Week 02 - Computer-aided design

This week we have the following tasks to complete:

• Model (raster, vector, 2D, 3D, render, animate, simulate, etc.) a possible final project
• Compress images and videos
• Post a description with design files on the class page

Choosing a CAD Program

We first received a brief introduction to the 3D software Blender by our local instructor Ferdi, which you can find on our lab page.For more detailed guidance, I referred to his full tutorial, available here. Besides Blender, I used Inventor for 3D modeling and EasyEDA for creating a PCB mockup of the dimmer module, which is already very close to the final PCB design. Concept sketches of my idea were drawn in Notability on my iPad for a better and more intuitive drawing experience. For image editing, I used GIMP with the BIMP extension to resize images more efficiently, primarily for screenshots. For other 2D modeling tasks, I used Inkscape.

To decide which 3D modeling software to use, I considered the following points:

1. What are the capabilities and limitations of the software?
2. How efficient is my workflow in this software?

I ultimately chose Inventor based on my prior experience with AutoCAD, Inventor, Fusion 360, SolidWorks, and CATIA. My first exposure to 3D modeling was in 2016 with AutoCAD, followed by a brief use of Fusion 360 in 2018. Since 2019, I have primarily used Inventor, as we had a dedicated course for it at university, and it felt the most natural to me due to my background in AutoCAD. Fusion 360 was a solid alternative at the time, but I found its timeline-based structure and single-file modeling approach less user-friendly. While I appreciated Fusion 360’s cloud-based system, I preferred local solutions with my own file management system and the Model Browser with it's feature-based parametric design tree in Inventor. One advantage of Fusion 360 is its integrated Eagle application, which simplifies PCB housing design. However, I no longer use Eagle, which I will elaborate on in week 06. In 2023, I learned and briefly used CATIA V5 and SolidWorks at university. I found CATIA to be a robust and highly versatile program, albeit lacking modern convenience features. In my opinion, mastering CATIA equips you to work with any similar CAD software. However, I stopped using CATIA mainly because of its limited sketching convenience. In Inventor, I appreciate the ability to use automatically generated midpoints, intersection points, and other relevant points for constraints and dimensioning when modeling.

Another issue in CATIA is constraint management in assemblies. While constraints function well, allowing for controlled degrees of freedom requires careful planning to avoid conflicts. In contrast, Inventor’s joint and constrain system simplifies assembly constraints by reducing the number of parameters to consider. Additionally, CATIA lacks an integrated standard parts catalog. While custom catalogs can be created or downloaded, I have found that Inventor’s built-in standard parts library usually contains everything I need.

For me, SolidWorks and Inventor function similarly, but I found SolidWork's menu structure less intuitive. Since I am more familiar with Inventor, I saw no advantage in switching. I rarely use finite element analysis (FEA) simulations—mainly for identifying weak spots in the optimization process—so differences in simulation capabilities did not influence my decision.

Even though technical drawings are used less frequently in digital fabrication processes such as CNC milling/turning, laser cutting, and 3D printing, they remain valuable for manual manufacturing. Our university provides useful drawing templates, which I slightly modified to better suit my needs.

Why Use Blender?

Inventor, Fusion 360, CATIA, SolidWorks, and similar programs are all parametric, feature-based CAD software, whereas Blender is a mesh-based modeling tool. For example, if you import an .stl file into Inventor, it displays a triangulated mesh of polygons, making parametric modifications extremely difficult. This is where Blender excels—it allows me to extend my skill set by enabling direct mesh manipulation.

Blender also simplifies rendering and animation compared to Inventor. While Inventor can generate animations and renderings, the process is cumbersome. One feature I plan to use in my documentation is Inventor’s ability to create exploded-view animations to illustrate assembly steps more clearly. Additionally, Blender provides superior texture libraries and better handling of flexible components like cables in motion. In Inventor, bending components realistically is challenging, as parts are rigid. Blender, on the other hand, allows easy parameter manipulation over time, making complex animations more achievable.

Getting Started with Inventor

After launching Inventor, you will see a screen similar to this:

The interface consists of three main sections. On the left, you will find the most important panel, where you can create and manage your projects and new files. The middle section will later display recently used files from the current project. At the top, in the ribbon, you will find settings and options and can also create new files.

