Page 1 of 3 123 LastLast
Results 1 to 10 of 21

Thread: How deep with a 3/8" compression?

  1. #1
    Join Date
    Dec 2015
    Posts
    38

    Default How deep with a 3/8" compression?

    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?

  2. #2
    Join Date
    Dec 2008
    Location
    Diamond Lake, WA
    Posts
    1,605

    Default

    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.
    Don
    Diamond Lake Custom Woodworks, LLC
    www.dlwoodworks.com
    ***********************************
    Life is not a journey to the grave with the intention of arriving safely in one pretty and well preserved piece; But to skid in broadside, thoroughly used up, worn out, bank accounts empty, credit cards maxed out, defiantly shouting "Geronimo"!

    If you make something idiot proof, all they do is create a better idiot.

  3. #3
    Join Date
    Dec 2011
    Location
    Piedmont, SD
    Posts
    653

    Default

    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

  4. #4
    Join Date
    Mar 2005
    Location
    Beckwith Decor Products, Derby/Wichita KS
    Posts
    604

    Default

    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
    Beckwith Decor Products
    Custom CNC Tooling/Onsrud Distributor


  5. #5
    Join Date
    Dec 2008
    Location
    Diamond Lake, WA
    Posts
    1,605

    Default

    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.
    Don
    Diamond Lake Custom Woodworks, LLC
    www.dlwoodworks.com
    ***********************************
    Life is not a journey to the grave with the intention of arriving safely in one pretty and well preserved piece; But to skid in broadside, thoroughly used up, worn out, bank accounts empty, credit cards maxed out, defiantly shouting "Geronimo"!

    If you make something idiot proof, all they do is create a better idiot.

  6. #6
    Join Date
    Dec 2015
    Posts
    38

    Default

    Quote Originally Posted by dlcw View Post
    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?

  7. #7
    Join Date
    Dec 2007
    Posts
    2,300

    Default

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

  8. #8
    Join Date
    Mar 2005
    Location
    Beckwith Decor Products, Derby/Wichita KS
    Posts
    604

    Default

    Quote Originally Posted by ClayM325 View Post
    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
    Beckwith Decor Products
    Custom CNC Tooling/Onsrud Distributor


  9. #9
    Join Date
    May 2014
    Location
    MA
    Posts
    434

    Default

    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.

  10. #10
    Join Date
    Dec 2015
    Posts
    38

    Default

    Quote Originally Posted by EricSchimel View Post
    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

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •