Results 1 to 9 of 9

Thread: Realistic Cutting/Rapid Speeds on Laguna/Axiom/Powermatic/Grizzly CNC Machines

  1. #1

    Question Realistic Cutting/Rapid Speeds on Laguna/Axiom/Powermatic/Grizzly CNC Machines

    I have a new-to-me Laguna iQ CNC machine. I'm slowly getting to know the machine and have been running it very conservatively.

    I've been doing a lot of reading about speeds/feeds, and I'm beginning to think that my conservative approach is needlessly slow and bad for bit life. By searching this forum, I found this amazing site - https://app.fswizard.com/ - which provides recommended speeds/feeds.

    As a somewhat silly example, according to this site, cutting a 1/2" slot through a sheet of 3/4" plywood in one pass using a carbide bit should be done at 14.8K RPM/227 IPM and will use 1.36 HP/0.5 ft-lb torque with a cutting force of 23 pounds. My spindle is 3HP @ 24K RPM = 0.7 ft-lb torque, so this is within the limits of my spindle. And my stepper motors feel like they'd easily lift 23 pounds, although I have no idea what I'm really talking about. But 227 IPM seems ludicrously fast for this operation even with step downs, let alone at full plywood thickness...

    As a more realistic example, according to the site, cutting 3/4" plywood with a 1/4" bit in one pass at ~100 IPM is barely pushing the machine (0.36 HP, 7 pounds cutting force).

    So, my question is, what are realistic maximum cutting speeds for Laguna iQ-style machines. And by extension, what about maximum rapid speeds? Axiom's marketing says 300 IPM rapids, Powermatic's says 200 IPM rapids and Grizzly's says 400 IPM CUTTING.

    I'm interested in knowing this so that when the website gives me insanely high feeds/speeds, I know at one point I need to start messing with other parameters because the machine simply won't ACCURATELY go that fast even if the spindle and the steppers have more than enough power.


    Also, as an aside, unless it's just "more power, more better" marketing, it seems that the spindles on these machines are WAY oversized relative to the capabilities of the machines themselves...or am I missing something?

    Thanks in advance.

  2. #2
    Join Date
    Mar 2003
    Location
    SE PA - Central Bucks County
    Posts
    60,562
    Many sites like that often assume an industrial level machine so you have to experiment with what you have to find out what works and produces both the desired quality/accuracy while also supporting adequate chip-load (which takes away heat from the tooling) and not breaking tools or overtaxing the steppers/servos. My opinion is that the level of machines you are asking about are really not suitable for single pass cutting in .75" sheet goods. Can they do it? Yes, but it's a chore. I personally use 2-3 passes with my Camaster Stinger II with heavy 900 oz NEMA 34 steppers and a 1.7kw spindle. That's with .357" or .25" tooling. I can run 1/2" but don't prefer that much waste on a 4x4 machine. My machine can rapid at 500-600 ipm, but that's not cutting speed. That's repositioning. I can push to 400 ipm in straight lines that have minimal load, but typically, I'm getting more like 200-300 ipm. Note, this is for 2D cutting. Add a lot of turns where acceleration/deceleration comes into play, the effective cutting speed necessarily drops a little.

    So my advise is that the various online resources for speeds/feeds are only a starting point and it's a best practice to start conservatively and work you way up on your own machine to the point that you are maximizing your throughput without killing quality. You have to get to know your machine and what works for it specifically. No calculator is going to do that for you.
    --

    The most expensive tool is the one you buy "cheaply" and often...

  3. #3
    You will have to experiment to find the sweet spot on your machine. Try running at the recommended chip load and see how it works, or start slower and increase the feed until cut quality suffers or the motor bogs down. I think a more typical bit diameter would be 3/8" for that material - you want a stiff enough bit without making a wasteful kerf. If your machine is powerful and stiff enough to run at the ideal rate and give a good quality cut that will allow the bit to run cool and have maximum life. If not you will have to run slower and have higher tooling costs for production. It would be easier on the tool to cut through in two steps at optimum speed than one pass at slow speed. Shops with heavy machines may run up towards 1,000 ipm with multi-flute bits.
    Last edited by Kevin Jenness; 01-05-2022 at 7:35 PM.

