How deep with a 3/8" compression?

[ClayM325]

I'm cutting some 5/8" Birch, and using a compression bit, but the first cut doesn't reach the downcut portion of the bit, and so I'm getting a lot of chipout on the top surface? Can I Cut the first pass deeper if I slow the feed speed? Any other suggestions?

[dlcw]

You want your first cut to first plunge about .25" Then start your ramp to depth. I always make my first cut a climb cut leaving about .025" of material. I then do a conventional cut about .025" thru the material. This process leaves a really smooth cut exactly on the line. That first plunge before ramping is important to eliminate that tear out.

[jTr]

You've got the right idea.
Some of the 3/8 compression bits require even more, like .30" or deeper. I usually go with .345 to .375" depth on first pass. Currently using Centurion bits, and the transition from up-cut tip to down-cut on remainder of shank is at ~ .0348", hence the setting listed. Works fine on my PRSAlpha with a 2.2HP spindle.

Your hold-down method, spindle/router horse power, and most certainly, type of machine need to be taken into consideration.. A desktop, for instance, is likely not going to do so well if you need this done in a hurry.

Still stuck? Try shopping for a different brand of bit - I've seen some that have as little as 3/16 -1/4" up-cut section at the tip. Just depends on whether you can dial it in as mentioned above, or if it's necessary to find a more compatible bit to suit your purposes.

Jeff

[garyb]

Mortise compression have shorter upcut lenghts.
if your running an alpha with spindle then 5/8 birch with a 3/8 compression is a one pass cut.
FYI, I cut 3/4 birch in one pass 546ipm 14k with 3/8 mortise compression (60-123PLR) You would have to figure what works for your machine
Gary

[dlcw]

Personally I cut everything with a 1/4" mortise compression. Like mentioned, a mortise compression has much less up cut spiral thus you don't need to plunge as deep into the material.

For 5/8" Applyeply (like baltic birch) with my particular setup (PRSAlpha 2.2hp spindle, pretty strong vacuum holddown system), I will make 3/8" deep passes at 5IPS @13K RPM.

In softer 3/4" plywood, I will make my first cut all the way to the point of just leaving the .025" skin. Then conventional cut all the way thru. I go 6IPS at 14K RPM. The bits I use have no problem cutting that much plywood at those speeds and feeds on my machine.

One thing Gary taught me, many years ago, you can push these machines pretty hard. I was always hesitant about cutting fast. But as the saying goes, a bit that is screaming as it cuts is a hungry bit. Either increase your feed rate or decrease your RPM's. When you've reached the sweet spot for your machine, the vacuum hold down system (if it resides in your shop with you) is MUCH louder than the cutting bit. When done cutting, you should be able to grab the bit with your fingers (TURN THE SPINDLE OFF FIRST) and it should be room temp. If hot, the bit is spinning to fast (friction) for the feed rate rate you've selected.

The problem I've seen with the Shopbot machines is the inherent flex in the machine. That is why I've switched to the two-way cutting process. Like Gary says, you can cut a piece of plywood with a 3/8" compression bit in one pass. I've found the accuracy of part dimensions using the method to be off a little (but that's probably because my machine isn't as tight as it could be). A climb cut will push the bit away the your cut line. A conventional cut pulls the bit towards the cut line. For parts I cut on my machine, I can go straight from the CNC to the edgebander with no sanding or edge cleanup needed.

Your mileage may vary!! So you need to experiment and figure out what works best for your machine.

[ClayM325]

Personally I cut everything with a 1/4" mortise compression. Like mentioned, a mortise compression has much less up cut spiral thus you don't need to plunge as deep into the material.

For 5/8" Applyeply (like baltic birch) with my particular setup (PRSAlpha 2.2hp spindle, pretty strong vacuum holddown system), I will make 3/8" deep passes at 5IPS @13K RPM.

In softer 3/4" plywood, I will make my first cut all the way to the point of just leaving the .025" skin. Then conventional cut all the way thru. I go 6IPS at 14K RPM. The bits I use have no problem cutting that much plywood at those speeds and feeds on my machine.

One thing Gary taught me, many years ago, you can push these machines pretty hard. I was always hesitant about cutting fast. But as the saying goes, a bit that is screaming as it cuts is a hungry bit. Either increase your feed rate or decrease your RPM's. When you've reached the sweet spot for your machine, the vacuum hold down system (if it resides in your shop with you) is MUCH louder than the cutting bit. When done cutting, you should be able to grab the bit with your fingers (TURN THE SPINDLE OFF FIRST) and it should be room temp. If hot, the bit is spinning to fast (friction) for the feed rate rate you've selected.

The problem I've seen with the Shopbot machines is the inherent flex in the machine. That is why I've switched to the two-way cutting process. Like Gary says, you can cut a piece of plywood with a 3/8" compression bit in one pass. I've found the accuracy of part dimensions using the method to be off a little (but that's probably because my machine isn't as tight as it could be). A climb cut will push the bit away the your cut line. A conventional cut pulls the bit towards the cut line. For parts I cut on my machine, I can go straight from the CNC to the edgebander with no sanding or edge cleanup needed.

Your mileage may vary!! So you need to experiment and figure out what works best for your machine.

Damn. My bits are always screaming. My tool is a PRS Standard and 5hp spindle, but it’s 12-18k and I run at 6ips and 14k. I’ll try lowering rpm a little. Think the motors on the standard can handle cutting all the way through in a pass?

[jerry_stanek]

I cut 3/4 ply in one pass with my PRS standard

[garyb]

Damn. My bits are always screaming. My tool is a PRS Standard and 5hp spindle, but it’s 12-18k and I run at 6ips and 14k. I’ll try lowering rpm a little. Think the motors on the standard can handle cutting all the way through in a pass?

Are you within the chiploads for the tool you are using? As Don noted, if a tool is screaming then typically it means its hungry, not getting enough material. However if you are within chipload ratings for the tool and its still screaming then I would be looking at the tool.

Yes your machine can handle cutting it in one pass, if you do your regular maintenance and have everything tight and adjusted correctly, your machine will preform as intended. I did it on a 2000- 2001 vintage prt for years.
Gary

[EricSchimel]

Depending on your machine setup you can cut with a 3/8 bit pretty fast:

https://youtu.be/wnBVQkTIng4

This is at full depth. Granted this is a best case scenario here, I'm cutting Luan, I don't care about squareness, and I was just having fun.

For "real" work to keep things nice and square I like to cut with a 1/4" compression in three passes, the first one at .375, the second one leaving a .04" onion skin (and .005 larger than the actual cut I need). Then I come back in reverse and take away that last .04 on Z and .005 and I get a laser finish with just about any bit. Also the parts are dead square (I've also obsessively squared my gantry too)

If you're getting screaming others are right: Slow down your spindle speed and speed up your cutting speed. Personally my safe "always works on plywood" speed is around 4-5 IPS at 12k RPM. Another note on the screaming: Onsrud two flue upsprials always seem to scream somewhat, especially in corners. I've found that compressions (with the right feeds and speeds) don't scream at all.

[ClayM325]

Depending on your machine setup you can cut with a 3/8 bit pretty fast:

https://youtu.be/wnBVQkTIng4

This is at full depth. Granted this is a best case scenario here, I'm cutting Luan, I don't care about squareness, and I was just having fun.

For "real" work to keep things nice and square I like to cut with a 1/4" compression in three passes, the first one at .375, the second one leaving a .04" onion skin (and .005 larger than the actual cut I need). Then I come back in reverse and take away that last .04 on Z and .005 and I get a laser finish with just about any bit. Also the parts are dead square (I've also obsessively squared my gantry too)

If you're getting screaming others are right: Slow down your spindle speed and speed up your cutting speed. Personally my safe "always works on plywood" speed is around 4-5 IPS at 12k RPM. Another note on the screaming: Onsrud two flue upsprials always seem to scream somewhat, especially in corners. I've found that compressions (with the right feeds and speeds) don't scream at all.

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

[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.

[guitarwes]

I'm an idiot, I misread his reply thinking he was asking why they were screaming the corners. :confused: