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草圖工作台(Sketcher Workbench)是一獨立模組，可用於繪製2D(平面)物件。但是，它通常與 零件設計工作台(PartDesign Workbench)結合使用。一個具有封閉輪廓外型的草圖通常用 來建立實體物件 .
1. 開啟FreeCAD, 使用檔案 → 開新檔案新增一空白文件.
- 按滑鼠右鍵，或在鍵盤上按一下 ，可在編輯模式下取消選擇目前啟用的工具。
- 離開草圖編輯模式，按一下複合檢視/任務上方的 按鈕，或按二次鍵盤的 按鍵。
- 要再次進入編輯模式，在樹狀檢視中該草圖名稱上點二下 ；或點選該草圖，再按一下 。
- 2.1. 選擇草圖平面，即XY，XZ或YZ基準面三選一。您亦可選擇相反方向的基準面，或是平行偏移於選定基準面一定距離的平面做為新基準面。
- 2.2. 將使用預設平面和選項。
- 2.3. 按下 開始建構該草圖。
- 3.1. 按下 ，進入建構線模式。
- 3.2. 按下 。
- 3.3. 在草圖中將滑鼠游標靠近原點，該點將高亮顯示並且在游標的右方將顯示 共點(重疊)拘束。
- 3.4. 點選一下該點(滑鼠左鍵)，然後移動游標準備建立一條新的直線。移動一下游標位置使線段長度大約
30 mm，再點一下(滑鼠左鍵)就會產生一新線段。在此步驟中的長度並不需要非常精確； 在後續步驟中將設定此線段的尺寸。
- 3.5. 重複步驟3.4，再繪製出四條大約呈星型的建構線(見下圖)。不需太在意他們的尺寸或位置，只需要將它們畫在四個像限。
- 3.6. 現在再按一下 切換建構線模式到一般模式。
註1: 此時3D view 中繼續點擊以繪製出更多的線段。如要離開 工具，按一下滑鼠右鍵或按一下鍵盤上的 鍵。By doing this the pointer won't create lines any more, it will just be a pointer allowing us to select the objects we just created. In this pointer mode we can pick and drag the endpoints of each line to adjust its placement.工具仍在作用中。這表示我們可以在
Note 2: do not press tree view.a second time as this will exit the sketch edit mode. If you do this, re-enter the edit mode by double clicking on the sketch in the
Take a look at the task panel again. The Solver messages section already indicates that the sketch is under-constrained, and it mentions the number of degrees of freedom.
Look at the Constraints and Elements sections to see the new listed constraints and lines. Once your sketches have many elements, it may be difficult to select them in the 3D view, so you can use these lists to select the object that you wish exactly.
Real geometry must make a closed shape if it is to be used as a profile that can be extruded by tools such as.
Make sure you are not in construction mode by clicking on, if you have not previously exited this mode.
4. Create a circle.
- 4.1. Click on .
- 4.2. Click on the origin of the sketch to position its center point.
- 4.3. Click anywhere in the 3D view to set the circumference radius as a distance from the origin. Make it approximately
8 mm. Again the dimension will be fixed later.
5. Create a series of arcs.
- 5.1. Click on .
- 5.2. Approach the endpoint of one of the construction lines, and click on it. This will set the center point of the circular arc to be coincident with this line's endpoint.
- 5.3. Click once in the 3D view at an arbitrary location to set simultaneously the radius of the arc, and the first endpoint of it. Define an approximate radius of
- 5.4. Move the pointer in an anti-clockwise direction to trace an arc that has its concavity pointing towards the origin of the sketch. Click to set the final endpoint of the arc, defining a circular arc that approximately sweeps
180°or half a circle.
- 5.5. Repeat these steps with each construction line, so that each of them has a circular arc at its tip. We will call these O-arcs for outwards-arcs.
Circular arcs added at the endpoints of the construction lines. Also a central circle.
6. Create an arc between each pair of the previous O-arcs.
- 6.1. Still with the tool active, click somewhere between two O-arcs but further away from the origin of the sketch, to set the center point of a new arc.
- 6.2. Click somewhere close to the endpoint of one O-arc, and move the pointer to sweep another arc finishing close to another endpoint of a different O-arc, as if you were trying to join the endpoints. This time the concavity must point away from the origin.
- 6.3. Repeat these steps, so that each pair of O-arcs has a new arc between them. We will call these I-arcs for inwards-arcs.
To summarize, the O-arcs should have their curvature pointing outwards, and their concavity pointing towards the origin of the sketch; the I-arcs should have their curvature pointing inwards, and their concavity pointing away from the same origin.
Circular arcs added between the first set of arcs placed.
Take a look at the task panel again. Due to the new geometrical elements that we have drawn, the Solver messages section indicates even more degrees of freedom. A degree of freedom (DOF) indicates a possible movement of one element. For example, a point can be moved both in horizontal and vertical directions, so it has two degrees of freedom. A line is defined by two points, therefore in total it has four degrees of freedom. If we fix one of those points, then the entire system has only two degrees of freedom available; if we additionally fix the horizontal movement of the remaining point, we only have one degree of freedom left; and if we also fix the vertical movement of this point, then the last degree of freedom disappears, and the line cannot move from its position any more.
Up to now when we have drawn lines and curves, the sketcher has added automatic constraints for us, those that keep the lines tied to the origin, and the O-arcs tied to the construction lines. But we haven't added other explicit constraints so the geometrical shapes can still be moved in many directions. Constraints are "rules" that tell us under which conditions a geometrical object can move and by how much. They are used to eliminate the degrees of freedom so that the sketch has a stable shape. If we eliminate all degrees of freedom, then the sketch is fully constrained, and has a fixed shape, that is, its points cannot move at all. In general, it is a good idea to fully constrain sketches because this will result in stable models.
