Fortgeschrittenes Modul: Bearbeitung einer komplexen 3D-Datei

Für dieses Modul müssen Sie zuvor Modul 2 des Grundkurses absolviert haben.

Haben Sie ein 3D-Netzobjekt von einer Design-Sharing-Website modelliert oder heruntergeladen und möchten Sie es bearbeiten? Hier erfahren Sie, wie Sie es importieren und für die Bearbeitung in Autodesk Fusion vorbereiten können.

Laden Sie die Beispieldatei „Nefertitis Gesicht“ hier herunter.

Die Beispieldatei ist eine .3mf-Datei, die zum Speichern von 3D-Modellen im Netzformat verwendet wird.

Eine 3D-Datei in Mesh-Modellierung (oder polygonal auf Französisch) besteht aus der Manipulation eines Netzes, das die Oberfläche des Objekts darstellt. Diese Art der Modellierung eignet sich gut für Animationen oder Videospiele, kurz gesagt, wenn Sie sehr organische Formen erstellen möchten.

Grundsätzlich verwenden Fusion und andere Industriedesign-Software keine Mesh-Modellierung, da diese Ungenauigkeiten mit sich bringt. Sie verwenden ein anderes System, das einfach als parametrische Modellierung bezeichnet wird. Diese Art der Modellierung ist viel genauer und flexibler als Meshes, lässt jedoch weniger Kreativität in Bezug auf das Design zu.

Dennoch werden viele parametrische 3D-Dateien, die Sie im Internet finden können, in Mesh konvertiert, da dies der für den 3D-Druck erforderliche Dateityp ist. Wenn Sie beispielsweise Designs von Thingiverse herunterladen, ist die Wahrscheinlichkeit groß, dass die Datei im .stl- oder .3mf-Format vorliegt. Am besten suchen Sie nach Dateien im Format .step oder .f3d, die Sie direkt in Fusion öffnen können!

Unser Beispiel hier ist eine Gesichtsskulptur, daher ist es sinnvoll, dass es sich um eine Mesh-Datei handelt, die wir jedoch in eine parametrische Datei konvertieren können.

Zu Ihrer Information: Dieses Modell ist eine modifizierte Version dieses Modells, das Sie auf Thingiverse finden:
https://www.thingiverse.com/thing:1822326

Start by creating a new file, ensure you are in the Design workspace, and select Insert > Insert Mesh.

Click on Select from my computer…, navigate to the folder where the Nefertuto.3mf file is saved and select it.

Normally, it is positioned on the correct plane (XY) because the .3mf format saves this type of positioning information.

You can rotate/move the object as you wish using the transformation tools. Make sure that the object is centred and placed at Z=0mm using the Centre and Move To Ground tools in the menu on the right.

Once everything is correct, click OK.

You can see that the object Nefertiti_face has appeared in the Browser with a small prismatic logo, indicating that this object is a mesh.

Although it is entirely possible to use the file directly as a mesh for machining, we will still convert it into a parametric object so that it can be easily manipulated in Fusion.

To do this, click on the Mesh tab:

Then in Modify > Convert Mesh.

In the menu on the right-hand side, click on Body Select and click on our object.
Leave the rest as it is.

An alert message like this may appear:

‘This mesh has more than 10,000 triangles. The calculation may take a long time.’

Depending on the complexity of the subject, the calculation time may be quite long. This example takes 4 seconds to calculate on a computer with a relatively powerful processor (AMD Ryzen 7 6800HS (3.20 GHz)).

You can then return to the Solid tab. You can see that the Nefertit_face object has changed its icon, meaning that the object is a Parametric Solid.

We will add a base to our object because the goal is to have a final object that can be easily cut out of the stock. Create a new Create > Sketch on the XY plane (we have hidden the body here to access the plane).

Select Create > Ellipse.

Place the first point in the center of the document, then enter 55 mm for the horizontal distance and 0 deg, and left-click to confirm.

Then enter 40 mm for the vertical distance:

Confirm by pressing Enter.
You can finish the sketch by clicking Finish sketch.

Create > Extrude and extrude the Ellipse by 2.66 mm. Make sure that Operation is set to Join.

Click OK to confirm the operation. The base is now complete.
We can now move on to the Manufacturing tab.

