Catia V5 Tutorial: 3D Modeling for 3D printing with Catia V5


1. Catia V5 Models: Design a printable 3D file

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 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.

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.

Catia tutorial image 

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

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.


  • Standard drill


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.

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.

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.

Catia tutorial image 

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.