FreeCAD v1.0 2025 Ultimate Beginners Course Extended Version

Think of FreeCAD like a fabrication shop, with multiple workbenches, each equipped with specialized tools. While these workbenches can function independently, they often interact to create a seamless workflow.

You can access the workbenches from the drop-down menu in the top toolbar. FreeCAD offers a variety of workbenches, including:
Assembly workbenches for complex designs
CAM workbench for CNC machining
Drafting workbench for 2D drawings
Part Design workbench for parametric modeling

The Part Design workbench is ideal for beginners because it guides you through a structured, linear workflow. In this course, we’ll focus on three essential FreeCAD workbenches:
✅ Sketcher Workbench – for creating geometry
✅ Part Design Workbench – for performing design operations

✅ Assembly Workbench – for creating Assemblies and Sub Assemblies.

By mastering these, you’ll be able to create precise and functional 3D models with confidence!

The FreeCAD workspace consists of toolbars and panels that help you navigate and create your 3D models efficiently.

Creating a New Document & Understanding the 3D View

When you create a new document, you’ll notice the 3D View panel—this is where your model takes shape. On the left-hand side, you’ll see several panes:
Model pane – Contains your project structure
Task pane – Displays options for active tools
Two tabs beneath the Model pane for additional settings

You can rearrange panels by clicking and holding the Task pane, then dragging it to a new position. To save space, you can combine panels by hovering over the left side until the area highlights in blue, then releasing the mouse button.

Troubleshooting Hidden Panels & Dividers

If a panel disappears, it’s often due to the divider being moved too far down. To restore it:
✅ Hover over the divider until it’s visible
✅ Click and drag upwards to bring the pane back

Entering Full-Screen Mode & Managing Report View

To maximize your workspace, go to:
View → Full Screen

You may also see the Report View panel at the bottom. If you don’t need it:
Disable it via View → Panels → Report View
To prevent error messages from constantly appearing, go to Edit → Preferences → General, then uncheck:
✅ Show Report View on Error
✅ Show Report View on Warning

With these settings adjusted, you're now ready to explore 3D navigation in FreeCAD!

To begin navigating the 3D view in FreeCAD, you first need to choose your preferred navigation style. You can select it from the drop-down menu. If you're transitioning from another CAD software, you can use familiar keyboard shortcuts and mouse movements—for example, styles similar to Blender or TinkerCAD.

Personally, I prefer the touchpad control style. Once selected, the drop-down will change to Touchpad, and when you hover over it, you'll see the control instructions. This style is perfect for laptop users with touchpads, but you can also use your mouse.

3D View Controls

Let’s go over the basic controls to get comfortable navigating your model in the 3D view:

Zoom
To zoom in and out, use the touchpad or mouse wheel. You’ll notice the scaling changing on the right-hand side of the screen as you zoom.

Rotate
To rotate the model, hold down the Alt key and move the mouse. A rotate icon will appear, and the center of rotation will be indicated in pink. You can rotate your model up, down, left, and right.

Pan
To move the model around the screen, hold Shift and move your mouse. This will allow you to pan your view left and right.

3D Cube & Axis
On the top-right corner, you’ll notice a 3D Cube. As you rotate your model, the cube rotates with it, helping you understand your model’s orientation. Below the cube, there’s an axis showing the X, Y, and Z coordinates.

Customizing the Interface

You can modify the 3D view interface to better suit your needs. Go to:
Edit → Preferences
Then, under the Display tab, click 3D View to adjust the coordinate system and other widgets such as the 3D cube.

To make the coordinate system more visible:
✅ Increase its size by 30% and click Enter.

Using the 3D Cube

The 3D cube is a handy tool for quickly selecting different views.
Click on the cube to switch between Top, Front, Right, etc.
You can also rotate the cube by holding Alt and moving the mouse.
Use the arrows to change perspectives, or click the edges of the cube to jump directly to those views.

At any time, you can hit the Home key to reset your view.

To get started, we’re modeling in the Part Design Workbench. If you haven’t selected it already, go ahead and choose it from the drop-down menu. Once selected, the Part Design toolbar will become active.

Creating a Body

In Part Design, every part you create is contained within a Body. This is essentially a container that holds your part. Once you create a body, you’ll notice that in the Tree View (on the left side), the Body will appear.

? Origin Visibility
Inside the Body, you’ll find the Origin, which contains the planes and axes for your design. However, you might not see the Origin at first. Here’s how to make it visible:
✅ Click to unselect the Body – This will make the Origin appear in bold in the Tree View.
✅ To toggle visibility, click the eye icon beside the Origin or simply press the Space bar when the Origin is selected.

By clicking on some blank space in the workspace, you can now see the planes and axes of the Origin.

Activating the Body

You’ll notice that the active Body is highlighted in bold in the Tree View. If it's not showing as bold, double-click on the Body or right-click and make sure that the active body is checked.

This makes the body the focus for the operations you’ll perform next in your design.

In FreeCAD, sketches are the foundation of most parts in the Part Design Workbench. Let’s dive into creating our first sketch.

Creating a Sketch

To create a sketch, simply select the Sketch icon from the Part Design toolbar. FreeCAD will prompt you to attach the sketch to a plane. You can select the plane by clicking directly on the screen or choosing from the panel on the left. For this example, let’s select the XY plane and hit OK.

You’ll now see that the Navigation Cube shows the Top view, and the XY plane becomes visible. By default, the plane is invisible, but since we’ve revealed it in the Tree View, it’s now shown. You can toggle its visibility by clicking it and pressing the Space bar.

Repositioning the View

FreeCAD will automatically adjust your view to be perpendicular to the plane you selected. You can reposition the view using your navigation shortcuts. To view them, roll over the navigation drop-down at the bottom. If you want to change angles, use the shortcuts or rotate the view as needed.

Now, let's begin sketching the geometry for our base plate. We'll draw one side and later use the Mirror operation to duplicate it. The Mirror is just one of many tools in Part Design, and it’s a great way to demonstrate symmetry.

• The red line represents the X-axis (horizontal), and the green line is the Y-axis (vertical).

