How deep with a 3/8" compression?

[garyb]

What about the onsrud 2 flute downcuts? That's what I usuallhy use that really screams

Clay
Need a litttle more info, what tool number are you using? is this when your cutting 5/8" birch ply? what are your feed, speed and stepdown, is the scream continuous thru the whole cut or mostly at ramping speeds, are you cutting climb or conventional? are you doing an LP toolpath for the final pass?
If you would like to discuss, your welcome to call me
Gary

Eric, I see you noted the scream in the corners, what is your ramping feedrate?

[EricSchimel]

I hear that screaming on those downcut bits too, although less so. That's why in most cases I just stick with compression bits as it's so much easier to tune those out. I tried just about everything to turn out the screaming bits, and while I can tune it out on straight cuts, the only way I figured I'd be able to do it in the corners, or during ramp downs is if the spindle speed could throttle up and down with feedrate. That's not something you can do on a ShopBot (or any other CNC machine of this class) that I'm aware of.

[coryatjohn]

I think you can change the speed of the spindle if you edit the machine code yourself. A lot of work and probably not worth the effort unless it's a file you run all the time.

[garyb]

Eric, same applies to you as Clay, if you supply me all the info on the tool, settings, material etc I will be happy to look deeper into your issue.
I haven't run Shopbot control software in some time but I'm sure you would have corner ramping adjustments now. These will give you a much quicker response than any rpm via vfd can give you, a ramp down into a corner and back up on a 90° turn will be over by the time the vdf can change the rpm.
Gary

[EricSchimel]

I've already solved the problem: I just don't use those double flute spirals from Onsrud unless I have to. When I do, they only scream in the very corners for a split second. The rest of the cuts sound perfect. This means that I've solved it for about 95% or more of the cutting distance in any given job. On the fly spindle speed changes would likely solve that last 5% if they were possible, but for 5% it's not worth me trying to invent something when I can in most cases just use a different bit or just live with a little noise.

[ClayM325]

Clay
Need a litttle more info, what tool number are you using? is this when your cutting 5/8" birch ply? what are your feed, speed and stepdown, is the scream continuous thru the whole cut or mostly at ramping speeds, are you cutting climb or conventional? are you doing an LP toolpath for the final pass?
If you would like to discuss, your welcome to call me
Gary

Eric, I see you noted the scream in the corners, what is your ramping feedrate?

Bit number is 57-924. I use them to cut 5/8", 1/2", and 3/4" plywood (Araucoply). Ive been running at 6ips,14k rpm, and screams all the time. Ive been doing it that way for 2.5 years since I got my machine. Didn't know better

[garyb]

Yes Clay I can see why its screaming, you are way off on the chipload for that tool.
The grind for that tool is designed for hard/soft woods which runs a lower feedrate, and not recommended for the plys your cutting, the recommended is the 60-100 series which includes the MW, C, MC and PLR tools.
For the 57-924 the chipload is .007 You didn't say, so I will assume your using .375 stepdown, at 14000rpm that would calculate your feedrate to 196ipm (3.2ips). At the 6ips (360ipm) you have been running at would calculate your rpm out to 25700rpm not the 14k you have been using.
Now if your cutting in one pass and not reducing the chipload then your multiplying the problem so the tool is screaming and burning up long before its expected life.

If you don't know how to figure your feeds and speeds the following are you 2 main formulas, you will find these at the bottom of the chipload charts in the back of the Onsrud catalog as well.
Feedrate (ipm) = RPM x # of cutting edges x chipload
RPM = Feedrate / (# of cutting edges x chipload)
Now these are based on the stepdown of 1 x the tool diameter, 2 x the tool diameter reduce the chipload by 25% and by 50% for 3 times the tool diameter.

All Onsrud tools have a chipload figured by the factory for that tool, as noted you will find that list by material in the back of the catalog which you can have mailed out or download as a pdf.
Gary

[ClayM325]

Yes Clay I can see why its screaming, you are way off on the chipload for that tool.
The grind for that tool is designed for hard/soft woods which runs a lower feedrate, and not recommended for the plys your cutting, the recommended is the 60-100 series which includes the MW, C, MC and PLR tools.
For the 57-924 the chipload is .007 You didn't say, so I will assume your using .375 stepdown, at 14000rpm that would calculate your feedrate to 196ipm (3.2ips). At the 6ips (360ipm) you have been running at would calculate your rpm out to 25700rpm not the 14k you have been using.
Now if your cutting in one pass and not reducing the chipload then your multiplying the problem so the tool is screaming and burning up long before its expected life.

If you don't know how to figure your feeds and speeds the following are you 2 main formulas, you will find these at the bottom of the chipload charts in the back of the Onsrud catalog as well.
Feedrate (ipm) = RPM x # of cutting edges x chipload
RPM = Feedrate / (# of cutting edges x chipload)
Now these are based on the stepdown of 1 x the tool diameter, 2 x the tool diameter reduce the chipload by 25% and by 50% for 3 times the tool diameter.

All Onsrud tools have a chipload figured by the factory for that tool, as noted you will find that list by material in the back of the catalog which you can have mailed out or download as a pdf.
Gary

By step down are you referring to how deep I cut per pass? If so then yes its .375 for 3/4

[guitarwes]

When I do, they only scream in the very corners for a split second. The rest of the cuts sound perfect.

I have the same problem. I've contributed it to the machine ramping down in speed to make the corner. Otherwise it just purrs right on thru on the straight cuts.

[dlcw]

I have the same problem. I've contributed it to the machine ramping down in speed to make the corner. Otherwise it just purrs right on thru on the straight cuts.

Slowing down to make a turn will let the bit scream in the turns. No big deal. If it's screaming while running at full speed, then it's an RPM or feed speed issue.