Featured image of 2019 FreeCAD Tutorial for 3D Printing: 5 Easy Lessons

2019 FreeCAD Tutorial for 3D Printing: 5 Easy Lessons

Rocío Jaimes Gutierrez
Nov 2, 2019

Check out this awesome FreeCAD tutorial where you can easily learn how to create your first design and bring it to life with 3D printing! No CAD or 3D printing experience required.

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Welcome to our FreeCAD tutorial for 3D printing! FreeCAD is a 3D parametric modeling program, designed for creating and customizing real-life objects. The beauty of this program lies in the complete ease with which you can modify your designs, while still being an open-source platform that is completely free to use.

In the 5 lessons of this FreeCAD tutorial, you will learn the basic commands and tools to visualize your ideas on screen, ready for 3D printing. We will show you how to construct a seemingly simple object, step by step, to familiarize you with important features.  By the end of the tutorial, you will be ready to print your first self-constructed CAD model.

After each instruction, you will find pictures that highlight the steps you will need to take.

Lessons

  1. Setup
  2. How to Cut Objects
  3. Fillets & Pattern
  4. The Revolution Feature & How to Cut with Two Objects
  5. 3D Printing

Lesson 1: Setup

In the first lesson of this FreeCAD tutorial, you will learn the basics of handling the program.

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FreeCAD Tutorial for 3D Printing

1.1 Download FreeCAD

Image of FreeCAD Tutorial for 3D Printing: 1.1 Download FreeCAD

To start, you need to first download and install FreeCAD. The program is available for free from FreeCAD.com. There are versions that support Windows (32-Bit, 64-Bit), Mac (64-Bit), and Linux (64-Bit AppImage).

If you want to ensure that FreeCAD is appropriate for your specific project, make sure to visit the FreeCAD forum.

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FreeCAD Tutorial for 3D Printing

1.2 Getting Your Units Right

Before you start with a project you will have to decide what units you are going to use. In this FreeCAD tutorial, we will be using the metric system, which is generally more friendly with the majority of 3D printing software.

When you open FreeCAD, you should see something comparable to this:

FreeCAD tutorial, create a new project
Create a new project.

Click on “Create new”. Now you can set your preferred navigation style. For this tutorial, we will use Blender. Rightclick > Navigation styles > Blender.

The menu allows you to use navigational gestures similar to other CAD programs. This can be useful if you use other software or plan to switch to another program later.

freecad tutorial

You are ready to get going! Follow these steps to change the units.

How to change units in FreeCAD

  1. Click on Edit > Preferences
    Free Cad tutorial
  2. Select General in the popped up window
    freecad tutorial set to English
  3. Go to Units and change the User System to “Standard” and confirm by pressing “OK”
    freecad tutorial metric system
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FreeCAD Tutorial for 3D Printing

1.3 Get Your Views Organized

Now, we will start a new document by pressing CTRL+N. You will see a new, unnamed tab open in the bottom left side of the window.

If the Combo View window on the left is already open, you can skip the next step.

FreeCAD Tutorial

Open the Combo View by clicking on View > Panels> Combo View

freecad turial set combo view

This window is very useful for issuing commands quickly. It also contains the Tree and Property view which allow you to have a closer look at the structure of your project.

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FreeCAD Tutorial for 3D Printing

1.4 Sketch a Base

To build a three-dimensional object, you will first have to sketch a base.

  1. Change your Workbox from Start to Part Design. This will enable the option Create Sketch under the Task tab in our combo view window.
    freecad tutial part design
  2. Make sure you are under the Tasks bar in Combo View. Click on Create body followed by Create sketch. This will pop up a new window, where you can choose which plane to sketch on.
    freecad tutial create body
    Create body
    freecad turial create sketch
    Create sketch

    FreeCAD tutorial create sketch
    Select plane: create a sketch

  3. Now choose the XY-Plane. In the latest FreeCAD release, you can proceed by clicking OK.
    freecad turial xy plane
    If you have an older version, uncheck Reverse Direction and zero the offset. In this window, the cube on the right will show you the selected plane. The Reverse Direction option will switch to the opposite plane. With the option Offset, you can change the height of the plane. Press OK to continue.

    First change your Workbox to Part Design. Then click on Create Sketch.
    First, change your Workbox to Part Design. Then click on Create Sketch.

