Manual:Traditional modeling, the CSG way/ro

CSG înseamnă Constructive Solid Geometry Constructive Solid Geometryși descrie maniera cea mai simplă de a lucra cu geometria 3D solidă, care creează obiecte complexe prin adăugarea/eliminarea unor elemente de volum prin utilizarea operațiilor booleene cum ar fi unirea, scăderea sau intersecția solidelor.

FreeCAD poate gestiona multe tipuri de geometrie, dar tipul preferat și mai util de obiecte 3D pe care dorim să-l proiectăm cu FreeCAD, adică obiecte din lumea reală, este fără îndoială, solid,BREP geometry, geometria BREP, care în mod principal sprijinită de către atelierul Part  Part Workbench. Contrar la plasele cu ochiuri poligonale polygon meshes, care sunt realizate numai din puncte și triunghiuri, obiectele BREP(B-Rep de la Boundary Representation) au fațetele lor definite de curbe matematice, care permit o precizie absolută, indiferent de scală.



Diferența dintre cele două poate fi comparată cu diferența dintre imaginile bitmap și vectori. Ca și în cazul imaginilor bitmap, rețelele poligonale au suprafețele lor curbate împărțite într-o serie de puncte. Dacă o priviți îndeaproape, nu va fi o suprafață curbată, ci o suprafață fațetată. În ambele imagini vectoriale datele B-REP, poziția oricărui punct de pe o curbă nu este stocată în geometrie, ci calculată din voleu, cu precizie exactă.

În FreeCAD, toate geometriile bazate pe BREP sunt tratate de o altă piesă de software open source OpenCasCade, OpenCasCade. Interfața principală dintre FreeCAD și kernelul OpenCasCade este Atelierul(Workbench). Majoritatea atelierelor de lucru își construiesc funcționalitatea pe atelierul Part.

Deși alte benzi de lucru oferă adesea instrumente mai avansate pentru a construi și manipula geometria, deoarece acestea manipulează obiecte Part, este foarte util să știm cum funcționează aceste obiecte intern și să poată folosi instrumentele Part deoarece, fiind mai simple, pot foarte des să vă ajute să ocoliți problemele instrumentelor mai inteligente care nu reușesc a rezolva corect aceleași probleme.

Pentru a ilustra lucrul Atelierului, vom folosi acest model, folosind doar operațiunile CSG (cu excepția șuruburilor, pentru care vom folosi unul dintre addon-uri și cotele/dimensiunile pe care se vor vedea în următorul capitol):



Let's create a new document (Ctrl+N or menu File -> New Document), switch to the Part Workbench, and begin with the first foot:


 * Press the [[Image:Part_Box.png|16px]] Cube button
 * Select the Cube, then set the following properties (in the Data tab):
 * Length: 80mm (or 8cm, or 0.8m, FreeCAD works in any unit)
 * Width: 80mm
 * Height: 75cm
 * Duplicate the Cube by pressing Ctrl+C then Ctrl+V (or menu Edit -> Copy and Paste)
 * Select the new object named Cube001 that has been created
 * Change its position by editing its Placement property:
 * Position x: 8mm
 * Position y: 8mm

You should obtain two high cubes, one 8mm apart from the other:




 * Now we can subtract one from the other: Select the first one, that is, the one that will stay, then, with the CTRL key pressed, select the other one, that will be subtracted (the order is important) and press the [[Image:Part_Cut.png|16px]] Cut button:



Observe that the newly created object, called "Cut", still contains the two cubes we used as operands. In fact, the two cubes are still there in the document, they have merely been hidden and grouped under the Cut object in the tree view. You can still select them by expanding the arrow next to the Cut object, and, if you wish, turn them visible again by right-clicking them or change any of their properties.


 * Now let's create the three other feet by duplicating our base cube 6 other times. Since it is still copied, you can simply paste (Ctrl+V) 6 times. Change their position as follows:
 * Cube002: x: 0, y: 80cm
 * Cube003: x: 8mm, y: 79.2cm
 * Cube004: x: 120cm, y: 0
 * Cube005: x: 119.2cm, y: 8mm
 * Cube006: x: 120cm, y: 80cm
 * Cube007: x: 119.2cm, y: 79.2cm


 * Now let's do the three other cuts, selecting first the "host" cube then the cube to be cut off. We now have four Cut objects:



You might have been thinking that, instead of duplicating the base cube six times, we could have duplicated the complete foot three times. This is totally true, as always in FreeCAD, there are many ways to achieve a same result. This is a precious thing to remember, because, as we will advance into more complex objects, some operations might not give the correct result and we often need to try other ways.


 * We will now make holes for the screws, using the same Cut method. Since we need 8 holes, two in each foot, we could make 8 objects to be subtracted. Instead, let's explore other ways and make 4 tubes, that will be reused by two of the feet. So let's create four tubes by using the [[Image:Part_Cylinder.png|16px]] Cylinder tool. You can again, make only one and duplicate it afterwards. Give all cylinders a radius of 6mm. This time, we will need to rotate them, which is also done via the Placement property under the Data tab (Note: change the Axis property before setting the Angle, or the rotation will not be applied):
 * Cylinder: height: 130cm, angle: 90°, axis: x:0,y:1, position: x:-10mm, y:40mm, z:72cm
 * Cylinder001: height: 130cm, angle: 90°, axis: x:0,y:1, position: x:-10mm, y:84cm, z:72cm
 * Cylinder002: height: 90cm, angle: 90°, axis: x:-1,y:0, position: x:40mm, y:-10mm, z:70cm
 * Cylinder003: height: 90cm, angle: 90°, axis: x:-1,y:0, position: x:124cm, y:-10mm, z:70cm



You will notice that the cylinders are a bit longer than needed. This is because, as in all solid-based 3D applications, boolean operations in FreeCAD are sometimes oversensitive to face-on-face situations and might fail. By doing this, we put ourselves on the safe side.


 * Now let's do the subtractions. Select the first foot, then, with CTRL pressed, select one of the tubes that crosses it, press the Cut button. The hole will be done, and the tube hidden. Find it in the tree view by expanding the pierced foot.
 * Select another foot pierced by this hidden tube, then repeat the operation, this time Ctrl+ selecting the tube in the tree view, as it is hidden in the 3D view (you can also make it visible again and select it in the 3D view). Repeat this for the other feet until each of them has its two holes:



As you can see, each foot has become a quite long series of operations. All this stays parametric, and you can go change any parameter of any of the older operations anytime. In FreeCAD, we often refer to this pile as "modeling history", since it in fact carries all the history of the operations you did.

Another particularity of FreeCAD is that the concept of 3D object and the concept of 3D operation tend to blend into one same thing. The Cut is at the same time an operation, and the 3D object resulting from this operation. In FreeCAD this is called a "feature", rather than object or operation.


 * Now let's do the tabletop, it will be a simple block of wood, let's do it with another Box with length: 126cm, width: 86cm, height: 8cm, position: x: 10mm, y: 10mm, z, 67cm. In the View tab, you can give it a nice brownish, wood-like color by changing its Shape Color property:



Notice that, although the legs are 8mm thick, we placed it 10mm away, leaving 2mm between them. This is not necessary, of course, it won't happen with the real table, but it is a common thing to do in that kind of "assembled" models, it helps people who look at the model to understand that these are independent parts, that will need to be attached together manually later.

Now that our five pieces are complete, it is a good time to give them more proper names than "Cut015". By right-clicking the objects in the tree view (or pressing F2), you can rename them to something more meaningful to yourself or to another person who would open your file later. It is often said that simply giving proper names to your objects is much more important than the way you model them.


 * We will now place some screws. There is nowadays an extremely useful addon developed by a member of the FreeCAD community, that you can find on the FreeCAD addons repository, called Fasteners, that makes the insertion of screws very easy. Installing additional workbenches is easy and described on the addons pages.
 * Once you have installed the Fasteners Workbench and restarted FreeCAD, it will appear in the workbenches list, and we can switch to it. Adding a screw to one of our holes is done by first selecting the circular edge of our hole:




 * Then we can press one of the screw buttons of the Fasteners Workbench, for example the EN 1665 Hexagon bolt with flanges, heavy series. The screw will be placed and aligned with our hole, and the diameter will automatically be selected to match the size of our hole. Sometimes the screw will be placed inverted, which we can correct by flipping its invert property. We can also set its offset to 2mm, to follow the same rule we used between the tabletop and the feet:




 * Repeat this for all the holes, and our table is complete!

The internal structure of Part objects

As we saw above, it is possible in FreeCAD to select not only whole objects, but parts of them, such as the circular border of our screw hole. This is a good time to have a quick look at how Part objects are constructed internally. Every workbench that produces Part geometry will be based on these:


 * Vertices: These are points (usually endpoints) on which all the rest is built. For example, a line has two vertices.
 * Edges: the edges are linear geometry like lines, arcs, ellipses or NURBS curves. They usually have two vertices, but some special cases have only one (a closed circle for example).
 * Wires: A wire is a sequence of edges connected by their endpoints. It can contain edges of any type, and it can be closed or not.
 * Faces: Faces can be planar or curved, and can be formed by one closed wire, which forms the border of the face, or more than one, in case the face has holes.
 * Shells: Shells are simply a group of faces connected by their edges. It can be open or closed.
 * Solids: When a shell is tightly closed, that is, it has no "leak", it becomes a solid. Solids carry the notion of inside and outside. Many workbenches rely on this to make sure the objects they produce can be built in the real world.
 * Compounds: Compounds are simply aggregates of other shapes, no matter their type, into a single shape.

In the 3D view, you can select individual vertices, edges or faces. Selecting one of these also selects the whole object.

A note about shared design

You might look at the table above, and think its design is not good. The tightening of the feet with the tabletop is probably too weak. You might want to add reinforcing pieces, or simply you have other ideas to make it better. This is where sharing becomes interesting. You can download the file made during this exercise from the link below, and modify it to make it better. Then, if you share that improved file, others might be able to make it even better, or use your well-designed table in their projects. Your design might then give other ideas to other people, and maybe you will have helped a tiny bit to make a better world...

Downloads


 * The file produced in this exercise: https://github.com/yorikvanhavre/FreeCAD-manual/blob/master/files/table.FCStd

Read more


 * The Part Workbench
 * The FreeCAD addons repository
 * The Fasteners Workbench