Creating a New Project

Before starting, we need to create a project instead of using the default project folder. To do this, navigate to the right panel, click on the three dots, and then select "Settings." In the new window, you will see all existing Inventor projects on your system. If you haven't moved any, they will be listed there.

To create a new project, click the "New" button at the bottom.

In the newly opened window, select "Single User Project," click "Next," assign a project name, and choose a storage location. Finally, click "Finish."

Note that multiple projects cannot be edited simultaneously in the same window. If necessary, open multiple windows, each containing one project. You can switch between projects on the home screen by clicking the small triangle next to the three dots. If you have already created or edited parts within the selected project, your home screen will look like this:

Creating new part

To create a new part, navigate to the right panel and click "New" (Ctrl + N). In the new window, select a suitable template. If you want to create a part, choose a part template. If you need a different file type, use the appropriate template. In my case, I use university-provided templates since I have already customized the sketch templates.

Now, let's create a basic part. This example will showcase useful tools, ranging from basic to more advanced functions. Upon creating a new part, the interface appears as follows:

At the top, the ribbon contains most of the tools and settings needed for designing your part. On the left, the parametric design tree displays the hierarchy of applied features, while the main area shows your working model.

General Navigation and Workflow Shortcuts

Most tools in Inventor rely on sketches, so we begin by creating a 2D sketch. Navigate to the top left corner and click "2D Sketch" (S), then select a reference plane. A reference plane can be one of the three origin planes, a flat modeled surface, or a workplane generated using various options.

For this example, I use the YZ plane, but the choice does not matter here. Best practice is to model your part in the correct orientation from the beginning, as this ensures consistency when assembling and exporting the model later. Maintaining the correct orientation from the start simplifies further processing, especially when working with assemblies or exporting to other software. The navigation cube in the upper right corner indicates the global orientation.

Scetching

In the first sketching step, create a rough shape that includes all necessary outer lines. In this case, I used the "Line" (L) tool.

Sketching Shortcuts

In the second step, apply constraints to remove degrees of freedom. The goal is a fully constrained sketch, except when working with splines without a descriptive formula. Start by applying constraints, followed by dimensions.

The first constraint will fix the general YZ movement. Use the "Coincident Constraint" on the automatic generated center point of the bottom line and align it with the origin.

This removes two degrees of freedom. The number of remaining degrees of freedom is displayed in the bottom right corner.

To use the "Revolve" command effectively, change the bottom line to a "Centerline" so that Inventor recognizes it automatically as the axis of rotation.

Now, let's add dimensions. Each dimension receives automatically increasing identifier like "d0" or "d100." You can reference dimensions in formulas, ensuring that modifying one parameter updates all associated features.

To check for unconstrained elements, attempt to move sketch entities. If necessary, use Right Click → Show All Degrees of Freedom to identify missing constraints.

A "Vertical Constraint" ensures that elements are parallel to the Y-axis, which was applied here to maintain the correct orientation. Similarly, a "Horizontal Constraint" aligns elements with the X-axis.

With a fully constrained sketch, use the "Revolve" tool (R) to create a 3D object.

Inventor automatically recognizes the closed loop and the centerline. If you have multiple closed loops from projections that are not construction lines, or if you intentionally create multiple loops, you may need to select them manually. If needed, you can configure the revolve tool further, specifying the rotation direction, the extent, and whether it should be a union, subtract, or intersect operation. Similar options are available for most tools that generate a 3D object from a 2D sketch.

Next, we create a work plane to reference a new sketch. Over the years, the automatic work plane generation has improved significantly, so I mostly just click "Plane," and it works. However, for beginners, I recommend analyzing the details to understand in which direction to select the geometries.

In this case, it is a tangential plane to the revolved curve and parallel to the YZ-plane.

In this sketch, I want to ensure that the center of the sketched geometry coincides with the origin. To achieve this, I used two lines and defined them as construction lines (similar to centerlines). The advantage is that Inventor does not recognize them as part of a loop, so the sketch remains a single closed loop instead of four separate ones.

With dimensions, it is possible to reference other dimensions and use mathematical functions. A concise list of possible commands can be found on the Autodesk help page. This list primarily applies to iLogic, a powerful system that enables cross-referencing parameters across multiple files, chaining default tools with sketches into macros, and much more. I have only scratched the surface of its capabilities over the years.

