Deflection angle is the angle between the Z axis and the direction of the deflected center line at the given Z coordinate.

The formula for reduced stress is listed in the Engineer's Handbook.

Graph

Displays diagram of selected graph.

Double-click the graphical representation of graph or support to display appropriate edit dialog box where you can change values of load and support. However, you cannot delete loads and supports on the Graphs tab, you can do it in the Calculation tab only.

Results

To display the Results area on the right side of the Graphs tabs, double-click the double line on the right or click the chevron.

The area displays calculated values such as the size of resistance in supports, deflection, and rotation in the place of the supports and loads, maximum bending and torsion stress, angle of twist, and mass of the shaft.

The following items are displayed in the Results pane:

Note: For more information on the calculated parameters, see the Engineer's Handbook chapters for shafts and beams.

The Load and Support lists include some of the important values at the position of every load and support. For a continuous load, the values are listed both for the beginning and for the end of the load.

  • Results
    • Length (L)
    • Mass (Mass)
    • Maximal Bending Stress (smax)
    • Maximal Shear Stress (ts)
    • Maximal Torsional Stress (t)
    • Maximal Tension Stress (sT)
    • Maximal Reduced Stress (sred)
    • Maximal Deflection (fmax)
    • Angle of Twist (j)
    • Deflection in Y Axis (fY)
    • Deflection in X Axis (fX)
  • Support
      • Support Force in Z axis (FZ)
      • Support Force in Y axis (FY)
      • Support Force in X axis (FX)
      • Yielding in Y axis (YY)
      • Yielding in X Axis (YX)
      • Deflection in Y axis (fY)
      • Deflection in X axis (fX)

Options

Use this dialog box to specify the 3D preview settings and visibility of 2D preview in the Design and Calculation tabs.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft icon_dacc_shaft_toolbar_14.png and in the Design or Calculation tab, click Options.

Note: Some options are available only if you open Options dialog box from the Calculation tab.

3D Preview

Section Edge Features (Fillet, Chamfer,...)

Specify the visibility of 3D edge features.

Show - Section edge features is always visible.

Hide - Section edge features is hidden.

Show Only for Selected Section - 3D edge features is visible for selected section only.

Section Middle Features (Keyway, ...)

Specify the visibility of 3D middle features.

Show - Section middle features is always visible.

Hide - Section middle features is hidden.

Show Only for Selected Section - 3D middle features is visible for selected section only.

Bores

Specify the visibility of 3D bores.

Show - 3D bores is always visible.

Hide - 3D bores is hidden.

Show Only for Selected Section - 3D bores is visible for selected section only.

Bore Edge Features (Fillet, Chamfer, ...)

Specify the visibility of bore edge features.

Show - Bore edge features is always visible.

Hide - Bore edge features is hidden.

Show Only for Selected Section - Bore edge features is visible for selected section only.

Bore Middle Features (Retaining Ring, ...)

Specify the visibility of bore middle features.

Show - Bore middle features is always visible.

Hide - Bore middle features hidden.

Show Only for Selected Section - Bore middle features is visible for selected section only.

Apply same settings also for 2D preview

Select to apply the same settings for 2D preview on the Design and Calculation tabs.

If no placement show in default (X-axis, YZ-plane, XY-plane)

Select to create 3D preview of the shaft in the default position in the graphics window.

Note: If you change this option you must restart the Shaft Generator to enable the option.

Show Shaft Coordinate System

Select to show 3D shaft coordinate system.

Automatically Scale Loads and Supports

Select to scale supports and loads while zooming, and set the scale value.

Note: This option is available only if you open Options dialog box from the Calculation tab.

2D Preview

Always Hide

Select to always hide 2D preview. 2D preview is hidden in the tab (Design or Calculation) where you made the selection. It means that you can have 2D preview hidden independently in Design and Calculation tabs.

Always Show

Select to always show 2D preview. 2D preview is shown in the tab (Design or Calculation) where you made the selection. It means that you can have 2D preview shown independently in Design and Calculation tabs.

