Sweep

This task shows you how to define a sweep.

1. Click any icon requiring a shape definition. For example, launch the Shellable capability , then click the Sweep icon.

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 Sweep 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 Sketch.2 as the profile you wish to sweep.

   If you launch the command with no profile previously defined, just access the Sketcher by clicking the icon available in the dialog box and sketch the profile you need.

   Path

3. Click the Center curve field and select Sketch.1 or click the Sketcher icon to sketch the center curve you need.

   Checking the Between points option defines the sweep between two points along the path (other than the endpoints). You merely need to select the points of your choice to define Point 1 and Point 2.

   The Profile/Surface needs to be between the two points along the path. When if the Profile/Surface is outside of the two points, the feature will be created from the spot of the sketch on the path keeping the same length of the distance between the two points.

   Control

4. You can control the sweep position by choosing one of the following options:

   Keep angle: keeps the angle value between the sketch plane used for the profile and the tangent of the center curve.

   Pulling direction: sweeps the profile with respect to a specified direction. To define this direction, you can select a plane or an edge.

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

   Create Line: for more information, 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

   Reference surface: the angle value between axis h and the reference surface is constant.

   
   For the purposes of our scenario, use the Keep angle option.
   Checking the Cut end option cuts the sweep's end profile so that it is normal to the end of the selected center curve.

   The Move profile to path option will sweep the sketch such that:

   • the anchor point travels along the path

   • the anchor direction remains parallel to either the pull direction or the normal to the reference surface

   The Move profile to path capability allows the user to obtain a simple associative between the profile and the path, and also allows a single sketch to be swept along multiple paths.

   To access the Move profile to path capability in Sweep, you need to follow the steps:

   • Sets the Profile Control to either Pulling direction or Reference surface.

   • Turns on the Move profile to path checkbox.

   • Builds the profile with the following understanding:

     • The origin of the sketch plane (i.e. 0,0) will be swept along the path.

     • The vertical axis of the sketch plane (i.e. 0,1) will be kept parallel to either the Pulling direction (if profile control is set to Pull direction) or the normal to the Reference surface (if profile control is set to Reference surface).

   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 a neutral element Profile plane: The default neutral element defines a neutral curve on which the drafted face will lie. Plane/Surface: If this is chosen, the Selection field is active. You just need to select the plane or surface of interest. 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. 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 a creation of the Prism to choose Draft Properties in the pull down menu. See Faces to draft section. a neutral element Profile plane: The default neutral element defines a neutral curve on which the drafted face will lie. Plane/Surface: If this is chosen, the Selection field is active. You just need to select the plane or surface of interest. 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, 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. Three options are available: 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.

   
   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 if you wish to fillet lateral edges. Then, you merely need to set the radius value of your choice.

8. Check the First radius option if you wish to fillet top edges. Then, you merely need to set the radius value of your choice.

9. Check the Second radius option if you wish to fillet the opposite bottom edges. Then, you merely need to set the radius value of your choice.

   Thick

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

    Three additional options display:

11. To add thickness to the inside of the profile, for example, enter 9mm in the Thickness1 field.

12. To add thickness to the outside of the profile, for example enter 3mm in the Thickness2 field . The application previews the new thickness.

13. To add material equally to both sides of the profile, check Neutral fiber and click Preview to see the result. The thickness you defined 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.