CNC Router Noise

[Turtle49]

This issue has been troubling me a lot lately.

About a year and a half ago I had my Porter cable rebuilt. After that, the noise I got during a 1/4" deep profile cut was unbearable. To the point I would leave the shop and go into an adjacent room until that portion of the gcode finished. Of course this decreased my productivity quite a bit.

So I decided something had to be done. So I looked into getting a spindle but the cost for the transition was more than I was comfortable with. So after talking to a few people and getting a lot of advice. I made a few changes that dramatically reduced the amount of noise I was getting.

First I replaced my porter cable with a Ridgid R2900. It has soft start and is very quiet. I picked up some 1/2" thick plastic from West Marine and cut out two spacers. Because the Ridgid and Porter cable are different diameters.
(one note here: if you use plastic spacers as I did, and you have a zero plate. You will need to run a ground wire to the router so the zero plate can complete it's circuit.)
I did have to shim a couple of places to get the bit re-squared to the table surface. But I am now getting very nice cuts and the router noise has been reduced.

In addition to the basic router noise the Porter cable was also having issues at the lower rpm's. At 10,000 rpm, the tone of the motor would fluctuate up and down. And I can only assume that the rpm's were fluctuating as well. The Ridgid does not do this. At 10,000 rpm the noise is very consistent.

Which brings me to the second change I made. Feeds, speeds and cutting depths.

Before I was running high rpm (21,000) and low feed rates (65 ipm). Keep in mind that I cut primarily hard woods. My cut depth was alway around one diameter deep (1/4" bit = 1/4" cut depth).
In reading about chip load I figured that I needed to reduce my rpm to 10,000 and increase my feed to between 100 and 140 ipm. Now that calculation is based on the Onsrud tables with a one diameter cut depth. But I use Centurion router bits (which I believe are slightly superior at less cost). But the chips looked very good in Oak at 100 ipm so I stuck with it. But because I was running faster I decided I could reduce my cut depth to 1/2 diameter and only take a small time hit in the process.
I improved this more by changing to a dual profile tool path scheme. For the roughing pass on a 0.75" board I run at 10,000 rpm with a 0.125 cut depth. But I only run it down 0.625" into the board. Also the roughing profile has a 0.020" cutting allowance built in. After that path is complete I follow up with a finish pass. 10,000 rpm, 40 ipm at the full 0.75" depth (one pass) no cutting allowance. This gives me a nice clean edge without any "step lines" that have to be sanded out. I should also note that I run this same scheme on my pocket cuts too.

While there is still a bit of noise during the profile cuts, it is vastly reduced from what I started with. And the other bits VCarve, 1/8" etc. Are so quiet that, the dust collection noise makes me keep looking to see if the router has stopped for a bit change or not.

I hope this helps somebody else....
Tim

[knighttoolworks]

try cutting purpleheart man talk about noise. reducing rms just makes a lower pitch squeal. a roughing bit helps but they are expensive and leave marks on the edges.

[jasond]

I have some 4 flute 1/4 bits, cutting .125 in pine, I cant even hear myself think, I need to use earplugs with those bits. 2 flute bits cutting the same is manageable, I can carry on a conversation about 20 ft from the machine, still noisy, but livable.

[Turtle49]

I have some 4 flute 1/4 bits, cutting .125 in pine, I cant even hear myself think, I need to use earplugs with those bits. 2 flute bits cutting the same is manageable, I can carry on a conversation about 20 ft from the machine, still noisy, but livable.

With a four flute you would need to be running an extremely fast feed rate to hit your chip load.

Right now with my current settings and my two flute upcut in a softer would like cherry or a soft piece of walnut there is hardly any "whine". But in oak or Padauk there is a bit, but I could still talk just a few feet away from the machine.

I have considered going to a single flute, but when I have done it before I had a lot of chatter on the edges.

Tim

[jasond]

I am still new to the cnc stuff (last fall), unless I am cutting something at a slower IPM, I usually run the router on full (hitachi) 24k.

So I guess with a 4 flute, I could do a lot deeper cuts in things like pine to hit my best speed?

[olf20]

Thanks for the information Tim!!
Do you think the Ridgid R2900 helped with the noise, or your change in the
feed, depth, and speed?
Do you think the plastic spacers help?
I also went to two flute bits and increased my feed rate which helped.
I still feel that if I was able to reduce the speed of the router motor that
the noise would be reduced.
I'm still looking for a way to get the noise down so we can run during
working hours. I hate to think that we have to enclose the machine.

olf20 / Bob

[Adrian]

I've spent a lot of time lately adjusting the RPM's and feedrates on my machine to lower the bit noise and it's been very succesful for the most part.

To paraphrase what someone on the ShopBot forum told me imagine that a noisy bit wants more more to eat.

The tricky bit is adjusting the rates to suit the parts you're cutting. Settings that work for a series of cabinet doors won't work for a bunch of 10 inch profile cut letters because the machine can't reach the speed it's set to around corners and short distances etc.

As an example I used to cut MDF cabinet doors with a two flute spiral bit (6.35mm dia and pass depth) at 4ipm @18k and the screaming from the bit was loud. Now I do it at 6ipm @12k and I only get a slight squeal when turning a corner.

[Turtle49]

Good morning Bob,
I am glad the info helped.

Do you think the Ridgid R2900 helped with the noise, or your change in the
feed, depth, and speed?

The Ridgid definitely helped reduce the router noise. That is the noise that the router motor itself generates.

But the main reason I changed was because of the rpm/tone fluctuations that I was getting with the Porter cable. I believe, but I may be wrong, that the Ridgid has a feed back circuit that helps maintain rpm's under load.

All in all I think it is a better router. I thought at first that I wouldn't like giving up the quick release collet on the Porter cable. But the Ridgid has one of those push buttons that allow you to change the bit with one wrench, while pushing the button. It turns out, the button works very well when a router is on a CNC. But I should mention that the 2900 is an older version. It came with 1/2" and 1/4" collets, the newer version comes with a 1/2" collet and a 1/4" reducer. I also believe that the newer versions are not quite as tall.

Do you think the plastic spacers help?

The plastic spacers were chosen mostly because I haven't ever cut aluminum before. I don't think they do anything to reduce the high frequency whine caused by the router. So, no I don't think they help in that way. But they do work fine for holding the router and not deflecting under load.



As Adrian just stated the biggest thing you can do to reduce noise is get the bit cutting at it's rated chip load. When it cuts to slow at high rpm's at creates that extremely high pitch that is the most offensive.

Tim

[Turtle49]

I am still new to the cnc stuff (last fall), unless I am cutting something at a slower IPM, I usually run the router on full (hitachi) 24k.

So I guess with a 4 flute, I could do a lot deeper cuts in things like pine to hit my best speed?

Hi Jason,
The formula to calculate your chipload is: Feedrate / (RPM x # of flutes)

Onsrud tells me that the target chip load for a 1/4" end mill in hardwoods should be between 0.005"-0.007".

So if you run at 24k your feed rate for a four flute bit should be between 480ipm and 672ipm. At 10k the feed rate reduces to 200ipm to 280ipm. And dropping to a two flute bit cuts those last feed rates in half.

I hope that makes sense.
Tim

[Gnarly Gnu]

As an example I used to cut MDF cabinet doors with a two flute spiral bit (6.35mm dia and pass depth) at 4ipm @18k and the screaming from the bit was loud. Now I do it at 6ipm @12k and I only get a slight squeal when turning a corner.

That would be inches per second, not minute right?

I run my 2 flute quarter inch bits in MDF at about 6 ips / 360 ipm at about 15k RPM. I found the power appears to drop off or something in my HSD spindle if I run it much slower, the cut isn't as clean anyway.

Squealing on direction change is generally bit deflection - you will see very fine chatter marks on the cut edge when this happens. The only cure I know is to have less of the but protruding from the chuck - I often get my quarter inch bits cut shorter so I don't have to hang as much length out, makes a big difference.