About Creating Both Side Drafts

The Draft Both Sides capability allows you to draft faces on each side of a parting element you determine.

Topics discussed are:

This page discusses:

See Also
Creating Auto Drafts for Casting

Mode

The app offers two modes for creating both sides drafts.

  • Reflect/Reflect: the neutral faces are the filleted edges and the faces to draft are automatically defined by the neutral elements as being the tangent faces. This mode is available in all three computational methods.
  • Neutral/Neutral: the neutral selected faces can be propagated by tangency, and the faces to draft can be defined either by the user or automatically by the neutral elements. When this mode is chosen, radius values are displayed in the geometry. This mode is available only in Independent, and Fitted computational methods.

Computation Methods

Three computation methods are available for creating both sides drafts.

  • Independent: you need to specify two angle values, as shown in the scenario above.

  • Driving/Driven: the angle value you specify for one face affects the angle value of the second face. By default, 1st Side Driving is the selected side, meaning that the angle value you specified for the face selected first is the driving value. You can change and select 2nd Side Driving instead.

    Sometimes, some resulting faces of the "Driven draft" are not apt for being removed from molds. In this case, we recommend you to check this using the draft analysis capability. For more information about draft analysis capability, see FreeStyle Shaper, Optimizer & Profiler User's Guide: Analyzing Shapes: Analyzing Draft Angle.

  • Fitted: performs a draft operation on two opposite sides of the part while adjusting the resulting faces on the parting element you chose.

Pulling Direction

You can define the pulling direction by selecting the reference element.

Contextual commands creating the reference elements you need are available from the Selection box:

  • Create Line: For more information, see Generative Shape Design User's Guide: Creating Wireframe Geometry: Creating Lines.
  • Create Plane: For more information, see Generative Shape Design User's Guide: Creating Wireframe Geometry: Creating Planes.
  • X Axis: the X axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Y Axis: the Y axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Z Axis: the Z axis of the current coordinate system origin (0,0,0) becomes the direction.

If you create any of these elements, the app then displays the corresponding icon next to the Selection box. Clicking this icon enables you to edit the element.

Parting Element Adjustment

You can set the Parting Element Adjustment to remove some transversal sharp edges.

The resulting drafted faces of a draft both sides fitted are adjusted on the parting surface. This constraint may lead to transversal sharp edges. In some cases (forging for instance), this constraint may not be useful and these transversal sharp edges may be unwanted. In such cases, you may need to set the Parting Element Adjustment to remove some transversal sharp edges.

Methodology

This option allows you to authorize the resulting drafted faces to join not exactly on the parting surface, but slightly above or below, in order to minimize the number of transversal sharp edges once the part is drafted. It actually gives you the ability to specify a tolerance of such vertical deviation. This vertical tolerance (the entered value) corresponds to the maximum distance the user can afford between the point where the skins locally join and the parting surface, distance calculated along the pulling direction. So the bigger this tolerance is, the less transversal sharp edges there will be, but the further from the parting surface the two drafted skins can join.

In the following figure, the parting element adjustment would correspond to the maximum authorized distance between A or B (point of skins adjustment) and the red line (parting), along the pulling direction. This vertical tolerance in fine defines how far A or B can be from the parting surface.

Pulling Direction



The red line represents the Parting Element.

The purple lines represent the Drafted skins joining strictly on the parting element.

The orange lines represent the Drafted skins joining below the parting element.

The green lines represent the Drafted skins joining above the parting element.

The tolerance is only available for both sides fitted drafts through the Draft Both Sides functionality.

Automatic Relimitation

This capability is applicable when the ribbon propagation encounters the first twist in the draft skin while creating a draft for a single body.

It will reduce some steps and design time. With this capability, drafts will not fail in case of twist, but instead drafts the maximum ribbon and leaves undrafted the twisted zones. The twist problem basically arises because of the following reasons:

  • When reflect/neutral curve tends to become parallel to the pulling direction.

  • When there is a collision between non-adjacent draft faces. This happens when reflect/neutral curve is not a straight line and we have relatively large draft angle.

Consider a solid part to be drafted. The input data such as pulling direction, parting surface, draft angle value are specified.



Starting from the selection (leftmost figure below), the maximum draft creates the longest draft ribbon on the solid, until a twisted surface stops the draft progression (rightmost figure below). Now the draft operation does not fail because of twist.





To draft the whole body, the procedure can be repeated by creating another maximum draft, selecting new faces (left figure below). Once more, some twisted surface can interrupt the draft ribbon (right figure below).





The cap faces are created at the location where draft ribbon propagation stops because of twist. Finally you can fill this portion and joins those with the draft result to get final result.



  • The maximum both sides draft capability is applicable only with the Draft Both Sides function with Fitted option and Advanced Draft function.

  • If you selects faces to draft such that, they are separated by a twist, then the draft operation will fail with a Multi-Ribbon error. This is because, draft ribbon propagation in a direction stops as soon as first twist is encountered. A new ribbon is required to cover the remaining faces to draft (if any) which were selected by you. The multiple ribbons are not yet supported in Draft Both Sides with Fitted option.

More about Advanced Draft

This section provides you information on the advanced draft.

  • The draft operation can be initialized only if the faces to draft and neutral elements of two sides lay one above another with respect to the pulling direction. This is a limitation to avoid bad performance in initialization phase.
  • There should be at least one common edge between the whole set of faces to draft and each neutral face selected. This is applicable only in Neutral/Neutral mode with Fitted computation method.
  • The draft ribbon propagation fails if the tangent propagation on neutral faces leads to a face to draft or vice versa. So in general for draft operation to succeed the common edges between neutral faces and faces to draft should be sharp. This is applicable only in Neutral/Neutral mode with Fitted computation method.
  • The features in the body to be drafted may get lost because of sewing of draft skin to the body. Sometimes it may cause failure of draft operation.

Editing Drafts Created With Advanced Draft

You can edit the drafts created using Advanced Draft command.

Double-clicking on both side draft features created using Advanced Draft displays the Draft Both Sides dialog box in which changing parameters will be done more easily.

Parting Line Adjustment

This section provides you methodology of using the Parting Line Adjustment option.

Methodology

The Parting Line Adjustment option thus adds material to the 3D shape. If then you decide to use it, you should keep in mind that you need to enter reasonable values not to add too much material prior to machining processes. Usually, 0.1mm set as the default value provided by the app, proves to be efficient most of the time.

Concerning draft angle values, again make sure the value you enter does not add too much material. In the worst cases, this would prevent you from removing parts from molds.

In other words, a successful draft operation requires a fine tuning between the draft angle value you set and the parting line adjustment you may perform. The challenge being to add the minimum material to the 3D shape.

Tip: Remember that you can always check curvatures by performing surface curvature analysis and draft validity using the draft analysis capability. For more information about surface curvature analyses capability, see FreeStyle Shaper, Optimizer & Profiler User's Guide: Analyzing Shapes: Analyzing Surfacic Curvature.