• These axes intersect at the origin, the center of the Body.

Creating a Rectangle

Select the Rectangle tool from the toolbar. Move your mouse to the center of the 3D view, and you’ll see the coordinates displayed on the right-hand side. As you move closer to the Y-axis, the numbers will decrease to zero and increase as you move to the right.

Now, let’s create our rectangle:

1. Position the mouse around -50 mm on the X-axis and click once to set the starting point.

2. Move down to draw the rectangle and, before clicking again, enter 50 mm for the top dimension and 50 mm for the side dimension. Press Tab to switch between the dimensions, then hit Enter to set them. The rectangle is now dimensioned.

Constraining the Sketch

You’ll notice that the rectangle has degrees of freedom (DOF), meaning it can still be moved. Our goal is to fully constrain the sketch, which means all its points and dimensions are fixed.

• Add a Symmetry Constraint: Select the top point of the rectangle (highlighted in green), and then select the middle point (origin). This makes the top points symmetrical along the horizontal axis. Once done, the sketch will turn green, indicating it’s fully constrained.

Adding Fillets and Constraints

Next, let’s round off the corners using a Fillet:

1. Select the Fillet tool from the toolbar (right-click if you can’t see it).

2. Hover over one line, click once, then hover over the other line and click again to create the fillet.

Now, let's apply a radius to the fillet:

1. Select the Dimensioning tool, then click on the fillet to set its radius. Enter 10 mm and hit Enter.

To ensure symmetry between the two fillets, we’ll make them equal:

1. Select one fillet edge, then the other. Use the Equal Constraint to ensure both fillets have the same radius.

Now the fillets are fully constrained, and the sketch is complete!

Adding Holes

Next, we’ll add holes to our design. We’ll use circles to create two holes:

1. Select the Circle tool and hover over the fillet’s center to snap to the coincident constraint.

2. Draw the circle, then select the other point to add a second circle.

3. Use the Equal Constraint to make the circles the same size, then apply the Dimensioning tool to set their diameter to 10 mm.

Once we’ve applied the constraints, we can move on. Everything is now fully constrained, meaning the sketch is locked in place.

Saving the Project

Now that we’ve created our first sketch, let’s save the project:

1. Go to File → Save and name the file Base Part. Hit Enter.

Congratulations, you’ve just completed your first fully constrained sketch in FreeCAD’s Part Design Workbench!

To create volume in FreeCAD, we can use additive operations. These are extrusion tools that convert a 2D sketch into a 3D object by extruding it in different directions. The most basic of these tools is the Pad, which extrudes your sketch in a straight direction.

Using the Pad Tool to Extrude a Sketch

Before we begin, make sure that the sketch you want to extrude is selected. You can do this by clicking on the sketch in the Tree View. Once selected, click the Pad operation in the Part Design toolbar.

The length of the extrusion is controlled by the length parameter. For this example, let's set the length to 5 mm. Once you’ve entered the desired value, click OK.

Understanding the 3D Update

After clicking OK, you’ll see that the model has been updated in the 3D View. The Pad tool has extruded the sketch by 5 mm, adding volume to your part. This creates a feature in the model.

Tracking the Operation in the Tree View

On the left side, in the Tree View, you’ll see an icon next to the Pad operation. This icon represents the Pad feature. This is called a Tip. Each time you add an operation, a new icon will appear in the Tree View in a linear order. The Tip will move to the next icon as you add more features to your part.

In FreeCAD, volume can also be removed from a design using subtractive operations. The Pocket operation is used for this purpose. Instead of adding material to the shape like the Pad tool, Pocket removes material, creating cutouts in your design.

Setting Up the Pocket Operation

For this example, we need to clear out a section on the top of an existing feature. It’s crucial to look at the shape from different viewpoints to properly envision how the pocket will be sketched. If we examine the cross-section of the part, we see it’s a single profile.

1. Select the Face for the Sketch
   Start by selecting the side face of your existing feature. Next, click New Sketch to begin a new sketch on this selected face.

2. Attaching the Sketch to the Face
   After selecting the face, the Task View will show the sketch attached to the flat face in Map Mode. This means that your new sketch is now mapped directly to the face of the object, ready for modifications.

Sketching the Profile for the Pocket

Now, let’s begin sketching the profile for the pocket:

1. Importing External Geometry
   In the Task View, use the External Geometry tool to import the top edge of the part. This tool allows you to constrain geometry from the imported edge to build your profile.

2. Drawing with Polyline
   Using the Polyline tool, sketch the profile you want to subtract. Start by aligning it to the vertical axis and connecting the lines at angles. Use the Point-on-Object constraint to attach the sketch to the imported geometry, ensuring proper alignment.

3. Constraining the Geometry
   After the geometry is complete, use the Dimension tool to set precise measurements. Set the height of the vertical line and other dimensions to fully constrain the sketch. The goal is to ensure your sketch has zero degrees of freedom, meaning it’s fully constrained.

Performing the Pocket Operation

Once your sketch is ready and fully constrained, it’s time to use the Pocket tool to subtract material:

1. Selecting the Pocket Operation
   With the sketch selected, click the Pocket operation from the toolbar. This operation removes material along the defined profile.

2. Setting the Pocket Depth
   Instead of manually typing the pocket depth, choose the option to remove material through all. This ensures that the pocket cuts through the entire length of the part.

3. Finalizing the Pocket
   Once you’re satisfied with the preview, click OK to finalize the operation. This removes material from the top section of the feature, leaving you with a clean pocket.

Conclusion

We’ve successfully used the Pocket operation to subtract volume from our design. This is the final step in creating a pocket, and now your design has a neat cutout as part of the overall geometry.

In FreeCAD, it's a good practice to rename the body to make it more descriptive and easier to manage, especially in complex designs.

Renaming the Body

1. Right-Click to Rename
   First, locate the body in the Tree View. Right-click on it and select Rename from the context menu. For clarity and better organization, rename it to something more descriptive, such as Base.

2. Adding Comments for Clarity
   You can also add a description to the body that will be displayed in the Tree View. This is particularly useful if you are working on larger projects with multiple parts. To enable this feature:

   • Right-click in the Tree View and select Tree Settings.