Before we move on to more advanced 3D operations, here are some useful 3D modeling shortcuts:

In the next step, I create a 3D sketch, which can be found in the context menu under 2D Sketch.

When using 3D sketches, always consider that they have more degrees of freedom. A line in 2D has two translational and one rotational degree of freedom. In 3D, it has three translational and three rotational degrees of freedom. I recommend avoiding them unless necessary or if an alternative method is more complex. Here, only projections are used, so there will be no issues with degrees of freedom, as the sketch references the previous 2D sketch and the revolving operation.

The "Project to Surface" operation allows wrapping the previous 2D sketch onto the revolved surface from step one.

The next step aims to create an extrusion in a cylindrical coordinate system along the radial direction. The geometry also varies along the Z-axis in cylindrical coordinates, making it unsuitable for the revolve function. While a similar result could be achieved using the Sweep tool, this would require additional sketches, making modifications more complex. Instead, the "Split" command is used to separate the surfaces.

To use this tool, first select a closed loop and then choose the surface to be split.

The tool is limited to one closed loop at a time, so it must be applied multiple times for all projected loops. The easiest way to accomplish this is by sharing the sketch—right-click on it and select "Share Sketch." This moves the sketch one level above the split tool in the feature tree.

After applying the split tool to all projected closed loops, the result looks like this:

Now, we create an extrusion-like effect in the radial direction of the cylindrical coordinate system.

The "Thicken/Offset" tool functions similarly to the extrusion tool but operates relative to the selected surface rather than perpendicular to a plane.

Earlier, it was mentioned that you can use parameters and reference dimensions in Inventor. Additionally, it is possible to use an Excel table to store parameters and reference them within the design. The advantage of this approach is that multiple parts can refer to a single parameter, ensuring consistency across components. You can perform calculations either in Excel or directly within Inventor. To use this feature, navigate to the Manage tab in the ribbon and click on Parameters.

This window provides access to all parameters used in the part file. In the lower left corner, you will find a Link button, which allows you to add a previously created Excel table.

Locate your xml file and open it.

The structure of the table is quite simple. A name and a value are mandatory. By default, my template interprets values in millimeters (mm), but in other templates, it might be inches. If another unit is required, such as degrees (°), centimeters (cm), meters (m), or inches (in), it can be specified by appending the unit to the value in the same cell.

To utilize these parameters in your model, click on the small arrow next to the parameter field and select List Parameters, where they are sorted alphabetically. However, it is not necessary to maintain an alphabetical order in the Excel table; I personally categorize them for better organization. Alternatively, you can manually enter the parameter name in the text field instead of selecting it from the list, which merely provides an overview of all available parameters.

A particularly useful function is the Hole tool, especially when clearance holes for countersunk screws are needed. This can be achieved by selecting the second hole type and choosing the required screw and fit. The following settings correspond to DIN EN ISO 2009 M2 screws.

Inventor can automatically calculate the weight of parts and display the center of gravity within an assembly. To use this, Inventor requires the part's density, which can be specified by selecting the appropriate material. I recommend using the Autodesk material library rather than the default Inventor library.

Based on the selected material, the part's texture is automatically applied but can be adjusted manually if needed. In this case, the cover will be laser-cut from acrylic, and the corresponding texture is translucent, providing a more realistic representation of the final product.

Creating a New Assembly

To create an assembly, first, choose an assembly template. In my case, I use the one provided by my university.

Assembly Shortcuts

To place a part, navigate to the ribbon and click Place or use the context menu for additional import options. For example, if you want to import a pre-existing 3D model of a connector or PCB, use Place Imported CAD File. To insert a screw from the standard parts library, click Place from Content Center.

To import a .STEP file, select Place Imported CAD File, choose the required file, click OK, and use the following settings in the new window to create a solid model.

The Content Center contains a variety of standard parts, including bearings, bushings, screws, pipes, and more.

In an assembly, degrees of freedom function similarly to those in part modeling. To check which degrees of freedom remain, navigate to the View tab in the ribbon and select Degrees of Freedom on the left side.

To fully constrain an assembly, individual parts must be constrained to other components. However, constraints only restrict relative degrees of freedom between parts and do not prevent the entire assembly from moving as a unit in space. To ensure absolute stability, at least one part must be grounded. To do this, right-click on the part in the Browser on the right-hand side and select Grounded.

