Prepare your model for 3D printing with CATIA V5
This tutorial is for 3D printing enthusiasts who are already familiar with CATIA and would like to know the tricks for making a 3D printable model with CATIA.
Throughout this tutorial, you will learn the best practices for modeling, correcting and exporting an object to be 3D printed. By the end of this tutorial, you’ll have mastered:
- Modeling for 3D Printing with CATIA V5
- Analysing and exporting your 3D model
- Fixing common errors
- Transform a 3D scan into a printable model
CATIA is a modeling program geared toward the modeling of industrial objects, but it can be used for much more than just that. Its function relies on the use of waves and NURBS for the base of its functions. Unlike many other programs, CATIA does not rely on a single function of meshing, which relies entirely on flat surfaces giving the impression of curves, instead it relies on a system of nurbs which take the average of those edges for a truly smooth surface. The system allows for a higher level of precision than other methods. Instead of polygonal modeling, CATIA relies on dimensional sketches which make measuring and resizing the object much more accurate. With a system based on these parameters, exporting becomes quick, easy, and surprisingly light as each individual file understands a large number of nurbs.
Though this type of system can make the creation of specific and organic forms (like a face) somewhat complicated. It also limits importable files to only other wave-based files (.iges and .step more specifically).
It is possible to export directly from CATIA to .STL with a high level of control and precision. This gives users the opportunity to model for 3D printing directly from the program, provided a couple of rules are respected.
You do not need to be an expert or know all of the minute details of CATIA to understand this tutorial. However, it is important to be comfortable with the basic elements of the program as this tutorial focuses specifically on the best practices for creating a 3D printable model. Thus this tutorial does not go into the basic principles of the program.
CATIA is paid professional software. It is possible to obtain a license from Dassault Systèmes, CATIA’s creator. There is also a student edition, available whatever the school / university you come from, for a fee of 99 euros with your student card.
Modeling for 3D Printing
A couple of good practices must be followed in order to create an effective 3D model. New limits arise with new materials and it's important to keep in mind that what you’re creating on the screen will become a physical object, limited by a different set of physics, namely gravity. In this part of the tutorial, you will learn the key notions for creating a model that can be 3D printed through CATIA.
CATIA modeling relies on a system of splines (spline modeling), which allows for extreme precision. That, coupled with CATIA’s body volumization system, a system in which classic constraints are automatically treated, make for even further precision. CATIA only generates coherent solids which are thus easily translated into a physical object.
It is also important to follow the following rules:
- The various bodies in your model cannot intersect
- All of the elements in your model must have a thickness
- The object must have a clear interior and exterior (this is generated automatically in CATIA)
- The file’s optimal size should be less than 50Mb after the export. This limit is generally enough for a file that does not lose any detail or information. The tutorial will go into further detail about exporting and file restrictions in a later chapter dedicated to mesh exportation.
- Finally, as previously mentioned, you must not forget that the digital object will become a physical one: a small and thin structure cannot support a top-heavy design. Keep the material's restrictions (minimum thicknesses, resistance, etc.) in mind when designing. To do so, you can check our material page.
With the exception of assembled folders, mobile pieces, and other designs that are physically separated, its essential that your file has only one body within it. Files which have more than one body will be covered in a later chapter dedicated to moving and assembled pieces).
Model a correct closed volume
CATIA offers two main types of models: Solid and surface. For these there are two different workbenches you can use: Part design exclusively for solid modeling and Generative Shape Design for both surface and solid modeling.
Solid modeling involves different bodies, within which the functions are contained. Note that a body can contain any number of functions, but it is nevertheless essential to work on multiple bodies if one wishes to be able to perform Boolean operations between them.
Surface modeling mainly uses geometrical sets that contain the geometric elements (points, lines, splines, maps ...) necessary to create surfaces.
Whether solid or surface modeling, it is important to create as many bodies / sets as you have different materials to be applied to your model.