   • Then, choose Show Descriptions to activate the description column.

Editing the Description

1. Adding a Description
   Once the Description column is visible, click on the body (in this case, the Base body). Make sure the cursor is placed in the Description field.

2. Edit the Description
   Press F2 on your keyboard to start editing the description. For version control, you can type something like Version 1.0, which helps keep track of different versions and revisions of your model.

3. Saving the Description
   Once you've entered the description, hit Enter to save it. Now the Base body has a clear, descriptive label with a version number visible in the Tree View.

Conclusion

Renaming bodies and adding descriptions in FreeCAD is a great way to keep your project organized and easy to understand, especially when collaborating or revisiting your work later. With these simple steps, you can streamline your workflow and manage complex designs with ease.

In FreeCAD, mirroring is a useful operation to duplicate and reflect parts across a specific plane. Here's how you can mirror your base part across the desired axis.

Mirroring the Base Part

1. Select the Base
   Start by selecting the base you want to mirror. In the Tree View, you can easily select the entire base. However, there are other ways to select features. If you click on blank space, it will unselect everything, allowing you to select specific elements like faces or features individually.

   • Click once on the face to select it.

   • Clicking again selects the entire feature, and a third click will select the body itself.

2. Using the Mirror Tool
   Once the body is selected, click on the Mirror tool in the toolbar. FreeCAD will prompt you to choose whether to mirror the body or the tool shapes.

3. Select the Mirrored Object
   Since you want to mirror the entire body, ensure you select the body option. The model will now be mirrored, but it may be in the wrong plane.

4. Adjust the Mirror Plane
   You’ll need to adjust the mirror plane. By default, it might mirror along the wrong axis. To correct this:

   • In the Plane dropdown, choose YZ to mirror the part across the YZ plane.

5. Finalizing the Mirror
   Once you’ve set the correct plane, hit OK to accept the mirrored part. You’ll now have an exact duplicate of your base part, mirrored across the YZ plane.

Conclusion

Using the Mirror operation in FreeCAD makes duplicating and creating symmetrical parts quick and efficient. Whether working on assemblies or individual features, this tool saves time and helps maintain design consistency. With these steps, you'll be able to create fully mirrored parts with ease!

When working in FreeCAD, there are several ways to start a new part. You can either create a new file or continue from your existing one. In this guide, we'll explore how to add a new body to your current project and sketch a part.

Step 1: Hiding the Current Part

Before you start creating a new part, it’s advisable to hide your existing body. Select the body in the Tree View and press the spacebar to hide it. This will help you focus on the new part you're creating.

Step 2: Creating a New Body

Now, create a new body for your part:

1. Create New Body
   Click the Create New Body button. This new body will be bolded, indicating it’s the active body. Any new sketches or operations will apply to this active body.

2. Sketching on the XY Plane
   To begin your new sketch, choose the XY plane. The dimensions of your part will be 25 mm by 50 mm.

3. Scaling the View
   Use the zoom shortcuts to scale your 3D view and get the right proportions for your part. Adjust the view until the model appears correctly.

Step 3: Creating the Sketch

1. Using the Polyline Tool
   You can use the Polyline Tool (M key) to create the sketch. Begin by selecting the vertical axis and clicking once to start your line. Draw out the shape by cycling through the different drawing modes (pressing the M key). You'll alternate between straight lines and arcs.

   • Arc: After drawing a line, hit M to switch to an arc mode. Create an arc by clicking twice and adjusting the shape as needed.

2. Adding Constraints
   After creating the basic shape, it's time to add constraints:

   • Horizontal/Vertical Constraints: Apply constraints to ensure that lines are straight and properly aligned.

   • Tangency Constraint: Use the Tangency Tool to make lines smooth and curve into arcs seamlessly.

   • Equal Constraint: Make sure arcs and lines are symmetrical or equal in size.

   • Symmetry Constraint: Ensure certain features are mirrored over a reference point (e.g., the vertical axis).

3. Dimensioning
   Next, use the Dimension Tool to set the required dimensions. Set the overall width to 25 mm and the height to 50 mm. Dimension the circles and arcs as needed (e.g., radius of 10 mm for the arc).

Step 4: Completing the Sketch

1. Finishing the Sketch
   After you have added all the constraints and dimensions, check that the sketch is fully constrained (green). Once done, close the sketch.

2. Padding the Sketch
   With the sketch selected, use the Pad Tool to extrude the shape. Set the Pad Length to 5 mm.

3. Rename the Body
   To keep things organized, right-click on the body and rename it to something descriptive (e.g., "Base").

Step 5: Adding a New Bracket

Now that the base part is created, let’s move on to the bracket.

1. Create New Sketch on a Face
   Select the face of the base part where you want to attach the bracket sketch. Click New Sketch and attach it to the selected face.

2. Import Geometry
   Use the External Geometry Tool to import reference points from the base part. These points will help you constrain the sketch accurately.

3. Creating the Bracket Shape
   Use the Line Tool and Arc Tool to sketch the bracket's profile. Again, use constraints (tangency, vertical, etc.) to ensure the bracket fits properly with the base part.

4. Dimension the Bracket
   As before, use the Dimension Tool to set the appropriate distances and sizes for the bracket. For example, set the radius of arcs and the distance between the bracket's points.

5. Pad the Bracket
   After completing the bracket sketch, use the Pad Tool to extrude it. Set the desired length for the bracket (e.g., 5 mm). You may need to reverse the direction of the pad if it’s not in the correct orientation.

Step 6: Finalizing the Design

1. Rename the Bracket Body
   To keep your project organized, right-click on the bracket body and rename it to "Bracket".

2. Save Your Work
   Don’t forget to save your work before moving on to the next steps.

Conclusion

You’ve now successfully created a new part, including a base and a bracket, and added sketches, constraints, and pads to it. By using tools like the PolyLine, Arc, and Pad, and organizing your parts in bodies, you can efficiently create and manage complex designs in FreeCAD.

