FreeCAD Tutorials

I don’t really have much of a CAD background, so I’ve been playing around with lots of the available (i.e. free) CAD tools to see if any of them click with me. I’m a software developer, so OpenSCAD makes the most sense, but I’ve found Autodesk Inventor Fusion to make the most sense out of the more traditional CAD tools I’ve tried. FreeCAD is really what I want to be using, but I’m finding the learning curve to be pretty steep.

Are there any great tutorials, books, example FreeCAD part design workflows you’d recommend to someone just getting started?

I’ve looked through tutorial links on FreeCAD’s site and watched several of the videos they link to, but I feel like I’m still missing a basic explanation of the workflow I should use. I can understand the concept behind sketching & then pad/pocket to extrude out a basic shape, but I don’t quite understand how I should be locking down the degrees of freedom within the sketch.

  • Adam

Hello Adam,

Here’s a list of the most recent FreeCAD tutorials on YouTube, I believe they are not referenced in the FreeCAD wiki.

One thing to keep in mind is that FreeCAD is open source software, developed by a very small team of people in their spare time. The developers cannot spare time to write documentation, they have to rely on the community, which is very small as well, actually a few orders of magnitude smaller than say the Blender community. Which is why there is not much learning material.

So far there’s been only one book published by Packt Publishing. It’s more of an introduction to FreeCAD than an extensive reference book. It looks like it’s not available in print anymore, just in ebook format.

I’ve been thinking of making FreeCAD tutorials but I already spend a lot of time helping newcomers on the FreeCAD forum where my handle is normandc.

Locking down degrees of freedom is done by applying constraints. To use constraints you need to select a sketch object first. When you hover over the icons, a tooltip will appear.

This is the Sketcher constraints toolbar.
I am using the development release of FreeCAD, I know the order of the icons was changed, but I don’t remember if that change was done for the stable release 0.13.1828 or after that.

To the left of the separator are the geometric constraints, to the right the dimensional constraints. You should always prioritize the geometric constraints. For example, rather than dimensioning two lines that share the same length, apply the

equality constraint between them - in case you need to change their size, you’ll only have one dim to change, not two.

You can apply the equality constraint to arcs and circles, this will apply to their radii.

With arcs and circles joined to lines or other arcs and circles, always make sure they are tangent by applying

tangent constraints. If the objects are not joined, select the endpoints of each then apply the tangent constraint: this will join the points together and apply the tangency at the same time.


symmetric constraint is very useful but should be used sparingly in the sketch. The Sketcher is still very young, v0.13 is only the second stable release which includes it. I’ve witnessed that when many symmetric constraints are used in the same sketch, it can lock up elements that are not fully constrained. This is a bug that will need to be addressed by the devs.

The symmetric constraint can for example be used to center a rectangle on the Sketch origin. Simply select two diagonally opposed points on the rectangle, then the origin point, then apply the symmetric constraint.
I recommend centering a rectangle to the origin because this will allow you to use mirrored features later on.

When using dimensional constraints, use the

length constraint sparingly. It should only be used when you need to set an angled dimension. For vertical and horizontal dimensions, use the

horizontal and

vertical distance constraints. This advice comes directly from the developer of the Sketcher internal solver, who told me the length constraint requires more calculation by the solver.

Of course this only covers the surface of the matter. If you want you can supply me a sketch you’ve done and I’ll give you specific advice on it. If you don’t mind hearing a funny French Canadian accent, I’ll even be willing to record a video. :stuck_out_tongue:

Hope this helps,


Awesome info Norm!

I’ll spend some time this weekend watching those YouTube videos & I’ll probably buy the ebook too. I have a really simple part that I designed in Inventor Fusion that I’d like to recreate in FreeCAD. I’ll give that a go over the weekend and if it doesn’t click, I may post my attempt here and get your suggestions as to what I’m doing wrong.

That being said, is FreeCAD what you’d recommend for a free/low cost CAD and/or solid modeling tool? I’m really surprised there aren’t hobbyist versions of AutoCAD, SolidWorks, etc. I have a project I’m trying to slowly prototype out (automatic wet cat food feeder using a TEC to keep the food container cool). I’d like to be working with reasonably good tools and doing this design the right way more or less, but $5000+ for “pro” tools is a bit too much at this point.

Thanks again for the great links. I’ll also go over to the FreeCAD forum and check things out there too - I don’t know why I didn’t think of that.

