Feeds and Speed and Plunge rates...


Page 1 of 2 12 LastLast
Results 1 to 12 of 20

Thread: Feeds and Speed and Plunge rates...

  1. #1
    Registered
    Join Date
    Mar 2010
    Location
    United States
    Posts
    433
    Downloads
    0
    Uploads
    0

    Default Feeds and Speed and Plunge rates...

    Feeds and Speed and Plunge rates...

    I'm finding a lot of information on Aluminum and other machining material but struggling to find Wood and MDF speeds and feeds, seems like a common question on the forum. Is there a repository, etc.?

    Is there guideline to follow when plunging, are people having better success with some speeds than other, best practices?

    I know the common reply is that it depends on your machine, I get that to some extent but at some point don't most machines have the same capability?

    For instance if your taking light passes at light depths shouldn't most machines be able to fit into a standard speed and feed and plunge rate formula based upon bit type?

    Adam,

    Similar Threads:


  2. #2
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    31696
    Downloads
    0
    Uploads
    0

    Default

    If you go fast enough, even a light pass becomes a heavy pass.
    Personally, I always try to ramp into the material rather than plunge. With wood, you can usually ramp in at full cutting speeds.

    What size bits, and how fast can your machine go?

    You can usually cut wood far faster than most people think, but machine rigidity and spindle power will usually limit the speed that you can achieve good quality cuts at.

    Onsrud has chip load charts on their website for all types of wood and panel materials and their different lines of bits.

    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  3. #3
    Gold Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5324
    Downloads
    0
    Uploads
    0

    Default

    As gerry says, it's almost always better to ramp or helix in, unless you can't. When I do plunge I like to cut the feedrate at least in half, though if you ramp in you usually can at your feedrate. You can download Onsrud's catalogs which have their recommended chiploads. I use the chipload numbers to get my feeds, then adjust the DOC to my machine.

    I prefer not to take light passes at light depths. It's a great way to unevenly wear your tools down. Also it's a less ridgid cut. Obviously, not all of us have machines as ridgid and powerful as commercial machines. But you should try to cut as close to your bit diameter for depth, at least for pocketing. When profiling I'll go 1/2 to 2/3 of my pocketing depth, because the tool is fully engaged in the work.



  4. #4
    Registered
    Join Date
    Mar 2010
    Location
    United States
    Posts
    433
    Downloads
    0
    Uploads
    0

    Default

    Thanks for the great info as usual your experience is helpful to those of us just getting started.

    "What size bits, and how fast can your machine go?"

    I'm thinking the majority of work will be done with 2 flute (1/4-1/2) carbide bits but obviously would change with the type of material and finish I'm looking for.

    As far as how fast my machine will go that's a great question... what's the best way to test what the machine is capable of?

    " You can download Onsrud's catalogs which have their recommended chiploads."

    Already have done that thanks, working on figuring out the math on a worksheet so its little bit handier than having to recalculate each time.

    "Helix" in can someone explain that one?

    Adam,

    Last edited by adam_m; 01-21-2014 at 06:20 AM.


  5. #5
    Gold Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5324
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by adam_m View Post
    Thanks for the great info as usual your experience is helpful to those of us just getting started.

    "What size bits, and how fast can your machine go?"

    I'm thinking the majority of work will be done with 2 flute (1/4-1/2) carbide bits but obviously would change with the type of material and finish I'm looking for.

    As far as how fast my machine will go that's a great question... what's the best way to test what the machine is capable of?

    " You can download Onsrud's catalogs which have their recommended chiploads."

    Already have done that thanks, working on figuring out the math on a worksheet so its little bit handier than having to recalculate each time.

    "Helix" in can someone explain that one?

    Adam,
    In a helix-in or spiral-in move, the tool does exactly that, helix or spiral move down to cut depth before proceeding (usually done in pocketing.)

    As to how fast your machine can go, only you can figure that out. You've probably got your rapids speed set already. That has nothing to do with your feedrate; that is determined based on your spindle speed, chipload and the number of flutes. You'll just have to do some experimenting.



