偏移曲線

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

   

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。

     

     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。

     

     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。

   

   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。

     

   • 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。

     

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。

     

     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。

       

     • 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。

       

   • 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。

     

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

8. Click the Targets field and select one or more target faces in the graphics area to constrain the curve to those faces. If no faces are selected, this is the same as all faces being selected.

   

   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. 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：

  

• 偏移曲線可以在相同面上彼此交錯：

  

• 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：

  

In addition to the surfacing tools, curves are used to create the basic building blocks of surfaces.

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.