藉由在周圍面上偏移邊線來建立與延伸和/或分割新的曲線。

Offset curve creates a new curve by offsetting the edges of surrounding faces, allowing you to create and control a profile without additional sketches or features. In this example, offset the outer edges of the top face, then split. Use other surfacing tools to raise an area for manufacturing to apply a texture.

Since the offset and split reference depend on the clip, any changes to the clip profile automatically update the split profile as well. Click Offset curve from the feature toolbar, then select one or more edges to offset in the graphics area. Select multiple edges to create a single chained curve or multiple disjointed curves.

Separate curves can overlap within the same face without error, but edges that branch within the same feature cannot be selected. Enter an offset Distance and Offset type. Geodesic calculates the offset using geodesic distance in the 2-dimensional space of the target faces. Euclidean calculates the offset using Euclidean distance in the 3-dimensional space. If required, flip the offset curve to the opposite side of the selected edge.

Select a Gap fill from the dropdown. Linear fills the gap with a linear edge. Round fills the gap with a rounded edge tangent to the two curves on either side of the gap fill. Select an offset Scope from the dropdown. Choose Offset and extend to extend both curve ends to the edges of the face.

Check Trim to control the start and end points of the curve. Enter a value or use the arrow manipulators. Equal trim trims the curve equally on both the start and end of the trim. With Equal trim selected, one manipulator adjusts both ends. When accepted, both offset options do not split any faces.

Offset, extend and split extends both ends of the curve to the edges of the face and splits the face at the offset. It does not create a separate curve. Click the Targets field and select one or more target faces in the graphics area to constrain the curve to those faces. When accepted, the offset only appears on those faces. Selecting no faces is the same as selecting all faces in the model.

Check Approximate to simplify a complex curve. Onshape rebuilds the curve to a new mathematical specification. Set the parameters to control how Onshape simplifies the curve. Set the Target degree, Maximum number of control points, and Tolerance. Check Keep start derivative and Keep end derivative to preserve the curve’s tangency at both ends of the curve. Check Show deviation to view the maximum deviation between the original and reapproximated curves. The Approximate option displays the original curve in yellow and the new approximated curve in magenta.

  1. Select the Offset curve icon () on the Feature toolbar.

    「偏移曲線」對話方塊

  2. 在圖形區域中選擇一或多條要偏移的曲線。
  3. 輸入從原始邊線的偏移距離數值。

  4. 從下拉清單中選擇「偏移類型」：

    • 測地線 - 使用測地線距離計算偏移。系統會在目標面的 2D 空間計算距離。

      「測地線」偏移類型

      黃色是選取的邊線，紫紅色則是偏移的邊線 (左圖)。測量顯示從邊線到偏移曲線如何計算測地線距離 (右圖)。

    • 歐幾里德 - 使用歐幾里德距離計算偏移。系統會在 3D 空間中計算距離。

      「歐幾里德」偏移類型

      黃色是選取的邊線，紫紅色則是偏移的邊線 (左圖)。測量顯示從邊線到偏移曲線如何計算歐幾里德距離 (右圖)。

  5. 選擇性地按一下「反轉」箭頭來將偏移曲線反轉到所選邊線的另一邊。

    反轉偏移曲線

    預設 (左圖) 與反轉的偏移曲線 (右圖)

  6. 從下拉清單中選擇「間距填補」：

    • 線性 - 使用線性邊填補間距。

      使用線性間距填補的偏移曲線

    • 圓形 - 使用與間距填補邊上兩條曲線相切的圓形邊來填補間距。

      使用「圓形」間距填補的偏移曲線

  7. 從下拉清單中選擇下列的「範圍」選項之一：

    • 偏移 - 將曲線從邊線偏移。

    • 偏移和延伸 - 將曲線兩端延伸至面的邊上。

      偏移曲線分別設定為無與延伸

      處理之後：無 (左圖) 與延伸 (右圖)

      • 如果選取了「偏移和延伸」，系統會提供「修剪」控制項。核取「修剪」並輸入「開始修剪」與「結束修剪」的數值，或使用開始與結束修剪箭頭操控器來在圖形區域中視覺放置修剪的開始與結束。