Although gussets and ribs do not have dedicated operations in FreeCAD, they can easily be modeled with some thoughtful sketching techniques. Let’s walk through the process of creating a gusset using external geometry and applying a chamfer as a dress-up operation.

Step 1: Selecting the Face and Creating the Sketch

We’ll begin by creating a gusset that runs along a face and across the bottom of a part.

1. Select the Face
   Click on the face of the object where the gusset will be placed. This will be the face to which the gusset will be attached.

2. Create a Sketch
   Once the face is selected, create a new sketch mapped to this face. The sketch will intersect with the bottom of the object.

3. View Section Tool
   To see the entire sketching plane more clearly, use the View Section Tool. This will help visualize how the gusset interacts with the rest of the geometry.

Step 2: Importing Geometry and Sketching the Gusset

Next, we’ll import geometry and create the sketch for the gusset:

1. Import External Geometry
   Switch to the left view and use the Create External Geometry Tool to import the line of the face you are working on. This line will serve as the reference for your rectangle.

2. Create the Rectangle
   Use the Rectangle Tool to draw a rectangle starting at the imported geometry. Attach one of the points of the rectangle to the line using the Point on Object Constraint.

3. Add Constraints

   • Select the top two points of the rectangle and then the vertical axis. Use the Symmetry Constraint to center the rectangle along the vertical axis.

   • Apply the Dimensioning Tool:

     • Set the top line dimension to 5 mm.

     • Set the vertical line dimension to 20 mm.

4. Fully Constrained Sketch
   Once your dimensions are set, the sketch will be fully constrained. Now, you can close the sketch.

Step 3: Padding the Gusset

1. Pad the Sketch
   With the sketch selected, use the Pad Tool to extrude the gusset. Set the Pad Length to 20 mm to extend the gusset outward from the face. This creates the gusset.

2. Automatic Face Merging
   Notice that the newly created gusset may merge with the previous face. FreeCAD automatically refines the feature, merging these faces.

Step 4: Creating an Angled Cutout with a Chamfer

Now, let’s add an angled cutout on the top edge of the gusset using a chamfer.

1. Select the Edges
   Choose the top edge of the gusset and the adjacent edge where you want the chamfer to be applied.

2. Apply the Chamfer
   Click on the Chamfer Tool. As you adjust the chamfer size, you’ll see material being removed from the edges.

3. Adjusting the Chamfer

   • Increase the chamfer size and notice how the chamfer moves along the edges.

   • If you try to set the chamfer size to 20 mm, you may encounter an error because the chamfer would cross the edge. To resolve this, reduce the chamfer size slightly (e.g., 19.99 mm) to avoid the issue.

4. Finalizing the Chamfer
   Once the chamfer is correctly applied, click OK to finalize the operation. Your gusset is now complete with the angled cutout.

Step 5: Modifying the Pad and Dealing with Parametric Modeling

1. Modifying the Pad Length
   Since FreeCAD uses parametric modeling, you can modify previous operations. For example, if you change the pad length from 20 mm to 23 mm, everything should update without issues.

2. Handling Errors
   However, if you change the pad length to 18 mm, you might encounter an error with the chamfer, indicated by an exclamation mark. This happens because the chamfer crosses the edge where it should not.

3. Fixing the Error
   To fix this, cancel the chamfer operation and reset the pad length back to 20 mm. This resolves the issue and allows you to continue working on the model.

Step 6: Saving the Model

Once the gusset and chamfer are properly set, don’t forget to save your work.

Conclusion

By following these steps, you've successfully created a gusset using external geometry, added constraints, padded the sketch, and applied a chamfer as a dress-up operation. We also discussed how to handle parametric modifications and errors in FreeCAD, helping you build a robust part.

In this method, we create the gusset in one go using a single sketch, reducing the number of operations and simplifying the model's design.

Step 1: Opening the Base Part and Setting the Active Body

1. Open the Base Part
   Upon opening the part, you’ll notice that there are two bodies in the document: bracket and base. The base body is hidden by default.

2. Activate the Bracket Body
   Since there are multiple bodies, FreeCAD will prompt you to select an active body when starting a new operation. To avoid this, double-click the bracket in the tree view, which will activate it and show it in bold.

Step 2: Deleting Unwanted Features

1. Remove Previous Features
   Delete the previous chamfer and pad operations to reset the design and start fresh. With the pad deleted, the sketch becomes free, and you can delete it as well.

2. Plan the New Sketch
   You will now create a triangle-shaped gusset that will be padded from a central point.

Step 3: Creating the Sketch on the XZ Plane

1. Selecting the Right Plane for the Sketch
   You will need to create the new sketch on the XZ plane:

   • You can create the sketch by selecting the XZ plane directly (if nothing is selected), which attaches to the base plane of the active body.

   • Alternatively, you can choose an existing face of the model (like the face of the pad) to attach the sketch. In this case, select the face and create a new sketch attached to it.

2. Understanding the Sketching Plane Orientation

   • In FreeCAD, the Z axis is normal to the sketching plane, and the X and Y axes follow the direction of the view. Ensure that the sketch plane aligns properly with the geometry.

3. Adjust the Attachment

   • After attaching the sketch to the face, check the attachment settings. You may need to adjust the Z-axis offset to position the sketch properly.

   • Set the Z-offset to -25 mm to position the sketch in the right place relative to the model.

Step 4: Using the View Section Tool for Better Visualization

To sketch easily with a clear view of the area, use the view section tool to cut through the volume in front of the sketch plane. This helps you view the area inside and ensure proper alignment while creating the gusset.

Step 5: Sketching the Gusset

1. Importing External Geometry

   • Use the Create External Geometry Tool to import the lines you need for the gusset. This helps you align your new sketch with the existing geometry.

   • Attach the geometry from the face and use the point-on-object constraint to define the relationships between the lines.

2. Creating the Triangle Shape

   • Use the polyline tool to create the triangular shape for the gusset. Attach the endpoints of the polyline to the external geometry using coincident constraints.

   • Close the shape and apply a horizontal/vertical constraint to ensure proper alignment.