Automatically Scale Loads and Supports

Select to scale supports and loads while zooming, and set the scale value.

Note: This option is available only if you open Options dialog box from the Calculation tab.

Show Section Features in Calculation Results report

Select to show section features in the HTML report.

Note: This option is available only if you open Options dialog box from the Calculation tab.

Show Bores and Bores Features in Calculation Results report

Select to show bores and bore features in the HTML report.

Note: This option is available only if you open Options dialog box from the Calculation tab.

Show Loads&Supports in Calculation Results report

Select to show loads and supports in the HTML report.

Note: This option is available only if you open Options dialog box from the Calculation tab.

Show Section Features when Calculation/Graph tab is active

Select to display section features (keyway, groove, wrench opening, for example) in the 2D preview in the Calculation and Graph tabs.

Show Bores and Bores Features when Calculation/Graph tab is active

Select to display bores and bore features in the 2D preview in the Calculation and Graph tabs.

Show Loads&Supports Designation

Select to show the loads and supports designation such as F1, F2, q1 in the 2D preview in the Calculation and Graph tabs.

Note: This option is available only if you open Options dialog box from the Calculation tab.

 

Template Description

Displays list of shaft templates.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft icon_cmd_design_shaft_32x32.pngand on the Design tab, in More Options, click Add.

You can create each new shaft from a template. When you open the Shaft Generator, click Set to apply the template to the currently designed shaft.

Any new shaft can be used as a template. Save it to the Templates Library on the hard drive, and the next time you create a shaft, the new template is available.

The name of template must be unique. If you try to save the template and the name exists, you are prompted to set a different name.

Set

Applies selected template to a current content of the shaft.

Add

Adds a newly designed shaft to the template library.

Delete

Deletes the selected shaft template.

 

Tips:

  • When you double-click a template, you can change the template description, if needed.
  • Drag a template to reorder it within the library.

 

Cylinder

Use the dialog box to enter parameters for cylinder.

Note: You can insert an unlimited number of middle features to a cylinder.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Sections in the Sections drop-down list. On the toolbar, click Insert Cylindericon_dacc_shaft_toolbar_02.png

Dimensions

Enables Cylinder dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. The column is not editable.

Size

Click the Size field to insert a value, or select a value from displayed list.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended and available dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Preview

Displays schematic image of the cylinder section.

 

Cone

Use the dialog box to enter parameters for cone.

Note: No cone middle features are available. Only chamfer and fillet are available for edge features.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Sections in the Sections drop-down list. On the toolbar, click Insert Coneicon_static_dacc_shaft_toolbar_03.png

Dimensions

Enables cone dimensions editing.

Unlock the edit field to enable automatic update of the value in case you change the shaft parameters that influence such value. For example, if you lock the First Diameter value, and you update the diameter of previous shaft section, the cone diameter value updates automatically.

Note: Only parameters that require automatic update have the lock available.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value, or select a value from the displayed list.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Same as Previous from the context menu to enter the diameter value of the previous shaft section.

Click Connect to Previous from the context menu to enter the diameter value of the previous shaft section, and to connect the cone to the previous shaft section. The edit field is locked and value is automatically updated when you change the diameter of the previous shaft section.

Click Same as Next from the context menu to enter the diameter value of the next shaft section.

Click Connect to Next from the context menu to enter the diameter value of the next shaft section, and connect the cone to the next shaft section. The edit field is locked and value is automatically updated when you change the diameter of the next shaft section.

Note: Displayed options in the context menu depend on the shape of the designed shaft.

Description

Displays the description of the parameter. The name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Preview

Displays schematic image of the cone section.

 

Cylinder - inside shaft bore

Use the dialog box to enter parameters for cylinder as an inside shaft bore.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Bore on the left or Bore on the right in the Sections drop-down list. On the toolbar, click Insert Cylindrical Bore icon_static_dacc_shaft_toolbar_09.pngicon_static_dacc_shaft_toolbar_06.png

Dimensions

Enables cylinder dimensions editing.

