Prism

1. Click any icon requiring a shape definition. For example, launch the Shellable capability . The Prism is the default shape proposed by the application.

Profile/Surface

All the Shape features have a Profile/Surface as part of the Prism geometry definition. You can select an existing sketch, a sketch output, a sketch output profile profile or surface as a Profile/Surface of the Prism definition. If you launch the command with no profile previously defined, you can access to the Sketcher by clicking the icon available in the dialog box and sketch the profile you need.

You can also select any face originated by Functional Features of any Functional Body. In this case, the face needs to be the original untrimmed (unmerged) of the feature.

You can also select any topological (trimmed) face of any Part Design body that is not the Part Body containing the active Functional Body.

2. Select the rectangle you have prepared for Profile/Surface.

   Limits/Distance

   All the Prism Shapes of the Functional features have two boundaries at the opposite sides of the extrusion direction. For Shape Features and Rib Functional Feature they are called First length and Second length. For some Functional Features (Cutout and Pocket) there are Floor and Opening on each side. By default, the application specifies the length of your prism.

There are following four ways of defining lengths. Depending on the Shape Feature you are defining, the length option selections vary. Length: entering a value. Thru All: the feature extends the protected volume itself along the prism extrusion direction outside the boundaries of the Functional Body. To Shell: the feature extends to trim the volumes at an offset of the shell. Shape Features: Cavity, Added, Protected, Internal, and Core Functional Features: Cutout, Pocket, Boss, Rib, and Reinforcement Feature Modifiers: Remove Feature and Intersect Feature

To Shell option for length in functional features will be available only when shellable feature is present in solid functional set. If no shellable feature is present in PartBody, the To Shell option will not be displayed in the length for concerned functional features.

• To Plane/Surface: the plane or surface you select trims the prism. In alternative to the selection of a plane/surface you can select a sketch, a sketch Output or a sketch Output Profile as profile, in this case a surface is automatically extruded along the sketch plane normal. It is also possible to trim the prism at an Offset distance from the plane or surface. If existing planes or surfaces do not meet your needs, you can use any of these creation contextual commands available from the empty field:

  • Create Plane: you can create a plane by using one of the method described in Creating Planes.

  • XY Plane: the XY plane of the current coordinate system origin (0,0,0) becomes the trimming element.

  • YZ Plane: the YZ plane of the current coordinate system origin (0,0,0) becomes the trimming element.

  • ZX Plane: the ZX plane of the current coordinate system origin (0,0,0) becomes the trimming element.

  • Create Join: joins surfaces or curves. See Joining Surfaces or Curves.

  • Create Extract: generates separate elements from non-connex sub-elements. See Extracting Geometry.

3. Enter the value of your choice the First length field to define the feature length from the sketch plane. If you prefer, you can drag the LIM1 manipulator in the geometry area.

   For the purpose of our scenario, enter 18mm.

   Optionally, you can also enter a value in the Second length field to define the feature length in the opposite direction.

   Checking the Mirrored extent option extrudes the profile in the opposite direction using the same length value as the one defined for the first length.

   Clicking the Reverse Direction button reverses the extrusion direction. Another way of reversing the direction is by clicking the arrow in the geometry area.

   Direction

4. Click the Direction tab.

   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.

    You can also use any of the following creation contextual commands:

   Create Point: For more information, see Creating Points Create Line: see Creating Lines. Create Plane: see Creating Planes Edit Components: edits the coordinates of the direction's components. X Axis Y Axis Z Axis Compass direction

   Clicking the Reverse Direction button reverses the extrusion direction.

   For the purpose of our scenario, use Normal to profile .

   Draft

5. Click the Draft tab.

   The Draft behavior field provides three options:

   None: there is no draft. Intrinsic to feature: you can perform a draft operation by defining the followings: an angle value You can enter the angle value. a neutral element You need to define a neutral element. Draft Properties: you can perform a draft operation by defining the followings with the faces to be drafted. Note: You need to define a Draft Properties prior to the creation of the Prism to choose Draft Properties in the pull down menu. See Faces to draft section. a neutral element Faces to draft

   Neutral element

   Profile plane: It is the default neutral element (defines a neutral curve on which the drafted face will lie).

   First limit: Automatically select a face.

   Second limit: Automatically select an alternate face.

   Plane/Surface: If this is chosen, the Selection field is active. You need to select the plane or surface of interest. From R16 onwards, you can select a sketch. When the sketch is selected, a GSD surface will be automatically built internally.

   Use parting element: This option will be available when Draft properties is selected. The Neutral element is equivalent to the selected Draft Properties Parting element.

   Faces to draft

   Faces to draft functionality can control which faces are drafted. There are three options:

   All lateral faces: It is the default neutral element (defines a neutral curve on which the drafted face will lie).

   Selected by pull direction: It will automatically select the faces to draft to be those that are parallel to the pull direction vector.

   Select profile curves: This method allows you to specify what faces to draft by picking curves of the boundary profile. I.e.: the defining profile curve for the face. You need to select Curves. There are two options available: First limit Second limit

   Parting element

   When the Profile Plane or Plane/Surface options are chosen to define the neutral element, then the Parting=Neutral  option is active by default. Moreover, when Parting=Neutral  is active, the Draft both sides option becomes active too. If Draft both sides is on, the draft will be symmetrical on the parting element. Parting=Neutral: If this is chosen, the plane or surface you selected as the neutral element is also used as the parting element. Draft both sides: If this is chosen, the draft operation applies to both opposite directions from the parting element. Draft fillets: If this is chosen, the fillets are applied before the draft is created. Sometime small edges that do not lie on the parting surface might be created. With this option, the fillets will become the variable radius fillets instead of the constant fillet and it prevents to generate the extra edges.

   Without Draft Fillets option                     With Draft Fillets option

   For the purpose of our scenario, set the Intrinsic to feature option, the profile plane as the neutral element and then enter the value of your choice to define the draft angle.

   Fillet

6. Click the Fillet tab.

7. Check the Lateral radius option to fillet lateral edges. You merely need to set the radius value of your choice. For example, enter 6mm.

   Checking the First radius option lets you fillet top edges. You merely need to set the radius value of your choice.

   Checking the Second radius option lets you fillet bottom edges. You merely need to set the radius value of your choice.

You can add lateral fillets to the end faces of open sketches when the Fillet profile ends option is combined with one or multiple of the radius options. Here are simple examples of the Fillet profile ends option.

8. Check the Thick option. This option enables you to add material to both sides of the profile.

9. Enter 10mm in the Thickness1 field and click Preview. Thickness is added to the inside of the profile.

10. Enter 15mm in the Thickness2 field and click Preview. Thickness is added to the outside of the profile.

11. Enter 10mm and check Neutral fiber and click Preview to see the result. The Neutral fiber option adds the same thickness to both sides of the profile. The thickness you define for Thickness1 is evenly distributed.

    Core (Specific to Shellable Features)

    The Core capability enables you to define a core body (offset) for a shellable feature.