3. Fully Constraining the Sketch

   • Add a dimension to the height of the triangle to fully constrain the sketch (e.g., set the height to 25 mm).

   • After dimensioning and fully constraining the sketch, you can proceed to create the pad.

Step 6: Padding the Gusset

1. Pad the Sketch

   • With the sketch selected, apply the pad operation. Set the pad length to 5 mm.

   • Select the option to make the pad symmetric to the plane so that the gusset will extend equally on both sides of the sketching plane.

2. Adjusting the Pad Length

   • You can change the length of the pad to adjust the gusset size. For instance, set the pad to 15 mm for a larger gusset.

   • If needed, undo any changes by pressing Ctrl + Z to revert to the previous state.

Conclusion

By following this alternative approach, you've created a gusset in a much simpler way, using a single sketch and reducing the number of operations. This method not only simplifies the design but also helps in reducing potential issues and improves the stability of the model.

In FreeCAD, changing the appearance of parts, whether by adding materials or adjusting colors, is a great way to visually differentiate components, especially when preparing for presentations or visualizing the design.

Methods for Changing Appearance in FreeCAD

1. Applying Materials (Appearance):

   • Step 1: With the base part file loaded and the bracket as your active body, right-click on the model in the tree view.

   • Step 2: From the context menu, select Appearance (not Material). The Appearance window will appear on the left, showing a list of available materials.

   • Step 3: Choose a material (e.g., Aluminum), and you will immediately see the appearance change in the 3D view of your part.

   • Step 4: After selecting the material, simply close the Appearance panel to apply the changes.

2. Changing Appearance for Another Part:

   • Step 1: If you want to change the appearance of another part (e.g., the base plate), click on the base plate in the tree view.

   • Step 2: Press the space bar to hide or unhide parts and toggle visibility if necessary.

   • Step 3: Right-click on the base plate and choose Appearance again.

   • Step 4: In the Appearance panel, select a different material such as Chrome to apply a new appearance. Close the panel after applying.

3. Adjusting Colors:

   • Step 1: Select the part you'd like to color (e.g., base plate).

   • Step 2: In the View tab, scroll down to Shape Appearance and expand it.

   • Step 3: Click on the Diffuse Color field, which allows you to modify the object's color.

   • Step 4: In the color panel that pops up, select a color of your choice, and click OK to apply it.

This process can make your design more aesthetically pleasing or just help differentiate parts during your design process.

In this video, you'll explore the key differences between two widely used file formats in the world of 3D design and printing: STL and STEP. Whether you're a beginner or experienced in 3D printing and CAD modeling, understanding the nuances of these formats is crucial for choosing the right one for your projects.

Exporting models in FreeCAD is a straightforward process, but there are some important details to keep in mind depending on the format and your workflow.

How to Export Models from FreeCAD:

1. Select the Body to Export:

   • Step 1: In the Tree View, select the body you want to export.

   • Step 2: Go to File in the menu bar and select Export.

2. Choose the Export Format:

   • Step 3: In the Export dialog, you'll see a dropdown with various file formats, including STEP, STL, and more.

     • For 3D printing, STL is commonly used.

     • For CAD interoperability, STEP is a good choice.

   • Step 4: Select the format you want (e.g., STL) and hit Save.

3. Importing Exported Files:

   • Step 5: If you'd like to check the exported file, go to File → Import, select your exported file (e.g., STL), and open it.

     • You will now see the imported model in the Tree View. You can hide or show components using the spacebar.

4. Exporting Different Stages of the Model:

   • Step 6: You can export your model at various stages. For instance, if you're working on different features (like a pad, chamfer, or other operations), you can export the model after each operation.

   • Step 7: Right-click the part (e.g., pad) in the Tree View, press the spacebar to show it, then export the model at that stage.

     • Each time you export, the features up to that point are included in the exported file.

Exporting Multiple Parts Together:

1. Selecting Multiple Parts:

   • Step 1: You can export multiple parts at once by selecting them. Hold Ctrl and click to select multiple components in the Tree View (e.g., base and bracket).

   • Step 2: With both parts selected, go to File → Export.

   • Step 3: Name the export file and click Save.

2. Importing Multiple Parts:

   • Step 4: When you import this file back into FreeCAD, you’ll see both parts embedded together inside the STL as separate components.

Handling Meshes:

1. Mesh Workbench:

   • Step 1: After exporting and importing the mesh, you can use the Mesh Workbench for advanced operations on the mesh.

   • Step 2: If you want to split components within the mesh, select Meshes → Split by Components.

   • Step 3: This will break the mesh into separate components, allowing you to manipulate each one independently. You can also use Transform to adjust each component's position.

Things to Keep in Mind:

• File Extensions: Some file formats can have multiple extensions. For example, STL might be saved with .stl or .STL. Ensure you select the correct extension for your needs.

• Mesh Visualization: When you import a mesh, it will appear in the Tree View. If necessary, you can delete the mesh or transform it into separate components.

• Exporting Operations: Exporting at different stages of your design can be useful for version control or when you need to see how a design looks at specific operations (e.g., after the chamfer operation).

This process allows you to create step-by-step exports, keep track of different iterations, and ensure you can share your designs across different software tools or 3D printers.

In this lesson, we’ll explore a different operation in Part Design—extruding material in a circular fashion using a profile. This technique is called a revolve.

Instead of creating a new body in the same project, we’ll start a new document. This will help us understand how to combine multiple files into one assembly later.

Setting Up the Sketch

1. Ensure we’re in Part Design mode from the dropdown.

2. Create a new body and a new sketch.

3. Sketch from the side using the polyline tool, focusing on a quarter cross-section of the part.

The full height of the sketch is approximately 10 mm, so we’ll scale out for better visibility. We’ll revolve the material around the X-axis, leaving a void in the center.

Drawing the Sketch

• Start away from the axis to create the necessary gap.

• Draw a 10 mm line, then zoom in if needed.

• Extend 2.5 mm outward while ensuring horizontal and vertical constraints apply automatically.

• Draw upward by 5 mm, then close toward the vertical axis to complete the profile.

• Right-click to cancel the tool.