Unlock the edit field to enable automatic update of the value in case you change the shaft parameters that influence such value. For example, if you lock Length value, and you update the length of designed shaft, the length of inside cone updates automatically.

Note: Only parameters that require automatic update have the lock available.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value, or select a value from displayed list.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Calculate from the context menu to automatically calculate a hollow through the length of the shaft (from a hollow on the left to a hollow on the right).

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Preview

Displays schematic image of the cylinder section.

 

Cone - inside shaft bore

Use the dialog box to enter parameters for cone as an inside shaft bore.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Bore on the left or Bore on the right in the Sections drop-down list. On the toolbar, click Insert Conical Bore icon_static_dacc_shaft_toolbar_07.pngicon_static_dacc_shaft_toolbar_10.png

Dimensions

Enables cone dimensions editing.

Unlock the edit field to enable automatic update of the value in case you change the shaft parameters that influence that value. For example, if you lock the Length value and update the length of designed shaft, the length of the inside cone updates automatically.

Note: Only parameters that require automatic update have the lock available.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value, or select a value from displayed list.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Calculate from the context menu to automatically calculate a hollow through the length of the shaft (from a hollow on the left to a hollow on the right).

Click Values from the context menu to see the list of recommended and available dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Preview

Displays schematic image of the cone section.

 

Split Selected Section

Enables you to split selected shaft section. The length of the shaft remains unchanged.

Note: Split Selected Section command is available if you select cylinders only.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. In the Design tab, click Split Selected Section in the Sections toolbaricon_static_dacc_shaft_toolbar_05.png

Select the section either in 2D preview of the Design tab or in the graphics window and click Split Section. Cylinder dialog box is displayed with two Section Length edit fields. One of them is enabled because its length is automatically changed based on dimension inserted in the enabled Section Length field.

By default, the selected shaft section is split in half. You can change the dimensions of divided sections by clicking an enabled Section Length value. The other half is spit section is calculated according to inserted value. For example, the original length of the section is 80 mm. When you click the Split Section command, Cylinder dialog box displays. Section Length L1 is 50 mm and is enabled for edit. Section Length L2 edit is 50 mm and is disabled for edit. Change the value in Section Length L1 edit field to 30 mm. Section Length L2 value automatically changes to 70 mm. Remember that length of the split section remains the same. In the Cylinder dialog box, click OK.

In 3D preview in the graphics window it is now possible to change the section length without changing the length of shaft. Select the cylinder and hold the Ctrl key while dragging the 3D grip. You change the dimension of the section but not whole length of shaft.

 

Geometry Definition

Enables you to measure shaft geometry.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. In the Design tab, click Specify shaft by picking geometry in assembly in the Sections toolbaricon_static_dacc_shaft_toolbar_08.png

You can measure the shaft geometry by selecting cylindrical, planar faces, work planes or sketches. The section diameter and length are read from selected face.

Note: Conical faces are not supported in this release.

Section length and diameter can be defined also by selection of two cylindrical edges. By selecting planar face or work plane the length of section can be modified.

The second option is to select part/assembly sketch and read the geometry from it. Function ignores chamfers, fillets, or other curve which are not parallel with sketch centerline. To select sketch it is necessary to have it properly defined, it means if you call the Inventor Revolve feature it automatically select all entities for profile and centerline

Note: If the sketch contains entities for inner bores, this version cannot work with it. It is not supported.

The sections order can be change by clicking the Flip command.

Note: If the placement is not specified then shaft is not mated.

icon_dacc_shaft_geometry_definition_01.png

Click to select faces, sketches or sketch entities.

Sketches are selected by default, to select sketch entity press and keep Alt.

Note: You cannot combine to select sketches or faces. If you select face first then it is not possible to select sketch and vice versa. Use CTRL + click the selected entity to cancel its selection

icon_flip_direction.png

Changes sections order in section tree (from left or from right).

dacc_shaft_geometry_definition_02.png

Provides a preview of the designed shaft based on the current selections.

