Machining a simple slot for a box (undercut)

What would be the best way to make a box with a slot at the top for the lid to slide into? it’s something I could do with a dremel, a wheel bit and a jig, but on the other hand, I have a precise machine now, so how hard is it to tell it to drop down a bit away from the edge, go in sideways, run along the length and back, go a bit deeper, then back out and up? Like so:

Each side of the box is a different piece, it is not done in a single piece of wood. You need to do the 4 sides of the box with the slot, the base and the cover, then bond all together with white glue for example.

Yep, I know how the box in the pic was done (this is the best I could find after quick Googling), but I’d like to cut the entire bottom of my box out of one piece of wood, no seams or joints.

Better example:

The box is easy to do. About the slot you will need a special mill, probably it exist, but I’m lost about it, maybe someone else can help you. Sorry

-David

1 Like

T-Slot Cutter

Hi, I’ve been searching, and this is what I’ve found, from my point of view maybe the easier way to do what you want is empty the box with a normal bit. And then develop a home made g-code .nc file: start, speed […] move to the middle of the hole made; move to the first point and with lineal moves G01 […] stop rotating, move the safety position, end.

This don’t looks easy, but the Meshcam don’t support at this moment this kind of cutters.

If you do, post the project!

-David

There are some other CAM packages in which you can do this kind of thing much more easily, but it could be done in MeshCAM, you’d just have to bend the way the software works a bit. You would define a tool as an end-mill that has the diameter of the shank of your cutter, plus however much air-gap you want so the shank isn’t rubbing against the side-wall, keeping in mind that the further the tool-shank is from the wall, the more shallow the cut groove is.

Then in your CAD pacakge you would then create a custom geometry based on your box design, that creates a pocket that super-imposes on where the grooves should go, but starts further out in open-air so that the tool can plunge down in air, travel along the material, and then retract out in open air again. Then you create and run only a water-line and pencil clean-up pass with your under-cutting slot tool, after you’ve cut the rest of the piece, without taking it out or changing your work-origin so that everything stays aligned.

It’s tricky, but doable. A cheap/simple slot-cutter option is a Dremel high-speed bit like [this one][1], part #199:
http://mdm.boschwebservices.com/files/Dremel%20High%20Speed%20Cutter%20199%20(EN)%20r19751v15.jpg

At some point I can try to make a “how-to” for this, but unfortunately I’ve got a few things in line in front of it, so it may be a week or two.
[1]: http://www.dremel.com/en-us/Accessories/Pages/ProductDetail.aspx?pid=199

I discussed the design and manufacture of a similar box to the first on the Shapeoko Projects site: http://www.shapeoko.com/projects/project.php?id=1 (hinged, not sliding lid though)

For the version made from a single piece of wood, one would typically want some additional tools:

Hi; when doing this kind of cut in Meshcam, how can you ensure that the initial “plunge” is in the open air section of your model? i.e. Meshcam just thinks you’re making a groove, whereas you’re trying to trick it into plunging down to the final Z level off the edge of your piece and then waterline carving the groove. But there’s nothing stopping Meshcam from just plunging straight down in the middle of your object since it doesn’t know about the undercut, correct?

Also, I have a more general question, if you don’t mind the thread hijack :slight_smile: . I’m new to cnc so I don’t really have a good feel for what actions the nomad is doing is due to gcode and what is due to carbinemotion. Could you describe, super high level, what needs to be done to send custom gcode to the nomad? Here are a few examples of something I’d like to try:

  1. t slot cutting or dovetail cutting like in this original post of this thread (but perhaps from another program that can handle this natively)

  2. threadmilling (again, probably from another program)

  3. just turning the spindle on and moving the cutter around (for use with edge finder, for example)

I guess what I’m wondering is like all the homing behavior and the pausing to let you switch cutting tools and the z-axis poke that the nomad does to test the length of the endmill: is that something that the nomad knows how to do on its own, or is that behavior in the gcode coming out from Meshcam? Or, more succinctly, say I have a bunch of gcode that I generated elsewhere which will do a threadmill for a single hole sitting around in a text file; can I just load it straight into carbidemotion and send it, or do I need to put a bunch of stuff before and after that code to make it work?

As UnionNine said, there is no way to define to MeshCAM where the plunge occurs, so it is a crapshoot. This is how to implement his workflow. (I had actually thought this up before reading his post so it might not be exactly what he had in mind…)

Make the box to the full height and the interior to the full depth, and open out to one end at the level of the bottom of the slot:

Make a second STL file, to the full height of the box but without the interior, but an open-ended recess at the bottom level of the slot and with the length and width of the slot:

Make a pencil-only finishing path with this second model, geometry only, zero margin, don’t machine top of stock.

The second workpiece must be aligned to the existing box workpiece like this:

If MeshCAM makes the initial plunge outside the original workpiece, this will cut the groove with the slotting cutter shown above. But there is no way to enforce the location of the initial plunge, Reversing the workpiece left-to-right might influence where the plunge is, but I have not done that experimentation. The cutter actually needs to be the full height of the groove (Woodruff cutters are the most useful), or else you need to repeat the pencil cut while fiddling with the depth.

But the straightforward and guaranteed way to do the box is in two simple pieces. Here is the lower piece

and here is the upper piece

and when glued together you get this

It is all simple top-down machining. Note the green arrows in both screenshots. You need to put a radius on the standing rib on the bottom piece to allow for the cutter radius on the top piece.

A further note is if you use a slotting/Woodruff cutter for the one-piece design, the radius at the closed slot corners will be much larger than in the two-piece design.

Yeah, that’s what I was imagining as well. And yep, it’s definitely possible with two pieces, but I was hoping to do a single piece (and out of aluminum). Basically, I wanted to see if I could make something like the red piece on the vise that comes with the nomad: http://shop.carbide3d.com/collections/frontpage/products/low-profile-vise - a long dovetail cut out of a single piece of aluminum.

After doing more research on CNC in general, it looks like something like this would be easy to do using MDI (manual data input), which I believe the Nomad supports, where you could just do the exact cut you wanted. Anybody know how to do this on the Nomad?

First, MeshCAM does seem consistent about starting and ending the pencil cut at the open end of the geometry (as I had hoped).

Even when the stock is at a non-orthogonal angle (but good luck setting the Program Zero! :wink: )

This single-pass approach will likely work in wood, but kjl in aluminum you’re more than likely in the realm of hand-written gcode to make incremental cuts to stay within the Nomad’s spindle torque limit

Conceptually that is a really easy toolpath to hand-code but you’d need to do the layout in 2D CAD or by hand and keep each spiral pass to maybe .005-.010" apart.

You’d

  1. Move to the starting X, Y
  2. Move down to the appropriate Z depth
  3. Move to each next X, Y waypoint on the path
  4. At the end, move back up

gcode is just a text file, so you’d do it in a text editor (or if you’re really good use some kind of script to generate the code) and then just load the gcode like any other gcode file.

1 Like