This removes all degrees of freedom from the selected part. Typically, I ground a central component that serves as the foundation for the assembly or the most critical part.

Constraints in an assembly function similarly to sketch constraints. However, if movement is required for a part, Joints should be used instead. Joints allow the definition of specific limitations on degrees of freedom while maintaining controlled motion.

Creating 2D Files in Inventor

Every 2D sketch is inherently two-dimensional and can be exported for laser cutting, for example. To prepare a sketch for export, create a new sketch and project the contour to be cut onto it. This ensures that no unwanted geometry, such as construction lines, is included in the export.

Make sure to select only the contours that need to be cut. For example, when cutting a part with countersunk holes, ensure that you select the inner diameter of the holes rather than the outer one. There are two primary methods to select geometry for projection:

1. Manually selecting each detail individually.
2. Clicking on a surface to project all details from that surface at once.

As a final step, navigate to the parametric design tree, select the newly created sketch, and rename it by pressing F2 or using the right-click menu. I usually name these sketches laser for clarity.

Next, right-click on the sketch in the design tree and select "Export Sketch As...". In the export window, choose a destination folder, enter a filename, and click Save. The sketch will be saved as a .DXF file.

Using Inkscape

To create the rough shape, I used the Rectangle Tool (R).

To make it more precise, I adjusted its dimensions and position using the settings in the ribbon.

Next, I needed to convert the rectangle into a path. To do this, navigate to Path → Object to Path (Ctrl + Shift + C). This converts the rectangle into an editable path.

To round the corners, I used the Node Tool (N) and applied the "Add Corners LPE" option.

First, I selected all corners to ensure uniform manipulation. Then, I adjusted one of the corner handles while using the rulers on the left and top for reference.

To create a path for the holes, I set the fill opacity to 0 so I could see what I was doing while ensuring that the stroke remained black.

Finally, I used the Ellipse/Arc Tool (E) to add circles for the holes, following the same approach as when creating the rectangle. The dimension and position settings are crucial to ensuring everything aligns correctly later.

I designed the following files this week:

Blender

In the Blender introduction, Ferdi showed us how to model this monkey pillar and create animations.

Video and Image Compression

For image compression, I used GIMP along with the Bimp plugin to enable batch processing. For video compression, I experimented with both HandBrake and FFmpeg.

What Caused Problems?

While preparing this week's documentation, I made two mistakes while resizing screenshots using Bimp. First, I navigated to Files --> Batch Image Manipulation..., added the images I wanted to modify, and selected an output folder.

I applied a resize operation, but the following mistakes occurred: First, I forgot to disable the height setting, which resulted in an automatically generated aspect ratio based on the first image. These parameters were then applied to all images, leading to incorrect resizing where some images first hit the vertical parameter, when "Preserve" aspect ratio was enabled. In a second attempt, I deactivated the vertical resizing but forgot to change the aspect ratio setting from "Stretch" to "Preserve," resulting in distorted images.

What Did I Learn This Week?

Key takeaways from this week include:

• Pay more attention to secondary tasks to avoid rework—always double-check your settings (see "What Caused Problems?").
• Inventor allows projecting 2D sketches onto surfaces in 3D sketches. Previously, this was achieved using Sheet Metal tools combined with other modeling techniques. However, a limitation arose: the applied 2D sketch had to be 0.001 mm smaller or larger than the circumference of the cylindrical object for a nearly proper fit a perfect fit was impossible.
• Setting up a 3D printer teaches unexpected lessons—such as the importance of gummy bears. With larger printers, you get bigger bags of gummy bears! For context, two out of three boxes for our Prusa XL finally arrived. In my spare time, I started assembling it. So far, I have installed the frame and movement system. In the next few days, I will install the heatbed and hotends (if they arrive on time).

What Do I Want to Improve Next Week?

I aim to document work directly on the webpage rather than summarizing it afterward. Writing daily or immediately after work, could improve efficiency. I will experiment with this approach next week.

Design Files

remote_top_inkscape.svg

inventor_final_project_250205.zip

monkey_tower.blend

To create this page, I used ChatGPT to check my syntax and grammar.

Copyright 2025 < Benedikt Feit > - Creative Commons Attribution Non Commercial

Source code hosted at gitlab.fabcloud.org