Spindle Speeds

[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.!