Creating a simple part with PartDesign/it



Questo tutorial ha lo scopo di insegnare ai principianti di FreeCAD alcune funzioni di base attraverso un esempio. Dopo aver scoperto alcune nozioni di base nella Documentazione utente è possibile disegnare una prima parte passo dopo passo.

In questo tutorial ci occuperemo in particolare di:


 * Usare l'ambiente Part Design per disegnare degli schizzi.
 * Usare le funzioni Pad e Pocket.
 * Cambiare il colore e la trasparenza.
 * Spostare la parte manualmente.
 * Visualizzare le quote di riferimento nello schizzo.
 * Modificare una o più dimensioni.
 * Usare della geometria esterna e usare un piano di riferimento per centrare un foro.

Usare l'ambiente Part Design per disegnare degli schizzi.
Creare un nuovo documento e passare all'ambiente usando il selettore degli ambienti (etichettato con il numero 6 nell'immagine collegata) o andando al menu Visualizza → Ambienti. FreeCAD si avvia con le barre degli strumenti in alto, la vista combinata a sinistra e la vista 3D a destra.

Creare il corpo:

Premere Crea corpo. Nota: non confondere il corpo, che ha l'icona è blu, con il contenitore di Parte che la cui icona è gialla. Nella scheda Modello sotto la barra laterale della Vista Combinata, sotto l'etichetta del documento appare un nuovo oggetto con l'etichetta "Body", che è attualmente "Senza nome" poiché non abbiamo ancora salvato il nuovo documento. Il Body è un contenitore in cui le funzioni di Part Design sono disposte in sequenza per formare un singolo solido. Contiene i propri assi e piani di riferimento. Se è evidenziato in azzurro nell'albero del modello, significa che è attivo, vale a dire che possiamo modificare gli elementi in esso contenuti e aggiungervi nuovi elementi. Se non è evidenziato, fare doppio clic o fare clic con il pulsante destro del mouse e selezionare "Attiva/disattiva corpo" nel menu contestuale. Davanti all'etichetta Body, c'è un'icona blu identica a quella sopra e una freccia o un segno più, a seconda del sistema operativo in uso. Facendo clic sulla freccia o sul segno più davanti a Body si espande il suo contenuto. A questo punto, contiene solo un elemento con l'etichetta "Origine". Anche davanti a Origine c'è una freccia o un segno più. Fare clic su di esso per espandere il suo contenuto. Rivela i suddetti assi e piani di riferimento come mostrato nell'immagine qui sotto: Il Corpo attivo appena creato con il suo contenuto espanso. L'Origine è di colore grigio, disattivata, il che indica che il suo contenuto non è visibile nella vista 3D. Per rendere visibile il contenuto di  Origin  nella vista 3D selezionare  Origin  e premere la barra spaziatrice sulla tastiera. Ora  Origin  appare in nero nell'albero. Premere nuovamente la barra spaziatrice per nascondere il suo contenuto nella vista 3D. Fare nuovamente clic sulla freccia o sul segno più davanti a "Origin" per comprimere il suo contenuto nell'albero del modello. Prima di continuare, cogliamo l'occasione per rinominare il corpo.

Rinominare il corpo:

Nell'albero del modello, fare clic sul corpo con il tasto destro del mouse. Selezionare Rinomina e digitare un nome, ad esempio "Body part1" e premere per confermare.

Creare lo schizzo:

Tracciamo ora lo schizzo che definisce la forma generale della parte. Uno schizzo è una sagoma che descrive un profilo da applicare a una funzione per produrre una forma. Può essere "positivo" o "additivo", come un pad per esempio; o "negativo" o "sottrattivo", come una tasca.

Qui, poiché la forma generale della parte è regolare lungo l'asse Y, creeremo il pad lungo questo asse.

Premere Nuovo schizzo. Ora la vista combinata passa alla scheda Azioni e visualizza la finestra di dialogo Seleziona funzione. Questa finestra di dialogo si aspetta la selezione di un piano a cui allegare lo schizzo ed elenca i piani disponibili. Selezionare "Piano XZ (Piano base)" e premere. L'interfaccia ora cambia, subentra lo Sketcher e sopra la vista 3D appaiono le sue barre degli strumenti. Ci troviamo sul piano XZ del corpo per tracciare lo schizzo.

