Shells are parametric features used for cast and molded parts. Material from the part interior is removed, leaving a hollow cavity. Changes to the dimensions of either the part or the shell automatically resize both.

By default, Autodesk Inventor LT provides a precise shell feature. If a precise solution does not exist and approximation is enabled, an approximation is attempted.

How are shells defined?

To define a shell, you specify one or more part faces to remove from one or more bodies, leaving the remaining faces for shell walls. You set the thickness of the shell wall and indicate the direction relative to the current part face. If no faces are specified for removal, the shell creates a hollow part.

Do all shell walls have to be the same thickness?

It is a good practice to specify a uniform wall thickness, because uniform wall thickness helps prevent distortion during manufacture and cooling. If necessary, specific walls can have a different thickness.

How do precise and approximate solutions differ?

In a precise solution, each point of the original surface has a corresponding point on the offset surface. The distance between the two points is equal to the specified thickness. An approximate solution enables Autodesk Inventor LT to deviate from the specified distance in an attempt to find an acceptable solution.

You can control where the deviation is allowed to occur, as well as the accuracy of the approximation. Keep in mind that the more accurate the approximation, the longer it takes to compute. Approximate solutions are provided only when a precise solution does not exist and when an approximate solution can be found. If approximate solutions are not acceptable, you can turn off this option .

Each time approximation is used, the tolerance of the deviation is reported upon selecting OK.

Can features be added after a shell is created?

Because shells remove material from the entire part, features added to a part after the shell is applied is not shelled. For example, if you sketch and extrude a solid feature on a shell wall, the extrusion is not shelled.

To make sure that all features are included in a shell feature, use one of the following methods:

Sketch all features on the part before you create the shell.
Use the browser to reorder features. Move all sketched features above the shell in the hierarchy.

Procedures

Create a shell feature

On the 3D Model tab, Modify panel, click Shell to remove material from a part interior, creating a cavity with walls of a specified thickness. By default, Autodesk Inventor LT provides a precise shelling solution. When a precise solution does not exist, Autodesk Inventor LT attempts an approximation.

Start with a single feature or a part.

On the ribbon, click 3D Model tabModify panel Shell.
Click Remove Faces, and select the faces to remove in the graphics window. If multiple tangent faces are highlighted with a single selection, and this selection is not ideal, clear the check box for the Automatic Face Chain option before selecting.
If you preselected a face, it is automatically highlighted.
Click Solids if available in a multi-body part file to choose the participating solids.
Click a direction button to specify the direction of the shell offset from the surface of the selected face (inside, outside, or both).
Enter the default face thickness.
To change how approximate shelling solutions are computed, click the More tab.
- To prevent approximate shelling, clear the Allow approximation check box.
- To determine where the deviation is distributed, click the arrow to select from the list.
- To specify the accuracy of the computation, select the appropriate option. If Specify tolerance is selected, enter a tolerance in the box.
To change the thickness of a specific shell face, click More.
Click in the row, then select one or more faces.
In the Thickness box, enter the face thickness.
Continue to change face thickness, as needed.
Click OK.
If an approximation is used, click OK in the message box to accept the results or Edit to return to the Shell dialog box More tab.
Show Me how to create a shell feature

Show Me how to create a shell with unique face thicknesses

NoteTo reset a shell face to its original thickness, click in the Thickness box for that face, then press Delete.

References

Shell

Removes material from a part interior, creating a hollow cavity with walls of a specified thickness. Selected faces can be removed to form a shell opening.

Access:

Ribbon: 3D Model tab

Modify panel

Shell

Shell tab

Direction Specifies shell boundary relative to the part face.

Inside Offsets the shell wall to the part interior. The external wall of the original part becomes the external wall of the shell.

Outside Offsets the shell wall to the exterior of the part. The external wall of the original part is the internal wall of the shell.

Both Sides Offsets the shell wall equal distances to the inside and outside the part. Adds half of the shell thickness to the thickness of the part.

Remove faces Selects part faces to remove, leaving the remaining faces as the shell walls.

Click to activate the part, then select the faces to remove. To reclaim a face, press and hold Ctrl and select the face.

Selected faces are removed. Thickness is applied to remaining faces to create shell walls. If no part faces are selected for removal, the shell cavity is entirely enclosed within the part.

Automatic Face Chain Enables or disables the automatic selection of multiple tangent continuous faces. Default setting is On. Uncheck to allow individual tangent face selection.

Solids Selects the participating solid bodies in a multi-body part file. Not available if the part contains only one body.

Thickness Specifies the thickness to be applied uniformly to shell walls. Part surfaces not selected for removal become shell walls. To use the thickness value in a parameter table, highlight the value in the box, and then right-click to cut, copy, paste, or delete it.

More tab

Allow approximation

When no precise solution exists, allows a deviation from the specified thickness while computing the shell feature. A precise solution creates a shell where each point on the original surface has a corresponding point on the shell surface. The distance between these two points is the specified thickness.

Select whether to allow an approximate solution, and then click the arrow to select the deviation type from the list. Click a command to choose a computation option.

Mean deviation is divided to fall both above and below the specified thickness.

Never too thin preserves minimum thickness. The deviation must fall above the specified thickness.

Never too thick preserves maximum thickness. The deviation must fall below the specified thickness.

Optimized	Computes using a tolerance that allows a minimal compute time.
Specify tolerance	Computes using the specified tolerance. Considerable computation time can be required. Click the command and then specify a tolerance.

(More)

You can override the default thickness to apply a unique thickness to selected walls. Click in the row to activate, then select faces.
Select	Displays the number of selected faces to which the new thickness applies.
Thickness	Sets new thickness for selected faces.
Deleting a row resets the shell walls to the default thickness.

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