[Cosha]

I have an issue with cutting out parts from 25mm marine Ply...

Im using 6mm 2-Flute Router bits (for wood)
Feedrate of 800mm min
Spindle speed of 10k
1mm plunge per pass

Im cutting out parts, so im going all the way down to 24.5mm

Vaccume for clearning chips is fine and works ok and sucking up all the rubbish...

My issue is of trust, it just does not feel like or sound like i should be doing it this way. It makes a good ammound of noise (Even inside a sound box)


I been looking all day for recomended feed rates etc...and im now totaly confused!

Any help? :cheers:

[stevespo]

Those are some very modest numbers. Cutting wood is noisy. Is it the volume that you're finding objectionable, or the particular pitch? Does it sound like something is wrong?

What type of machine and spindle are you using to cut the parts? That is probably going to determine your feedrates more so than the ideal chip load on the tool in question.

For instance, assuming a conservative 2% (.004") chip load and adequate mass, rigidity and spindle power (HP) I would be moving at least 80 IPM (2000 mm/min) and taking a full 6mm depth of cut.

Feed Rate Calculator

Tools designed for cutting plywood and other engineered wood products can support MUCH higher chiploads and feedrates. A 1/4" Onsrud 60-100 series tool can support a .016" chipload, and a 4x increase in speed to 320 IPM and 8000 mm/min, with a 1x diameter depth of cut.

Onsrud Plywood Chiploads

Your average woodworking router bit cannot manage that performance. I regularly cut 1/4" birch (hardwood) ply in one pass with an 1/8" single flute, double compression tool at speeds of 250 IPM and faster. This is an aluminum frame router with a 2.2kW spindle at 16-24K RPM.

So, the limiting factors are the tool in question, CNC machine, spindle and workholding.

Steve

[TDA]

Short answer:

Sounds like you are cutting too slow. With the specs you listed I would start at .1mm per tooth per rev which would be 2000mm/min. But my guess is your sweet spot will actually be much faster then that (2x-3x).

Don't fall into the trap that cutting slower is better. The problem is that the tool needs the cut material to cool it. If the pieces are too small then it's like spinning your tires. It makes some noise and burns up the tires (bits).

Long answer:

RPM:

RPM will be dependent on the tool you are using. Different manufacturers use different tool geometries which will mean they all have different good RPMs.

What you can do is try to get the SFPM recommendation for the material you are trying to cut then use the following. (3.82xSFPM)/tool diameter. So lets say your SFPM is 1200 (random number. I don't know that material) that would be (3.82*1200)/0.2364 (sorry don't have the metric formula handy)=19390RPM.

A simple way of thinking of this is that you are trying to get a good impact velocity for the flute of the tool. Too fast and you will have extra noise and kill your tool faster. Too slow and you will limit your feed and possibly have other issues, torque comes to mind.

Plunge:

A good plunge rate is always a game of trade offs. Go deeper and you finish sooner but you have to worry about tool deflection and increase your chances of breaking your tool.

A good place to start is usually 1 diameter of the cutter. So if you have a 6mm cutter that would be 6mm per pass plunge. You can increase your plunge but you put more stress on the tool and can increase tool deflection (the tool actually bends as it cuts). If you are having trouble with a material then you can decrease the plunge and it will take stress off the tool. This is almost always a better option then lowering the feed rate.

Feed:

Rule of thumb is based on a percentage of the cutter diameter. However, the best feed will vary with the tool geometry and material being cut.

If you want to know for sure where you should be, get some scrap material and run a test. Write some code that will start you at one corner then start with your starting feed and cut a "V" then repeat the code increasing the feed at every end point (see code below).

Here's a code example to show you want I mean. If you try to use this you need to zero your machine in the bottom corner piece of your material with your Z being zeroed at the face of the material being cut. This code also lacks a header, one would need to be added. Again, this is an example I just wrote up to demonstrate the process. If you use it in any way you need to check that it will work on your CNC and check the code for errors.

I TAKE NO RESPONSIBLY IF YOU USE THIS CODE AND SCREW SOMETHING UP.

