Spindle RPMs and feed rate issue

[dminnery]

Hi All, I could some input.
I have a Bosch Colt(1hp) on my new Romaxx and my feedrate to RPM ratio seems out of line.

I'm using maple primarily(3/4" thick), .1" depth with each pass, Onsrud solid carbide up cut bit, 2 flute (Onsrud rep recommended).

The problem is that I find I have to run the router at around 30k RPM otherwise the router bogs down and begins to vibrate. The feed rate is limited because of this situation, and can't go much over 35. If I push it the bits get pretty warm and that's not a good thing.
I've tried both conventional and climb cuts.

I see plenty of folks reporting running the same .1" depth @ 10k RPM and at a much faster feedrate. What am I missing? My router is variable from 15k-32k. I'll be using a 2hp Porter Cable in about a week.

I'm using a shop vac and a dust foot which has worked well, so chips are not the issue.

This leads me to believe I'm not using the best bit for my needs, any recommendations or other thoughts?
Thanks,
David

[louieatienza]

Hi All, I could some input.
I have a Bosch Colt(1hp) on my new Romaxx and my feedrate to RPM ratio seems out of line.

I'm using maple primarily(3/4" thick), .1" depth with each pass, Onsrud solid carbide up cut bit, 2 flute (Onsrud rep recommended).

The problem is that I find I have to run the router at around 30k RPM otherwise the router bogs down and begins to vibrate. The feed rate is limited because of this situation, and can't go much over 35. If I push it the bits get pretty warm and that's not a good thing.
I've tried both conventional and climb cuts.

I see plenty of folks reporting running the same .1" depth @ 10k RPM and at a much faster feedrate. What am I missing? My router is variable from 15k-32k. I'll be using a 2hp Porter Cable in about a week.

I'm using a shop vac and a dust foot which has worked well, so chips are not the issue.

This leads me to believe I'm not using the best bit for my needs, any recommendations or other thoughts?
Thanks,
David

The problem I believe is more your router; it may not be powerful enough for the task at hand. Unless you have a SuperPID, you'll have a loss of power at lower speeds. You would be better off in the mean time to raise your feedrate and decrease your depth of cut, until you get your new router.

For your bit, in 1/4" (52-200) the recommended chipload is .005-.007" at 1/4" doc. At 32000rpm, that equals a theoretical feedrate of 320-448ipm! While your Romaxx is capable of that, your router definitely is not!

I would suggest starting at about 120-150ipm, 15krpm, and .05"doc, and move in .01" increments intil the cut quality goes bad. Then just back off .01"

If this does not work, then I would suggest trying a single flute upcut spiral, which you can run at almost max rpm....

[txcncman]

You are probably using the wrong bit for maple. I missed what diameter you are cutting.

[dminnery]

Thanks Louie, I'll give that a try until I get a bigger router.

TXCNCMAN-it's a 1/4" bit, Onsrud 52-287. I talked to a rep at Onsrud and this was what he recommended. Though perhaps it's note the best match to this small router.

thanks for the help.

[txcncman]

Just remember, an Onsrud rep is going to only recommend Onsrud tools. I might suggest a 'O' Flute bit for your consideration. Also, as already suggested (sorta) run max RPM and max feed rate and adjust depth of cut until you get bad quality cut or bog the router down. Then back off 0.010-0.020".

[michaelthomas]

rpm x number of flutes x chipload(cut per tooth)=feedrate in ipm for best longevity.

Chipload on solid wood for a 1/4" bit is maybe .006 to .010......mdf maybe .008 to .012.

30000 x 2 x.006 ish= 360 ipm.

.006 chipload is less than I used to run for a 1/4" onsrud bit......but its probably still liveable.

I believe I ran around .009 per tooth on solid wood, and .012 per tooth on MDF with a 1/4" bit. This was on a machine that had a surplus of spindle power, though.

After you look at that formula......you will see that the rep was not making a very good suggestion.

Bits wear to the point of uselessness very quickly when they aren't
taking chiploads close to what they are designed for. Too small a chipload will create lot of heat via friction and destroy the bit in short order.

A single flute would be much better than two.....although you still wont be able to get close to the feed speed you need to keep it lasting as long as it could at the rpm where your router max its best power. Power in the 5000-10000 range would probably suit your machine much better......along with a single O.

They are right in suggesting that you don't have enough power as well.

[louieatienza]

To add to what Michael has mentioned, it is not always easy to achieve the recommended chploads on hobby machines. The spindles on commercial machines can be 15-50HP and can cut at speeds faster than most of us rapid.