  4. #4
    Join Date
    Oct 2009
    Location
    Marquette, MI USA
    Posts
    499
    Matt...
    Your assumptions are correct, but you are missing what may be the most important spec: The ability of the machine frame to withstand cutting force, i.e., deflection. This affects the ability to cut smooth accurately sized parts. This is what each user must "dial in". Each of us needs to experiment to obtain our best feeds and speeds to get the desired edge quality and accuracy.

    Along with machine frame specs, hold down, material type, sharpness of bit will determine optimum feedrates.
    Gary Campbell
    CNC Replacement & Upgrade Controllers
    FabMaster ATC-40 Bridgemill

  5. #5
    Not sure from reading your post but you may be intermixing "rapids" and "feeds"? Rapids are no cutting, moving from point to point, how fast the machine moves from one start point to the next with no tool engagement. This would hopefully be as fast as any particular machine can run as per the manufacturer's specs for the components (steppers/servos etc).

    Your cutting feeds (and tool wear) are of course exactly that. While you can dial down your rapids while your learning just to make sure you have a few extra milliseconds to catch a crash or other issue due to bad code its best for these to be as wide open as possible as all those moves are doing zero production work for you. So if you have your safe z heights correct you should be running all of those wide open.

    Be careful with the FS tool wizard as it can be very conservative. Its great you found the FS wizard its calculator I use by default and its a good starting point. Your reference of a 1/2" tool (assuming 2 flute) full depth in 3/4" ply really doesnt apply as your machine will never be able to push the tool fast enough (feed rate) or you will have to run the tool rpm so slow, it will be unrealistic.

    The larger HP spindles are moreso there so you can run a tool at a lower RPM and still have the power (due to HP loss across the power curve). I have 10hp spindle, 600ipm max feed speed, and what I consider a very rigid machine in its class, and in most cases I cant push my machine fast enough to run 1/2" tooling. My feed speeds would need to be up in the 1000-1100ipm range and I still wouldnt be running the spindle wide open. What I do wind up doing is running a 3/8" compression at 600ipm and 14K rpms (well below the 24K the spindle maxes out at) to do exactly as you are thinking, save the tool.

    Your on the right track that if your running slow your burning up tools. They are just sitting there grinding themselves to death generating heat. Use a calculator to get you a starting point then start using your eyes and ears, run your machine fast as you can while generating a good chip and dont be afraid to break a few tools. Try a few 1/4" compressions, try a few 3/8" compressions (you can buy cheaper ones to start) and start at your calculator start point and quickly start ramping up your feeds using your ear and looking at the chips. You'll know when your at the sweetspot a few moments before the tool breaks. Back it down from there and thats your money maker.

  6. #6
    Thanks, guys, for your responses. Glad to hear my thinking is on the right track.

    For the heck of it, because I'm hyper-analytical, I decided to crunch some numbers to get a SUPER-ROUGH, THEORETICAL sense of what my machine MIGHT be capable of. Basically, I found some formulas online for stepper motor RPM vs. amps and lead screw force, and used my stepper motor specs to run the calcs. I also measured the amps required to move my gantry (on the Y-axis, which is moving the X- and Z- axes and is therefore the hardest to move) at various speeds and baked that in.

    The result, which you can view here - https://docs.google.com/spreadsheets...it?usp=sharing - shows with numbers what is logically obvious:

    As speed goes up, the available power remaining to push router bits through stuff diminishes, and since bigger bits use more force at a higher ideal speed, this results in theoretical maximum bit diameters for given scenarios (permutations of pass depth and material).