There are two principal types of constraints:
- Geometric constraints define characteristics of the shapes without specifying exact dimensions, for example, horizontality, verticality, parallelism, perpendicularity, and tangency.
- Datum constraints define characteristics of the shapes by specifying dimensions, for example, a numeric length or an angle.
Equal length and radius
7. Geometrically constrain the lines and arcs.
- 7.1 Select all five construction lines. You only need to click once to select an element.
- 7.2. Press .
- Note: this creates only four constraints. The constraints are chained, the first line has the same length as the second one, which has the same length as the third one, which again has the same length as the fourth one, which has the same length as the fifth one. So in this case, the first and the fifth have the same length.
- 7.3. Select all five O-arcs, those centered on an endpoint of a construction line.
- 7.4. Press .
- 7.5. Repeat with all I-arcs, those between the O-arcs.
- Note: again the constraints are chained. Therefore all O-arcs will have the same radius, and all I-arcs will have the same radius. At this moment, the specific value of these lengths is not fixed. You may use the pointer to drag a point and see how the sketch is updated while respecting the constraints in place.
- 7.6. Select the construction line that is closest to the vertical axis.
- 7.7. Press Point on object constraint was already placed, keeping the construction line vertical. In this case, no additional Vertical constraint is necessary. (optional). If you drew the construction line downwards over the Y axis, an automatic
Note: as you add constraints, overlay symbols indicating the type of constraint appear over the geometry in the 3D view. If these symbols obfuscate your view, you can hide them by unchecking the constraint in the task panel. Also note that the number of degrees of freedom decreases after adding each constraint.
Note 2: if you wish to temporarily disable the constraint, you may select it and press. When you want to apply it again, press again the same button.
Sketch with equality constraints applied to the construction lines, and to the two sets of arcs.
8. Apply tangency to the arcs.
- 8.1. Select one endpoint of an O-arc and then the closest endpoint of the adjacent I-arc.
- 8.2. Press . This makes the two adjacent arcs connect smoothly at their endpoints.
- 8.3. Repeat for all endpoints of the O-arcs and I-arcs to obtain a closed profile.
Note: applying the tangential constraint very often will move the geometry around in order to produce a smooth connection. You may have to use the pointer to reposition the points a bit before applying the next tangential constraint. Try placing the endpoints in such a way that two arcs aren't too far apart, so they can be connected with a short line rather than a long line.
As of this step, we have now created a closed profile, as all arcs have been tied together. Now we can provide datum constraints to fix the shape of the sketch. While the dimensions of lines and arcs remain unfixed, we can drag the points of the sketch and observe how the entire sketch changes.
Sketch with tangential constraints applied to the arcs, which closes the shape.
These constraints specify the numerical distances between two points, and angles between two lines.
Distances and angles
9. Adjust the size of the construction lines.
- 9.1. Select the vertically constrained construction line.
- 9.2. Press .
- 9.3. Set the length to
30 mm. Because all construction lines are constrained to have the same length, all these lines adjust their sizes at the same time.
10. Adjust the angle between the construction lines.
- 10.1. Select the vertical construction line and the construction line closest to it.
- 10.2. Press .
- 10.3. Set the angle to
- 10.4. Repeat the same procedure for each pair of construction lines, and use the same angle.
- Note: at this stage, the sketch may have very few degrees of freedom left, meaning that its shape cannot be changed too much. If you attempt to add more constraints, these may cause a conflict with the previously added constraints. If this is the case, do not add these constraints, and proceed with the next steps.
Sketch with length constraint applied to one vertical construction line (left), and angle constraints to three pairs of construction lines (right).
11. Adjust the size of the arcs.
- 11.1. Select one of the O-arcs, centered on the endpoint of a construction line.
- 11.2. Press .
- 11.3. Set the radius to
8 mm. Because all O-arcs are constrained to have the same radius, all these arcs adjust their sizes at the same time.
- 11.4. Select one of the I-arcs, between two O-arcs.
- 11.5. Press .
- 11.6. Set the radius to
11 mm. Because all I-arcs are constrained to have the same radius, all these arcs adjust their sizes at the same time.
Sketch with radius constraints applied to the outwards arcs (left), and inwards arcs (right).
- 11.7. Finally, select the circle in the center of the sketch, press
8 mm. , and set the value to
We should end up with a fully constrained sketch. It can be confirmed by noticing the change in color of the real geometry, and by the message that is shown in the task panel.
Sketch with all geometrical and datum constraints applied.
12. Now that we have a fully constrained sketch, it can be used to create a solid body.
- 12.1. Exit the sketch edit mode by pressing the tree view and the 3D view. button, or pressing twice. The sketch should appear in the
- 12.2. Switch to the PartDesign Workbench.
- 12.3. With the sketch selected in the tree view, press , choose the default XY-plane, and press . The sketch should appear now inside the Body.
- 12.4. Select the sketch, and then press , choose the default options, and press to create a solid extrusion.
Left: fully constrained sketch with only the most important constraints showing. Right: solid extrusion produced with PartDesign Pad.
Constraining a sketch can be done in many different ways. In general, it is recommended to use geometrical constraints first, and minimize the number of datum constraints, as this simplifies the task of the internal constraint solver. To investigate this, repeat this example, now adding the constraints in different order.
- First constrain the construction lines before drawing the arcs.
- Or constrain the size of the arcs before making them tangent.
- Or set the angle of the construction lines before adding more elements.
- Try using other construction geometry.