Router Speed

[Oldbill]

I am using a Bosch colt router (variable speed) and mostly 1/8" upward spiral flute bits. The problem I seem to be having is that the material being cut by the bit stays in the toolpath and I have to constanly vacuum it out.
I don't want to leave the material in the toolpath so that the bit has to run up against it again on the 2nd or 3rd pass.
I mostly use baltic birch ply and have tried running the router at various speeds. Is there a set rule on what the speed of a router bit is in relationship with the feed?

Thanks,

Bill

Similar Threads:

• Need Help!- Router Speed Controler
• Build Thread- Super-PID speed controller installation to Fixed speed Router
• Router Speed Control
• Router speed
• Router speed control

[ger21]

Is there a set rule on what the speed of a router bit is in relationship with the feed?

Thanks,

Bill

Bit manufacturers will specify a chip load, which is how much material is cut per flute per revolution of the tool. Feedrate = chipload x # of flutes x rpm. For example, if the chip load is .003, and your spinning a 2 flute tool at 20,000 rpm, feedrate = .003 x 2 x 20000 = 120ipm

If you don't know the chip load, you could find a similar tool at https://www.onsrud.com/xdoc/FeedSpeeds and use their chip load charts.

Unfortunately, I don't think optimizing your feedate will get the chips out of your cut. Especially with smaller tools, but even with 1/2" bits you'll still get this problem. The best option would probably be to blow compressed air on the cut, but vacuuming is better than nothing.

[Oldbill]

Thanks Gerry, this will help alot.

Regards,

Bill

[harryn]

Hi, my router is a bosch 1613 evs with approx 3 - 3.5 hp and 1/2 in collet.

Most of my historical cutting work has been on an outdoor project on western red cedar, which cut remarkably slowly and dulls bits fast. (I have been told it is because this wood has a high sand content, but I don't really know)

Yesterday I was working on my DIY cnc router project and was (hand) cutting some 20 mm thick finish grade plywood (0.715 in - it is what H Depot had) with a new porter cable 3/4 in cutting diameter x 1.X long 2 flute straight cutting carbide bit. (no bearing) The bit spec'd 20 K rpm, so that is where I ran it.

I was really amazed by how fast and easily it cut, so I started to play around with moving the router faster and counting off seconds to cut. I moved the router faster until I could hear the motor tone change. I was able to cut both 1/2 depth and full depth through the plywood at approx 1 - 2 inches per second, so nominally 60 - 120 in per minute. This seems like a likely upper limit to my cutting speed for this setup.

2 Questions
- Is this about what is "normal" for a router with this kind of setup ?
- I read about industrial routers with 10 x that cutting speed. I assume these things are spinning at some amazing rpms or are they using bits with a lot of flutes and deep cuts ?

Thanks

[ger21]

What's "normal" can vary quite a bit. But that's not bad for a 3/4" diameter bit.

With a handheld router, you're speed will be limited by the routers power. Harder materials need more power to cut. However, you can buy bits that need less power to cut, which will let you increase your speed. Spiral bits will cut faster than straight carbide tipped. Spirals with chipbreakers even faster. Spiral roughers even faster, but they leave a rippled edge that will require cleanup with another tool.

A few weeks ago, I had to route small countertops out of 40 sheets of Avonite solid surface, which is a nasty polyester material. I used a 2 flute spiral to start, and it was shot after 3 sheets. I then decided to make a roughing bit pass, and a 1/32" cleanup pass with the same type of 2 flute spiral I started with. I was able to double my speed, so the 2 passes took the same amount of time as the 1 pass before, and I got over 20 sheets before needing to change the bit.

With a high HP spindle, you actually don't spin it any faster. Each flute just takes a bigger bite. When the bites get too big, you use more flutes, but usually not more than 3.

10-15HP will let you blast through pretty much anything, and you can't slow it down.

[sploo]

Feedrate = chipload x # of flutes x rpm. For example, if the chip load is .003, and your spinning a 2 flute tool at 20,000 rpm, feedrate = .003 x 2 x 20000 = 120ipm

With a high HP spindle, you actually don't spin it any faster. Each flute just takes a bigger bite. When the bites get too big, you use more flutes, but usually not more than 3.

So... if you're not varying the rpm (much) and you've got loads of HP (so you can cut fast), am I right in thinking that means you're going to choose a tool with either a higher chip load/more flutes/both of the above?

The feedrate calculation tells you how fast you should be cutting, but what I've never understood is how you work out how fast you can cut with your machine. Is it just a case of try it and see, or are there rules of thumb as to what kind of HP you need to be able to handle certain chip loads (or ipm speeds)?

10-15HP will let you blast through pretty much anything, and you can't slow it down.

Truly scary. My machine, router, dust extractor... heck, all the tools in my garage... probably don't add up to 15HP

[ger21]

So... if you're not varying the rpm (much) and you've got loads of HP (so you can cut fast), am I right in thinking that means you're going to choose a tool with either a higher chip load/more flutes/both of the above?

Yes, you use a tool that will let you cut faster, whether it can take a bigger bite (higher chipload), or more bites.(more flutes)

The feedrate calculation tells you how fast you should be cutting, but what I've never understood is how you work out how fast you can cut with your machine. Is it just a case of try it and see, or are there rules of thumb as to what kind of HP you need to be able to handle certain chip loads (or ipm speeds)?

If your spindle slows down when cutting, then you're probably going to fast for the power you have. With a low power (handheld router) spindle, it'll be very much try and see. Different materials will cut very differently and may require different speeds.

With a "real" spindle, which won't slow down on you, the general rule is to cut as fast as you can while still getting an acceptable quality cut. As feedrates increase, eventually the quality suffers when you take too big a cut.

[sploo]

Thanks for the info Gerry.

I think I've probably pushed my machine (a K2 KG3925) as fast as I'm happy with for MDF cutting (about 120ipm, 1/4" upcut spiral, 1/4" deep cut). I've occasionally tried going a little deeper, but there's a definite change in 'tone' of the sound, plus the cut quality does suffer a bit too.

I guess the pro machines are a completely different game - much more rigid, much more powerful spindles. I was just wondering how you guys work out how fast you can go!

I had wondered about getting a router with more HP (my current unit is a 2.25hp PC892). I guess a 3.25HP PC7518 is about as high as I could go, but I don't know if it would make much difference.

A 'proper' spindle is a bit out of my price range, but I suppose on these hobbyist aluminum machines (circa 220lbs), rigidity will be an issue with going fast.