You should be cutting at 50-75mm/sec at 16,000 rpm, not 5mm/sec.
Can you post a picture of the bit?
What kind of machine is this?
Hi,
I'm milling a profile cut full depth on a 10mm plywood piece.
I'm using an 8mm, 3-flute endmill, downcut.
My settings were:
16000 RPM
5mm/sec feedrate
A few things in the attached images are clear to see:
1 - some of the paths generate a "twirly" piece of chipping. Why is that?
2 - The finished quality is not good. There are chipped off parts at the surface. It looks like what an upcut should do, but I have a downcut. What causes this effect?
3 - The plywood get's darker as it burns, which is not something I want.
During the milling, my RPM was too low and the axis "lagged" by about 5mm, so I had to restart the Z position because the bit was getting 'stuck' too much and being pulled the wrong way, so I realized i need to raise the RPM to make it go smoother into the wood. When I raised the RPM to 21000, the wood was getting a bit darker because of burn. Is there some balance here i'm missing?
Attached are the images.
Thank you!
Similar Threads:
You should be cutting at 50-75mm/sec at 16,000 rpm, not 5mm/sec.
Can you post a picture of the bit?
What kind of machine is this?
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
I'm using a Stepcraft 840, with a MM-1000 spindle.
The bit is attached in an image here.
It doesn't make sense to me to run it at that feedrate... The machine max is 3000mm/min, so that's 50/sec, but it's not recommended (according to them) to run it at 100%.
If I did it at 5mm/sec and 16000rpm, and it "lagged" because the wood was pushing on the bit too fast, making the axis go out of sync, that will probably have a much much worse effect if I try to up the feedrate to x10 of that... right?
What do you think?
Thanks
Toi don’t have enough power on a stepcraft to perform such deep cuts. Try doing several passes with eg 2-3mm doc
Sent from my iPhone using Tapatalk
That's not a downcut bit.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
A stepcraft can’t cut that deep in one pass. Take from 1mm to 3mm passes with a higher speed.
The stepcrafts tiny steppers can’t handle bigger loads and the frame isn’t rigid enough for cutting deep passes with a single cut.
So go with light passes and keep the machine cleaned and lubed and it will work.
Sent from my iPhone using Tapatalk
Ah, my mistake indeed..
Thank you for the clarification
Do you have any suggestions about the other issues I mentioned..?
Try running faster but not so deep. If you only took 5 mm at a time and taking two passes to cut through, it would go smoother. Also, 4-flute bits like that are better suited to steel than wood. You only need one or two flutes for wood. With 4, it's equivalent to running at twice the RPM.
[FONT=Verdana]Andrew Werby[/FONT]
[URL="http://www.computersculpture.com/"]Website[/URL]
Hi,
Okay thanks. I think also compression bits would work better.
You say 'try running faster... 5mm at a time', but this is an 8mm diameter bit, and my pass depth was 3mm... so 5mm would be deeper than what I did.
Try a smaller bit, either 1/4" or 6mm, like this:
https://www.amanatool.com/46202-soli...-down-cut.html
Lower the rpm to 10,000-12,000, and try 3mm depth @ 10-15mm/sec
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
@ger21,
But lowering the RPM and raising the feedrate would make the bit cut less smoothly and go faster through the wood... isn't that the opposite of what I'm trying to achieve?
No.... this info is incorrect.
the RPM is calculated to how fast the cutter is passing the material.... this is termed Cutting Speed (usually in SurfaceFeet/Minute or Metres/Minute). Once you calculate the RPM, you then multiply that by chip thickness, multiplied by the number of teeth on the cutter.
RPM = CS / (Cutter Dia x Pi) x 1000.....metric CS m/min
Feedrate = RPM x Feed per tooth x number of teeth
so... a 2 flute is run 2x faster than 1 flute... but a 4 flute is programmed 2x faster than a 2 flute.
your issue may be your feed is too slow to create a chip, it would make only dust..plus going slow also creates heat and allow burning of the wood.
A 4 flute (steel cutting geom) doesn't have deep flutes for chip evacuation. So look for cutters made specifically for wood. You could utilize cutters designed for aluminium, as these have sharper edges, uncoated, and a greater helix angle for slicing instead of a scraping like action on the softer materials.
Dust/chips should be removed from around the cutter to help minimise heat generation & to keep the cutter edges sharp. A vacuum system (1st choice) or a simple air blow (messier but would improve the part finish and extend tool life)
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi,
I'm a bit confused from all the answers.
When I try to put my bit data into FSWizard for example, the result is to run the 8mm bit at 110 mm/sec, with 8700 RPM... MY machine can only go 50 mm/sec maximum, and i'm still confused - if I go at maximum feedrate but spin really slow, that will break my machine no?? It's like dragging a very slow spinning object really fast into something.. I can't image how 8000rpm + 50mm/sec is better than 16000rpm + 25mm/sec...
You need to adjust the depth of cut to compensate for the weak machine.
Try what I said above, 10,000-12,000, and maybe 15-20mm/sec, but start at 1mm depth.
Higher rpm and slower feedrates will generate a lot of heat and destroy your bits, as you've already seen.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Thanks ger21!
I'll try that. Compensating by reducing depth seems like a viable solution.
I'll report back with good/bad results.
[I'm a bit confused by your reply, Superman. How is what I wrote incorrect? Since according to your formula, feedrate is determined by the RPM times the number of teeth (or flutes) on a tool , and doubling those doubles the feedrate, it's the same thing as doubling the RPM, no? If I'm missing something here, please point it out in terms mere mortals can understand...]
[FONT=Verdana]Andrew Werby[/FONT]
[URL="http://www.computersculpture.com/"]Website[/URL]
[FONT=Verdana]Andrew Werby[/FONT]
[URL="http://www.computersculpture.com/"]Website[/URL]
RPM is calculated on the diameter of the cutter to suit the material being machined.
so... changing a cutter from 4 flute to 2 flute means that the feedrate is only to be altered ...altering the RPM changes the cutting speed that has designed for that cutter geometry.
you may not be locked in to what is specified by the tool manufacturers, but what works for your application/setup.
say... a 10mm dia x 2 flute verses 10mm x 4 flute.... both run at the same RPM but the 4 flute would be programmed at 2x the feed as a 2 flute
take material steel for example
a HSS runs about 25 m/min. so the RPM using 10mm dia is set around S800, dia 5mm would be S1600. if you double RPM, your cutter runs the risk of not lasting too long.
That's not to say you cannot do it, you need to weigh the pros and cons.
The principle of thinking that doubling RPM is the same as halving feed is incorrect.... the time is quicker, but you have actually doubled the recommended cutting speed that the manufacturers have designed the tools to be optimally run best
Last edited by Superman; 01-26-2019 at 07:28 PM.
[Not necessarily - you might have been going too slow before. As far as the formula's concerned, it's the same thing. Tool manufacturers typically specify a feedrate as a unit per tooth per revolution, as well as a SFM, which varies according to the material being cut. As long as you don't exceed these values, the tool should work fine. Here's a typical manufacturer's chart, which illustrates what I'm talking about: Niagara Cutter ]
[FONT=Verdana]Andrew Werby[/FONT]
[URL="http://www.computersculpture.com/"]Website[/URL]