G90G0 (Absolute programming, rapid)
X0Y0   (Zero position)
Z-6F10 (Plunge 6mm into material)
G91    (Incremental programming) 
X25Y6F2000   (Move 25mm in X and 6mm up in Y at 2000mm/min)
X-25Y6F2000 (Move back to starting X and 6mm up in Y at 2000mm/min)
X25Y6F2100   (Move 25mm in X and 6mm up in Y at 2100mm/min) 
X-25Y6F2100 (Move back to starting X and 6mm up in Y at 2100mm/min)
X25Y6F2200  (Move 25mm in X and 6mm up in Y at 2200mm/min)
X-25Y6F2200 (Move back to starting X and 6mm up in Y at 2200mm/min)
X25Y6F2300  (Move 25mm in X and 6mm up in Y at 2300mm/min)
X-25Y6F2300 (Move back to starting X and 6mm up in Y at 2300mm/min)
X25Y6F2400  (Move 25mm in X and 6mm up in Y at 2400mm/min)
X-25Y6F2400 (Move back to starting X and 6mm up in Y at 2400mm/min)
X25Y6F2500  (Move 25mm in X and 6mm up in Y at 2500mm/min)
X-25Y6F2500 (Move back to starting X and 6mm up in Y at 2500mm/min)
X25Y6F2600  (Move 25mm in X and 6mm up in Y at 2600mm/min)
X-25Y6F2600 (Move back to starting X and 6mm up in Y at 2600mm/min)
G90 (Absolute programming)
Z10 (Lift tool 10mm above material)

This will allow you to test what feedrate works best for you. Each "V" will be a different feed rate and you can then evaluate them right next to each other. You will also hear a changes in the sound of the cut as you go. If it starts to sound really bad stop the cut as you are probably exceeding the tools ability.

Machine:

Keep in mind that all of the above can be effected by your CNC. Runout, flex, backlash, spindle/router specs, and tooling. All of those can limit how you need to cut.

[Cosha]

Thank you both for taking the time to reply and the expert answers!

My spindle is a Kress 800 spinning full power! Machine is a 25mm ply all around machine, it has minimal runout and flying gantry!

It uses acme lead screw and brass nuts

800mm feed rate is what i can use i could use 1000mm at a push but i start to get some stalling at the max and min at both extremes of the bed, the part is only 100mm wide so i should get away with it!

Uncomfortable is not the word, it's an ultra high pitch scream that makes the cats and dogs i'n the area run for cover! It does not burn the wood, but re noise it makes suggest it is!

I been round wood working shops for some time ( day job is a weapons tech for the British MOD ) so used to noisy machinery!

I just think I'm tryin to do too much for my machine, I'm acualy cutting a new machine from my cnc machine!

I think all i can do it index my bass with a few pins, do a 1mm cut of the part, cut around with a jig saw, replace the part onto the indexing pins and re start the cuts!

Minimal material to cut for the router then!

The way it is going now, i just don't feel very comfortable around it, and my gut feeling is to stop, before i do damage to the machine or myself!

If money was no objective i would buy a machine from a shop, but i'n the real world i don't have the funding! Alot of DIY machines are doing a great job!

I will push my limits to the max to see what happens and I'll take a 2mm pass each time!

As you can image there is so much info on the forum almost too much sometimes!

Thank you for the code. I did learn a little g code when i first started building my machine I'm sure it will be fine!

Again thank you very much for the replies!

[stevespo]

Your Kress will go to 30K RPM, but you're only running it at 10K RPM because your machine is only capable of 80-100 cm/min cutting speeds. That seems very reasonable and achieves a conservative chip load.

I don't know what else to suggest. That kind of noise sounds like spindle bearings, not cutting noise. Is there some vibration/resonant frequency thing that is happening with the machine when the spindle is cutting? The culprit could be the plywood construction and some small vibrating part. Something that is loose?

I get a small whine when my spindle is running at about 20K RPM. The noise is actually coming from the aluminum frame which must be attuned to that frequency. A little slower, or a little faster and it's quiet.

Might still be worth trying a new (carbide) cutting tool that is designed for plywood. Could save you a lot of aggravation and cut down on noise.

Good luck!

Steve

[ger21]

Is it a 2 flute carbide tipped bit, or a spiral bit? I've heard the noise you're talking about. Even when hand routing.
Sometimes smaller bits can really scream. A larger bit can be a lot quieter.

800mm = 31 ipm, which is waaaay too slow for 10,000 rpm. You really should be cutting at closer to 3m/min at 10,000rpm. Going faster would very likely be quieter, and would greatly extend tool life.

[Cosha]

Hi Steve,

I just got home, my feedrate is now 1400mm/m & it is comfortable at that, if i push it uptoo say 1500mm/m or more it messes the harmonics of the machine and stalls...

