填補

定義邊界並使用邊界條件 (而不需使用參考曲面) 來細修曲面以建立一個曲面 (或從曲面建立零件)。

填補：桌面版

影片範例

影片字幕

The Fill feature connects boundary edges to create surface geometry. Deciding on whether to use Boundary surface, Loft, or Fill feature depends on the application. The Boundary surface and Loft features require 4-sides to the boundaries, whereas the Fill feature can utilize as many boundary segments as needed. This is especially useful when holes and gaps with several surfaces must be patched with a single feature. A Loft or Boundary surface provide more control and result in higher-quality surfaces.

The Fill surface feature can be used to repair imported models, patch the area of a model that contains complex geometry, or simply enclose a surface model to create a solid part. To create a surface with the Fill feature, the sections must have fully connected edges to form a single chain.

Start a new Fill feature. Select the edges of a part, surface, sketched or 3D curve. As each entity is selected, two red dots indicate the start and end of the selected boundary chain. To create a surface, the boundary must be completely closed. If not, the red dots remain visible in the graphics area. Pay close attention to these indicators. In some situations, a small interruption in the boundary prevents a closed chain. As a best practice, use the Create selection option. Under the Edges tab, select “Loop/Chain connected” to quickly select the entire boundary. Once the boundary has been completely closed, the red dots are removed from the graphics area. A Fill surface can still be created if a portion of a boundary completes a chain but does not stop where it connects to other entities.

The New option creates a new surface and is visible in the Parts list under Surfaces. Add, adds the surface to other surfaces defined in the merge scope. Select Match position, Tangency, or Curvature in the Continuity dropdown to set boundary conditions. If the portion of the boundary is a sketch entity and the option to match tangency is selected, Onshape respects the direction normal to that sketch plane. Interior edges, 3D fit splines, projected curves, and bridging curves can only match position. A composite curve can be used to match tangency or curvature, only when edges of a surface have created the curve. Onshape analyzes the underlying surfaces that form the composite curve and can match the appropriate continuity. When choosing Position, the fill surface maintains G0 continuity to the surrounding geometry. Choosing tangency ensures G1 continuity, and matching curvature ensures G2 continuity. When tangency or curvature are selected, apply finer control by specifying adjacent faces.

A guide for the Fill feature is similar to a guide for a Loft feature for manipulating the surface geometry. Use curves or vertices as guides. Using vertices as a guide, the surface passes through those points while satisfying the boundary conditions. Using curves as a guide, the surface geometry accurately follows specific or sampled points along the curve. Precise follows the guide curve exactly as defined. Sampled takes a sampled number of points that follow the curve the fill surface passes through. This option is helpful if the fill surface is heavily constrained. For this reason, “sampled” may be used to loosen the constraints for the guides and results in a smoother surface. The number of sampling points can be changed by increasing or decreasing the sample size.

Check Show ISO curves to evaluate the flow of the filled surface visually. Adjust the Count value to increase or decrease the amount of curves displayed.

步驟

按一下。
請選擇邊線，也就是填補的邊界。

建立選取項目 工具在選擇相關的邊線時是相當有用的。
選擇性地為每個所選邊線或曲線定義連續性 (您可以從小視角立方體功能表中選擇 [斑馬條紋] 來查看效果)：

位置 - 使邊線在沒有互為相切或曲率關係的狀況下交會
相切 - 在邊界與新曲面 (就像有參考曲面一樣) 間建立一個隱含的相切 (垂直於曲面的平面)。僅能在選取的草圖中作用，無法用於其他的平坦曲線上。選擇性使用，選取時系統會啟用「相鄰面」欄位。選取任何一個面，其基礎幾何須與至少一個輪廓零件的曲線重合 (面與邊線不需相交或是同一零件的一部分)。
曲率 - 與相鄰曲面的實際曲線相配。選擇性使用，選取時系統會啟用「相鄰面」欄位。選取任何一個面，其基礎幾何須與至少一個輪廓零件的曲線重合 (面與邊線不需相交或是同一零件的一部分)。
例如，已為下方選擇的最左側邊線選取了連續性選項。注意到在視覺顯示條紋間的不同：
位置：
相切：
曲率：

