Spindle Speeds

[Lodds]

Guys
Are there any "rule of thumb" when looking at spindle speeds for different size cutters and for cutting timber? I appreciate that it is not an easy answer but i just need a starting point as I keep finding new ways to fill my workshop with smoke.

Thanks

[m_c]

The key is you always want to be cutting, never rubbing. This is something that applies to any material you're trying to machine.

Spindle speed is a product of how fast your machine can move, recommended surface cutter speed (aka the diameter of the cutter), and spindle power.
Try running some figures through some of the feed/speed calculators like https://app.fswizard.com/

This will give you some ball park figures, but will still need some experimentation for specific cutters/machines.

[JAZZCNC]

Usually if your smoking it's because your feeds are too low rather than spindle speeds being too high.

What size cutters are you using and in what material.? Give us some idea of the feeds n speeds your using.

Also, the machine makes a BIG difference because if your machine can't handle the loads or travel fast enough to cut correctly then you always going to struggle. This is why Feeds n speeds calculators don't often work for DIY machines as they assume an industrial spec machine is used.

[Muzzer]

Good point to check the required spindle power for a planned operation. As well as checking the spindle motor is powerful enough, it's often worth checking how much or little of its capability you are making use of.

Lots of Youtube warriors seem scared to get anywhere near what their machines can achieve and have little idea where that is because they never check. My larger machine has "only" 3kW but when you see what 3kW can do, it can be quite a revelation. If you experiment and go a little too far, what do you have to lose? Cutters aren't expensive and underwear can be washed.

There are a few free f&s apps beyond the fswizard that include spindle power estimates. And many VFDs can display the actual load as a % of max.

[Kitwn]

Good point to check the required spindle power for a planned operation. As well as checking the spindle motor is powerful enough, it's often worth checking how much or little of its capability you are making use of.

Lots of Youtube warriors seem scared to get anywhere near what their machines can achieve and have little idea where that is because they never check. My larger machine has "only" 3kW but when you see what 3kW can do, it can be quite a revelation. If you experiment and go a little too far, what do you have to lose? Cutters aren't expensive and underwear can be washed.

There are a few free f&s apps beyond the fswizard that include spindle power estimates. And many VFDs can display the actual load as a % of max.

I once read a forum entry somewhere that suggested the way to set your feedrate was to increase it until the tool breaks then back off 10% and replace the tool. I prefer to use HSMAdvisor but it's a worthy experiment if you have a handful of 3-6mm tools you're willing to sacrifice. I'm not sure I'd deliberately push my machine that hard with anything larger. Make your own mind up depending on what you have.

Regarding the strength of DIY machines, you're better reducing the depth of cut or tool engagement more than the feedrate if you're getting inaccurate cuts since the cause of smoke, as Dean implies, is not moving the tool through the material fast enough. This leads to rubbing, localised heating and smoke.

[Lodds]

Usually if your smoking it's because your feeds are too low rather than spindle speeds being too high.

What size cutters are you using and in what material.? Give us some idea of the feeds n speeds your using.

Also, the machine makes a BIG difference because if your machine can't handle the loads or travel fast enough to cut correctly then you always going to struggle. This is why Feeds n speeds calculators don't often work for DIY machines as they assume an industrial spec machine is used.

Material is chipboard (just to practice on) RPM I have varied from 10,000 to 24000 (max) machine is a C-Beam from Open Builds

[JAZZCNC]

Material is chipboard (just to practice on) RPM I have varied from 10,000 to 24000 (max) machine is a C-Beam from Open Builds

Well, that's two details which don't help.!. . .But you didn't answer my questions regards speeds n feeds your using.

[Lodds]

Well, that's two details which don't help.!. . .But you didn't answer my questions regards speeds n feeds your using.

perhaps this will help
28980

[erniehatt]

I am new here, and I am using a Chinese 6040 machine with a 2.2kw spindle, for plywood I run at 10,000 rpm 254 feed and 80 plunge, with a 3mm end mill,and get excellent results, the top edges are very clean.
I intend to try Aluminium next, so some experimenting is needed.

[Clive S]

How many flutes ??

That is way too slow. I don't know what machine you have but I would start by triple those speeds ie. 1800mm/min at 14000 rpm

Be prepared to break a few cutters.

