Thick solid question.


This is my first post on this forum. It’s about a question that I have after following the YouTube tutorial of Irv regarding 3D printing basics. In that tutorial, Irv shows us how to remove material from a solid shape using the “Make a thick solid” button in Part Design:

[ATTACH=JSON]{“alt”:“Click image for larger version Name: MakeAThickSolid_Button.png Views: 0 Size: 1.3 KB ID: 16144”,“data-align”:“none”,“data-attachmentid”:“16144”,“data-size”:“full”,“title”:“MakeAThickSolid_Button.png”}[/ATTACH]

I’ve made something similar: a box to hook onto a DIN rail. However, that box has an “appendix” compared to the model shown in the video: a kind of “hook” to snap the box on the DIN rail:

[ATTACH=JSON]{“alt”:“Click image for larger version Name: din_rail_box.png Views: 0 Size: 74.0 KB ID: 16145”,“data-align”:“none”,“data-attachmentid”:“16145”,“data-size”:“full”,“title”:“din_rail_box.png”}[/ATTACH]

This is a screenshot taken from the Cura slicer. Mind the “hook” at the left of the model that is used to hang the box on the DIN rail.

My question: can the same technique be applied to take away the material, seen the fact there’s an “appendix” in the above model?

What I’ve done now is to select the top surface of the initial block and added a new sketch with a beam-alike shape which is a bit smaller than the initial model and then created a pocket and pushed the pocket downwards until I end up with a bottom thickness of 2mm. The result is perfect, but I’m not sure if this is the way a real 3D developer would do it.

Curious to hear what others think of this.

PS: If anyone is interested in the FreeCAD sources of the above, pls. let me know. I can share this with others.

Oops: forgot maybe the most important info…
Using FreeCAD 0.19 on a Windows 10 Home Edition machine

Best rgds,



Not sure if I understand your question, but I give it a shot. I think you ask if it is possible to create the box and remove the grove to mount the box to the rail.

I personally would draw the side of the box as a master sketch.

Basically the bright yellow side facing to the viewer in your picture without the mount. Then I would pad the face of the box section.

The result is a block you can put onto your rail, but it of course lacks the opening. This can be achieved by a simple function named “thickness”. The name is a little confusing, but the basic function is to apply material on the outside to create a box, BUT if you select the checkbox (Apply thickness towards the inside or so) you simply specify the wall size you want and add on all faces you want to be open to the list.

Next select the lines of the mount bracket and a pad. I added a length reference to the master sketch, so both pads are the same and you can change it.

The result will be a container like above in just three steps plus a sketch. I just did a rough outline without any real world measurements and the connector will be wrong, but you will get what I was to achieve here.

All you need to do at the end is to add chamfer and fillets. There are multiple ways of designing stuff in CAD. There is no right or wrong. Well, with FreeCAD editing on faces is wrong and especially the official version of FreeCAD is buggy like hell in reference department. Google “FreeCAD TNP” and you will see. I used this version made by RealThunder to create the example and can recommend it. It works like a different application.

I used a feature names master sketch. I basically drew multiple lines into one sketch. The entire sketch cannot be padded, but you can select multiple parts of it, create a binder and pad only that binder. With the real thunder version the binders will automatically created when padding/pocketing shapes from the master sketch.

The master sketch way you can have everything on a plane in a top down view within a single sketch and you can use what you need at a time. e.g. two circles in the same sketch. One is for the screw hole and through all, while the second is only a few mm deep to take the screw head. No need to reference the anchor point of the circles twice, which you would need with separate sketches.

ExampleBox.FCStd (34.9 KB)

@Geit First off, thanks for your extended answer!

To make sure I expressed myself correctly: my issue was not about the grove to mount the box. My question was related to remove the material from the original shape, so that I finally have a kind of box in which I can put stuff (like screws, nails, bolts,…) and that I can hang the box on a DIN rail.

Let me show some extra images:

A view on the initial sketch which has the box in the correct shape but where the “body” is still solid material but on which you can already see the layout of my second sketch of which the purpose is to “push” the material away so that I have a “hollow” box:


A view on the box after I have “pushed away” the material by means of my second sketch (still visible):


So, it’s not about the DIN rail hook. That was the easy part…

I started my project by drawing the side view of the box like so:


As you can see, the DIN rail hook is already there. Then I padded the shape to a length of 150mm, resulting in the first image of this post.

But then I needed to remove most of the material and I’ve done this by means of a second sketch, as I already explained near the second image of this post.

Hope I made my question more clear now.

FYI: To be complete, I also added the FreeCAD file to this post.

Best rgds,


DIN_Box_GVC_70mm_deep.FCStd (59.4 KB)

I included my example file above and used the thicken approach to remove the material. The problem there is that the rail hook would be made hollow, which, depending on the size, will fail as the rail hook is to small to have e.g. 2mm walls all around. So the thicken operation fails. Thats why I used two sketches for that and padded the rail mount hock later on.

Your approach is fine too. I would use a datum plane on the flat bottom axis (the one where you just need a rectangle to pocket up). Then you change the Z offset to the wall size of your box and now you can put a sketch onto the datum plane as if it is XY/XZ/YZ.

The usage of datum planes also helps to avoid creating links on faces (TNP mentioned above). It is possible to move a sketch itself e.g. created on XY plane by changing that offset, but I would prefer using a datum plane, as you can name that and used it as often as required to put multiple sketches. Also if you decide to move the DatumPlane, all sketches will move automatically.

Just name it DP_InnerBottom and e.g. If you want to add a hole to the box for draining water later on, you add a new sketch onto the existing datum plane, draw a circle, pocket and done. Without an additional reference or thinking, because the bottom of the box is the DatumPlane.

You can of course add datum planes to a face, but that will break with the official branch of FreeCAD, if you change other stuff created before in the working tree (again TNP). But even that has advantages as you just need to fix the DatumPlane reference and all linked sketches will follow.

If you use measurement references you can avoid those issues, too. I see on your middle image the sketch you used to pocket the contents to the inside. By referencing the height of the box as sketch z offset and pocket size this is a valid box. The approach I used was using the inner bottom of the box (wall size is the offset from the bottom of the box) and simply use pocket though all as there is nothing above which must not be removed.

As you can see there is no real right or wrong. Just use the way that works for you and try to avoid placing sketches on faces if possible. Also keep in mind that setting DatumPlanes may be an additional step, but they make your model clear. If you later on want to add another feature you can use that plane instead of finding out how to place a sketch at the same position again. Naming sketchs/pad/pocket/datumplanes is key. Yes, you need to type more, but when returning in a year to modify the model, you will back in in no time.