  • Adam

Well I guess it depends on whether it’s enough for what you’re planning. I’ll be honest, the software is nowhere complete yet, and some parts of it can get buggy. It does not have a 3D relationship-based assembly module yet, so to assemble parts together it’s a little like in AutoCAD: you need to place your parts manually, and the assembly won’t be parametric. But it’s doable, thousands of designers have been doing the same in AutoCAD for decades. It’s just that when the assembly module comes out, it will be a whole lot easier.

If you need more than that, then you could look at the free commercial software that’s available.

I am firmly commited to using open source software for my own needs, so it’s one reason for me to stick with FreeCAD. Helping people get the hang of this software is one of the ways I’m helping the project. I’ve also done a little icon work in v0.13 and I manage packages for Ubuntu Linux.

These corporations have no interest in the hobbyist market, apart from Autodesk which offers “dumbed down” versions of their software. Dassault which owns SolidWorks has DraftSight, a free AutoCAD-clone, but it’s 2D only - and the reason they are offering it free is not to get some hobbyist market, but to hurt Autodesk’s business and attract AutoCAD users to SolidWorks.

You could look at Geomatic Design (formerly Alibre) but the personal edition is very limited, and the pro one is not cheap, but still a lot less than SolidWorks.

@Norm - I spent the weekend watching the videos, reading over the FreeCAD book, browsing the forum a bit in addition to your tips in this thread. I’m happy to report I was finally able to get my part designed just like I wanted within FreeCAD thanks to your help.

FreeCAD Bracket Design

FreeCAD Bracket Printed on TAZ

FreeCAD Bracket Assembled with TEC & Heat Sinks

I still have plenty more work to do on the design (and I more printer tuning - the Z-wobble is making it hard to slide the heat sinks in the slots), but I’m really happy with the progress. FreeCAD definitely has quite the learning curve and lots and lots of strange things going on (my mesh wouldn’t export with the channel in the side until I added fillets for some reason) in addition to quite a few crashes (stable v13 on Win & unstabke v14 on Ubuntu), but it got the job done.

Thanks again for pointing me in the right direction Norm!

  • Adam

Thanks for the great FreeCAD video tutorials!

In your tutorial videos, there is an origin point in the Sketch. I am unable to center to the origin because there is no center origin in Sketch mode. In the Solver Messages it indicates Under-constrained sketch with 3 degrees of freedom.

I am unable to close and apply a Pad without getting the following error message…

Creating a face from sketch failed.

Tutorial Photo with Origin Point…

Photo of No Origin Point in FreeCAD…

I appreciate your help.

Hey Adam,

I’m late to reply but nice work! :slight_smile: Glad I could help.

The origin point was introduced in the latest stable release of FreeCAD, v0.13.1828. If you don’t have it, that means you have an older and obsolete version of FreeCAD.

I see from your screen capture that you are using Mac OS X. To be blunt, that OS is the worst to use FreeCAD on, because none of the developers own Macs, the Mac builds are provided by one or two volunteers. And these volunteers do not stick around long enough to troubleshoot and fix their builds’ bugs.

You may want to try this new one:

This error means your sketch profile is probably not closed. Check each of your corners, pick the point with your mouse and drag it. You may discover the end points of your segments (line or arc) are not connected to each other. It’s essential that they be constrained with a coincident (point on point) constraint. If you can’t find out what the problem is, please attach your file and I’ll have a look at it.

Scratch what I wrote previously.

If you are attempting to pad the sketch in the screen capture you provided, the error is caused by intersecting elements in your sketch. The way Pad works internally is it creates a face from the profile in the sketch, then it extrudes the face to build a solid. For the face step to succeed, the sketch needs to contain a single enclosed profile. This profile main contain other closed profiles, but they must not cross the outer profile.

In your sketch, you have an inner rectangle with circles placed on each of its corners. Those are intersecting elements and cannot produce a valid face. There’s also a small diagonal line joining the upper left corner of the outer rectangle and the upper left circle.

I understand that you used this line and rectangle to position your circles, but they are making the face fail. To fix this, you need to turn them into construction lines. Construction lines are of blue color in a sketch, and when you leave the sketch edit mode they are discarded by the system and made invisible. Which means they won’t prevent the Pad operation. Select the lines, then click on the “Toggle construction mode” icon in the Sketcher toolbar.

Thank you for all the information!

I will post once I’ve followed your careful instructions.

This is just an update on something I wrote very long ago, in case someone stumbles on this topic:

This is no longer the case, OS X is now very well supported as a few Mac guys have joined the development.