Prepare your model for 3D printing with Inventor
In this tutorial we’d like to underline, to Autodesk Inventor users, some peculiarities of the software that are better to keep in mind when modeling for 3D Printing.
Since in 3D printing we aim to produce correctly meshed models, to be exported as .stl files, it’s reassuring to know that a 3D model obtained through Inventor will almost certainly result in a closed manifold and correctly shelled mesh. But still, besides paying attention to meeting the design rules (Related to the material guides) some care is necessary in order to produce a correct .stl file in the exporting phase of the modeling process. These steps, along with the description of some tools to check the model and some other tips, will be covered in this tutorial.
By the end of this tutorial you should be able to:
- Design a printable 3D file that can be used on 3D printers using Inventor
- Export valid file from Inventor
- Translate a mesh into an Inventor modeling file and fix errors
Inventor is one of the world’s most used pieces of 3D mechanical CAD design software for creating 3D digital prototypes used in the design, visualization and simulation of products. It uses a parametric solid modeling techniques, that makes it very suitable for the design process of engineered mechanisms and geometric-like exterior shapes, allowing for quick changes and adaptation of the geometric characteristics through a very intuitive workflow. On the other hand, this modeling style is very unsuitable for the creation of free-form shaped products, i.e. more ‘organic’ shapes.
Previous, basic knowledge of the software is required in order to get the most from this tutorial. Autodesk provides lots of great videos and tutorials for getting started with Inventor.
The version used in this tutorial is Autodesk Inventor 2014. You can download the student edition of Autodesk Inventor for free. This version fully reproduces the features of the commercially available software, and doesn’t produce any kind of watermark or other limitations in the output .stl files.
Designing a 3D printable model
Model for a closed, manifold and correctly shelled mesh
As you probably already know, 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 an .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 an .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 is 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, as noted before, 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 choosen (Join Cut or Intersect ).
Otherwise, selecting ‘New solid’ when creating a new feature, produces what will be recognised 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’).
Hollow your model with patterns
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 cost, 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 property you are aiming for.
But just hollowing your model doesn’t affect your product if your hollow 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, conferring aesthetic pleasure while reducing the amount of material and therefore the cost of the product. Lets now see how this can be made 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 type 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 ( ).
In this way we are then able, through the feature ‘Split’ ( ) separate the area of the logo from the rest of the surface. 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 like in this case, and choose the wall thickness you want to achieve, depending on the material. For instance, for 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.
Colors and textures
Inventor allows us to very simply and intuitively 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 the amazing 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 link above), you can easily apply colors to your model with the command ‘Adjust’ tool , and select a colour 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 colours will be stored in the file!
Measure the model
The first way to check if we have modeled correctly, respecting 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 cut away 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. In 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 reading their distance (Wall thickness) in the active window.
Analyse and export a mesh
When you’re done modeling and you are satisfied with the model you have produced, it means you are ready to prepare your .stl file for 3d printing.
What you have modeled so far with Inventor is a solid component, with mathematical data that needs to be translated into a ‘mesh’, made of polygons, vertices, and edges, in order to make it understandable for a 3d printer.
It’s important to be sure about every detail of our model before ‘meshing’ it, as the .stl file produced won’t be easily modifiable. So check wall thicknesses, clearances, and all the other parameters related to the material you would like to use for your print.
To translate your file into a mesh, access the ‘3D Print Preview’ environment by clicking ( )>Print>3D Print Preview.
A new window will open on your screen, showing your meshed model, with a specific toolbar that allows you to check and change some features of your mesh before exporting it.
Let’s see what kind of information we can access through this toolbar, starting from the right side.
defines the size of your file in its actual state. This value is related to the number of polygons (Facets) in the model, so the higher the number, the higher the size of the file. We recommend to keep the size of your model under 50 MB in order the make it easy to handle for our systems.
displays the number of polygons in your model. This number defines the surface definition of your printed object, so a higher number of facets will result in a smoother surface, closer in definition to your digital design. We suggest to set 1,000,000 facets as the absolute upper limit in your mesh in order to keep the file under 50 MB and easy to handle. Anyway, after some years of 3d printing, we can truly say that this limit is way higher than what is actually necessary to have the smoothest surface quality at this scale, as there is no visible difference in surface quality over 250,000 facets. Aiming for about 300,000 facets is a good compromise to ensure a great surface quality and a light, handy file.
will close the current 3D Print Preview.
gives you access to the most important part of this preview, the ‘STL File Save As Options’ window.
The format of the .stl file can be left as Binary, and the default units will be the ones used for modeling.
The ‘Resolution’ part of the window provides us with some options to define the quality of our mesh (And consequently its size). You can choose between 3 default settings, ‘High’, ‘Medium’ and ‘Low’, or a custom one.
Every time you choose one of these settings, press ‘OK’ and look at the preview window to see how your model has been affected by the change (Checking ‘Facets’ number), it will update in a few seconds.
Try first with the default settings, then if none of them fits your needs, go with the custom one, trying to change the ‘Max Edge Length’ value (Max length that every polygon’s edge can have) and leaving the others unchanged.
The ‘Show Facets Edges’ button ( ) lets you visualize how the object is meshed on the viewer.
When you have found what you think is the right configuration for your model, you can press ‘Save Copy As’ ( ) to export your object as an .stl file, ready to be uploaded to Sculpteo.
Translate a mesh into an Inventor modeling file and fix errors
Although Inventor allows you to import .stl mesh files, it doesn’t let you change or modify them as a normal modeling file. This means there is no way to add features or change shapes on .stl models that you may perhaps find on an online library. This format, .stl, in fact has been designed specifically to transfer data to 3d printing machines, and not for sharing modeling projects (check all the formats we accept on Sculpteo).
So if .stl is the format you have to modify, and you don’t have access to a better file format, then to bypass this limitation, you need to convert your .stl into a .dxf file, that Inventor is able to read as a modeling source.
To do so, you can use an online free tool, thanks to the great work of the guys of ‘CadForum’. You can go to CadForum's converter and simply select your file, and choose .dxf as target format, it will be automatically converted.
Once you are in possession of your .dxf converted .stl file, you can import it into Inventor and translate it into a modifiable 3d modeling file. Open a new file and select .dxf from the ‘File Type’ menu.
Select your file and press ‘Open’, and a .dxf import wizard, which allows you to choose its configuration options, will now start. The default settings are normally fine, just remember to check the ‘3d solid’ box in the last panel.
Press ‘End’ to close the wizard, you will see your model being converted into a surface modeling file, this operation may take a while, depending on the number of polygons in your model.
The last step in order to obtain a solid model from your .stl mesh is to stitch the surfaces you’ve created (Derived from the polygon faces of the mesh). To to so, choose ‘Stitch’ ( ), select the model and press ‘Apply’ on the ‘Stitch’ window. After some more seconds you will see it changing color and becoming a solid, that can be modified like a native file.
The defects of this process derive from the fact that what Inventor is doing is translating all the mesh’s polygons into surfaces to be stitched together, so it would be quite a different file compared to the one that would come out modeling it by ourselves, and the quality of the non-flat surfaces will depend on the quality of the mesh from which they derive. But on the other hand, a high definition mesh would take quite a long time to be calculated by the software. A good compromise needs to be found. Generally, we recommend you avoid translating meshes bigger than 100.000 polygons.
Take a look to what we mean by ‘the quality of the non-flat surfaces will depend on the quality of the mesh from which they derive’ on this cut away view.