  4. Under the Tasks bar, new options will pop up. Here we can change the Grid properties. Check all the grid options and set the Grid size to 10 mm. Unchecking “Show grid” will hide the grid and “Grid size” will vary the spacing of the grid. Selecting Grid Snap will automatically snap a point to the closest gridlines.
    freecad turial 10grid
  5. Select the sketch tool Create a Rectangle. When you move your cursor over the coordinate system you can see the current coordinates right next to your cursor. Click on the IV quadrant of the coordinate system (bottom-right quadrant) in the point 40.0, -40.0. You may notice how the points snap to the grid, this lets you work more precisely. Make your rectangle 80.0 x 80.0 (drag and drop the rectangle in -40.0, 40.0).
    freecad tutorial create a rectangle
    Set Grid options and select draw rectangle
    FreeCAD tutorial

    FreeCAD automatically sets constraints to your sketch, which you can see in the Constraints window on the left. Click on Close to exit the Sketch. You can now extrude the sketch to a three-dimensional object.

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FreeCAD Tutorial for 3D Printing

1.5 Setting New Points

  1. Select the Pad command under the Task section in the Combo View.
    Freecad tutorial Pad
    If you don’t see these options, go back to Model and select the sketch. Then move to the Tasks tab.
  2. Set the length to 60mm, the tab to Dimension and uncheck Symmetric to Plane and Reversed.
  3. Length will determine how far your object is extruded. The option Reversed will extrude the sketch in the opposite direction.

freecad tutorial pad options
2nd length will be enabled by switching the Dimension tab to Two Dimensions and will extrude the object on two sides. We will not use this function for our model. Go back to Dimension and click OK.
freecad tutorial pad in two dimesions

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FreeCAD Tutorial for 3D Printing

1.6 Moving Objects & The Different View Windows

Image of FreeCAD Tutorial for 3D Printing: 1.6 Moving Objects & The Different View Windows
Different points of view. 1 Isometric view, 2 Front view.

You can also move the object around and take a look at it from different sides.

  1. Holding the middle mouse button and moving your mouse will rotate the object. Note that this function is available after right-clicking and selecting Blender under Navigation styles.
  2. You can also select different angles of view. The different views can be found in the central row of the FreeCAD toolbar. The axonometric view projects the object to appear as three dimensional. You can also choose to look at one specific side.
  3. If you lose track of your object press on the magnifying glass on the left of the view toolbar. This will center your entire project.
    freecad tutorial handlense
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Lesson 2: How to Trim or Subtract Objects

To begin with Lesson 2 of this FreeCAD tutorial, open the last lesson’s project and switch your Workbox to Part Design. First, we want to hollow out our box with the cut feature.

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FreeCAD Tutorial for 3D Printing

2.1 Basic Trim Tool

Set the dimensions of the Pocket feature found in the combo view.

  1. Select the Top plane by switching to the Top view in the view menu and clicking on the visible face of your box. Now create a new sketch under Task in the Combo View window.
    freecad tutorial
  2. Set your grid to 5mm and check Grid Snap. Now draw a rectangle starting at -35.0, 35.0 and give it the dimensions 70.0 x -70.0. It should offset 5mm from the edges of your box. Click to confirm the rectangle and close the sketch.
    freecad tutorial sketchhole
  3. Continue by clicking on the Pocket feature, under the Pad feature in the Combo View. This feature will cut everything inside your recently drawn rectangle. You can change the direction and the limit the cut in the Type selection. Set Type to Dimension and your length to 55.0 mm so the floor is 5 mm thick. Also, rename the created pocket to “Hole” by pressing F2. When you switch to isometric view you can see the hole in the box.
    freecad tutorial pocket
    freecad tutorial hole

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FreeCAD Tutorial for 3D Printing

2.2 Offset

  1. To keep the lid (which we will create shortly) in place, you will have to create a rim around the top of the box. Switch to the axonometric view and select the Top plane of the box. Do not select the floor or walls of your box! Change the Grid size to 5mm and enable grid snap. Now create a rectangle aligned with the top edges of your box starting at -40, 40.0, close the sketch when finished and rename the sketch to Rim 1. To access the Offset tool, switch your Workbox from Part Design to Draft.
    freecad turorial axiometric view

    FreeCAD tutorial Rim

    freecad tutorial rim ax view
  2. Redefine your working plane by clicking on Set Working Plane and then on the Top plane of your box. A grid should become visible. To show or hide the grid go to Draft > Utilities > Toggle Grid. The height working plane will determine the drafting level. Drafting on different levels will allow you to extrude the drafts into one object.
    FreeCAD tutorial Toggle Grid

    FreeCAD tutorial Toggle grid view
  3. Select the sketch “Rim 1″ in the Model section and select under Task the Offset tool. Check Copy so “Rim 1″ remains after the offset. When using the offset tool it is very important to keep your cursor in the modeling window. You will notice a rectangle following your cursor. Without moving your mouse, type -2.5 and press enter. This will offset your sketch by 2.5mm to the inside. Also, rename “D Wire001″ to “Draft”.
    freecad tutorial offeset
    Modify objects: Offset

    freecad tutorial offeset 2.5
    Set offset.