Modified Current Shaft

Select this option to modify only section dimensions. Section, features, loads and supports remain unchanged. If a section is mission, generator adds it automatically

By default, section, features, loads and supports are deleted.

 

Chamfer

Adds a chamfer on an edge of the shaft section. You can add only one chamfer on the shaft edge.

You can insert a chamfer either on the left or on the right of the selected shaft section.

Note: For already created chamfer you cannot change the method how the chamfer was created.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the First edge features or Second edge features drop-down menus, select Chamfericon_dacc_shaft_feature_left_02.pngicon_dacc_shaft_feature_right_02.png

Method

Specifies how the chamfer is constructed.

Distance

Creates a chamfer with the same offset distance from the edge on both faces. Selects a single edge, multiple edges, or chained edges. Corner setback appearance may be specified.

Distance and Angle

Creates a chamfer defined by an offset from an edge and an angle from one face to the offset. Any edge or all edges of a selected face may be chamfered at once.

Two Distances

Creates a chamfer on a single edge with a specified distance for each face. Edges may be chained together.

Distance and Angle

Specifies the extent of selected chamfer method.

Distance

Creates a chamfer with the same offset distance from the edge on both faces. Selects a single edge, multiple edges, or chained edges. Corner setback appearance may be specified.

Distance and Angle

Creates a chamfer defined by an offset from an edge and an angle from one face to the offset. Any edge or all edges of a selected face may be chamfered at once.

Two Distances

Creates a chamfer on a single edge with a specified distance for each face. Edges may be chained together.

 

icon_tolerance_ok.gif

Confirms the component's input.

icon_tolerance_cancel.gif

Closes the dialog box.

 

Fillet

Adds a fillet on an edge of the shaft section. You can add only one fillet on the shaft edge.

You can insert fillet either on the left or on the right of the selected shaft section.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the First edge features or Second edge features drop-down menus, select Fillet.icon_dacc_shaft_feature_left_03.pngicon_dacc_shaft_feature_right_03.png
  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cone in the tree control. In the First edge features drop-down menu, select Fillet.icon_dacc_shaft_feature_left_03.png

 

Radius

Specifies the fillet radius for the selected set of edges. To change the radius, click the radius value, then enter the new radius.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

icon_tolerance_ok.gif

Confirms the component's input.

icon_tolerance_cancel.gif

Closes the dialog box.

 

Through Hole

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the Second edge features drop-down menu, select Add Through Holeicon_static_dacc_shaft_el_feature_06.png

Dimensions

Enables Through Hole dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to specify how the hole position is measured within the shaft section.

Measure from first edge

Select to measure the through hole position from the left edge of the section.

Measure from second edge

Select to measure the through hole position from the right edge of the section.

Centered

Select to place the through hole to the center of the section.

Note: If you select the Centered option, you cannot specify the Distance value.

Preview

Displays schematic image of the hole feature.

 

Keyway

Use the dialog box to enter parameters for keyway feature.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the Second edge features drop-down menu, select Add Keyway grooveicon_static_dacc_shaft_el_feature_02.png

Dimensions

Enables keyway dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to specify how the keyway position is measured within the shaft section.

Use the second drop-down menu to select a key from the Content Center.

Note: To select a standard key from Content Center you must be connected to Content Center server. Also, you cannot select component from Content Center if the Custom box is checked..

Based on your selection of a key from Content Center, the keyway data is read by Shaft Component Generator and data is used for keyway groove values. Key is not inserted with the shaft.

Type of the keyway groove is set automatically according to the key type.

Measure from first edge

Select to measure the keyway position from the left edge of the section.

Measure from second edge

Select to measure the keyway position from the right edge of the section.

Centered

Select to place the keyway to the center of the section.

Note: If you select the Centered option, you cannot specify the Distance value.

Preview

Displays schematic image of the keyway feature.

Custom

Check the box to insert user values for keyway dimensions.

Note: You cannot edit values that are grayed out. They are calculated automatically.