  6. #6
    Registered
    Join Date
    Mar 2010
    Location
    United States
    Posts
    433
    Downloads
    0
    Uploads
    0

    Default

    So I have Keeling motors on my machine.

    NEMA 23 Stepper Motor: KL23H2100-35-4B (1/4” Dual shaft with a flat) 381 oz-in
    Specification (Inductance 2.8 mH) Can be used for G540, G251, G250 or any other driver
    381 oz In. Hybrid Motor
    1.8° /200 Steps Per Rev.
    3.5 Amps Current Per Phase
    4-wire Bi-polar, NEMA 23 Frame
    From their website it looks like this is the calculation:

    Motor Tuning:
    Finally we’ll get to actually spin some motors. The first thing in the tuning process is to
    calculate how many steps per unit of travel we have. This depends on a few things:
    In case of a step motor:
    • The amount of steps per revolution, most commonly 200.
    • The step resolution of the motor drive, if you set at 8
    • And finally, the thread pitch of the screw. (How far the table moves with each rotation
    of the screw) let say it has a 5TPI pitch.

    So Step per should be 200 x 8 x 5 = 8000.

    I'm assuming the 200spi is maximum free without any tension?

    So, if you wanted to test to see what the Maximum is where would you adjust since everything else i fixed the Steps Per Inch?

    I now realize that what I have set in Mach3 is based on the G540 and not from Keeling... attached.

    Does the G540 come into play at all when tuning the motors?

    Adam,

    Attached Thumbnails Attached Thumbnails Feeds and Speed and Plunge rates...-snag-0032-jpg  


  7. #7
    Gold Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5324
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by adam_m View Post
    So I have Keeling motors on my machine.



    From their website it looks like this is the calculation:




    I'm assuming the 200spi is maximum free without any tension?

    So, if you wanted to test to see what the Maximum is where would you adjust since everything else i fixed the Steps Per Inch?

    I now realize that what I have set in Mach3 is based on the G540 and not from Keeling... attached.

    Does the G540 come into play at all when tuning the motors?

    Adam,
    20000 steps/inch? With a G540 (which has 10x microstepping) I'd have to guess you're using 10tpi leadscrews? I don't know what your power supply is, but if it's 48v, you probably can get 1000-1200rpm out of your steppers, which I would guess give you a rapids speed of about 100-120ipm. It looks your acceleration could be a bit higher; experimentation is needed. You basically raise each number (velocity, accel) till you stall the axis, then drop down about 10-20%, and that's your max velocity and acceleration. Do it for each axis.

    For wood, I like the spindle to be between 10krpm-15krpm. So for a 1/4" 2-flute bit, with a chipload rating of .004", that would be a theoretical feedrate of 80-120ipm at 1/4" doc. Can your machine handle that? Only way to find out is to test it. 120ipm is probably the upper limit of your machine and you may not have enough torque available to cut at that speed. The only way to reduce the feedrate is to also reduce the spindle speed as they are directly proportional. I would try the low chipload number at the slowest spindle speed possible for each tool, then do test cuts starting at half tool diameter for depth and going progressively deeper till it's apparant your spindle is getting bogged down, then back off a little and that's your tool depth. Is there a magic umber? No, it's different for all machines since all machines have different specs. Higher horsepower spindles can handle higher chiploads. You may or may not be able to cut at the recommended minimum. There's always some compromise.

    There is another number, sfm, or surface feet per minute, which is used to determine the max speed of the tool, but we don't have to worry about it here since we likely won''t be able to reach that max given your machine specs. There may be a minimal sfm, but that likely won't apply either since we can only work with what we got for our DIY machine and may not even reach the minimum sfm for a specific too.



  8. #8
    Registered
    Join Date
    Mar 2010
    Location
    United States
    Posts
    433
    Downloads
    0
    Uploads
    0

    Default

    Great information louieatienza, I'll certainly be testing all kinds of scenarios after I get the axis setup correctly..