Applying Dimensions & Constraints

1. Use the dimension tool to set the top length to 5 mm.

2. Set the horizontal segment to 2.5 mm.

3. Define the center gap for the revolve by setting the distance to 2.5 mm, creating a 2.5 mm radius hole when revolved.

4. Select all three lines and use the equal constraint to maintain proportionality.

Revolving the Sketch

1. Close the sketch and toggle the axis cross in View to see the revolve direction.

2. Select the sketch and choose the Revolve operation.

3. By default, it revolves around the Z-axis, but we need the horizontal axis. Adjust the settings accordingly.

4. We can also select the Base Z, X, or Y planes if needed.

Finalizing the Bushing

• Click OK to complete the revolve.

• Right-click on the body, select Rename, and change it to "Bushing".

• Save the part as "Revolve Parts", as we’ll be using this technique for upcoming components.

That’s it! We’ve successfully created a bushing using the revolve tool. Now, let’s move on to the next part of the design! ?

In this lesson, we’re going to create an axle by starting with a new body. First, click on the bushing and hide it by pressing the space bar.

Next, let's create a new sketch and zoom out. Remember, we can use the home key to reposition. Select the XZ plane for this sketch.

Now, let’s explore a different tool for the axle—the trim tool. We'll revolve this shape around the horizontal axis. Place the rectangle coincident to that line, then set the dimensions:

• Length: 60 mm (press Tab)

• Width: 2.5 mm (press Enter)

Zoom in to check the shape. Right-click, then select the center origin point and apply a symmetrical constraint.

Adding Another Rectangle

Now, let’s add another rectangle:

• Hover over the bottom line of the first rectangle and attach a point-on-object constraint.

• Set the length to 30 mm (Tab), width to 5 mm (Enter).

• Escape the tool, then select the two points and use the vertical axis to make them symmetrical.

Fixing Sketch Errors

If the sketch is invalid, check for extra constraints. In this case, the center section causes an issue. Use the trim tool to remove unnecessary lines:

1. Right-click and choose Trim Edge.

2. Hover over edges until they highlight in green.

3. Click to remove the unwanted lines.

Final Adjustments

Double-click the 5 mm height and set it to 2.5 mm. If a point-on-object constraint is missing, select the two points and apply the coincident constraint. Ensure the horizontal constraint is applied to keep the shape aligned.

Now, we have a fully constrained sketch! Adjust constraints as needed, then close the sketch and use the revolve tool. Since we sketched along an axis, this will not create a hole. Select the horizontal axis and hit OK.

Finally, rename the body to "Axle" (Right-click → Rename → Enter). Remember to save your work!

In this lesson, we’re going to create a roller using the mirror tool and the revolve operation.

Setting Up the Sketch

1. Create a new body, then hide the axle (click on it and press space bar).

2. Go to View → Toggle Axis Cross to remove unnecessary axis lines.

3. Create a new sketch on the XZ plane.

The roller is approximately 40 mm wide, so we’ll zoom in and position the sketch closer to the bottom to maximize the 3D view space.

Sketching the Roller Profile

We’ll use the Polyline tool to sketch on the left side of the vertical axis with a point-on-object constraint to ensure proper alignment.

• Start the sketch away from the axis to create a hole when revolved.

• Right-click to cancel the tool, then add constraints:

  • Base width: 20 mm

  • Height: 30 mm

  • Top length: 10 mm

  • Bottom length: 5 mm

  • Angle between the slanted edges: 110°

  • Additional length constraint: 5 mm

At this point, the sketch is fully constrained, but it’s only half of the desired shape.

Using the Sketch Mirror Tool

1. Since we want symmetry, we’ll mirror the sketch across the vertical axis.

2. Select the Mirroring (Symmetry) tool from the toolbar (or right-click and choose Symmetry).

3. Click the vertical axis to mirror the sketch across.

4. If needed, adjust the constraints to ensure a fully closed profile.

Revolving the Sketch to Form the Roller

1. Click on the sketch and select the Revolve operation.

2. Set the revolve axis to Horizontal Sketch Axis.

3. Click OK, and the roller is created!

Finalizing the Design

• Rename the body to "Roller" (Right-click → Rename → Enter).

• Save the part using Ctrl + S.

We’ve now completed all our parts! The roller is successfully modeled using the mirror and revolve tools, ensuring precision and efficiency. ?

We’ll take the two FreeCAD parts we created earlier – the bracket and the base plate – and bring them into FreeCAD Version 1’s new Assembly Workbench. In the Assembly Workbench, we will assemble these parts into a subassembly, then combine them with an additional part to create movement between the components.

Let’s get started by opening FreeCAD and creating a new document. Once the document is open, I’ll switch to the Assembly Workbench, which is an integrated feature in FreeCAD Version 1 and onwards.

Navigating the Assembly Workbench

When you’re in the Assembly Workbench, you’ll see a toolbar running across the top of the screen. You’ll notice that most of the tools are grayed out at first. This is normal! These tools become active once we start working within the assembly.

Creating a New Assembly

To create a new assembly:

1. Click on the New Assembly button.

2. You’ll notice that the origin and joints appear in the workspace.

The joints you see are crucial—they create constraints between different parts of your assembly. In this course, we will primarily work with bodies, but it’s important to note that assemblies can also be used as parts within other assemblies. We’ll explore this more in detail later.

To begin assembling our parts, we’ll use the Insert Component button. This button gives us instructions on how to add and manage parts in our assembly.

Inserting Parts

1. Left-click on a part to insert it into your assembly.

2. To remove a part, simply right-click on it.

3. To add multiple instances, hold down the Shift key while selecting the part.

Let’s go ahead and click the Insert Component button. At this point, FreeCAD is looking for parts within the current document. Since I’ve created a new document for our assembly, we can choose to add parts from the current file or an external one.

For now, let's open the Base Part file from our directory:
? File → Open
? Select the Base Part and click Open.

Saving and Grounding the Part

On the left-hand side, you’ll see the Base Part being loaded into our assembly. Now, we need to save the assembly document. A Save Document window will pop up. Let’s name this assembly:
Base Assembly
Then, click Save.

