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If your plan is to get your hands on an object you designed through Sculpteo’s 3d printing program, you need to produce a 3D mesh file and export it in any of the acceptable formats, usually a .stl file.
Mesh files are not necessarily used for 3D printing, so it is important to use characteristics that function with the program you plan on using it for, whether that be rendering, animation, or 3D printing. The most important characteristics for a 3D printing mesh (also the most common errors for non-printable meshes) are that must be manifold, oriented, and made of single shell parts. We recommend modeling with Autodesk Inventor as these characteristics are easily attainable.
Manifold essentially means that your mesh needs to be completely closed (Or ‘watertight’) and that each of its edges needs to be shared with two polygons. A solid in Inventor always produces this type of mesh; if it doesn’t, that means your current model is not yet a solid but a group of surfaces. It’s easy to recognize when your imported model is made of a solid or multiple surfaces because multiple surfaces do not look the same – they have a slightly transparent shade by default.
That type of problem can occur if a model is imported from another software, and then its converted to a .stl file or if surfaces are created directly in Inventor. If the element in Inventor is not a solid, the 3D Print Preview won’t allow us to export the model and will produce this message:
If this message appears, all we need to do in order to obtain a solid that is exportable as a manifold mesh, is to stitch these surfaces together using the command ‘Stitch’ (Press the command>select the surfaces>press ‘Apply’>press ‘Done’).
As for the orientation of the mesh, the inside and outside of a solid model are automatically determined. That which is mathematically full within the solid is defined as the internal area and there is no reason to manually define it.
The third important requirement is to have each separate part of our model made of just one shell. Once again, the software automates this process, and each time we create a new feature on the working model, a joining option can be chosen (Join Cut or Intersect ).
Otherwise, selecting ‘New solid’ when creating a new feature, produces what will be recognized as a separate shell in the mesh. To join two solids into one (And obtain one shell when meshed), the command ‘Combine’ is needed (Press the command>Select bodies to be joined>choose Join, Cut, or Intersect>press ‘Apply’).
There are several reasons why digital models for 3D printing should be hollowed but the main one regards the amount of material used to produce it. In 3D printing, unlike common production techniques, the cost to fabricate an object is not dictated by its shape complexity, but mainly by the amount of material that it requires. Making your object hollow will then strongly affect your product costs, sometimes decreasing it by up to 60 or 70%.
Another important reason to hollow your model is to keep your product lightweight if that’s a factor you are aiming for.
But just hollowing your model doesn’t affect your product if your hollowed part is not connected to the outside through at least two holes. The reason is related to the technology: “unprinted” material would be trapped inside your model with no way for it to escape.
In many examples of successful 3D printed products, we have seen designers taking advantage of this production driven restriction, creating patterns of cavities along the whole model surface. This confers aesthetic factors while reducing the amount of material and therefore the costs of the product. How can this be achieved with Inventor?
We are creating a simple cube (Primitive Box) and choosing one of its faces as 2D Sketch plane ( ).
Then press the ‘Insert AutoCAD File’ button ( ) to import the vectorial drawing you want to use as a cutting pattern on the surface (You can also import other types of files or draw something directly on the sketch plane).
We’ve uploaded the Sculpteo logo, then scaled it ( ) and moved it ( ) to the center of the surface.
Then what we need to do is to use the command ‘Project to 3D Sketch’ ( ) and select the surface on which the sketch is lying. Press OK and exit the sketch ( ).
We are then able to separate the area of the logo from the rest of the surface through the feature ‘Split’. Select the 3D Sketch just created with the ‘Split Tool’ and the surface which it belongs to as ‘Faces’. Press ‘Apply’.
The final step is to use the feature ‘Shell’ to hollow the model, removing the logo’s surface just created.
Pick the ‘Shell’ feature ( ) and select the face to remove. Deselect ‘automatic face chain’ if this face belongs to a bigger surface as in this case, and choose the wall thickness you want to achieve, depending on the material. For instance, Plastic material needs to be at least 0.8 mm and 2 mm to be considered as rigid. You can find more information about material specifications on our Materials page.
Now you can press ‘Apply’ to hollow the model, and engrave the logo.
Inventor allows us to very easily color the singular faces of our model or apply materials to them, but unfortunately, it doesn’t allow us the ability to export this information as proper files for Full Color 3D Printing.
To partially avoid this problem, ‘CadStudio’ created a plug-in called ‘VRML Translator for Inventor’, which gives the ability to export as a VRML file. VRML files keep track of color information and it’s accepted by Sculpteo uploader. You can find it on ‘CadStudio’ page (Trial version free, after 99 Euros).
However, this only partially solves the problem because VRML still do not support textures; it’s still not possible to make the most of the Full Color printing technology.
When you have installed the plug-in (instructions in the link above), you can easily apply colors to your model with the command ‘Adjust’ tool, and select a color directly from the color picker or by entering an RGB value, and choosing the faces where will be applied. With the above mentioned plug-in, a VRML will appear among the available exporting formats, and your colors will be stored in the file!
The first way to check if we have modeled correctly, and respected the design rules, is to manually do so by creating a new sketch in the model.
Let’s check for example the pitch of a thread. Choose ‘Create 2D Sketch’ ( ) and select the plane that is longitudinally crossing the bolt model then go to the cutaway view of the model by right click>Slice Graphic, to be able to evaluate the profile of the thread.
Let’s show its edges in the sketch with the command ‘Project Cut Edges’, that you can find in the ‘Project Geometry’ tab. This way, you would be able to snap to the geometry of your model that is intersecting the plane you chose.
Now with the tool ‘Line’ ( ) you can trace two consecutive oblique faces of the thread and connect their middle points. Use the tool ‘Dimension’ ( ) to measure the length of this line, and if it corresponds to your thread Pitch, it means you’ve modeled correctly. If what you want to measure is the distance or the angle between edges, points or faces of the model, or check the size of areas and loops of the faces, you should then access the features called ‘Measure’ under the ‘Inspect’ panel.
For example, it could be really important to check the wall thickness of your object at the end of modeling. Anything lower than 0.8 mm won’t, in fact, be 3D printable in any material. You can find more information about materials and their specifications on our Materials page.
You can measure it with the ‘Distance’ ( ) tool, selecting two opposite faces of a wall, and read their distance (Wall thickness) in the active window.