Then go to the Manufacture workspace.

Create a new Setup as usual, placing the working coordinates on the martyr in the Setup tab:

We are assuming here that our stock is 18 mm thick. Set the Stock Top Offset to 0 mm and check that the Stock Height (z) is less than 18 mm in the Stock tab. If it is thicker than this, feel free to change the size of the model by returning to the Design section and using Modify > Scale.

Tu peux valider le Setup.

Select the 3D > Pocket Clearing operation. This operation is easier to use than Adaptive Clearing, which we used for the ashtray, but allows for less precision. However, Pocket Clearing is generally much faster. Feel free to run tests and compare the results and machining times.

Select a 6 mm diameter end mill, select the appropriate speeds for your equipment, and go directly to the Geometry tab.

In this tab, select Machining Boundary: Selection, then click on the upper edge of the base.

In Tool Containment, select Tool outside boundary.

This option allows you to limit the machining area to the outer contour of this ellipse.

In the Passes tab, only change the Maximum Roughing Stepdown value to 1 mm. This value will determine the degree of finish of the operation: the smaller it is, the more defined the object will be; the larger it is, the more approximate the object will be. This will depend on your time objectives, the type of material, etc.

Above: Result for 1 mm passes -> 2 minutes and 10 seconds according to Fusion.

Above: Result for 5 mm passes -> 23 seconds of machining according to Fusion.

Don't forget to uncheck Stock to Leave.

Then, in the last tab, Linking, make sure that the Ramping Angle (deg) is set to 35 deg.

You can click OK to confirm the operation.

We will now use an operation to complete the 3D shape. We will use a conical hemispherical cutter (this one: https://www.fraisertools.com/en/zeta-covered-spiral-carving-2d-3d-router-bit.html) because this type of cutter allows for a level of precision that is difficult to achieve with a conventional straight hemispherical cutter. It is entirely possible to use one, but you will have to compromise on its diameter or the level of detail you want to achieve.

It is essential to use a hemispherical cutter because the aim here is to smooth out our roughing by breaking up the staircase effect and machining the details. This is impossible to do with a straight cutter.

There are different finishing operations in Fusion, each of which is more or less suited to a particular type of design. Here, we will use the most common operation, 3D > Parallel. Feel free to try them out depending on your design.

The setup is quite simple: just select the right milling cutter, in this case #22 - 3.2R1.6mm 2.5° ZETA face from the Fraiser Boss Ultimate kit.

In terms of settings, we will use those recommended by Fraiser here. If you are using a different milling cutter, check the manufacturer's specifications, but bear in mind that you can work quite quickly as this milling cutter does not have much to machine.

Then in Geometry, leave Machining Boundary set to Silhouette.

In the Passes tab, the only value to check is the Stepover value. This value defines the fineness between each tool path. If you notice that the surface of your machining is not perfect but has traces of the milling cutter, it is possible that this value is not small enough:

You can click OK to confirm the operation.

The purpose of this last operation is simply to machine the outline of the base in order to remove the engraving from the raw material. We will not go into detail here, as this operation is explained in other tutorials.

Select 2D > 2D Contour:

Then select a flat-end cutter (you can use the one from the first operation, for example).

In Geometry, select the bottom edge of the base and don't forget to add the tabs.

In Passes, don't forget to set the passes according to your preferences and your end mill:

Then, in Linking, activate Ramp and use our optimal values:

Ramping Angle: 35 deg
Maximum Ramp Stepdown: 300 mm
Ramp Clearance Height: 2.5 mm

You can then confirm the operation by clicking OK.

Nothing special here. Don't forget that you are changing tools and that you will need to export each operation one by one if you are using the license for personal use.

As for machining, there's nothing special here either.

We use the base here to easily cut the object out of the raw material with tabs. However, this may not be possible depending on the file type, and it is entirely possible to use 3D Pocket operations to cut all the way through. However, you will not be able to add tabs: you must either model them yourself or use the technique known as “Onion skinning”: leave 0.2 to 0.3 mm of material at the bottom of your cut, then finish by hand using a cutter.

If you use a good hemispherical cutter and the material is soft enough, you can cut directly into the raw material with the finishing pass. Be sure to test it first!