 

Plain Keyway Groove

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the First edge features drop-down menu, select Plain Keyway Grooveicon_static_dacc_shaft_feature_left_07.png

Dimensions

Enables plain keyway groove dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to select a key from the Content Center.

Note: To select a standard key from Content Center you must be connected to Content Center server. Also, you cannot select component from Content Center if the Custom box is checked.

Based on your selection of a key from Content Center, the key data is read by Shaft Component Generator and data is used for keyway groove values. Keyway is not inserted with the shaft.

Type of the keyway groove is set automatically according to the key type.

Preview

Displays schematic image of the plain keyway groove feature.

Custom

Check the box to insert user values for plain keyway groove dimensions.

Note: You cannot edit values that are grayed out. They are calculated automatically.

 

Keyway Groove with one rounded end

Use the dialog box to enter parameters for round keyway feature.

Note: Type of the keyway groove is set automatically according to the key type.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the First edge features drop-down menu, select Keyway Groove with one rounded endicon_static_dacc_shaft_feature_left_08.png

Dimensions

Enables keyway groove with one rounded end dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to select key from the Content Center.

Note: To select a key from Content Center you must be connected to Content Center server. Also, you cannot select component from Content Center if the Custom box is checked.

Based on your selection of a key from Content Center, the keyway data is read by Shaft Component Generator and data is used for keyway groove values. Key is not inserted with the shaft.

Type of the keyway groove is set automatically according to the key type.

Preview

Displays schematic image of the keyway groove with one rounded end feature.

Custom

Check the box to insert user values for keyway groove with one rounded end dimensions.

Note: You cannot edit values that are grayed out. They are calculated automatically.

 

Relief

Use the dialog box to enter parameters for relief feature.

Access:

  • To insert relief as a second edge feature: Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the Second edge features drop-down menu, select Reliefs.icon_static_dacc_shaft_feature_left_05.png
  • To insert relief as a section feature: Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the Section features drop-down menu, select Add Relief.icon_static_dacc_shaft_el_feature_05.png

Dimensions

Enables relief dimensions editing.

Use the drop-down menu to specify how the relief positions are measured within the shaft section.

Note: If you select Centered option, you cannot specify the Distance value.

Name

Displays the name of the parameter. The name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. The name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to specify how the relief position is measured within the shaft section.

Measure from first edge

Select to measure the relief position from the left edge of the section.

Measure from second edge

Select to measure the relief position from the right edge of the section.

Centered

Select to place the relief to the center of the section.

Note: If you select the Centered option, you cannot specify the Distance value.

Custom

Check the box to insert user values for relief dimensions.

Note: You cannot edit values that are grayed out. They are calculated automatically.

Preview

Displays schematic image of the relief feature.

 

Polygon

Use the dialog box to enter parameters for a polygon section.

Note: No edge features are available. Only Through hole is available for middle features.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, on the Sections drop-down list, select Sections. On the toolbar, click Insert Polygon.icon_static_dacc_shaft_toolbar_04.png

Dimensions

Edit polygon dimensions.

Unlock the edit field to enable automatic update of the value in case you change the shaft parameters that influence such value.

Note: Only parameters that require automatic update have the lock available.

Name

Displays the name of the parameter. The name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Description

Displays the description of the parameter. The name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Inscribed

Check the box to insert user values for inscribed polygon dimensions.

Note: You cannot edit values that are grayed out. They are calculated automatically.

Preview

Displays schematic image of the polygon section.

 

Groove

Use the dialog box to enter parameters for the groove feature.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the Section features drop-down menu, select Add Groove - A, or Add Groove - B.icon_static_dacc_shaft_el_feature_08.pngicon_static_dacc_shaft_el_feature_07.png

Dimensions

Use the drop-down menu to specify how the groove position is measured within the shaft section.

Enables groove dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to specify how the groove position is measured within the shaft section.

Measure from first edge

Select to measure the groove position from the left edge of the section.

Measure from second edge

Select to measure the groove position from the right edge of the section.