For 3D printing, it is best to only export files containing volume parts, not surface. In fact, the planar body has no thickness (the thickness is set zero), which can not be translated into anything "physical". Your 3D model must have a minimum thickness corresponding to the limits of the material used to be correctly interpreted by the 3D printer. We'll look at the solid bodies in the first step before treating surface bodies in a second step, the latter being less suitable for 3D printing.
Solid modeling : « Part Design » Workbench
Solid modeling is used for simple geometries and uses of such operations as "positive" (extrusion, revolution, rib ...) and "negative" (pocket hole, groove ...). It is sensible to create bodies for each operation, so you can easily tweak them against each other through Boolean operations. These boolean operations can be performed at any time of your modeling, although it is common to perform them gradually. They are applicable between all the body parts you have created and are accessible via the 'Insertion' tab > 'Boolean operations' or simply by right-clicking on the body in question in the tree. For 3D printing, the Boolean operation "add" applied successively to different bodies will get you a single body ready for printing.
Each function applied by CATIA generates a printable valid model in 3D volume terms, of course, you still need to respect the constraints of the material you want to use.
You can verify that your model is merged using a section view. This requires that the body belongs to a product. Then you can access the “assembly design" workbench, which contains the "section" tool, located in the toolbar at the bottom of your screen.
The "section" tool brings up a yellow plan scheme you can move manually or using the "positioning" tab. You also need to activate the "volumetric cut" icon present in the tool edition. Then clicking the "results" tab will generate a preview of the cut.
Before the merging the bodies, you can observe two distinct bodies that intersect.
After using "add", the two bodies are merged as shown in the screenshots below
If your model contains only simple geometric shapes, then it's highly recommended to use the "design part" workbench. We recommend as much as possible to work in solid bodies for 3D printing. Boolean operations in surface and volume are identical and have the same characteristics.
It may be the case, however, that you need to work on your model surface. In the following section, you will learn how to make a printable surface model.
Surface modeling : "Generative Shape Design" (GSD) workbench
Although surfaces are not directly usable for 3D printing, it is possible to use surface modeling by converting all surfaces into volume bodies before exporting. Therefore it must be modeled with a view to create a body which can be converted into solid.
For this you need to create a closed body with finite, seamless borders, paying special attention to the characteristic "watertight" mesh.
To better represent this idea, you have to imagine that the inside of the object is filled with water, which should not come out, regardless of orientation. The goal is to obtain a perfectly sealed body, "watertight".
The set of functions that allows you to convert a surface body to a solid body are represented by purple icons.
In the case that your set of surfaces is a fully closed volume, you have to use the "fill" function that will automatically handle filling the inside of your surfaces. The yellow surface becomes a purple volume.
In case your surfaces are not a fully closed volume, you can use the "thick surface". This feature will allow you to determine the thickness of your surface so that the latter can be physically printed. This tool offers you the ability to precisely control the size and direction of the thickness in question. Then consider recommendations with reference to the target material.
Finally, note that the GSD workbench offers a boolean tools panel to achieve the same Boolean operations as the Part Design workbench.
Hollowing your model
Making a hollow model is a common task in modeling for 3D printing. Indeed, it helps limit the amount of material used to what is strictly necessary, thereby limiting the cost of production. It is also essential for some materials (especially ceramics) which need constant thickness.
To hollow your model, you have several options.
With the hollowing function Sculpteo offers, you can easily hollow your model. Just upload your file to our site, then choose the location of the holes for material extraction and our algorithm does the rest, automatically adjusting wall thickness when you change material or scale.
It may also be interesting to create your object with hollowed out areas that do not require significant resistance, using a pattern or hollowing non-uniformly (transparency effects, thicker and thinner areas, etc.). Simply use the standard functions of material removal. You can find some examples below. (But unlike Sculpteo's Hollowing, this will not adapt to changing materials or scales.)
- Structural removal
- Shell removal
- Standard drill
If you want to hollow your model in more personalized way, CATIA also offers the "shell" function, fulfilling this role. You will have to choose one or more faces that are "opening out" and specify the wall thickness you want.