        有開始與結束修剪值的偏移曲線

      • 核取「同等修剪」來在修剪的開始與結束邊上同等地修剪。在選取了「同等修剪」的情況下，一個操控器會同時調整開始與結束的相同修剪。

        使用「同等修剪」的偏移曲線

    • 偏移、延伸和分割 - 偏移並將曲線兩端延伸至面的邊上，同時分割面以建立新的面。使用這個選項時，不會建立新的曲線。

      偏移曲線延伸與壓印，以及僅延伸

      選項：「偏移、延伸和分割」(左圖) 與「偏移和延伸」(右圖；顯示曲線)

  8. 按一下「目標」欄位，然後在圖形區域中選擇一或多個目標面來將曲線限制在這些面上。如果沒有選擇任何面，效果是與選擇所有的面一樣的。

    偏移曲線「目標」的範例

    設定目標為最上方面 (左圖)、中間面 (中間圖) 與不設定目標 (右圖)。

  9. Complex curves can be reapproximated to create simpler curves. Check Approximate to open options to reapproximate the curve. The original curve is displayed in orange, and the new approximated curve is displayed in magenta.

    • Target degree - Enter the target curve degree for the selected curve.
    • Maximum control points - Enter the maximum number of control points allowed for the selected curve.
    • Tolerance - Tolerance of the selected curve, as a length measurement. Enter the tolerance value.
    • Keep start derivative - Check to keep tangency at the beginning of the selected curve.
    • Keep end derivative - Check to keep tangency at the ending of the selected curve.
    • Show deviation - Check to view the maximum deviation between the original curve and the reapproximated curve.

    Options to reapproximate complex curves

  10. 按一下核取記號來接受新的偏移曲線。

  • 可以選擇多條邊線來建立連續的曲線：

    選擇多條邊線來建立連續的偏移曲線

  • 偏移曲線可以在相同面上彼此交錯：

    在相同面上交錯的多條偏移曲線

  • 選擇分支的邊線會產生錯誤。系統無法用這些分支的邊線建立偏移曲線：

    偏移曲線分支錯誤

除了曲面建構工具之外，還可使用曲線來建立曲面的基本建構塊。

This lists the collection of curve feature tools. This is not an exhaustive list. Additional Feature tools may be used when manipulating curves.

  • Sketch tools - Tools in the Sketch toolbar such as Line, Corner rectangle, Center point rectangle, Center point circle, 3 point circle, Tangent arc, 3 point arc, Spline, Point, and Construction used to create a sketch in a Part Studio.
  • Helix - Create a helix using a conical or cylindrical face, single axis or z-axis of a mate connector, or circular edge.
  • 3D fit spline - Create a 3D fit spline through a series of vertices. Creates a curve which is listed in the Parts list under Curves.
  • Projected curve - Create a curve from the projection of two sketches (Two sketches option) or from the projection of a curve on a face (Curve to face option).
  • Bridging curve - Create a Curve connecting any two points, vertices, or Mate connectors. The resulting Curve is listed in the Feature list and the Parts list.
  • Composite curve - Represent multiple edges as one Curve. Select multiple adjacent edges, sketch entities, and other curves. Selecting non-contiguous edges may result in multiple Curves created. Selections for each Curve must meet at their vertices. (Curves are listed in the Parts > Curves list.)
  • Intersection curve - Create a curve at the intersection of two or more surfaces or faces. The selections must intersect.
  • Trim curve - Trim or extend a curve by a distance or to a bounding entity.
  • Isocline - Create an isocline on a sloped face. An isocline runs on a face at positions where the face has a certain slope compared to its reference definition. The resulting isocline is listed in the Feature list and Parts list.
  • Offset curve - Create and extend and/or split a new curve by offsetting edges on surrounding faces.
  • Isoparametric curve - Create smooth curves that run along a face or surface in the U or V direction.
  • Edit curve - Edit an existing curve by selecting sketch entities or curves to apply a simplified approximation, elevate the degree, reposition control curve vertices and/or planarize into any 2D plane.
  • Routing curve - Create a multi-point curve across one or more planes in 3D space (routed path). This is useful for creating pipe routing, wiring, and NURBS curves for advanced surfacing.

iOS 與 Android 對偏移曲線特徵的支援僅限於顯示與編輯現有的曲線。僅能在桌面版 (瀏覽器) 平台上建立偏移曲線。無法在 iOS 或 Android 平台上建立偏移曲線。