Centered

Select to place the groove to the center of the section.

Note: If you select the Centered option, you cannot specify the Distance value.

Preview

Displays schematic image of the groove.

 

Retaining Ring Groove

Use the dialog box to enter parameters for the retaining ring feature.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the Section features drop-down menu, select Add Retaining Ring.icon_dacc_shaft_el_feature_03.png

Dimensions

Enables Retaining Ring Groove dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to specify how the retaining ring position is measured within the shaft section.

Use the second drop-down menu to select a retaining ring from the Content Center.

Note: To insert standard Retaining Ring from Content Center you must be connected to Content Center. Also, you cannot select component from Content Center if the Custom box is checked..

Measure from first edge

Select to measure the retaining ring position from the left edge of the section.

Measure from second edge

Select to measure the retaining ring position from the right edge of the section.

Preview

Displays schematic image of the retaining ring.

Custom

Uncheck the box to insert your own values.

Note: You cannot edit values that are grayed out. They are calculated automatically.

 

Wrench Opening

Use the dialog box to enter parameters for a wrench opening.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the Section features drop-down menu, select Add Wrench.icon_static_dacc_shaft_el_feature_04.png

Dimensions

Enables wrench opening dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Position

Use the drop-down menu to specify how the wrench opening position is measured within the shaft section.

Measure from first edge

Select to measure the wrench opening position from the left edge of the section.

Measure from second edge

Select to measure the wrench opening position from the right edge of the section.

Centered

Select to place the wrench opening to the center of the section.

Note: If you select the Centered option, you cannot specify the Distance value.

Preview

Displays schematic image of the wrench opening.

 

Thread

Use the dialog box to enter parameters for thread feature. Specify thread dimensions, thread type, nominal size, class, and direction. Thread data originates on a spreadsheet that you can customize by adding thread types and sizes.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the First edge features drop-down menu, select Threadicon_static_dacc_shaft_feature_left_061.png

Dimensions

Enables thread dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Thread

Defines the threads. Predefined thread types are specified on a spreadsheet whose default location is:

Microsoft Windows XP: Program Files ac.menuaro.gif Autodesk ac.menuaro.gif Inventor [version] ac.menuaro.gif Design Data.

Microsoft Vista: Users ac.menuaro.gif Public ac.menuaro.gif Documents ac.menuaro.gif Autodesk ac.menuaro.gif Inventor [version] ac.menuaro.gif Design Data.

To learn how to modify the spreadsheet, click here.

Thread Type

Use the drop-down list to select the thread type from the list defined in the spreadsheet.

Size

Depending on the selected thread type, Autodesk Inventor offers you a list of nominal sizes. Each nominal size has one or more pitches available. Each nominal size and pitch combination has one or more classes available.

Designation

Select the pitch from the list for the chosen thread diameter.

Note: If you use English units, the pitch is equal to 1 divided by the number of threads per inch.

Class

Use the drop-down menu to select the class of fit for the internal thread.

Note: For English threads, the letter A represents external threads and B represents internal threads. Use higher numbers for more accurate, closer fitting requirements. For instance, use 2B for screws, bolts, nuts, and other general applications, and use 3B for highly accurate and close-fitting requirements.

Direction

Specifies Right or Left hand direction for the threads wind.

Preview

Displays schematic image of the thread.

 

Thread - inside feature

Use the dialog box to enter parameters for thread inside feature.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, in the Sections drop-down list select Bore on the left or Bore on the right, and Insert Cylindrical Bore. In the First edge features drop-down menu, select Thread.icon_static_dacc_shaft_feature_left_061.png

Dimensions

Enables thread dimensions editing.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Click List Parameters to display list with parameters. Click to select the parameter and insert the value to the Size edit field.

Click Values from the context menu to see the list of recommended dimensions.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Thread

Defines the threads. Predefined thread types are specified on a spreadsheet whose default location is:

Microsoft Windows XP: Program Files ac.menuaro.gif Autodesk ac.menuaro.gif Inventor [version] ac.menuaro.gif Design Data.