The "shell" tool also lets you select faces in different thicknesses. This allows you to manually change the thickness of these shells. This tool is useful when there are sensitive areas that we mustn't hollow out.
If you use "shell" without selecting faces, remember to make two holes to allow the object to be emptied at the end of production. Without drain holes, an object, even with proper thickness, will be considered a solid object, because the blocked powder inside can not be evacuated, though its strength will be slightly lower because it will be full of "unfused" dust. Keeping drain holes is particularly important. To learn more about the diameter of the holes to be made depending on the material used, consult our materials pages.
Text and patterns
You can add text or raised patterns on your object using Sculpteo's tools but you can also do it in CATIA. If you want to add text to your model, you can:
- Use the CATIA text tool
- Or import an existing text or picture
Using CATIA text tool
- Open the "Drafting" workbench in mechanical design
- Use the "Reference" tool and choose your font and size and type your text
- Save your text in DWG or as DXF
- Return to the workbench "design part"
- Open a sketch
- Click File > Select, open your DWG or DXF file
- Select the text > edit copy
- Return to your sketch > paste edit
- Now you can work on your text like any sketch. We will extrude to obtain a solid body.
Import an existing text or picture
If you want to import text, drawings, graphics or other vectorized artwork directly into CATIA, you will need to use DWG or DXF formats using the same method as described above.
Mobile parts and assemblies
With 3D printing, you can print moving parts or articulated objects in one go - the resulting object will be fully assembled in the 3D printer, functional, and with permanently attached parts.
However, it must follow certain rules so that your object is functional.
For example, for a plastic object, you must leave a minimum clearance of 0.5 mm around the various bodies so that they are not fused together during 3D printing. For the modeling rules for each material, we invite you to visit our materials pages. We’ll see how to measure elements and distances in the next chapter.
To separate elements with a specific distance, use conventional constraints tools.
Colors and textures for a full color 3D print
CATIA incorporates a materials management solution, also used for its integrated 3D rendering solution (photostudio). However, the colors / materials information is not exportable. You cannot export a CATIA file while including textures.
Only one pre-export filter allows saving of the material information by separating the file zones (each different material will be considered a different mesh area). You can then export your CATIA file to other software to manage color / textures (e.g. Blender), assigning your textures there before exporting again.
This process is particularly laborious and involves many risks of failure, such as during the export of materials. So it is better if you want to make a large texture for your object, work directly in a software that manages textures, like Blender for example.
Furthermore, UV management is almost impossible with CATIA. Indeed, once exported, basic UV are unusable and unfolding an exported CATIA mesh is often a challenge that will waste more time than it will save.
To learn more about modeling with Blender for 3D printing, please see our tutorial Prepare your file for 3D printing with Blender .
Analysing and exporting your 3D model
Measuring elements and distances
While it is always easier to model directly using the right dimensions, thicknesses and distances, it is sometimes necessary to measure parts of an existing volume. CATIA has two tools: Absolute measurement and relative measurement.
The relative measurement tool calculates the distances between any type of geometry: points, lines, planes, surfaces ... The minimum distance is displayed. This tool measures either the distances between different bodies or simply a distance between different geometrical elements of a single body.
"Absolute measure" tool
The absolute measurement tool provides all the necessary information on a volume or a surface. It also helps with the "thickness measurement" to measure to a thousandth of a millimeter and very intuitively and quickly any thickness / length. In the case of a preparation of your CAD for 3D printing, absolute measurement tool will be used primarily to obtain volume information.
For dimensions, it is important to note that the concept of units is not valid for CATIA here. When exporting the file in a format other than native CATIA (.CATPart), the units are not retained. You'll need to define the unit and scale appropriately when you move to the Sculpteo interface.
This is the "tesselation" tool that allows you to generate the mesh. It is located in the sidebar.
You can then work on two main features, which will determine the accuracy of your model: sag and step.