Next, FreeCAD will ask if you want to ground the part (make it stationary). It’s necessary to have at least one grounded part in the assembly to prevent it from moving. You can ground the part now or later—let’s choose Yes for this part. You’ll see a small lock icon appear, indicating that the part is grounded.

Now the Base Part is in place, and we can move it around if needed. To move it, use the Handler tool. Simply drag the part to where you’d like to position it. For now, I’ll leave it in place and click off to finish.

Let’s start by adding the bracket part to the assembly. On the left-hand side of the screen, I’ll click on the bracket, and it will be added to the assembly. At this stage, we are only adding parts to the assembly, not yet attaching or positioning them.

Placing and Transforming Parts

Once the bracket is added, we can transform it into the desired position. Click on the part, and the transform icon will appear, allowing us to move it around the screen. You can either drag it with your mouse or double-click to move it.

If a part is locked, like in this case, the transform icon won’t appear, and you won’t be able to move it until it’s unlocked.

Checking the Assembly Structure

Now, let’s check the left-hand panel for what’s happening in the assembly. Under Joints, we’ll see the base and the bracket inside the assembly structure.

When you click on the eye icon next to the grounded joint, you can toggle the visibility of the joint. This is useful for organizing and identifying connected parts. You can also press the spacebar to quickly toggle between visibility states.

Creating Joints Between Parts

Next, let’s create a joint between the bracket and the base. To do this, I’ll use the navigation shortcuts with my mouse to adjust the view and position the parts correctly.

Now, to create the joint between the two circles:

1. Select the first circle (on the bracket).

2. Hold Ctrl and select the second circle (on the base).

3. Now, choose the appropriate joint type from the toolbar. In this case, I’ll choose the Fixed Joint, which will permanently connect the two parts (just like a bolt).

Adjusting Joint Options

Once the parts are connected, we’ll see a small axis appear, indicating the joint’s connection. There are options to adjust:
? Offset – Adjust the position between the parts (we’ll leave it at zero for now).
? Rotation – Adjust the rotational alignment of the parts (we don’t need any rotation for this one).
? Flip – Change the orientation of the parts. For example, flipping the joint will change the Z-axis direction from pointing upwards to downwards.

Once everything looks good, hit OK to confirm the joint. This Fixed Joint will keep the two parts connected, and there’s no need for additional rotational joints since this connection is fixed.

Now that we’ve added one bracket, let’s add another one to the opposite side. To do this, simply head back to the Insert Component button and select the second bracket. You’ll notice that this new part is added, but we still need to position it.

Positioning the Bracket

To move the bracket, click on it once to select it, then click again to activate the transform tool. This allows us to flip the part around and position it more easily. I’ll adjust this bracket’s position and place it around here.

Adding Constraints Between Parts

Now, let’s add a constraint between the bracket and the base. To do this, select the circle edge underneath the bracket and match it with the corresponding circle edge on the base.

You can also use a more direct method by selecting the fix joint tool without choosing any part first. This is similar to how constraints work in the Sketcher Workbench—you can either select geometry and apply the constraint or select the constraint first and then apply it to the geometry.

Once we select the fix joint, we’ll see the axis of the parts that we’re connecting. You can flip the parts if necessary, just like in the Sketcher Workbench, to get everything in the correct position. If needed, adjust the rotation to place the parts exactly where you want.

Adjusting and Confirming Constraints

With the two parts positioned, we can finalize our constraints. If you accidentally select the wrong constraint, you can simply use the dropdown menu to choose a different one. Once everything is in place, hit OK to confirm the constraints.

Creating a Subassembly

What we’ve just done is create a subassembly. The reason we’re doing this is that we want to use this same setup multiple times in our main assembly. Now, let’s save this subassembly so we can reuse it in our larger project.

Let’s take a closer look at the assembly we’ve created before adding any additional parts.

Viewing and Managing Joints

On the left-hand side, we can see all the joints in the assembly. For example, we have a fix joint and a grounded joint. If I click on a joint and press the spacebar, it will toggle the visibility of the joint. This is useful when you want to see where each part is connected.

In this case, we have two fixed joints and a grounded joint. To remove a joint, simply click on it and press Delete. Notice how the part becomes free once the joint is deleted. However, every assembly needs at least one grounded joint to stay in place. Without it, your assembly will become unstable.

Grounding the Assembly

Now, let’s place the grounded joint. I’ll navigate to the View menu and toggle the Axis Cross to see where the parts are located. I want to ground the assembly to the center of my view. To do this, I click on the base part and use the grounded joint. After grounding, I can zero out the position for the X, Y, and Z axes, making sure everything is centered.

This ensures the assembly is anchored at the center of the origin, which is important for accurate placement and further operations.

Managing Linked Parts

If you look to the left in the tree view, you’ll notice all parts are linked to the original file. For example, you can see the base part and its associated link object. It’s important to be cautious when removing parts from the assembly, as it can affect the original file.

For instance, if I try to delete the base part by pressing Delete, I’ll notice that it removes the part from the assembly but also affects the original file. This is because both files are open and interconnected.

Best Practices for Deleting Parts

To safely remove a part from the assembly without impacting the original file, you can use the tree view. Simply right-click on the part you want to delete and select Delete. This will remove the part from the assembly while keeping it intact in the original file.

If you accidentally delete a part, don’t worry! Just hit Ctrl+Z to undo the action.

Making the Assembly Active

Finally, when working with assemblies, it’s crucial that the assembly is active. You can tell if it’s active by the bold text in the tree view. If the assembly isn’t active, double-click it to make it active, or right-click and select Activate Object. Once active, all the tools will be available to edit your assembly.

If the assembly is not active, you’ll notice everything is grayed out, and you won’t be able to make changes.

In this video, we'll walk through the process of creating and using assemblies in FreeCAD —from making your first assembly to integrating it into a new file. You’ll gain a solid understanding of assembly structure, dependencies, and working with subassemblies and main assemblies.

Steps We'll Cover:

Creating the First Assembly

We start by creating our first assembly. Once it's saved, we’ll discuss dependencies and how to manage them, especially when alterations like deleting operations are made.

