Creating a Rest

You can use the Rest command to remove material from the active body to create a platform-like area. The area of the rest is an inner protected volume, which means that no other volumes within the same body can penetrate this area.

You can add a rest to a shelled or unshelled body. The results will vary, depending on the volume type that you select. If you add a rest to a shelled body, it creates supporting walls, if necessary.

Related Topics
More about Rests
Creating Functional Features
Using the Display Only Parents Option to Retrieve a Creation Context

  1. Click Rest in the Functional Features toolbar.

    The Rest dialog box appears.

  2. Select a closed profile.

    A rest requires a closed profile on the body indicating where the rest is to be created.

    Tip: If no profile is defined, clicking Sketcher enables you to sketch the profile you need.

  3. Enter 8mm in the First length box to define the distance from the sketch plane up to the bottom.

  4. To define the landing, enter 10mm in the Second length box to define the distance from the sketch plane up to the landing. Previewing the feature lets you get an idea of what the rest looks like. As a protected area, it is displayed in red:



  5. Select Mirrored extent to extrude the profile in the opposite direction using the same length value as the one defined for the first length.

  6. Click Reverse Direction to reverse the extrusion direction. Another way of reversing the direction is by clicking the arrow in the geometry area.

    By default, the Normal to profile option is checked, meaning that the profile is extruded normal to the sketch plane. If you wish to specify another direction, just uncheck the option, and then select a geometrical element to be used as the new reference. For the purposes of our scenario, keep the default option.

  7. Select the Draft tab to define a draft angle.

  8. In the Draft behaviour list, select Intrinsic to feature.

  9. Enter the desired value in the Angle box.

    The default neutral element (defines a neutral curve on which the drafted face will lie) is the Profile plane. The other possible neutral elements can be:


    • Bottom
    • Landing
    • Plane/Surface



    A Clearance volume angle box and associated Reverse button allows the clearance draft to be independent of the platform draft. This allows, for example, the platform draft to be used for aesthetic reasons (large draft value) and the clearance draft to be used for manufacturability (small draft value).

  10. Enter 7deg in the Angle box and 8deg in the Clearance volume angle box.

  11. Click Reverse button at Angle.



  12. Click the Fillet tab.

    Selecting Lateral radius check box enables you to fillet lateral edges. Then, you merely need to set the radius value of your choice. Select the Bottom radius check box to fillet bottom edges.

    Important: You can select the Draft fillets check box from the Fillet tab. For more information, see More About Draft Fillets.

  13. Select the Landing radius check box to fillet landing edges and enter 6mm as the radius value.



    If the rest is to be shelled, you can select Constant wall thickness check box. This propagates the fillets into the shell, thus maintaining a constant wall thickness.

  14. To define the wall, you can set one of the two options available from the Type drop down list:


    • Use body thickness: the rest wall thickness is that of the active shelled body thickness.

    • Enter thickness: simply enter the value you want. After this option is selected, the value box becomes available. Wall thickness values can only by positive values.

    You can control whether the wall is constructed inside or outside of the selected profile. The default is an inside wall thickness.

  15. Click OK to confirm and create the rest.

    The rest is created. The protected area is hidden. Rest.X is added to the specification tree in the Solid Functional Set.X node.