The sag is the maximum distance between the mesh and the real shape. "Step" meanwhile corresponds to the distance between two neighboring nodes. Since both are dependent each other, the default setting for step is 'disabled'. You choose on what basis you want to control the accuracy of your model's mesh.
We recommend that you keep the default setting and use the sag. Finally, note that the lower the values you choose, the more accurate your mesh will be, and of course heavier to export. Also note that the accuracy of the machines being one micron, it is unnecessary to enter a sag of less than 0.01mm.
Finally you can choose the grouped or separate option. If you have several pieces, the "grouped" option generates a single mesh for all parts. Conversely, choosing "distinct", CATIA generates independent mesh for each body part. Note that the mesh appears in the product / part which is activated in the tree.
To view the mesh, which is not the default view, you need to access the mesh properties that appear in the tree (right click > properties display mode, check "triangles").
"Mesh regeneration" tool
This tool allows you to automatically re-mesh the model. This can be useful if you have a complex shape to mesh.
An "Information" icon that informs you about the geometry of the mesh can be found at the bottom of the toolbar.
Automatic error detection
Once your mesh have been generated, you can use the "mesh cleaning" tool in the side toolbar. This tool is quite limited as it merely permits errors detection. We will see in the next chapter how to fix them. The following window will appear. Click on "analysis" to see if your model contains errors or not.
The mesh cleaning tool allows you to detect basic errors such as duplicated triangles, bad direction, edges and non-manifold vertices. A drop-down menu in front of each of the above errors allows you to assign a color to better identify the problem.
You can also apply filtering options of long edges and small angles, entering the values you want. Then clicking "apply", affected points or edges related to the problems identified will be removed, as shown in the images below.
Also note that the "structure" tab will allow you to manually change the orientation of your surfaces (We will explain this more precisely in the next chapter).
Choose a file format and export your model
CATIA works on a system of NURBS, which therefore allows you to easily save your model in STEP or IGES format. To do this, simply select one of these formats in the menu at the time of saving.
It is also possible, at the time of export, to convert your model to a file defined by a mesh, such as STL. It is indeed the most widely used format for 3D printing. Although CATIA does not directly support mesh modeling, you can generate one while exporting, which makes CATIA especially effective for 3D printing. CATIA allows import and export in this format, with quite a range of settings.
To export your model, you go through the STL rapid prototyping workbench (Start tab > Machining) or the Digitized Shape Editor module (Start > Form tab). The first workbench will be useful if you want to prepare your CAD model for 3D printing, while the second is more oriented towards processing point clouds from a 3D scanner. Both are quite similar except for a few tools.
Export is achieved by using the "STL export" button in the side toolbar.
If your design is an assembly, several options are available to you when exporting. If you generated one mesh per part, then you can get a .STL file for each part. To do so, click on the icon "STL export." Then click successively on the different meshes forming your assembly, and choose the "distinct" option. If, however, you want to get a single .STL file for your full assembly, then choose "grouped". But be careful, “grouped” doesn’t mean “merged”. It just means that you will have only one file for the whole assembly.
Some files, by their complexity or nature, will not be optimal candidates for export to .stl. They will generate either very large files (over 500MB), or simply not be exported from CATIA below a certain level of accuracy.
Files with many curved / rounded parts or large areas based on vector drawings with a large number of points (text, graphics, etc.), will generally generate very large files in .STL.
It would be better to export them to a "vector" IGES or STEP-type as mentioned above. These file formats are obviously supported on our website.
Fixing common errors
Before starting this chapter on repairing the most common issues when preparing your data for 3D printing, here is a description of some tools that will be useful later.
This tool allows you to select the mesh points you need to work on. You will be able to use conventional tools such as the selection tool or brush. The neighborhood tool lets you choose a whole part of a mesh, selected automatically by CATIA depending on your mesh geometry. Finally, the "pointing" mode will allow you to select items one by one, which is great for detailed touch-ups.
You can also choose to work at different levels: points, triangles, cloud, etc.
Translation / Rotation / Symmetry / Scale tools
You will find them in the “digitized shape editor” workbench. Their use is identical to the one you know in Part Design.
