[2muchsanding]

I've seen on different machine manufactures their advertised IPM, some up to 800ipm. I have the CNCRP Pro 4824 with NEMA34 electrics. Very ridged unit with a 3hp router.
My question is, how fast do people really push their machines. I've only cut up to 100ipm, 800ipm to me would be like light speed, even @250ipm.
I know materials and spindle vs router are probably the main factors, I think my gantry would handle most any speed without flex before the tool snaps. Well unless I'm using a 1/2 endmill or something really ridged.
I'm really not sure what mine is capable of.

 

[difalkner]

Typical cuts for me are at 18k rpm with a 3kW (4HP) water cooled spindle and probably 75% of what I cut is Walnut, Maple, and Cherry. The remaining 25% is cutting the Longworth chucks in 1/2" Baltic Birch -

- 1/32" end mill, 0.015" depth of cut, 15 ipm
- 1/16" end mill, 0.025" depth of cut, 20 ipm
- 3/32" end mill, 0.035" depth of cut, 25 ipm
- 1/8" downcut spiral, 0.100" depth of cut, 75 to 100 ipm
- 1/4" down or upcut spiral, 0.200" depth of cut, 150 to 200 ipm, usually in the middle at 175 ipm in hardwoods, 200 ipm in Baltic Birch but thinking about going to 250 ipm
- 1 1/2" flat bottom bit for surfacing the spoilboard, depth of cut as needed, anywhere from 200 ipm to 400 ipm and sometimes I'll drop the spindle speed to 15k or even 12k rpm but the last time I surfaced the spoilboard was at 18k rpm (that big cutter makes a LOT of noise at that speed :grin

V bits, 60° and 90°, usually about 75 ipm, it just depends on what I'm carving. If it's something big without a lot of detail I can double that speed.
Ball nose bits - 1/4", 3/8", and 1/2" are the same - it just depends on what I'm cutting

David

 

[MEBCWD]

One other thing to consider is acceleration and deceleration. With larger stepper motors the acceleration rate will be higher than rates for the small steppers on entry-level machines. Normally 800 IPM on these heavy-duty hobby machines is a rapid speed and you need to consider how long it takes to get to that top speed and how long will it take to slow down to set feed rates. Think about that mass (router/spindle) that you are going to push up to that top speed and how much force it takes. Then think about trying to slow down that mass that is moving at 800 IPM. The whole system from stand to gantry needs to be able to handle that constant acceleration and deceleration of that mass so you will probably never run at top rapid or feed rates. Trying to run the CNC at too high a rate will cause flexing that will cause poor cut quality and less than accurate sized parts.

That is where proper feed rates and spindle speeds for the bit you are using come into play. Calculating the correct settings allow you to run the machine at the optimum performance and helps keep you within the limits of the overall system.

 

[MEBCWD]

Typical cuts for me are at 18k rpm with a 3kW (4HP) water cooled spindle and probably 75% of what I cut is Walnut, Maple, and Cherry. The remaining 25% is cutting the Longworth chucks in 1/2" Baltic Birch -

- 1/32" end mill, 0.015" depth of cut, 15 ipm
- 1/16" end mill, 0.025" depth of cut, 20 ipm
- 3/32" end mill, 0.035" depth of cut, 25 ipm
- 1/8" downcut spiral, 0.100" depth of cut, 75 to 100 ipm
- 1/4" down or upcut spiral, 0.200" depth of cut, 150 to 200 ipm, usually in the middle at 175 ipm in hardwoods, 200 ipm in Baltic Birch but thinking about going to 250 ipm
- 1 1/2" flat bottom bit for surfacing the spoilboard, depth of cut as needed, anywhere from 200 ipm to 400 ipm and sometimes I'll drop the spindle speed to 15k or even 12k rpm but the last time I surfaced the spoilboard was at 18k rpm (that big cutter makes a LOT of noise at that speed :grin

V bits, 60° and 90°, usually about 75 ipm, it just depends on what I'm carving. If it's something big without a lot of detail I can double that speed.
Ball nose bits - 1/4", 3/8", and 1/2" are the same - it just depends on what I'm cutting

David

Those feed rates sound conservative to me. Even will all the flex in my Shark HD1 here are some of the feeds I use with spindle speed at 16k rpm

- 1/32" end mill, 0.02" depth of cut, 45 ipm
- 1/16" end mill, 0.0625" depth of cut, 100 ipm
- 60 deg and 90 deg v-bits at 100 ipm

Of course with the small steppers on the Shark HD1 it probably never gets to those feedrates.

Another thought is stepover of each bit but I usually calculate feeds based on a full width cut

 

[kp91]

I tend to listen to the router, just like working by hand or on a router table. The standard feeds and speeds are a good place to start, but listening to the router is best in my opinion. Even among the same species of wood sometimes it cuts easier or harder than others. I rarely cut anything over 80 IPM, and watching the 'actual' speed on the interface, it rarely gets up to that speed with all of the direction changes.

 

[BalloonEngineer]

Here is a quick video of a 3d carve in Corian 200ipm, .40 deep in one pass. 1/4" ball nose. Mach4 does display the "actual" speed during a carve. Corian cuts pretty fast, these are the type of carves I want to speed up.

[URL=https://vimeo.com/314282115]https://vimeo.com/314282115[/URL]

and here is a cut with a small 1/8" downcut at the same speed (in MDF).

[URL=https://vimeo.com/287521067]https://vimeo.com/287521067[/URL]

 

[beltramidave]

Just got this link this morning in case anyone is interested.
https://www.cnccookbook.com/feeds-s...+speeds+for+wood&utm_campaign=FeedsSpeedsWood

 

[difalkner]

I doubt it's actually reaching 200 ipm on such a short path, Richard. I see that on the Mach4 screen also and while I know the command is for 200 it just doesn't appear to be that fast. When I cut the Longworth chucks, especially the larger ones with greater arcs and larger diameter, it definitely hits 200 ipm.

Try setting the speed to 250 ipm or even 300 ipm on that same cut and see if you can tell a difference. I've tried going faster on small cuts and the only way I see a difference is if I have the acceleration set high, but then I stand a much greater chance of breaking bits.

Even with the NEMA 34 steppers and as quickly as the machine gets up to speed I just don't see a difference in small pockets and contours except that the machine jerks around a bit more. So I backed the acceleration down to 40 - started at 75, went to 60, then down to 50, but much more comfortable with the somewhat 'softer' acceleration setting of 40. It doesn't seem to matter on bits 1/4" and larger but I don't want to snap my 1/8" and smaller bits because the acceleration was too high. But then, as Mike pointed out, I'm a bit on the conservative side anyway... :grin:

David

 

[kolias]

Its all about listening to the machine and you can adjust all parameters thru Mach. I never push my cnc to the limits, I just try to make it run "happy"

Just run it slow to start and increase parameters slowly and eventually you will find your own parameters which are good for your machine. Numbers published are not good for all cnc's, each one has its own "happy" settings and it takes time to get there