    20000 steps/inch? With a G540 (which has 10x microstepping) I'd have to guess you're using 10tpi leadscrews? I don't know what your power supply is, but if it's 48v, you probably can get 1000-1200rpm out of your steppers, which I would guess give you a rapids speed of about 100-120ipm. It looks your acceleration could be a bit higher; experimentation is needed. You basically raise each number (velocity, accel) till you stall the axis, then drop down about 10-20%, and that's your max velocity and acceleration. Do it for each axis.
    Yes, sorry that was a typo 20000 as can be seen from the image. I am also running a 48v power supply...

    So this being a rack and pinion on the X and Y axis I gleaned this from CNCRouter's website.. missed it.

    A: The base resolution of the system is 190.986 steps per inch with a 200 steps per revolution stepper motor. Multiply this by however many microsteps your driver has. For example, with a G540 (10x microstep), your resolution would be 1909.86 steps per inch.

    "Stall" the axis, what does that look like or sound like?

    Adam,



  9. #9
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    31696
    Downloads
    0
    Uploads
    0

    Default

    Kind of a loud nasty grinding/buzzing type sound and the machine will stop. You can't miss it.

    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  10. #10
    Registered
    Join Date
    Mar 2010
    Location
    United States
    Posts
    433
    Downloads
    0
    Uploads
    0

    Default

    Loud noise... eek!

    So, I think I have the Motor tuning for my X,Y and A drives with the G540, Keeling motors and Rack and pinion (3:1) but would appreciate your review...

    The R&P system is based on a pinion with a 1" pitch circle. The total linear distance traveled per revolution of the pinion is thus 3.14159". With the 3:1 reduction, this means that the distance traveled per motor revolution is 3.14159 / 3, or 1.0472". If you have a stepper with 200 steps per revolution, this means you have 200 / 1.0472" = 190.9861 steps per inch, or 0.005236" per step. With 10x microstepping (like in the G540), you would have 1909.861 steps per inch, or 0.0005236" per step
    So these are what I assume to be legitimate settings for MACH for my X, Y and A axis.

    Steps 200 x 10 = 2000
    Velocity = 120
    Acceleration = 4
    Step Pulse = 5
    Dir Pulse = 5



    My Z is a 1/2-10 5start Acme, I think this is correct?

    Steps 200 x 10 x 2 = 4000
    Velocity = 30
    Acceleration = 2
    Step Pulse = 5
    Dir Pulse = 5


    Adam,



  11. #11
    Registered JerryBurks's Avatar
    Join Date
    Aug 2011
    Location
    USA
    Posts
    922
    Downloads
    0
    Uploads
    0

    Default

    The acceleration in your numbers is very low (assuming this is inch/sec^2). At that rate you will have the axis winding up and decelerating almost a second before the top speed or standstill are reached. It may even make fast jogging a bit difficult due to overshoot.

    As Gerry mentioned the stall noise is nasty and obvious when getting stuck in a long stroke with too high speed or too much mechanical load (usually no damage, though). But under some conditions, like stalling when going around a very small radius too fast or stopping too hard, the duration of the stall may be only a fraction of a second and can be missed if you don't pay good attention. Then the motor has slipped a few steps and you may only notice at the end of the run when the work is ruined.

    Box Joint and Dovetail CAM software here: WWW.TAILMAKER.NET


  12. #12
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    31696
    Downloads
    0
    Uploads
    0

    Default

    Both your velocities and accels are way low I think compared with other users of similar setups.
    I don't use rack and pinion, but I think most rack and pinion users are running at velocities of at least 400-500ipm, and accels closer to 30

    On my Z axis, with 1/2-10 single start and a Xylotex drive at 24V, my velocity is 55 with an accel of 5. I would think you should be able to run at least 4x faster than me.

    Also, I would think that your steps/inch on your rack and pinion is not correct, and will give you incorrect travel distances.

    To set your velocity, leave the accel where it's at, or bump it to at least 10. Then, start increasing the velocity in increments of 25, and jog back and forth at each speed. When you see a stall, then back off the velocity by 20%. That should be your velocity.

    Once the velocity is set, start increasing the accel, and again, jog back and forth until you see a stall. Then back off 20%. Now you have your accel setting.

    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


Page 1 of 2 12 LastLast

Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Feeds and Speed and Plunge rates...

Feeds and Speed and Plunge rates...