The size of the mesh depends directly on your export settings and of course the complexity of your model.
Some functions, such as the leave and text functions (based on a highly vectorized initial design) are particularly resource-hungry and will quickly increase the size of your exportedfile.
If your file is too large to be imported on Sculpteo, try lowering the level of detail specified in CATIA (or no arrow), or if your model incorporates many holidays / rounded or curved parts / sketches based on text or graphics vectorized, try to export in a more appropriate format for the file type, such as iges or step.
Overall mesh reduction
CATIA also provides a "decimate" tool, which reduces the number of triangles in
the mesh. This tool should be used with caution, since reducing the number
of triangles also reduces precision. This tool gives as much control as
possible for the reduction of triangles, with several options:
- Minimum length: This option allows you to keep maximum control while returning the minimum edge length you want. When you choose this option, a green sphere appears, allowing you to compare the size you selected with the size of your model. With this option, the edges whose length is greater than the value that you choose will not be changed, the mesh remains the same in non-affected areas.
- Targeted percentage: This is quite a random setting to reduce density to a defined percentage of triangles. The reduction can therefore be very fast, but without much predictability of the result. The mesh is usually completely changed.
Local mesh reduction
If you want to change only a part of the mesh, you can use the selection tool "activate". It offers several selection modes such as the ones we mentioned previously (brush or hatch., trap…). Choose the mode that suits you, select the area to decimate, and click OK. Then apply the "decimate" tool on the active area as seen above.
To get back to the rest of the mesh, click the "activate" tool again, select the mesh you were just decimating, click on "swap" and finally click on "activate all." You will then get a full mesh with locally depleted zones.
"Fill holes" tools
"Fill holes" is quite an efficient tool, offering many settings that can solve most cases of non-watertight meshes. To do this, click the icon located in the sidebar, the holes are then detected and a window opens with several options:
- The "hole size" allows you to select only the holes whose size is less than the value you have entered.
- The "points insertion" to select the arrow and / or the pitch of the mesh that will be generated for filling the hole. Again, the higher this value, the higher the precision of the mesh.
- Finally, the "shape" is useful for filling unflat surfaces. Do not hesitate to move the cursor position up for good continuity in the reconstruction.
Before validating and generating the filling surface, select or deselect with a single click, holes that will be affected by the repair. Green holes will be repaired, red ones will be ignored.
Then check the result of the reconstruction by performing a “zoom in” on the area to ensure the continuity of the surface generated with the initial surface is good. If necessary, repeat the operation by reducing the arrow and / or the not.
« Smooth » tool
This tool, which is represented by an iron in the toolbar is very easy to use. Just select some or all of your mesh, and each time you click on "apply" a smoothing operation will be performed. The more you repeat the operation, the smoother it becomes. After a number of operations, the algorithm plateaus and becomes less effective.
« Mesh offset » tool
If you forget to generate thickness of one or more surfaces in your model in the GSD workbench, it is always possible, even after your meshed model has been created, to generate thickness.
To do this, use the "mesh offset" tool, enter the value of the thickness, and remember to check the option "create the shell" to generate a closed body.
« Rough offset » tool
This tool allows you to precisely control the shape and quality of the shell you will generate. Click on the icon "offset distance". A black arrow represents the length of your shift and its direction.
The setting on the granularity directly affects the quality of the mesh of the generated shell. The higher is the granularity, the lower the accuracy (left image). Conversely, a high granularity will reduce the size of your exported file (right image).
Finally, the 3 direction icons allow you to control the shift.
As mentioned earlier in the tutorial, the orientation is especially important for the volume to be valid for 3D printing because it helps to determine the inside and outside of the shape.
If your body is a solid body in CATIA, you will not have any problem. CATIA allows only the creation of "consistent" solids.
If your body is a surface body, the orientation of the mesh is automatically managed by CATIA during creation. You can see it in the "mesh cleaning" tool "structure" tab and then selecting "orientation". You can then reverse the orientation of certain faces if necessary by clicking the corresponding arrows. In the unlikely event CATIA generates errors during export (complex files), the Sculpteo auto repair tools will be able to repair it automatically because the bodies generated by CATIA are easily adjustable.
CATIA operates on a principle of NURBS, so the generation of triangles occurs only once the mesh is generated, or when exporting. In both cases, the orientation of the triangles is uniform, and there are usually no problems.
Nevertheless, it is possible to use the "mesh cleaning" tool to check that everything is in order. Go to the "structure" tab, check "orientation" and see if blue areas appear on your mesh. If so, click on each of the arrows on the inverted triangles (blue), which then become yellow and click "apply". The affected triangles will be automatically flipped.
Automatic "Mesh cleaner" tool
Run a scan with the mesh cleaning tool, which notifies you of any non-manifold edges or points. If you are in the "suppression" tab, click "apply". Errors are suppressed but can sometimes leave holes in your mesh.
Don't hesitate to run several successive analyses since removing points / edges in the first analysis, can lead to the creation new points / non-manifold edges in a second analysis.
You can then fill using the tool "triangle creation" or "fill holes". If the repairs are fast, use the tool for creating triangles, you will then have to click successively on two edges to form a triangle, which appear in a blue color on your mesh.
Manual cleaning : "Delete points" tool
If you want to manually repair errors, be aware that there is a "striking points" tool in the digitized shape editor workbench. You just have to click the point to delete it, and click "apply". Points and their related edges will be removed.
In case there would be many holes, prefer the automatic hole filling tool
Self-intersections do not generate problems for export, and conversion to STL can take place regardless. It is only when printing that trouble arises. You will need to make sure your surfaces do not overlap. The following tools will therefore help you to precisely select surfaces.
This tool has exactly the same features as the "activate" tool. The difference is that when you click OK after defining the area of interest, the latter is separated from the rest of the mesh. You then get a CutMesh.1 and CutMesh.2 tree that correspond to the selected area and the unselected area.
This tool is the same as the cutting tool in GSD. First selecting the mesh that has to be cut, then the cutting element (which may be a plane, a surface or another mesh). You now have two new elements in the tree. By checking "Overview", a white line representing the cut appears on the mesh.
"Merge meshes" tool
This tool allows you to merge two or more meshes. It is useful when you want to, for example, assemble two meshes on which you want to make a cut or perform any cutting operations.
Multi-shell files are automatically handled by CATIA. You can choose to keep the different bodies at export, obtaining an .stl file for each body, or export a single .stl file containing all the bodies. In both cases, CATIA generates a file ready for 3D printing.
To repeat 3D prints (multiple copies of the same model), the most economical method, is to use the online Sculpteo tool which creates a series or batch (of at least 20 pieces), which will optimise the positioning and price of production.
Transform a 3D scan into a printable model
3D scanning and 3D printing are increasingly linked technologies, there are specific tools in CATIA to transform a 3D scan into a printable model. For this you have to go into the "Digitized Shape Editor" workbench that is in the "shape" menu.
This tool provides an easy and precise way to reduce the number of points from the scan (to reduce the file size). A green sphere appears, and represents the difference between two points. The higher the value, the greater the distance between two points and therefore the lower the number of points in the mesh will be.
After filtering, you obtain a lighter with a reduced number of points, which will depend on the size of the filter you applied.
"Mesh creation" tool
Creating a mesh from a point cloud operates in the same way as earlier, by clicking on "mesh creation", followed by setting the SAG depending on the desired level of accuracy.
- 2.1. Measuring elements and distances
- 2.2. Mesh generation
- 2.3. Mesh analysis
- 2.4. Choose a file format and export your model
- 2.5. Useful tools
- 2.6. Heavy file
- 2.7. Hole filling
- 2.8. Thickness
- 2.9. Normal orientation
- 2.10. Triangle orientation
- 2.11. Non-manifold edges/vertices
- 2.12. Self-intersections
- 2.13. Multishell files