[Kitwn]

How many flutes ??

That is way too slow. I don't know what machine you have but I would start by triple those speeds ie. 1800mm/min at 14000 rpm

Be prepared to break a few cutters.

I'm with Clive on this one. 3mm tools are cheap enough so keep the 1mm depth of cut (or maybe up it to 1.5mm, 50% of the tool diameter) and crank up the linear speed in steps until you break the tool. If you've been running at such low speeds up to now you will be pleasantly surprised at how fast you'll be able to cut even if your machine is not very rigid. I'd be fairly confident that you can cut at up to 3m/min (50mm/sec) in MDF with no problems. Just be aware that MDF dust is nasty stuff so a mask and dust extraction/vacuum cleaner are essential.



Kit

[Neale]

I was cutting some ply last night. 4mm single-flute carbide cutter, 24K RPM, 2000mm/min cutting speed, 3mm DOC. Probably could have gone at it harder but like a lot of my jobs, I was cutting fiddly bits and I wasn't confident about the hold-down method stopping the work moving. After all, with a handheld router I would be running these cutters at 26K RPM so that's not a problem. After that, it comes down to rigidity of the machine and how well you can clamp things. Just keep winding things up until it breaks!

[JAZZCNC]

I'm sorry but all this talk I keep seeing about keep winding it up until the tool breaks is total B@##~ks.! . . Just because the tool breaks doesn't mean you have found the limit. Tools can break for multitude of reasons which have nothing to do with speeds n feeds. Spindle runout, machine vibrations, material hard/soft spots, tool geometery, DOC etc etc.

just a simple tweak of any, one parameter can cause a tool to break, esp small tools, like wise a simple tweak of any one parameter can Stop the tool from braking and allow you to push far higher than you probably realise.
No two machines and work/material setups are the same so it's very difficult for anyone to recommend speeds n feeds unless machines are very closely matched. Even then materials and the quality of them play a huge part.

For instance MDF, most people think MDF is just MDF and all are the same, they are very much NOT, the cheap nasty stuff you find in B&Q etc cuts Soooo much diffferent to a quality grade MDF. So much so you can easily double the feeds with the same tool and machine setup because of how it chips and clears the cutter.

I have one particular customer who cuts nothing but MDF letters & shapes, 10hr days, 6 days a week using 4mm SF cutters with 4mm DOC @ 7mtr/min and hardly breaks a tool.
Before changing grades and using cheap MDF they were breaking cutters all the time and cutting at half the feeds.

Now the OP is battling with several fronts, Crappy material, Crappy machine design and probably using Crappy cutters going at least 6 times too slow and I'd also take a guess not even able to achieve the feeds required to cut correctly due to lack of power.!

The only thing I'd say is to ramp up the feeds and play with the parameters until you get cutting something like your happy with. Then push it some more if you want, but be prepared to break tools but don't think because the tool broke it's the limit, keep tweaking the parameters a little at the time and you'll get more, how much depends on many factors and just like a womens mind, it could all change again tomorrow when you get a different grade of material.!!

[Lodds]

.........
The only thing I'd say is to ramp up the feeds and play with the parameters until you get cutting something like your happy with. Then push it some more if you want, but be prepared to break tools but don't think because the tool broke it's the limit, keep tweaking the parameters a little at the time and you'll get more, how much depends on many factors and just like a womens mind, it could all change again tomorrow when you get a different grade of material.!!

Thank you, I will be trying that. From what I have read the way forward is exactly the opposite of what I have been doing.

Thanks everyone for your input, been very useful

T

[erniehatt]

Your info has been most helpful indeed, I am now getting a lot more out of the Machine.
You may be able to help me with one more set up, I have to cut some aluminium for some face plates, can you please give me some starting points. Thanks

[JAZZCNC]

Your info has been most helpful indeed, I am now getting a lot more out of the Machine.
You may be able to help me with one more set up, I have to cut some aluminium for some face plates, can you please give me some starting points. Thanks

Ahh now you are moving into a much trickier area to advise because many more variables come into play. The machine strength and material grade play a huge part as does the spindle quality and you will very much need to feel and ear your way thru this one.!

I need more info to help.

Material grade, Cutter size, # flutes, HSS or Carbide.