I only have 2.1amp stepper drives, not the best :-(

I also cleaned out all the crud in the screw threads and it seems more happier...i re-adjusted the X axis bearings and it seems to like it more!

My Kress has around 10hours run time so not alot and is smooth throughout the speed range...

Tomorrow i will record a video of the machine cutting at 2mm dept per pass to see what you think (And anyone else following) if you dont mind

I shall bump the spindle speed upto around 15-18k and see how it goes, again the router cutter is new - might not be now but ill give it a quick scrape on the inside flutes

i was about to order some single flute index tools, i dont cut any aluminium so it will work out ok for me!

just as reference here is a image of my humble machine :-(



....dont laugh

i have made a few nice bits with it like a dash board for a UAV

[Cosha]

Is it a 2 flute carbide tipped bit, or a spiral bit? I've heard the noise you're talking about. Even when hand routing.
Sometimes smaller bits can really scream. A larger bit can be a lot quieter.

800mm = 31 ipm, which is waaaay too slow for 10,000 rpm. You really should be cutting at closer to 3m/min at 10,000rpm. Going faster would very likely be quieter, and would greatly extend tool life.

Thank you for the input Ger!

Its a stright 2 flute TCT bit

[ger21]

A spiral would be a lot quieter, but more expensive.
I'd double your depth of cut, to 4mm, it might help with the noise a little. Or, it might just get louder.

[Cosha]

A spiral would be a lot quieter, but more expensive.
I'd double your depth of cut, to 4mm, it might help with the noise a little. Or, it might just get louder.

Its 10:30pm here, id better try tomorrow, i dont want to wake up my neighbour...saying that she is 89 lives on her own and...deaf

[TDA]

I shall bump the spindle speed upto around 15-18k and see how it goes

Don't raise your RPM. Steve was saying that it was good that you were using the lower RPM per below. The noise and cut will get worse it you up the RPMs.

Your Kress will go to 30K RPM, but you're only running it at 10K RPM because your machine is only capable of 80-100 cm/min cutting speeds. That seems very reasonable and achieves a conservative chip load.

just as reference here is a image of my humble machine :-(



....dont laugh

Looks ok to me. At the very least you've got a starting point and are making parts.

i have made a few nice bits with it like a dash board for a UAV

Looks neat. What is it used for?

A spiral would be a lot quieter, but more expensive.
I'd double your depth of cut, to 4mm, it might help with the noise a little. Or, it might just get louder.

Gerry is right on the cutter. A straight flute tool will almost always make more noise then a spiral tool. Increasing the DOC might help but I think with that cutter it's just going to make it chatter more.

One last thing. Are you climb or conventional cutting? It will make the straight flute problem worse if you are climb cutting.

[Cosha]

Don't raise your RPM. Steve was saying that it was good that you were using the lower RPM per below. The noise and cut will get worse it you up the RPMs.


Sorry i miss read that, ill keep it as low as poss




Looks ok to me. At the very least you've got a starting point and are making parts.

This is the second version, i built one from wood by hand, then that cut this one, weill engraved the outlines and cut by jigsaw

Looks neat. What is it used for?

Was to test a onboard altimeter, and for watching vermin over farming crops


Gerry is right on the cutter. A straight flute tool will almost always make more noise then a spiral tool. Increasing the DOC might help but I think with that cutter it's just going to make it chatter more.

One last thing. Are you climb or conventional cutting? It will make the straight flute problem worse if you are climb cutting.

Just a normal cut no climbing, meh whats does DOC stand for :-(

Thank you for taking the time to reply!

[TDA]

DOC = Depth of cut.

[Cosha]

DOC = Depth of cut.

I knew that

Ok i joke, i did not know that :-D

[mcphill]

If your axes are running full speed, it sounds to me from the suggestions that you should SLOW DOWN your spindle. If you can't speed up the axes, slow the spindle. Both actions have the same effect of the amount of material cut per tooth.

[Cosha]

YES! First part cut!

Pushing the machine to 1400mm a min and reducing the spindle speed to the lowest it would go, it cut through the 25mm marine ply like a hot knife through butter!

Thanks to your advice I'm a very happy chap! I can't thank you all enough! I stuck too 1mm DOC to be on the safe side and it sounded like the router bit wasn't spinning fast enough! I guess that a common mistake thinking the fast the spindle speed the better the cut! In fact now i know other wise!

The chips were actualy visable this time maybe 1mm chunks!


Thank you all Again very much!

[mcphill]

Great News! Congrats. :banana: