Basic Part Design Tutorial/pl

Ten poradnik zapozna nowego użytkownika z niektórymi narzędziami i technikami dostępnymi w Środowisku pracy Part Design. Ten poradnik nie jest kompletnym i wyczerpującym przewodnikiem po Środowisku PartDesign, a wiele narzędzi i możliwości nie zostało omówionych. Ten poradnik pozwoli użytkownikowi wykonać kroki niezbędne do modelowania części pokazanej na rysunku poniżej za pomocą szkiców.

Nim zaczniesz
Zdjęcia przedstawione w tym poradniku zostały wykonawane w programie FreeCAD z włączoną funkcją auto dopracowania, która usuwa dodatkowe niepotrzebne linie na powierzchniach czołowych. To ustawienie jest potencjalnie niebezpieczne, nie powinno być używane przez nowych użytkowników i może uszkodzić Twoje modele. Najlepszą radą jest, aby nie zmieniać tych ustawień z domyślnych wyłączonych.

Zadanie
W tym poradniku, za pomocą stanowiska roboczego Part Design utworzysz trójwymiarowy model bryłowy części pokazanej w Rysunek poniżej. Podane są wszystkie wymiary niezbędne do wykonania tego zadania. Rozpoczniesz od stworzenia kształtu rdzenia z bazowego szkicu, a następnie zbudujesz go na tym kształcie, dodając coś, co jest znane jako Cechy. Cechy te albo dodadzą materiał do bryły, albo usuną materiał z bryły za pomocą dodatkowych szkiców i towarzyszących im operacji na cechach. Przewodnik ten nie będzie wykorzystywał wszystkich funkcji i narzędzi dostępnych w środowisku Part Design, ale powinien wykorzystywać je na tyle, aby dać użytkownikowi tego przewodnika solidne podstawy, na których będzie mógł budować swoją wiedzę i umiejętności.

Część główna z wyciągnięciem
Zacznij od upewnienia się, że jesteś w obszarze stanowiska pracy Part Design. Gdy już tam będziesz, będzie trzeba stworzyć nowy dokument, jeśli jeszcze tego nie zrobiłeś. Dobrym zwyczajem jest częste zapisywanie pracy, więc zanim cokolwiek innego zapisze nowy dokument, nadaj mu dowolną nazwę. Teraz, gdy jest zapisany, zaczniemy od podstawowego szkicu. Aby rozpocząć ten szkic, kliknij na ikonę nowego szkicu na pasku narzędzi lub z menu Part Design, Nowy szkic. Po wywołaniu powinno wyświetlić się okno dialogowe z prośbą o wybranie orientacji szkicu i podanie przesunięcia. Nie będziemy używać przesunięcia, ale dla naszego szkicu podstawowego chcemy wybrać płaszczyznę YZ, jak pokazano na rysunku poniżej. Po wybraniu płaszczyzny YZ klikamy przycisk i możemy przystąpić do konstruowania pierwszego szkicu. Następnie należy użyć narzędzi a Polyline i wykonać kształt mniej więcej taki jak na następnym obrazku. Nie musi być on idealny, ponieważ kształt końcowy jest wykonywany z użyciem wiązań. Kiedy już będziesz miał podstawowy kształt, zaczniemy wprowadzać wiązania. Jeśli miałeś włączoną opcję Automatyczne wiązania, niektóre z tych wiązań zostaną zastosowane natychmiast, jeśli nie, wykonaj następujące czynności.


 * 1) Select the two horizontal lines with your mouse by clicking on them, and once selected, click on the Constraint Horizontal.png horizontal constraint.
 * 2) Select the vertical line on the right and then click on the Constraint Vertical.pngcal constraint.
 * 3) Select the start and end points of your polyline and click on the Constraint PointOnPoint.png coincident constraint to close the polyline.
 * 4) Select the bottom horizontal line and the right vertical line and apply and Constraint EqualLength.png equal constraint.
 * 5) Select either the horizontal or vertical line and apply either a corresponding Constraint HorizontalDistance.png horizontal or Constraint VerticalDistance.png vertical distance constraint and give it a value of 26 mm.
 * 6) Select the top horizontal line and apply the horizontal distance constraint and give it a value of 5 mm
 * 7) Select the lower left point, (vertice) of the horizontal line and the upper right point of the vertical line, then select the center point of the grid and apply the Constraint Symmetric.png symmetry constraint.

At this point you should have a fully constrained sketch as indicated by it changing color and the message shown in the Combo View. It should now look just like the image below. Now in the Combo View, click on the Close button to leave the sketch edit mode and select Pad from the toolbar or from the Part Design menu. This will give you a Pad dialog in the Combo View. Using that dialog, first using the Type pulldown menu, select Two dimensions. Drawing presented at the beginning of this tutorial says the part is 53 mm long. We do it by Padding our sketch both ways from the center plane to make up that distance i.e. make the pad symmetric in relation of sketch-plane. The reason for is seen later when creating features. For now, given we want it to be 53 mm long in total we will input 26.5 for Length, and 26.5 again for the Second length. Alternatively, you can provide a single length of 53 mm and click the Symmetric to plane check box. Once that is done we now have our base solid upon which we will add additional features to construct our part.

A video of the steps used in this portion of the tutorial is here: https://www.youtube.com/watch?v=UacO5Pa4gIM

Features with pocket and external geometry
Using the mouse or the view icons turn the model around so you can see its back. Once the back of the part is visible, select the back face by clicking on it as seen in the next image. After the face is selected, click on the New sketch icon in the toolbar or from the Part Design menu and that will map our next sketch to the back face of the part. Now select rectangle tool and place a rectangle on the rear face of the part in a similar fashion as shown below. Now following the steps listed, constrain the sketch.

Once that is done, click the Close button at the top of the Tasks tab in the Combo View window, then select Pocket tool from the toolbar or Part Design menu. Using this tool is the opposite of the Pad tool. As the Pad tool adds material to the part, the Pocket tool removes material from the part. Both operations are called features. In this Pocket operation we want to select Through all from the type pulldown-menu and then click the OK button.
 * 1) Select one of the horizontal lines apply a horizontal distance constraint and a value of 5 mm.
 * 2) Select one of the vertical lines and give it a vertical distance constraint and a value of 11 mm.
 * 3) Use Sketcher_External.png External geometry tool and select the upper right vertex of the face and click it so you are provided a point from the external geometry to link our sketch to. [[Image:PD_WB_Tutorial004.png|center]]
 * 4) Right click to end the External geometry mode
 * 5) Select that point you just made available with the External geometry tool and then select the upper right vertex of the rectangle and click on the coincident constraint. At this point the sketch should be fully constrained and look like the next image.

For the next operation, make sure that “Pocket” is selected in the Model tree view and once done, click on the Mirror feature on the toolbar or from the Part Design menu. In the Mirror dialog in the Combo View, select Horizontal sketch axis from the Plane pulldown menu. Then click OK. The Mirror feature works in this way because the base feature of our model was Padded both ways from the horizontal plane in the first operation with the base sketch. If all has gone well, you should now have a part that looks like the image below after you orbit it around to the front.

A video of the steps used in this portion of the tutorial is here: https://www.youtube.com/watch?v=nnVQDjUpS3o

Features with pad and external geometry
After taking a look, orbit back around and once again select the back face of the part and select that face to map the next sketch to. Select New sketch and make a new rectangle in the manner similar to what is shown below in the next image. Then proceed to add dimensional constraints to the rectangle.

Now selecting the upper left vertex of the rectangle and the external geometry point, click on the coincident constraint to fully constrain the sketch. Next we will click on the Pad feature and in the Pad dialog in the Combo View we want a length of 26 mm leaving the type as Dimension and then placing a check on the Reversed checkbox. Using the Reversed checkbox will cause the Pad to go into the part instead of away from the part. This operation provides with the following result. Once again use the Mirror feature to get the second pad. First ensure that created Pad is selected in the tree view, then click on Mirror in the toolbar of select it from the Part Design menu. We will repeat the operation we did for Pocket above and select Horizontal sketch axis from the Plane pulldown menu.
 * 1) Select a horizontal line and apply a horizontal distance constraint with a value of 16.7.
 * 2) Select a vertical line and apply a vertical distance constraint of 7 mm
 * 3) Using the External geometry tool, select the upper left vertex of the part face.

A video of the steps used in this portion of the tutorial is here: https://www.youtube.com/watch?v=DZOF21fNVDs

Feature with pocket and external geometry
At this point orbiting the part around to the front, we can see that our part is now starting to look like the part in the dimensioned drawing at the beginning of this tutorial. Once you have the view of the front, click on the sloped face with your mouse to select the face we will use for the next sketch. Here we will use the rectangle tool and place a rectangle in our sketch and once having done so, apply the following constraints.

Now using the dimensions from the drawing, apply the following constraints.
 * 1) Select a horizontal line and a vertical line, and after both are selected, click on the Equals constraint.
 * 2) Select either a horizontal or vertical line and apply a corresponding horizontal or vertical distance constraint with a value of 17 mm
 * 3) Using the External geometry tool, select the top right vertex as shown in the image below.


 * 1) Select the external geometry point and the upper right vertex of the now square sketch and apply a horizontal distance constraint of 7 mm
 * 2) Select the external geometry point and the upper right vertex of the now square sketch and apply a vertical distance constraint of 11 mm

The result should be as follows. At this point if we were to simply Pocket this sketch, the resulting hole would be perpendicular to the sloped face that it is mapped to, and this is not what we want. We want the hole to be perpendicular to the back face, but it's projected dimensions are not the 17 mm x 17 mm dimensions that are given in the drawing. Now we could do the math and calculate the dimensions needed, or we can use the tools provided in FreeCAD to make that projection for us. To do that, we are going to create a small Pad feature from the sketch we just made as a helper. We will use the External geometry tool to project the points of the base of that helper Pad on to the back face where we will place our final sketch that will pocket the hole through to finish the model.

So first, after clicking Close to exit the Sketch edit dialog, select Pad and provide a distance of 1 mm. Click OK and you should see the following result.

A video of the steps used in this portion of the tutorial is here: https://www.youtube.com/watch?v=a0hsJtbFW4Y

Next we will orbit back around to see the back face of the part once again and select the back face to map the final sketch to. Select New sketch from the toolbar or Part Design menu. Now in sketch edit mode, we will orbit back around to the front so we can see two perpendicular edges of the Pad we made in the last operation. Using the External geometry tool, select the connected horizontal and vertical edges at the base of the Pad with the External geometry tool. The image below shows the base edges to be selected with the External geometry tool. Now orbiting around to the back face, or alternatively double clicking on the active sketch in the Model tree view, you will see the two external geometry lines that we provided from the front of the model. Make a rectangle and using the coincident constraint, do the following.


 * 1) Select the upper left vertex of the rectangle and the upper left point of the external geometry and click on the coincident constraint.
 * 2) Click on the lower right vertex of the rectangle and the lower right point of the external geometry and click on the coincident constraint.

And we should end up with this. For the final step in this tutorial, we will select the Pocket feature from the toolbar or from the Part Design menu and from the Type pulldown select Through all and click toe OK button. A video of these steps of the tutorial is here: https://www.youtube.com/watch?v=dlQV9OkXWOI

Your model will have some extra lines on it compared to the images in this tutorial. To remove these extra lines, change to the OpenSCAD workbench, select Pocket001 (in v0.17 and later select Body) from the hierarchy tree, and click the Refine Shape tool:. This creates a refined version of the model that is parametrically linked to Pocket001 and so is also linked to the entire history of the model. If we change, for example, the numerical value of a distance constraint the Refined Shape will update. In contrast, the Part WorkBench also has a Refine Shape tool in the pulldown menu, and it creates a Refined Shape that is more like a snapshot of the model as it existed when the Refine Shape tool was used. If we change (for example again) the numerical value of a distance constraint, Refine Shape created from the Part Workbench remains the same and does not update.

This tutorial and your model are complete.

Additional Resources

 * Links to accompanying video have been included.
 * FreeCAD file for comparison (made with 0.16.6706) Download