[erniehatt]

Thanks, The material is just standard aluminium 1/4 inch thick.. The bit is also 1/4 inch 2 flute carbide. The machine is a 6040, the spindle is a water cooled 2.2kw

[erniehatt]

Thanks, The material is just standard aluminium 1/4 inch thick.. The bit is also 1/4 inch 2 flute carbide. The machine is a 6040, the spindle is a water cooled 2.2kw

[Clive S]

Thanks, The material is just standard aluminium 1/4 inch thick.. The bit is also 1/4 inch 2 flute carbide. The machine is a 6040, the spindle is a water cooled 2.2kw

There is a huge difference in the grades of aluminium from gummy to cast the grades have numbers like 6082.

The machining properties are different across the grades. Its the same with plastics and wood / MDF

[JAZZCNC]

Thanks, The material is just standard aluminium 1/4 inch thick.. The bit is also 1/4 inch 2 flute carbide. The machine is a 6040, the spindle is a water cooled 2.2kw

Ok well, there is no such thing as Standard aluminum, there are lots of grades and like Clive says huge differences in how they machine. Also, you don't say how long the cutter is which plays a large part in feeds n speeds.

I will give you some starters but they could be miles off. The machine sturdiness and tool quality play a big part when cutting aluminum and combined with not knowing the grade of Ali it's verging on impossible to advise with any accuracy. Again you'll need to use your Ear and listen to what the machine is saying to you and use lots of air to clear the chips and WD40 for lube.

I'm going to assume it's a lower grade like 1050 which is horrible stuff. Lots of people go wrong with this stuff by taking too shallow a depth of cut which results in a thin chip that gets too hot melts and sticks to the cutter. Taking deeper cuts produces a bigger chip that won't melt but it does mean you need to get the chips out of the cut before it gets re-cut which can cause other issues.

Try this and see how you get on, but again use your own judgment and ear to determine if your machine is handling it ok. Don't be surprised at the noise level, it's much louder than cutting woods, etc and could squeal loudly.

1.5mm Depth cut, 1000mm/min, 14000 to 16000rpm

These are very conservative feeds n speeds for a carbide cutter and I would expect to be cutting deeper and faster but without knowing your machine or the material grade then your better taking it easy, but not so easy chips start to melt.!

[erniehatt]

Ok,just found the receipt, it is 5083 aluminium.The cutter is a 6 mm straight 2 flute at 32 mm long

[Doddy]

Ok,just found the receipt, it is 5083 aluminium.

29050

Good luck!

Worth reading about the spec before investing a lot of time or cost with cutters.

(source: http://www.aalco.co.uk/datasheets/Aluminium-Alloy-5083-0-H111-Sheet-and-Plate_149.ashx )

[JAZZCNC]

Ok,just found the receipt, it is 5083 aluminium.The cutter is a 6 mm straight 2 flute at 32 mm long

Ok well, it's a good grade to cut, not so sticky. However, your cutter is quite long and being straight flutes not ideally suited to aluminium. The stick out will have a large effect on feeds and the straight flutes won't clear chips very well. So I'll say it again because cannot stress enough how important it is to clear the chips away, lots of Air and occassional spray of WD40 will be needed.

Given these new details, I would start with halfing those settings I gave before and work up changing one setting at a time to see the effect. 1st I would play with RPM, then Feed then DOC.

[JAZZCNC]

29050

Good luck!

Worth reading about the spec before investing a lot of time or cost with cutters.

(source: http://www.aalco.co.uk/datasheets/Aluminium-Alloy-5083-0-H111-Sheet-and-Plate_149.ashx )

Tells you absolutely nothing of any value for deciding cutting parameters other than hardness, which in aluminium doesn't mean so much because it's often full of hard n soft spots.

[erniehatt]

Thanks guys for the great help, I have a few items to come before I can design the plates, but I will try some different settings on some scrap.
To be honest I have been a bit afraid to try it, but now at least I have some faint idea.

[Lodds]

Taking this conversation on a step but still speeds and feeds related....

Does anyone have an opinion on a product called "GWizard"? It's a paid for program but might be a good starting point for us newbies. There is a 30day trial and on the surface seems informative, as I say it may be just a starting point for newbies?
https://www.cnccookbook.com/g-wizard-cnc-speeds-and-feeds-calculator/ :link: