I’ve been told by Tech Support that the maximum feed rate for a Benchtop Pro w/nema 23 is 200ips and a Pro 4824 nema 23 is 250ips.
We have many bits that specify higher feed rates … what is the recommended resolution to this issue?
If we shouldn’t exceed a certain feed rate, shouldn’t CNC12 impose this limit?
Run slower rpm on your spindle. Match up your spindle rpm to the feed rate you can reach. Cutters do not have to run at RPM max’d out.
Provide some example cutters and can give you some direct examples
WoodPeckers
Thats just a couple that we have that recommend feedrates about the machines limit
I did not see any recommended feed rate at those links.
You need this
Feed Rate Formula
Feed Rate=RPM X Number of Flutes X Chip Load
Feed Rate (IPM) =
Spindle Speed (RPM) × Flutes × Feed per Tooth (inches/tooth)
Example
• RPM = 18,000
• Flutes = 2
• Chip load = 0.005”
18,000 X 2 X 0.005 = 180 IPM
You could use that for the 3/8” compression or the ball nose…assuming you are cutting wood.
It’s good to understand the concept of chip load. It is a key component to getting good feed rates and good cutting.
Also learn about Surface Feet Per Minute (SFM) or also known as cutting speed for materials. Then how cutter diameter and spindle RPM impact the SFM you are cutting at.
There is a lot that goes into getting the right spindle RPM, SFM, and feed rate IPM (inches per minute)
For your skinny pointed V cutter if cutting wood you will most likely run it at the max spindle rpm, because with the tiny pointed diameter of the tip you are running a very low surface feet per minute and the chip load of .0015” to .002”.
So I’ve done alot of reading on chip load and for hardwood ideal is from .019 to ,021. so 18000 results in a IPM of 684 … way too fast for any AVID machine (servos are 600). To get below 250ipm with a 1/2” bit in hardwood i have to be at about 6500 RPM … well below the recommended minimum … so .. what am I missing?
I would consider chip loads that are 1/3 to 1/2 of those you listed. Maybe others can provide what they are using.
What specific bit are you looking at here… The flute count really matters here…
If you want to drop below 684 you drop your RPM too to hit the same chipload…
I do understand the math. The bit is the woodpeckers 2 flute at the top of the thread,
US3100C
to hit 250ipm on hardwood with “standard chip load” of .019-.021 takes me to 6500 rpm .. I can reduce depth of cut or ignore the chipload tables to get higher RPMs …..
The reason im here is because Fusion threw an error when we had a tool over 250ipm, the stated max for a NEMA23 Pro machine …Shouldn’t CNC12 throw an error as well? I assume at sustained rates over 250ipm something is going to break.
Hey Jim, this is a common question on the forum (tool manuf. recommended feeds/speeds/chip loads vs various machine configurations). It’s a rite of passage for any operator!
Regarding the question about CNC12 limiting rates, in my opinion the CAM software that contains all your tool data should act as the gatekeeper and not the control software.
Here are some other topics where community members have ‘chipped’ in with their approach:
Thanks David, yes, the CAM software should, and as I said Fusion goes a step further and warns you when your tool definition is beyond the machine limits. I’m running a maker space, I cannot be 100% sure that a members tool library or selection is consistent with the machine. As you know most of these packages provide a tool library … and we provide one as well to match the tools we provide. But in the end the design software can generate code the machine can’t handle. CNC12 warns me of all sorts of things … like drilling through the table … it knows about the machine … this seems like a reasonable request
I understand. The controller software, whether Mach4 or CNC12 (the ones I’ve used), will only transit as high as its profile is configured to allow for. That is to say, it does implement limitations, but does not alert the operator outright. Some software will show a ‘commanded’ and an ‘actual’ readout, and the operator is expected to be familiar with the equipment and why those values might differ (limitations, overrides, certain milling features, etc). A maker space, which is AWESOME btw, can’t expect everyone to be an expert on the equipment, and so I see where you’re coming from.
I’m not going to tell you how to run your shop, that’s not what you’re here for. If you’d like some additional ideas for your situation, I’m sure the community could share their experiences.
As speed increases (rpm), both holding torque and driving torque drop significantly on stepper motors. They are limiting the to 250 ipm to keep the rpm on the stepper motors in a usable range. Get outside of that and the motor will “lose steps” aka the motor tries to turn but doesn’t. At that point the machine has lost position and you will at the least scrap material if not have a machine/tool crash.
For your Woodpeckers I am guessing you will be cutting sheet goods and doing a lot of “slot” cutting as you profile parts out of a sheet? Try .008 chip load at 12K rpm. That will put you at 192 ipm. See how it cuts a slot. If it does will bump the chip load up to .009, then .010.
You will find the sweet spot and you most of the time can hear it it how the machine is cutting. If the cutter is REALLY screaming there is not enough chip load and the cutter is rubbing, which generates heat in the cutter.
It just takes time making cuts to find it.