Using an Assembly in Another File

After saving our assembly, we’ll open a new file, save it as a main assembly, and import our base assembly as a subassembly.

Managing Dependencies

We’ll explain the importance of managing dependencies, especially when importing a base assembly and whether to pull in base parts or the entire assembly.

Grounding and Moving Assemblies

You’ll learn how to ground assemblies and move them around. We’ll discuss how to unground and reposition parts within the assembly and how to manage the grounded joints for proper alignment.

Revolving and Assembling Parts

We’ll add revolve parts into our assemblies. Learn how to use fixed and revolute joints to properly position and connect components such as bushings, axles, and rollers.

Adjusting Parts and Joints

As we assemble, we’ll show you how to adjust parts into position, using offsets when needed and ensuring that each component is connected correctly.

Finishing the Assembly

Once all parts are in place, we’ll test the assembly to ensure everything rotates and fits as expected, giving you a fully functional design ready for further use.

In this video, we’ll walk through the process of creating a roller subassembly by combining bushings, axles, and the roller as a single assembly. This will help you streamline your design and learn how to manage smaller subassemblies within a larger project.

Steps We'll Cover:

Setting Up the New Document

To get started, we’ll close the current document and create a new one. We’ll save it as Roller Assembly and open it in the assembly workbench.

Importing Components

We’ll import the necessary components for the roller subassembly—this includes the axle, roller, and bushing—into our new file.

Grounding the Axle

The axle will be our grounded part. Since nothing in this assembly will move, we’ll ground it to provide a stable foundation for the other components.

Adding the Bushings

Next, we’ll add two bushings to the assembly, position them on either side of the axle, and rotate them to ensure the right alignment for the next steps.

Adding the Roller

The final part of our subassembly is the roller. After placing the roller, we’ll be ready to connect the components together with joints.

Changing the Appearance of Parts

Before we begin assembling, we’ll adjust the appearance of each component for better clarity in the assembly. We'll use predefined materials for each part:

Axle: Steel

Bushing: Jade

Roller: Brass or Gold

This will help visually distinguish between each part in the assembly tree and the workspace.

Starting the Assembly Process

Once the parts are prepared and appearances are set, we’ll begin assembling the components by attaching them using the necessary joints.

By the end of this video, you’ll be able to create and manage roller subassemblies effectively, grounding key components and assembling them in a way that ensures proper movement and function in your design.

In this video, we'll walk through the process of creating a subassembly for a roller using components such as bushings, axles, and rollers. We will cover the creation of joints, managing the appearance of parts, and how to integrate this subassembly into a main assembly.

Steps We’ll Cover:

Setting Up the Subassembly

We’ll begin by creating our roller subassembly, using a fix joint to constrain the components. We’ll learn how to add edges and faces to set up the assembly and ensure the correct alignment of parts like the axle, bushing, and roller.

Removing and Adjusting Joints

One essential step is learning how to remove joints if the assembly isn't aligned correctly. We'll go over how to delete or modify joints if components are not positioning as expected, ensuring perfect alignment.

Placing and Flipping Components

To achieve the correct positioning, we’ll use the flip tool to adjust parts. We’ll demonstrate how to rotate components such as the bushing and roller around different axes for precise placement.

Adjusting Appearance

We’ll change the appearance of our components for better visual organization. You’ll see how to apply materials like steel for the axle, jade for the bushings, and brass/gold for the roller. This helps visually distinguish the parts for easier assembly management.

Finalizing the Subassembly

Once the parts are correctly placed and the appearance is adjusted, we’ll save the roller subassembly and make it ready for use in our main assembly.

Integrating the Subassembly into the Main Assembly

We’ll open the main assembly and import the roller subassembly. After importing, we’ll add a revolute joint to connect the roller to the main assembly, ensuring it’s positioned correctly.

Grounding and Aligning Parts

In the main assembly, we’ll demonstrate how to ground the subassembly and align it with other components in the assembly. This ensures that the parts are fixed in place and aligned with the rest of the project.

Final Adjustments and Testing

Once everything is in place, we’ll make sure everything is connected, grounded, and aligned properly. We’ll refresh the assembly to check that all components are correctly linked and positioned.

By the end of this video, you’ll be able to create subassemblies, add and remove joints, adjust appearances, and integrate subassemblies seamlessly into your main assemblies. This workflow is essential for organizing complex designs and making your assemblies modular and efficient.

In this video, we’ll cover the steps to import and attach a roller subassembly into your main assembly. We’ll explore how to manage components and use joints for alignment and movement.

Steps We’ll Cover:

Opening the Main Assembly

Begin by opening the main assembly file. Ensure the assembly is activated – check that all buttons at the top are available for use. Once activated, double-click on the assembly file to make it active, allowing you to import additional components.

Importing the Roller Subassembly

We’ll now import the roller subassembly by opening the file and selecting the roller part. Simply double-click the roller assembly, and it will be added to the main assembly. You’ll see the roller subassembly appear in the file.

Attaching Components with Joints

Once the roller subassembly is imported, we’ll add a revolute joint between the two parts to connect them. Select the edges you want to join, and the parts will be aligned. Since the roller subassembly is not grounded, it will appear in an ungrounded state initially.

Adjusting Placement and Grounding Parts

If the subassembly is not grounded, it may not be positioned correctly. We’ll show you how to reposition and rotate the components. Simply double-click on the part, and the rotation tool will appear, allowing you to place the part as needed.

Grounding the Subassembly

To ensure that all components stay in place, we’ll ground the roller subassembly. Grounding the part will fix it in place, preventing it from moving. We’ll also explain that you can have multiple grounded parts within a single assembly.

Refreshing the Assembly

Once the parts are grounded, use the refresh tool to update the assembly and ensure everything is correctly aligned and connected.

Using the Assembly in Other Projects

With the two subassemblies successfully integrated, we can now use this combined assembly in other projects. This process is useful when creating modular designs, like a cabinet or chest of drawers, where you need to combine multiple subassemblies into a single final assembly.