    For example, using these numbers, that 1/2" bit scenario from my post above is basically the absolute max my machine will theoretically do (including my factored-in safety margin of 50%, to cover curves, bad math, bad theory, my stupidity, climb vs. conventional milling, etc., etc., etc.). Alternatively, a real-world scenario like trying to cut through 3/4" plywood using a 1/4" bit in one pass should, theoretically, be no problem for my machine.***

    ***There are two key assumptions in all of this:

    1. The FS Wizard site gives wood a Brinell hardness of 2, which is quite soft. From the reading I've been doing, MDF is ~4 and plywood is ~5. I have no idea how much this changes things, but I'm sure it has some impact.
    2. To @Gary Campbell's point, the machine has to be stiff enough, and the clamps strong enough, etc., etc. to put all this theoretical power into the workpiece, and the workpiece has to be able to take it without chipping, cracking, etc.

    Long story short, my net takeaway from all of this is that I've been babying my machine and it's theoretically quite a bit more capable than I thought. I do think 3/4" plywood in one pass using a 1/4" bit at 100 IPM is not only possible, but reasonable, and will save time and tool life. Now I just need to test it...!

    Also, for what it's worth, I tested my machine at 400 IPM today ("rapid-ing," not cutting anything) using a tape measure and a stopwatch and found it hit the speed I asked for and didn't appear to miss any steps (distance moved on the controller matched distance moved on the tape measure). Also, using my numbers, it seems the theoretical real-life maximum speed of my machine is somewhere between 400 IPM and 500 IPM.

    For those who enjoy this kind of armchair engineering, would love to hear your feedback. Thanks!

  7. #7
    Put down the calculator and cut some material.

  8. #8
    Join Date
    Oct 2009
    Location
    Marquette, MI USA
    Posts
    499
    Quote Originally Posted by Matt Culik View Post
    For those who enjoy this kind of armchair engineering, would love to hear your feedback. Thanks!
    +1 to what Kevin says.... and while you're at do these real world tests:

    Make a straight line cut 3-4" long with a 1/4" bit slow speed, mid-hi rpm and measure the slot to find out what diameter your wood thinks the bit is

    Set your rpm to 15k rpm, cut depth to 1/4" and feed to 60ipm
    Using that diameter cut outside circle and square vectors of 4 & 6" both climb and conventional direction starting at 60ipm and increasing by 60 to repeat
    Compare each set (climb vs. conventional) to determine how much machine deflection there is. (half of the difference)
    Then test at 1/2" cut depth and 3/4" if you wish
    Use your findings to determine what speeds are best for your products on your machine with your bits

    And ignore all "bit deflection" info from those who produce machines with inherent flex. Tungsten carbide is a crystalline compound, it will snap, not bend.

    For rapids, find the max speed you can travel with obvious failure. Set steppers at 60% of that speed, servos at 80%
    Last edited by Gary Campbell; 01-09-2022 at 8:39 AM.
    Gary Campbell
    CNC Replacement & Upgrade Controllers
    FabMaster ATC-40 Bridgemill

  9. #9
    Join Date
    May 2008
    Location
    MA
    Posts
    2,000
    Quote Originally Posted by Gary Campbell View Post
    +1 to what Kevin says.... and while you're at do these real world tests:

    Make a straight line cut 3-4" long with a 1/4" bit slow speed, mid-hi rpm and measure the slot to find out what diameter your wood thinks the bit is

    Set your rpm to 15k rpm, cut depth to 1/4" and feed to 60ipm
    Using that diameter cut outside circle and square vectors of 4 & 6" both climb and conventional direction starting at 60ipm and increasing by 60 to repeat
    Compare each set (climb vs. conventional) to determine how much machine deflection there is. (half of the difference)
    Then test at 1/2" cut depth and 3/4" if you wish
    Use your findings to determine what speeds are best for your products on your machine with your bits

    And ignore all "bit deflection" info from those who produce machines with inherent flex. Tungsten carbide is a crystalline compound, it will snap, not bend.

    For rapids, find the max speed you can travel with obvious failure. Set steppers at 60% of that speed, servos at 80%

    Thank you, awesome exercise!

Posting Permissions

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