Microsoft Vista: Users ac.menuaro.gif Public ac.menuaro.gif Documents ac.menuaro.gif Autodesk ac.menuaro.gif Inventor [version] ac.menuaro.gif Design Data.

 

To learn how to modify the spreadsheet, click here.

Thread Type

Use the drop-down list to select the thread type from the list defined in the spreadsheet.

Size

Depending on the selected thread type, Autodesk Inventor offers you a list of nominal sizes. Each nominal size has one or more pitches available. Each nominal size and pitch combination has one or more classes available.

Designation

Select pitch from the list for the chosen thread diameter.

Note: If you use English units, the pitch is equal to 1 divided by the number of threads per inch.

Class

Use the drop-down menu to select the class of fit for the internal thread.

Note: For English threads, the letter A represents external threads and B represents internal threads. Use higher numbers for more accurate, closer fitting requirements. For instance, use 2B for screws, bolts, nuts, and other general applications, and use 3B for highly accurate and close-fitting requirements.

Direction

Specifies Right or Left hand direction for the threads wind.

Preview

Displays schematic image of the thread.

 

Locknut Groove

Use the dialog to enter parameters for locknut groove feature.

Access:

Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. On the Design tab, select Cylinder in the tree control. In the First edge features drop-down menu, select Lock Nut Groove.icon_static_dacc_shaft_feature_left_04.png

Thread

Use the drop-down list to select the type of the thread.

Dimensions

Enables Locknut groove dimensions editing.

Use the drop-down menu to select a locknut groove from the Content Center.

Note: You must be connected to Content Center server and your computer configured to insert locknut groove from the Content Center.

Predefined thread types are specified on a spreadsheet whose default location is:

Microsoft Windows XP: Program Files ac.menuaro.gif Autodesk ac.menuaro.gif Inventor [version] ac.menuaro.gif Design Data.

Microsoft Vista: Users ac.menuaro.gif Public ac.menuaro.gif Documents ac.menuaro.gif Autodesk ac.menuaro.gif Inventor [version] ac.menuaro.gif Design Data.

Name

Displays the name of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Size

Click the Size field to insert a value.

Click Measure from the context menu to measure dimension in the Autodesk Inventor window.

Description

Displays the description of the parameter. Name of the dimension is used in the Calculation tab and in the Results pane. Column is not editable.

Custom

Check the box to insert user values for locknut groove dimensions.

Note: You cannot edit values that are grayed out. They are calculated automatically.

Preview

Displays schematic image of the locknut groove feature.

 

Axial Force

Use the dialog box to enter parameters for axial force of shaft.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. Click the Calculation tab, on the drop-down list in the Loads & Supports area, select Loads. Click Add Axial Force from the toolbar.icon_dacc_shaft_load_03.png
  • On the Loads & Supports area of the Calculation tab, select the Axial Force in the tree control, and click Loads properties.icon_custom_prop.gif
  • Double-click the force preview in the Autodesk Inventor window.

Properties

Distance from middle of section

Enter the value for distance measured from the beginning, middle, or end of the section defined by active position marker.

Force

Axial Force

Enter the value for axial force.

 

Common Load

Use the dialog box to enter parameters for common load of the shaft.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. Click the Calculation tab, in the Loads & Supports drop-down list select Loads, and in the toolbar click Add Common Load.icon_static_dacc_shaft_load_07.png
  • On the Loads & Supports area of the Calculation tab, select common load in the tree control, and click Loads properties.icon_custom_prop.gif
  • Double-click the load preview in the Autodesk Inventor window.

Enter the values of the Radial Force, Axial Force, Continuous Loads, Bending Moment, Torque, and Distance. Click OK to recalculate values.

 

Continuous Load

Use the dialog box to enter parameters for continuous load of the shaft.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. Click the Calculation tab, in the Loads & Supports drop-down list select Loads, and in the toolbar click Add Continuous Load.icon_dacc_shaft_load_03.png
  • On the Loads & Supports area of the Calculation tab, select continuous load in the tree control, and click Loads properties.icon_custom_prop.gif
  • Double-click the load preview in the Autodesk Inventor window.