Per facilitare la creazione dello schizzo, in "Controlli" nel pannello Azioni a sinistra, impostare le seguenti opzioni:
 * Visualizza la griglia: attivare
 * Dimensioni della griglia: 10 mm
 * Vincoli automatici: attivare

Tracciamo il seguente schizzo:



Iniziamo con i primi segmenti:

Selezionare lo strumento Linea. Fare clic sul punto di origine, assicurandoci innanzitutto che accanto al puntatore del mouse appaia un piccolo punto rosso. Cliccare il punto successivo sull'asse X a circa 10 quadrati a destra o a circa 100 mm. Per ora, non importa se il segmento non è esattamente 100 mm, gli daremo dopo una dimensione fissa che vincolerà questa lunghezza.

Fare lo stesso per gli altri segmenti, provare a mirare ai punti creati e che devono accendersi in giallo. Ciò significa che questi punti sono coincidenti. Si dovrebbe ottenere più o meno questo:



Notare le piccole linee rosse sopra e accanto ai segmenti disegnati: questi sono i vincoli orizzontali e verticali. Le linee sono costrette a rimanere orizzontali o verticali. Notare anche il simbolo a forma di piccolo arco a sinistra: significa che il punto è fissato all'asse Z.

Now pick different line segments with the left mouse button and while keeping the left button pressed, drag the mouse to try to move them: some are free, others not.

Applying constraints:

At the top of the combo box, in the Tasks panel, you can read the number of degrees of freedom of the already sketched elements: it must be about 6, the objective of the constraints is to reduce the number of degrees of freedom to 0.

The slanted line should be free to rotate at this time: we will give it an angle constraint to fix it.

Click on the slanted line, then the bottom line; once selected these lines will turn dark green; then click the Constraint_InternalAngle icon.



Enter a value of 30°. Both lines have a fixed angle now. The constraint was created to the left of the sketch; with the mouse, move it inside the profile.

We will now constrain the bottom line with a dimension: select it then click  Horizontal distance.

Enter a value of 100 mm. The vertical line on the right now aligns exactly with the grid's 10th square to the right of the origin.

Let's set the overall height to the profile by selecting the highest point on the left then the origin point. Click on Vertical Distance, enter a value of 50 mm.

Do the same for the horizontal length of the sloped line with another 50 mm vertical distance contraint.

Move the dimensions away from the profile for better visibility. You should now have something like this:



Notice that the number of degrees of freedom reduced to 2. These are the ends still open.

Tracing the arc

Click on Arc, position the center at approximately x = 80 y = 30; then click to define the first starting point of the arc on the upper horizontal line's right end point; then click to define the end of the arc to the right vertical line's upper end point (make sure the points are highlighted in yellow before clicking).

Give the radius a radius constraint: select the arc, then click on Radius then enter a value of 20 mm.

Now let's make the arc tangent to the lines it's connected to: select the arc, then the top line, then click on Tangent. A Constraint substitution message appears, click. Do the same for the tangent constraint on the other side of the arc.

We proceeded in two stages to create the sketch, but we could also have traced the profile completely before constraining it fully.

Fully constrained sketch:

If you worked well, you should get this:



The sketch has become green, which means that it is fully constrained. There is no longer any ambiguity, everything is perfectly defined. This is confirmed by the solver message at the top left. Also note that the center of the arc has moved slightly, indeed giving these last three constraints, FreeCAD has calculated the true position of the center.

If your sketch is not yet green, one or more points are not coincident (2 points can be superimposed yet not be coincident). Make a small window (capture window) around a point to select, and create a Coincident constraint. Note: don't mistake the Coincident constraint for the Sketcher Point; while their icons are very similar, the latter has a larger icon; it adds a lone point in the sketch.

Proceed in the same way with all the points.

If your sketch is still not green, verify that all lines (but the slanted one) have either a Horizontal or  Vertical constraint, and add if necessary.

