I have had the Nomad for four days and have been focused on learning Meshcam and how the different tool path parameters effect results. I started out using the Carbide Auto Toolpath parameters and found they were too fast. After slowing things down to the 35in feed with depth per pass and stepover half the cutter diameter I started getting better results.
The Meshcam Pro simulator is a great tool for understanding what is going on. Rather than for Pro users I would recommend that most new CNCers buy it and carefully look at the tool path simulations. You can even tell when you are cutting too deep for a given cutter by studying the waterline cuts. I also found out how 3D roughing and the parallel finish need to work together on some parts. If 3D roughing is turned off then the parallel path can take too deep of a cut and stall the Nomad causing it to jump off the tool path.
After learning speeds and how the different selections in the Toolpath parameters interact I was going to design s knife handle like the really good looking ones Apollo did. I did not have a knife with removable handles so I decided to just design the whole knife. The cut in the pic below was done with a 0.063in end mill, 35in feed, 0,03in depth per pass and 0.03 stopover. I will try the ball cutter next then both types of .125 cutters just to get a good feel for how results for the same Tool Path Parameters are effected by the different cutter size and styles. I am pleased with the first 3D cut, and will be working my way up to ‘Apollo Quality’…
And question about depth per pass - is that the plunge rate? If it is, I feel like half of the cutter diameter is very shallow, no?
EDIT: I realize now that depth is just that, how deep of a cut per pass. So I’m still a little consisted as to what plunge rate is.
And how long did it take to make that cut? For my duck blocks, it took about 30 minutes. I feel like I could have sped up the feed and plunge to get it done faster and still maintained quality. My machine actually shut down when I was starting a new blocks with faster rates due to a cut wire on the z motor.
Steve that’s a good 1/2 knife, I’m looking forward to seeing the other side when you cut it out
For using the other end-mills, I assume you mean that you’ll be generating equivalent tool-paths with the other tools, right? You’ll need to do that because to get the right chip-load on your tool you’ll need different feed-rates to get the performance you’re expecting. For a 1/8" cutter in a hardwood you’re looking for a chip-load of ~0.003-0.005" per tooth, so since the formula is:
Chip Load = feed rate ( ipm ) ÷ ( cutting rpm x number of cutting edges )
that works out like this to solve for feed rate instead:
chip load x rpm x cutting edges = feed rate
So we get: 0.003 x 5000 x 2 = 30ipm on the conservative side, and .005 x 5000 x 2 = 50ipm on the aggressive end, with the 1/8" tools.
Heres a page from PDS (a spindle manufacturer) for feeds and speeds in a fair number of materials.
The plunge rate is how quickly the z-axis moves down into the material. You generally want the plunge rate to be such that the tool engages at or below the chip-load you’re cutting laterally with, so in the case of hard-woods, 0.003-0.005 per revolution of the spindle should be good. That works out to 5000rpm x 0.003 = 15ipm for a safe plunge-rate.
UnionNine - thanks for the explanation. And regarding your formula, how does one determine the rpm of the spindal? You used 5000 in the example. Where do I find that number?
The spindle speed is set on a per-tool basis in MeshCam. You get to the tool settings through the “select tool” button in the tool-path settings window, which brings up a list of your available tools:
Then you can click on a tool and hit “edit” to pull up the tool settings for each tool:
You may want to define different “tools” for different material configurations even with the same actual cutter.
I’m posting this from my Surface, so it doesn’t have my full tool library that my main PC has… I’ve got quite a few different definitions in there!
I need to experiment with depth per pass, I started very conservative since initially I was having trouble with things being too fast.
I tried to upload the STL in case you wanted to try the knife, but STL is not an allowed
format to upload. I wonder if the boards owner might change that so we could exchange
STL files?
When I try other tool shapes and sizes I will generate specific tollbooth parameters for each tool.
On the PDS webpage you linked to it shows the chip load for .125" cutters being the same for hardwood, acrylic, and aluminum, which makes sense from the formula. Would the difference in cutting these materials be in depth per pass for roughing, and step-down for waterline? I am assuming the default 5000rpm setting for the spindle. This seems to be midrange for the Nomad, I expect they default to this for reliability considerations??
What depth per pass and Step-down values do you use for wood and acrylic? Are these calculated values or experimentally determined?
The shortest answer I can distill to answer your question is “adjust your feeds/speeds to accommodate your machine’s limitations and the cutting characteristics of the material, while trying to keep your chip-load as close to the “ideal” loading for your given tool as you can.”
For setting depth of cut for roughing, the recommended ratio limits for most tools is 1:1 depth to diameter to go at the recommended regular chip-load. The general rule-of-thumb if you want to take deeper cuts is to reduce your feed-rate by 25% for a 2x deep cut, and cut it to 50% the recommended chip-load when going 3x as deep as your cutter is wide. Due to the machine limitations, you’ll probably be adjusting both your feed and your spindle speed to achieve optimal chip-loads and the appropriate 1:1 depth ratio.
For finishing, your depth is primarily decided by the target finish quality. Smaller steps will reduce the “topo-map” look of your model because the cuts will more closely follow the curvature of your object, resulting in smaller “stairs” or “scallops” on your model. Therefore the “right” step-down is largely determined by the slope of the sidewall you’re finishing, and how smooth you want the final result. Bigger step-downs means more obvious steps, smaller step-down means less obvious stepping, but more tool-paths and time spent cutting.
On steep slopes you can use larger step-downs and save time and still have it look decent, but on shallow slopes the step-down needs to be smaller to really capture the contour. This is also why having parallel passes is more efficient when dealing with shallowly-sloped geometry, and as Randy has posted elsewhere you want to use the “angle limit” features and have those limits overlap so that you make sure everything gets covered with one finishing method or the other. Rob posted previously about this here in the GRZ software blog.
The correct spindle speed and material feed values are both experimentally derived and calculated, in that you can calculate the “ideal” values, but then you usually end up having to adjust because of some limitation of either your machine, or your material not exactly matching the definition you’re working from, or having some non-linear behavior.
Some materials just “like” to be cut faster/slower or with larger/smaller chip-loads than the standard tooling guideline for a given tool.