選擇會影響形狀的導引 (點、頂點、在草圖上的點或曲線)。所產生的曲面會與這些點相交，且點會落在邊界的內部。當選取了曲線時，曲面會穿出曲線，然後您可以從兩種計算類型中選擇：
1. 取樣 - 使用樣本大小來決定用來計算曲面的沿曲線頂點數量。較長的樣本大小可能會產生依循整個曲線的曲面：
  3 的取樣大小：
  
  10 的取樣大小：
取決於樣本的大小，曲面上可能會有波紋。
精準 - 使用明確的曲線來形成曲面。請注意，此選項需要非常小心地設計與選擇曲線。詳細資訊請參考下方的範例。
核取顯示 isocurves來評估其下曲面是如何被定義的。
會以網格呈現未經修剪的下方曲面以顯示 iso 參數式曲線，讓您能夠評估其下曲面的品質。
按一下。

範例

選取了曲面邊線與兩條橋接曲線來做為邊界，藉此建立一個新的曲面：

選取了曲面邊線與兩條橋接曲線來做為邊界，藉此建立一個新曲面的範例

導引頂點

選取「導引頂點」來進一步定義曲面的形狀：

導引頂點的範例

使用精準選項的導引

特別是當導引曲線使用 [精準] 選項時，如果曲線互相交會，相交必須是在一個點上，就像是曲線與點是互為相切的。同時當使用 [精準] 選項時，曲線必須碰觸邊界但不可超過邊界。

導引並未相交

導引並未相交的範例

導引相切交會

導引相切交會的範例

導引與邊界相接觸

導引與邊界相接觸的範例

導引未與邊界相接觸

當選取 [取樣] 時，這種狀況是可行的：

導引未與邊界相接觸的範例

但如果選擇了 [精準] 則不會成功。

導引在相切平面相交

導引在相切平面相交的範例

缺乏相切導致失敗

缺乏相切導致失敗的範例

導引符合相切準則

導引符合相切準則的範例

顯示 isocurves

已選取「顯示 isocurves」來顯示 iso 參數式曲線，讓您能夠評估其下曲面的品質：

已選取「顯示 iso 曲線」的範例

曲面建構工具集合組

This lists the collection of surface feature tools. This is not an exhaustive list. Additional Feature tools may be used when modeling surfaces. See Surfacing for additional information.

Thicken - Add depth to a surface. Create a new part or modify an existing one by giving thickness to a surface and converting it to a solid, adding or removing material from an existing part or surface, or intersecting parts in its path.
Enclose - Create a part by selecting all boundaries surrounding an empty space to form a solid. Use any set of surfaces and solids (including planes and faces) that intersect each other or connect at a boundary to create a volume. Create a new part or modify an existing one by adding, removing, or intersecting parts.
Fillet - Round sharp interior and exterior edges and define as a standard constant radius, more stylized conic, or variable by selecting Edge fillet. Optionally apply a Full round fillet to create a seamless blend of one or more faces between two opposing sides.
Face blend - Round sharp connected or disconnected interior and exterior faces to create a seamless blend between the faces or detach the blend to create new faces, defining a radius or constant width. Further define the blend cross section (rolling ball or swept profile), symmetry, control, trim, constraints, and limits.
Delete face - Remove geometry from a part. Select whether to heal the surrounding faces (by extending until they intersect), cap the void, or leave the void open. This Direct Editing tool is especially convenient if you don't have the parametric history of the part, as is often the case with an imported part.
Move face - Translate, rotate, or offset one or more selected faces. This Direct Editing tool is especially convenient if you don't have the parametric history of the part, as is often the case with an imported part.
Replace face - Trim a face or extend a face to a new surface. This Direct Editing tool is especially convenient if you don't have the parametric history of the part, as is often the case with an imported part.
偏移曲面 - 偏移一個現有面、曲面或草圖區域來建立新的曲面。將偏移距離設定為 0 來就地產生一個副本。
Boundary surface - Create or add a surface specified by its boundary profiles.
Fill - Create a surface (or a part from surfaces) by defining boundaries and refine the surface with boundary conditions (instead of requiring the use of reference surfaces).
移動邊界 - 移動曲面的邊界線以延伸或修剪曲面。
Ruled surface - Create a new or additional ruled surface from an existing edge or multiple edges of a sketch region.
Mutual trim - Trim two adjacent surfaces by extending intersections to complete the trim.
Constrained surface - Create a surface from a selection of points or mesh data within a specified tolerance. Display deviations and optimize for performance or smoothness.