  4. Disable your Draft grid as shown in 2. and switch your Workbox back to Part Design.
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FreeCAD Tutorial for 3D Printing

2.3 Alternative Method to Trim or Subtract From an Object

  1. Double click on “Rim 1” sketch to edit it. Set your grid to 2.5mm and check Grid Snap. Now draw a second rectangle right on top of “Draft” starting at (-37.5, 37.5) with a dimension of (70,70). Close the sketch. Now you can also delete “Draft” by clicking on it and pressing the delete button.
  2. Select “Rim 1″ again and cut it by using the Pocket feature. Set Type to Dimension and Length to 5 mm. This will cut the space inside the rectangles.
    freecad tutorial rim subtract
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Lesson 3: Fillets & Pattern

In Lesson 3 of this FreeCAD tutorial, you are going to learn how to multiply a piece and make corners round. To begin, open the box you created in Lesson 2.

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FreeCAD Tutorial for 3D Printing

3.1 The Pattern Feature

  1. The Pattern feature distributes an object equally. Before you can pattern an object, you need to create one. In this step, you are going to add little nubs on the bottom of your box. Switch your view to the Bottom and select the visible plane. You should see the bottom of your box. Now create a new sketch on this plane and set your grid size to 2.5mm, also check Grid Snap. Select Create a Circle and draw a circle in the upper right-hand corner of your box at -30.0, 30.0 with a radius of 5mm. Now close the sketch.
    freecad tutorial legs

    freecad tutorial legs coordinates 30,30
  2. Select the sketch drawn in 1. and extrude it with the Pad feature. Set Length to 5mm, uncheck Symmetric to Plane and Reverse. Press OK to finish and rename the pad to “Nub” by pressing F2.
    freecad tutorial pad legs

    freecad tutorial nub
  3. Now click on “Nub” again and select the Polar Pattern feature. Set Angle to 360.00, Occurrences to 4 and uncheck Reverse Direction. This tool creates a circular pattern of a part with a specific angle and occurrences. The angle determines the size of your pattern. For example, at 360° the objects will be arranged in a full circle, at 90° only inside a quarter of a circle. With Reverse Direction checked your pattern will go around clockwise.
    freecad tutorial nub polar patterns

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FreeCAD Tutorial for 3D Printing

3.2 The Fillet Feature

Now we will create a fillet from the circle pads with the radius of 2.4mm.

  1. Switch to bottom view and select all the Nubs. To select many parts hold down CTRL and click on different parts. To unselect a part just click on it again.
  2. Now select the Fillet feature. The adjustable radius determines the size of your fillet. The radius has to be smaller than the entity you create a fillet so set the radius to 4.9mm. The result should look like little knobs. Close the feature and rename the fillet to “Nub1″.
    freecad tutorial fillet 4.9
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FreeCAD Tutorial for 3D Printing

3.3 How to Give Corners a Fillet

First, create a rectangle on the existing rim. Cut it by 2.5mm and then select the outward rim of your box to create a fillet.

  1. Switch to top view and create a new sketch on the rim you created in Lesson 2.
  2. Now draw a rectangle on the right side starting at 35.0, 37.5 and make it 2.5 x -75.0. Exit the sketch and proceed to the next step.
  3. Create a new pocket with the sketch from 1., set the length to 2.5mm and uncheck reversed. Also, rename the pocket to “SmallRim”.
    freecad tutorial upper view fillet 2.5
    Draw a small rim by sketching a rectangle on the right side of the box.

    freecad tutorial smallrim
    A fillet will be made in the next step on the with the newly drawn rim.

  4. Now click on the outer edge of SmallRim and click on the Fillet feature. Set the radius to 2.4mm.

    freecad tutorial small rim applied
    Make a fillet with a 2.4mm radius.

