Page 2 of 3 FirstFirst 123 LastLast
Results 11 to 20 of 21

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

  1. #11
    Join Date
    Mar 2005
    Location
    Beckwith Decor Products, Derby/Wichita KS
    Posts
    594

    Default

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


  2. #12
    Join Date
    May 2014
    Location
    MA
    Posts
    409

    Default

    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.

  3. #13
    Join Date
    Mar 2013
    Location
    Memphis TN
    Posts
    629

    Default

    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.
    ShopBot Details:
    PRS Alpha 96x60x12
    4hp Spindle
    12" indexer
    Aspire
    Rhino

  4. #14
    Join Date
    Mar 2005
    Location
    Beckwith Decor Products, Derby/Wichita KS
    Posts
    594

    Default

    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
    Beckwith Decor Products
    ArtCam Trainer
    Custom CNC Tooling/Onsrud Distributor


  5. #15
    Join Date
    May 2014
    Location
    MA
    Posts
    409

    Default

    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.

  6. #16
    Join Date
    Dec 2015
    Posts
    38

    Default

    Quote Originally Posted by garyb View Post
    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

  7. #17
    Join Date
    Mar 2005
    Location
    Beckwith Decor Products, Derby/Wichita KS
    Posts
    594

    Default

    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
    Beckwith Decor Products
    ArtCam Trainer
    Custom CNC Tooling/Onsrud Distributor


  8. #18
    Join Date
    Dec 2015
    Posts
    38

    Default

    Quote Originally Posted by garyb View Post
    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

  9. #19
    Join Date
    Mar 2016
    Location
    Brooklet, Ga
    Posts
    185

    Default

    Quote Originally Posted by EricSchimel View Post
    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.
    2006 PRTalpha 96x48
    3hp SEV spindle
    Vcarve Pro8
    Always eager to consume large amounts of info, tips, and techniques!

  10. #20
    Join Date
    Dec 2008
    Location
    Diamond Lake, WA
    Posts
    1,573

    Default

    Quote Originally Posted by guitarwes View Post
    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.
    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.

Posting Permissions

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