While taking a shallower cut can help, in the long run, you'll wear the bottom of the bit faster than the side. And, the side is way more efficient at cutting than the bottom. Finally, the bit is stiffest closest to the collet, so the deeper you can cut, the less deflection you'll have.

Another thing: with a 1/4" groove, it will be hard for chips to clear. You don't want the bit re-cutting chips. Worse, your making too small a chip, so the chips don't pull the heat away from the bit. Then the dust in the kerf "pinches" between the bit and kerf walls, causing more friction and heat. And like Michael said, heat will cause the cutting edge to wear quickly.

[CptanPanic]

If unable to achieve feedrate with router, should he switch to different/smaller bit that has smaller chip load?

[ger21]

If unable to achieve feedrate with router, should he switch to different/smaller bit that has smaller chip load?

I wouldn't.

One, most bits smaller than 1/4" diameter aren't long enough to cut 3/4" material, which is what he's doing.

There's a pretty good chance that the high rpm's and low feedrate have already dulled your bit quite a bit.

Buy a couple of these from Ebay: 57-281 Onsrud Solid Carbide Double Edge Downcut Spiral Wood Rout | eBay

Reduce your depth of cut to about .03-.05, and up the feedrate to 200-300ipm, at maybe 20,000 rpm. The colt should be able to handle this. With a bigger router you can cut even faster at the same rpm, if the machine is rigid enough.

The shallow depth of cut should keep chips from packing in the cut, if you have decent dust collection.

An advantage to the downcut bits is that even when they start to dull, they still give provide a very high quality cut, so you can usually get much longer life from them.

I cut quite a bit of curved blanks to run through a shaper to make curved mouldings, and I use the shallow pass high feedrate technique to get cleaner cuts with no tearout. Even though the machine is capable of making one pass at 600ipm, the cut quality is much better with shallow passes.

[louieatienza]

If unable to achieve feedrate with router, should he switch to different/smaller bit that has smaller chip load?

In this particular case, the OP is cutting 3/4" solid maple. I don't know how well a 1/8" bit, if they had one with that cutting length, would work.

But using a bit with a smaller chopload would make things worse, since the smaller chips are a cause of the problem (too high RPM with too low feedrate.) This is why I and others suggested 1-flute bits, since they have a higher chipload and can be run at a higher RPM and lower feedrate than a 2-flute...

Another issue is tool engagement. When cutting a slot, half the tool's circumference is cutting. As you go deeper, the bit will rub on the sides already cut. A "trick" I use, though it increases the cycle time, is to offset your part outline in this case 3/8" then select both your part outline and offset chain and pocket it, using an offset toolpath, 50% stepover and climb-cut. This "relieves" one side of the bit and gives the chips a place to go.

On some more sophisticated CAM, you can do what's called "open pocketing" where the tool would approach the cut line from the outside in, allowing continuous tool engagement and preventing the bit from burying into the work. You could probably do this with other CAM by drawing a boundary defining your work piece and spiraling in with the offset toolpath if your CAM allows this.

[dminnery]

Thanks guys this is all great info!
Making shallower passes, .05 @ 15k rpm, definitely helped and the bit stayed cool even with even with a faster feedrate. I am hopeful that when I get my 2hp router this will all be more efficient and quality will improve as well.

I think I may also try offsetting (.02) the first cuts for rough cutting and then doing a final pass and see what I get.
I'm really trying to get a great profile on these cuts.

Thanks to all for the help, this has been tremendously helpful!
David

[dminnery]

Hi Guys,
I wanted to post an update and get your thoughts.
I installed the PC 892 2hp router the other day and had good results using a compression bit on baltic birch. Today I used the Onsrud 52-910, 1/4" carbide upcut 2 flute spiral bit on maple. The router bogged down alot, to the point that I ended up with a depth of around .07 with a feedrate of 30, rpm was 20k. It was painfully slow and very frustrating. On top of that the profile face was not smooth and I had to sand.

Earlier in the week I talked to a colleague who's doing the same type of work and has the same Romaxx, router and the same bit, He was doing a depth of .25" @ 100 feedrate and his rpms were 23k. I tried that and the router bogged down horribly, I backed off to .1 and it still wasn't great. Why am I having such different results!?

I tried my compression bit this evening @ .2" depth, 100 feedrate and an rpm of around 18k. I got some burn marks, but overall the results were much better.
I'm ordering a downcut spiral to try it out, but any downsides to using compression on wood if I can control the burning?

Very puzzled why I can't get the same results as my friend, thoughts?