Using Pad and Pocket features
Click on in the Tasks tab, at the top left corner. We automatically exit the Sketcher workbench, and the Part Design workbench is activated again. The Combo View switches back to the Model tab. If you left your Body part1 expanded, you will see a new Sketch element below Origin, and nested under the Body. At this point, let's save our document. Give it a name (for example "tutorial1", or any name that you find relevant). It is good practice to save your document often, for example after completing a sketch or a feature.

Click on Axonometric view then  Fit all, which gives a centered 3D isometric view.

Click on Pad, enter a length of 30 mm; check the Reversed box to reverse the direction of the Pad. Click, the shape is completed. In the Model tree, a Pad object (that we call feature) appears instead of the Sketch. In fact, it has claimed Sketch, since it is based on it; clicking on the arrow or plus sign in front of Pad to expand it will reveal the Sketch underneath, which was automatically made hidden (its label is grayed out).

Note that the shape created forms a solid.



Creating the hole

Click on the top (square) side of the part and click the icon to create a new sketch. FreeCAD creates a new sketch attached to this face. So we are on a plane parallel to the absolute plane XY, but offset in height from the height of the piece, i.e. 50 mm.

You can switch the 3D window to an axonometric view or stay in top view. At any time, you can return to Sketch view (the view is oriented to face the sketch plane) using the Sketcher ViewSketch icon.

Note that the origin of this new sketch is that of the body. They may be different, but here are confounded with the absolute origin.

With the Circle tool, click roughly in the center of the face and make a circle of any radius.

Select the circle then create a Radius constraint, enter a value of 5 mm.

Select the center of the circle then create a Lock constraint; double-click on the horizontal dimension and enter -65 mm (here we indicate a position relative to the origin of the sketch). Do the same for the vertical dimension (-15 mm). The circle takes its correct position and the sketch becomes green, indicating it is fully constrained:



Close the sketch; in the Model tree, a new Sketch001 object has appeared below Pad. While Sketch001 is still selected, click on Pocket.

Pocket is a feature called "subtractive", it removes material from our part, here in the form of a cylinder since the sketch is a circle. Set "Through all" to completely cut the part. Press to complete. In the Model tree, a new element labeled Pocket appears at the bottom of the Body part1, and claims Sketch001.

Changing color and transparency
It is possible to change the color of the part, it is often useful to distinguish a part among others. The transparency of the piece can also be modified, which is useful for visualizing its internals.

Select the Body part1 body and go to the lower part of the Combo View, click on the View tab; locate the Shape Color property; you may need to use the vertical scroll bar to the right to find it. You can also widen the Property column: hover your mouse pointer over the separating line between the Property and Value headers; when the pointer turns into a double-sided arrow, press and hold your left mouse button and drag sideways, then release. In the right column, click on the gray square, which opens the Select Color dialog. Pick another color then click OK. Next, again in the View tab, change the value of Transparency, for example to 50 and press to complete (0 = totally opaque, 100 = totally transparent).

The hole is now visible inside the part. This is often useful for seeing the hidden or internal faces of the model.

You can also vary "Line Color" and "Line Width" to change the line thickness and the color of the part outline.

Manually move the part
Go to the View menu and select Toggle axis cross. These are the absolute axes. You should see in the 3D view, the 3 axes X, Y, Z in red, green and blue. This landmark will help us to orient ourselves in space. This landmark is fixed and immutable, it is either the view that rotates or the object that rotates in this space.

Select the Body; at the bottom of the Combo View on the left, you can see this (the Data tab needs to be on the foreground, you may need to click on the Data tab to make it visible):



Click on the three small dots (if they don't appear, click on the Placement field), this opens a new dialog in the Tasks panel. Using the arrows you can vary the position and angles of the part. It is actually the position of the body (so its origin) that moves in space, the orientation of the 3D view does not change.

Another method: in the Combo View, select the Body and click on the right button of the mouse, then select Transform. A view like this appears:



Hold and drag the cones along the axes or the spheres to move the body in all directions.

Validate. Then reset angles and coordinates to 0.

Displaying reference dimensions in the sketch
It may be useful to know the dimensions of some parts of the sketch, from the internal calculation of FreeCAD. It can be used just for reference, or use them later to set other dimensions for example.

In the Model tree, if necessary expand Body part1 then Pad to show the first Sketch. Double-click on it (or right-click and select Edit sketch in the contextual menu) then click on Toggle Constraint. (Note: depending on your computer display resolution, this icon may not be visible. At the right end of the Constraints toolbar, you may find a button. Click on it to expand and access collapsed icons.) From now on, we can create reference dimensions rather than dimensional constraints: they will be blue and will have no influence on the shapes of the sketch from which they come, they are calculated automatically.

You can display these dimensions for example:



We can see for example that the arc has a length of 20 since it's tangent with the edges.

We can also see that FreeCAD calculates the left face (50-50xTAN 30 °), as well as the distance dimension of the axis of the arc with the origin.

Editing one or more dimensions
During modeling, you can vary the dimensions of the model. It's very simple: for the thickness of the piece, double-click Pad, then enter a new value, 40mm for example. In the lower part of the combo view, you can change this value as well. Validate, the shape of the object has changed.

Do the same for the total length of the piece: double-click on Sketch, then double-click on the 100 mm dimensional constraint, change it to 110 mm then validate.

We can see that the piece was enlarged, but the hole is no longer centered in the middle of the top face. That's because it has been constrained to the sketch origin. Which does not necessarily correspond to what one would like, the hole should remain in the center, whatever the size of the face.

Center the hole
First method using external geometry.

Edit again the sketch of the hole and erase its horizontal and vertical distance constraints.

Then click on External Geometry.

We will now create two lines in the sketch, but extracted from a shape (or feature) external to this one and previously defined: that of the Pad.

Click on a vertical edge at the top of the part. For example, the edge slope side.

A new magenta line will appear above the edge. Repeat for the other edge, on the rounded side.

We can now use these lines (and especially their end points) to centre the circle, however we must add two construction lines: for example the diagonals.

Click on Construction Mode, we switch to construction mode: the lines will be blue and will be discarded outside of the sketch editing mode. They will allow to fix the center of the circle. Create the diagonals in the same way that you drew the first lines. Make sure all points are coincident.

Then select the center of the circle, then the two blue diagonal lines and click on Point on object, the circle must be centred at the intersection of the diagonals, that is at the center of the face. The sketch must be green, completely constrained (it is essential). Note that besides the radius of the circle, it is no longer necessary to create dimensional constraints.



Leave the sketch, we see that the circle is well centred. (The pocket feature was not deleted, but modified). If you change the dimensions of the part again, the thickness or the length, the circle will remain centered on the face.

Avoid construction lines:

It is often possible to avoid creating construction lines. You can edit the sketch again, erase the construction lines and use a Symmetric constraint between the two opposite vertices of the external geometry lines and the centre of the circle (select points in this order):



We get exactly the same resultat for the position of the hole. In fact, thanks to the constraints available in the Sketcher workbench, there are many possible methods. This example shows that it is often better to choose the simplest method, thus limiting the number of objects created as well as the errors that might result.

Second method using a datum plane.

Here is another, faster method that is possible since version 0.17: the use of a datum plane and its attachment.

Start by erasing the "Pocket" function as well as the sketch of the hole. Select the top face and click Datum point: create a datum point in the active body. The attachment mode chosen must be "Center of mass".

As the face is rectangular, its center of mass corresponds to the center of its diagonals. Validate, and a datum point is created. Select the top face again and while holding down the CTRL key, select the point you just created in the Model tree, release CTRL and click Datum plane. A reference plane is created with the origin of the point. Click OK.

It is now very easy to center the circle! Select from the Model tree or in the 3D view the plane you created, and click on Create a sketch, a sketch is created with as origin, the origin of the plane. Then just trace the 5 mm radius circle on this origin, then validate (the sketch must be green imperatively).

You get with "Pocket", as created previously, the hole and it will always be centered.



This tutorial is completed, save this file, you can have fun exploring various features. Change other dimensions, make other shapes, put other holes on other faces, it is when making mistakes that we progress!

You can also continue with this other tutorial of a slightly more complicated part:

Basic Part Design Tutorial 017