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Lesson 4: The Revolve Tool & How to Trim or Subtract Surfaces with Two Objects

In lesson 5 of this FreeCAD tutorial, you will create the cover of your box. The cover will be curved and hollowed out with the Revolution feature. No, you are not going to overthrow a government, but you will create a solid curved shape around a sketch. To begin, open a new document and save it as “Box cover”. Then switch your Workbox to Part Design.

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FreeCAD Tutorial for 3D Printing

4.1 The Revolve Tool

  1. Create a new sketch on the XY-Plane, draw a rectangle starting at -40.00, 40.00 and make it 80.00 x -80.00. Rename the sketch to “Base”. This will be a new, independent body.
    freecad tutorial lid sketch
  2. Now extrude the sketch to 5mm height and rename it to “Base”. When finished, start a new sketch on top of the extruded box. Draw another rectangle starting at -40.00, 40.00 and make it 80.00 x -40.00. Rename it to “Base of Revolution”.
    freecad tutorial lid pad
    Extruded base

    freecad tutorial lid sketch revolution
    Sketch of the revolution

  3. To create a revolution click on ‘Base of Revolution’ first and then on the Revolve a Sketch feature. Set Axis to Horizontal Sketch Axis and Angle to 180°. Uncheck Symmetric to Plane and Reversed. Symmetric to Plane will equally distribute the feature on each side of the sketched plane.
    freecad tutorial lid revolution
  4. Hide the revolution you created in 3. by clicking on it in the Model view and pressing your spacebar. Now create a new sketch on top of the ‘Base’ extrusion. Set your grid to 2.5mm and draw a rectangle at (-37.50, 37.50) and make it 75.00 x -37.50. Create a new Revolution feature. Set the Axis to Horizontal and Angle to 180°. Uncheck Symmetric to Plane and Reversed.
    freecad tutorail second revolution sketch
    Inner sketch of your lid.
    freecad tutorial lid second revolution pad
    inner pad of your lid

    freecad tutorial second revolution lid
    Inner revolution. This object will be used to create a pocket in your lid, giving the box a larger space and using less filament when 3D printing.

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FreeCAD Tutorial for 3D Printing

4.2 Trim or Subtract Surfaces with Two Objects

  1. Switch your Workbox to Part and select Run a Boolean operation. Check Difference in the Boolean operation window. This will subtract the second shape from the first shape. Union will combine two objects, Intersection will extract the common part of two objects and Section will extract the common part of two objects as a non-solid.
    freecad tutorial lid cut
  2. The first shape should be your first revolution. This must be the largest revolution of the two. The second shape will be your smaller revolution. Click on Apply to confirm the subtraction.
  3. To finish we will create a new sketch at the bottom of ‘Base Extrude’. Draw a rectangle starting at -37.50, 37.50 and make it 75.50 x -75.50. Cut the sketch by a length of 5mm with the Cut feature.
    freecad tutorial lid final
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Lesson 5: 3D Printing

Now, you should be all set to 3D print your model.

If you don’t own or have access to a 3D printer, you always can use a 3D printing service like the ones that you find here: Craftcloud, the 3D printing and price comparison service from All3DP.

Be aware that minor modifications might be needed to tackle problems that may arise during the 3D printing process.

  1. You will probably need to add supports. The contact area between the print and the bed is only that which you added in the nub (unless you change the print orientation). Hence, expect that your print won’t adhere flawlessly without increasing the contact surface. You can also try setting your fillet in step 3.2 to 4.5 mm.
  2. You will need to support bridges. The distance between the nubs is far too long for the bottom of your box to hold firm.
  3. Remember to print both models at the same scale to ensure a perfect fit between the lid and the body.
  4. Post-processing the box can include polishing the surface and adding a hinge to hold your box open.
    3D printed box and rim
    3D printed box and rim
    3D printed box and lid.
    3D printed box and lid.

    Printed properly, the lid should fit perfectly on the box.

Playing with print orientation will lend different results, decide for yourself what you like best!
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Wrapping up

Congratulation on completing this FreeCAD Tutorial for 3D Printing!

If you have any questions or problems regarding this FreeCAD tutorial, please do not hesitate to leave a comment. Also, if you want to add suggestions for this course, please use our feedback forum – thanks!

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License: The text of "2019 FreeCAD Tutorial for 3D Printing: 5 Easy Lessons" by All3DP is licensed under a Creative Commons Attribution 4.0 International License.

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