Properties

Enter the value for distance measured from the beginning, middle, or end of the section defined by active position marker.

Loads

Select the option and enter the load values.

 

Bending Moment

Use the dialog box to enter parameters shaft bending moment.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. Click the Calculation tab, in the Loads & Supports drop-down list select Loads, and in the toolbar click Add Bending Moment.icon_dacc_shaft_load_05.png
  • On the Loads & Supports area of the Calculation tab, select Bending Moment in the tree control, and click Loads properties.icon_custom_prop.gif
  • Double-click the load preview in the Autodesk Inventor window.

Properties

Enter the value for distance measured from the beginning, middle, or end of the section defined by active position marker.

Moments

Depending on your selection, Moment with angle or Moment in X and Y axes, the additional options display in lower part of the area.

 

Moment with angle

 

 

 

Bending Moment enter the value of the bending moment.

 

 

Angle enter the angle value.

 

Moment in X and Y axes

 

 

 

Bending Moment in Y axis enter the value of the bending moment in the Y axis.

 

 

Bending Moment in X axis enter the value of the bending moment in the X axis.

 

Radial Force

Use the dialog to enter parameters for shaft radial force.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. Click the Calculation tab, in the drop-down list in the Loads & Supports area select Loads, click Add Radial Force from the toolbar.icon_dacc_shaft_load_02.png
  • On the Loads & Supports area of the Calculation tab, select Radial Force in the tree control, and click Loads properties.icon_custom_prop.gif
  • Double-click the load preview in the Autodesk Inventor window.

Properties

Enter the value for distance measured from the beginning, middle, or end of the section defined by active position marker.

Force

Depending on your selection, Force with angle or Force in X and Y axis, the additional options display in lower part of the area.

 

Force with angle

 

 

Force enter the value of the force.

 

 

Angle enter the angle value.

 

Force in XY and XZ planes

 

 

 

Force in Y axis enter the value of the force in the Y axis.

 

 

Force in X plane enter the value of the force in the X axis.

 

Supports

Use the dialog to enter parameters of shaft supports.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. Click the Calculation tab, in the Loads & Supports drop-down list select Supports, and in the toolbar click Add Fixed Support or Add Free Support.icon_dacc_shaft_load_09.pngicon_dacc_shaft_load_10.png
  • On the Loads & Supports area of the Calculation tab, select free or fixed support in the tree control, and click Support properties.icon_custom_prop.gif
  • Double-click the load preview in the Autodesk Inventor window.

Properties

Enter the distance value which defines the distance of the actual support from the left side of the section.

Support Type

Use the Type drop-down list to select the bearing in the assembly. Bearings data are entered to the edit fields. Plasticity is calculated automatically based on the parameters.

Note: The drop-down list is available if you uncheck the Custom box at the left lower corner of the dialog box.

Depending on your selected support type, the edit fields are enabled to change the values.

Outside Diameter

Enter the outside diameter value - diameter of the actual bearing.

Width

Enter the width of the actual bearing. Only for cylindrical, sealed needle roller bearings. For taper roller bearings, the input parameter is the width the outside circle.

Yielding

Define the plasticity.

Custom

Uncheck the box to be able to select the type of support.

 

Torque

Use the dialog box to enter parameters of shaft torque.

Access:

  • Ribbon: Design tab ac.menuaro.gif Power Transmission panel ac.menuaro.gif Shaft. Click the Calculation tab, In the Loads & Supports drop-down list select Loads, and in the toolbar click Add Torque.icon_dacc_shaft_load_06.png
  • On the Loads & Supports area of the Calculation tab, select Torque in the tree control, and click Loads properties.icon_custom_prop.gif
  • Double-click the torque preview in the Autodesk Inventor window.

Properties

Enter the value for distance measured from the middle of the section.

Moment

Enter the torque value.