Delving into the Gcode seems a little daunting to me right now. Will explore using Fusion360 for the GCode later on. I did do a finishing pass. Hmmm. Thoughts?.
Have you played with spline travel?
I haven’t received my Nomad yet…so I’m not sure if it will even run with Motion / CAM gCode / etc (I’m a CNC noob still)
Having said that…tweaking spline travel has greatly improved the quality of my 3D prints, and is a substantial drop in rigid motion // wear and tear on my Lulzbots. If nothing else I’m testing driving it thru Motion for (hopefully) smoother movements all around. (possibly to fake/fudge a helixed movement pattern for threading)
The results are crazy impressive. Seam cross-section closeup | Details | Hackaday.io (edit)
I wouldn’t use it for general machining. Just thinking out loud for thread possibilities.
A (drill and) tap operation in CNC requires a reversible spindle (to back out after the tap is done), considerable horsepower and torque (to push the tap through the stock), G code support, and lubrication.
The Nomad does not support the “rigid tap” and “drill program” G codes, does not have a reversible spindle, and does not have the horsepower or torque to handle a tap operation. Also, tapping requires very slow speeds - lower than what the Nomad can do.
Yes, we can make precision holes with end mills. Yes, we can drill softer materials without the “drill program” G code (CAREFULLY!).
Yes, lubrication can be done manually. Do not place a body part in the work volume of a CNC machine! It is disaster waiting to happen - just don’t do it.
However, in general, the Nomad is not suitable for drill and tap operations (due to the other limitations).
But using a threadmill instead of a tap, given you can make the appropriate gcode that the Nomad can ingest, should be possible. No need to reverse spindle, and can take multiple passes to lessen required spindle horsepower and rigidity.
I’ve been trying to find a good tool that makes gcode the nomad can use, but have been unsuccessful thus far. Most I’ve found want to use gcodes (tool radius offset, and others) that aren’t supported by the nomad; Fusion 360 has yet to implement threadmill tools, and defining a workaround of a dovetail or similar I have difficulty getting the proper thread diameters, but not sure exactly why.
I was able to get fusion360 to give me threadmilling paths. I’m at work so I can’t check my job exactly, but you’re right in that they don’t support the threadmiling shape in the tool library. However, a while ago I spent some time researching this on the fusion360 forums, and I think (again, I don’t have fusion360 in front of me so this is just memory), the way to do it was simply to define a flat endmill with the same outer diameter as the threadmill, and then under the drilling operations in fusion there is a threadmiling operation which will generate a valid pass (you can even define a very small step over and it will give you a multi pass operation where it widens the thread on each pass). Iirc this workaround (flat endmill) was originally suggested by a fusion360 employee providing support on the forums.
Iirc there is a way to define the actual geometry of the screw hole + threads, but that this was not the way to generate the pass. I think you just model the hole, define an operation to drill that out first with a separate pass (drill or pocket or contour, etc.), and then you create a threadmill operation on that hole, and in the operation dialog you specify the pitch (M5x.8) and then it’ll generate the threadmilling pass for you…
Let me know if you need help and I can dig up my fusion project tonight or this weekend and tell you exactly how I did it…
edit: after posting this I got thinking maybe I should forget the drill op of the minor diameter, and just model a 3mm hole and see if that is the problem. maybe even saying I want a M3x0.5 thread is instead using the hole max of 2.5mm; I’ll go give that a try…
Thanks kjl; I did read that info also, and basically that is the method I’ve been trying (I defined a dovetail instead of a flat endmill…like a slotting mill)… I do get a toolpath but it is the wrong sizing and that’s the part I just am struggling with.
For example… I create a sheet 10mm x 10mm x 3mm thick, and I make a 2.5mm hole (cylinder) in the exact middle.
I go into CAM and drill a 2.5mm hole, then do a threadmill operation at M3x0.5 (3mm, 0.5mm pitch).
The threadmill I am using has a diameter of 2.2352mm (0.088"), so I have a simple tool defined with a diameter of 2.2352.
The toolpath generated is a nice helical spirial, except the diameter is too small, so basically the toolpath puts the 2.2mm mill down in the previously drilled 2.5mm hole, and makes a nice little helical upcut but only with a diameter of about 0.18mm instead of 3mm.
The actual gcode below shows a XY of 0.094 +/-
So that’s where I’m stumped… somehow doing a threadmill op and saying M3x0.5 and a tool of diameter 2mm makes a helical toolpath that is too small. Hmmm…
G0 X-0.015 Y0.079
G43 Z15. H2
G1 Z-3. F10.
G3 Y-0.094 I0.047 J-0.047
X0.094 Y0.094 Z-2.75 I0.094 J0.094
X-0.094 Y-0.094 Z-2.5 I-0.094 J-0.094
X0.094 Y0.094 Z-2.25 I0.094 J0.094
X-0.094 Y-0.094 Z-2. I-0.094 J-0.094
X0.094 Y0.094 Z-1.75 I0.094 J0.094
X-0.094 Y-0.094 Z-1.5 I-0.094 J-0.094
X0.094 Y0.094 Z-1.25 I0.094 J0.094
X-0.094 Y-0.094 Z-1. I-0.094 J-0.094
X0.094 Y0.094 Z-0.75 I0.094 J0.094
X-0.094 Y-0.094 Z-0.5 I-0.094 J-0.094
X0.094 Y0.094 Z-0.25 I0.094 J0.094
X-0.094 Y-0.094 Z0. I-0.094 J-0.094
X0. I0.047 J0.047
G1 X0.079 Y-0.015
Nope, that wasn’t it… it DID increase the diameter of the helical, but not enough.
Not sure how a 2.232mm diameter tool is expected to make a 3mm thread with X and Y values of +/- 0.27.
I guess there is some part of this I just don’t understand. Seems like it should be simple enough… but…
G0 X-0.033 Y0.237
G43 Z15. H2
G1 Z-2.776 F10.
X-0.039 Y0.232 Z-2.834
X-0.054 Y0.216 Z-2.888
X-0.08 Y0.191 Z-2.935
X-0.112 Y0.158 Z-2.97
X-0.15 Y0.12 Z-2.992
X-0.191 Y0.079 Z-3.
G3 Y-0.27 I0.135 J-0.135
X0.27 Y0.27 Z-2.75 I0.27 J0.27
X-0.27 Y-0.27 Z-2.5 I-0.27 J-0.27
X0.27 Y0.27 Z-2.25 I0.27 J0.27
X-0.27 Y-0.27 Z-2. I-0.27 J-0.27
X0.27 Y0.27 Z-1.75 I0.27 J0.27
X-0.27 Y-0.27 Z-1.5 I-0.27 J-0.27
X0.27 Y0.27 Z-1.25 I0.27 J0.27
X-0.27 Y-0.27 Z-1. I-0.27 J-0.27
X0.27 Y0.27 Z-0.75 I0.27 J0.27
X-0.27 Y-0.27 Z-0.5 I-0.27 J-0.27
X0.27 Y0.27 Z-0.25 I0.27 J0.27
X-0.27 Y-0.27 Z0. I-0.27 J-0.27
X0. I0.135 J0.135
G1 X0.079 Y-0.191
X0.12 Y-0.15 Z0.008
X0.158 Y-0.112 Z0.03
X0.191 Y-0.08 Z0.065
X0.216 Y-0.054 Z0.112
X0.232 Y-0.039 Z0.166
X0.237 Y-0.033 Z0.224
Hey hey - this is a success
Note that both X and Y are 0.27, so this point is on the diagonal, not on the X or Y axis - it’s really sqrt(.27^2+.27^2) distance from the center,
sqrt(.27^2+.27^2)+2.2352/2 = 1.4994, so this is a 3mm outer diameter!
Ah HA ! Thanks so much. That was the bit of knowledge I was missing. I guess I’ll go fire up the mill and give it try
You are a superstar! Thank you for the help.
Quick Pic of outcome in plexi as a test… will try some aluminum now…
Video of happy little M3 threadmill doing it’s thing:
What mill did you use? those be close to the top of my ‘to buy’ list.
I got my threadmills from lakshore carbide.
This particular one is:
Awesome! I have a bunch of stuff (drills, a threadmill, some aluminum plate) that I originally bought to make a new bed for the nomad, so I eagerly await any feeds and speeds info you may have … though now that I have some experience with the nomad I imagine making a new bed will be hours and hours of milling!
Drill and tap (threadmill) sequence…
CAM is in the youtube description.
I’m pleasantly surprised that threadmills work this will in a Nomad.
We don’t call this is a drill and tap - this is a drill and threadmill. They are distinct operations, each with advantages and disadvantages.
Tapping is MUCH FASTER than threadmilling… but one needs a unique tap for each direction, size, and thread count. Lots of holes - tapping is faster than threadmilling. Tapping can go into really deep holes but blind taps - not all the way through a hole - aren’t so nice. They cut through tough materials like butter.
Tapping requires very slow speeds - lower than what the Nomad can do.
Threadmilling is nice in that one needs a small number of tools - one? - to cover a wide range of hole sizes and directions. They are designed for use in high speed mills - 30K, 40K, 60K RPM - which is why I’m surprised this comes off well in a Nomad (and why I didn’t even mention them above).
That was more for search-ability than correct nomenclature. Most people have heard of a tap and know what it does… I figured people new to cnc may not have heard of thread milling. (even Google thinks I always want to buy a new 3mm Treadmill… not!)
I have a different profile tool from Maritool that I’m going to try some M6 holes tonight. I’m a bit skeptical with regard to the rigidity of the Nomad, hence the reason why I took it really slow with the M3, but we’ll see.
That was more for search-ability than correct nomenclature.
True, that is why I changed the name of the entire posting.
I’m very pleasantly surprised that threadmills work.
For those truly adventurous, they make threadmills that combine a threadmill (top) and end mill (bottom)! One can do the drilling, change spindle speed and program in the middle of the hole making, and threadmill! I’ve never had the courage to use such things and I don’t think the Nomad has a “Z” to make such devices very useful - the tools tend to be a bit long.
If you continue to have success, I will have to get some 0.125" shank threadmills and give it a try. BobCAD-CAM has all of the necessary support to do this kind of thing.
You can even make external threads with a threadmill!
You can even make external threads with a threadmill!
Yup… not that any of use will make screws or bolts or thread pipes…
I’m hoping to use threading aaaaaalot. Haha. I’m glad this is all getting worked out now. Great job guys!