Announcement

Collapse
No announcement yet.

Feedback on Feed and Speed Calculators

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts
  • Feedback on Feed and Speed Calculators


    Hello Ladies and Gentlemen,

    I recently ordered my stinger i and it is currently in production. I'm new to CNC machinery and took it upon myself to learn as much as I can before it arrives. I followed this forum and did research on CNC machines. I'm hoping my first cut won't result in a disaster. There was so much to wrap my head around; Aspire, WinCNC, CAD...etc....

    So when I discovered feed and speed rates and learned it was not an exact science it boggled my brain. How did we not figure this out? I learned there was so many variables that a simple formula would only put us in the ballpark.

    During my slow adventure of trying to figure all this out, I found two software feed and speed calculators. One is from CNC Cookbook, GWizard G-Code Editor, and the other is an Apple App in the App store, FSWizard Pro.

    Each lets you select material, tools, and enter some other data and POOF!, you get your feed and speed rate. But this is where I ran into a problem.

    With my newly acquired machine I will primarily be working on Wood, Ply and hard wood. In both calculators I entered the exact information:

    Material: Hardwood
    Tool: Carbide Endmill, .5 D, 2 flutes
    Cut Depth: .25
    Cut Width:.25

    G-Wizard= 5561 RPM and 161.269 Speed
    FSWizard Pro= 9172 RPM and 237.74 Speed

    I'm assuming both programs are in inches.

    Does this seem right? Why such a large gap in numbers? Anyone have feedback on any of these programs? Should i even bother with these calculators?

    BTW FSWizard costs 17.99 in the apple app store and G-Wizard is subscription: 79/yr, 129/3yrs, or 249 for a life subscription.

    Thanks in advance.

    -Romeo (that is my real name)
    Stinger I
    1.7 KW (2.27HP) HSD Spindle
    Indexing Lathe
    Digitizing Probe
    Laser Cross
    FTC
    T-Slots
    Aspire 3, Cut 3D, WinCNC
  • #2

    The first thing I see is it looks like the tool diameter is 1/2 inch and the cut diameter is 1/4 inch. Most programs wouldn't allow it by toolpathed that way. Could that be throwing off the calculations?

    Secondly, why are we up on the forum at 2:30 in the morning? Shouldn't we be sleeping?
    Kevin Tringle
    Stinger II 4X4 w/1.0Spindle
    Graphtec FC5100-75 Plotter/Cutter
    AutoCAD 2010-Flexi-Sign-V-Carve Pro

    Comment

    • #3

      Why are we up on the forum at 2:30 in the morning? Shouldn't we be sleeping?
      Sleep what's that
      Romeo,

      I see that you have ordered a router I think you might have a problem dialing in the following
      G-Wizard= 5561 RPM
      FSWizard Pro= 9172 RPM

      I tend to cut around 14000 / 16000 rpm and adjust my feedrate as needed.
      Mick Martin
      mickmartin3@comcast.net
      CAMaster Cobra 508 ATC + Recoil + Popup Pins
      Digitize Touch Probe
      Wincnc Handheld Serial Keypad + Wireless Pendant
      Hurricane vacuum
      WinCNC + Aspire 9.5 + PhotoVCarve + EnRoute 5
      www.mickmartinwoodworking.com/

      The search function on the forum is your best friend!

      Comment

      • #4

        Hi,

        First, welcome to the owners club! :)

        For my Stinger I I find that for a majority of wood cutting (hardwood and plywood) a speed of about 15K-17K RPM and a X/Y feedrate of about 100 ipm with the Z of 30 ipm does pretty well. As mentioned above, the depth of cut is adjusted to what works and sounds about right ( one half diameter of bit is a good starting point). I am sure one can go a bit faster but I mostly do one-off parts and these numbers usually get me started.

        As for bits, a couple different 1/4 inch bits, and a 60 and 90 degree 'V' bit will do many interesting things to get you started. If you have not used a CNC before a 'V' bit is a good one to start with. The hard part that not many talk about is how to fixture the workpiece. You will likely find that to be the most challenging part of the entire process.

        Robert
        Stinger I Router / WinCNC
        SprutCAM, V-Carve,ZW3D
        Tormach PC1100 / Mach3

        Comment

        • #5

          in the beginning try running shallower depths to see chipload, increase depth to comfort level if you get powder it is to hot, if it breaks it is too cold.
          James McGrew
          CAMaster ATC 508
          The principle of Measure twice cut once has not been replaced by a CNC

          www.mcgrewwoodwork.com

          https://www.facebook.com/pg/Mcgrew-W...=page_internal

          Camera 1 ATC Closeup !
          https://video.nest.com/live/esNTrZ

          fixed 4-27-2020

          Comment

          • #6

            Romeo...
            Welcome!

            The real answer is that there is no real answer. Most of the chipload calculators out there are tilted towards high horsepower machines, maybe even milling. Big iron. Forget them.

            As you can see from the responses above there is variation even between accomplished users. What will be the common thread between them is that they will recommend "starting points". We all have our goto numbers that we know will work, and we tune from there. Different rpm and/or feedrates are required to get the best cuts for each different combination of machine, bit and material.

            I like to recommend to new users some conservative guidelines to start.

            Use a 1/4" or larger bit
            Start at 15000 rpm and be prepared to go down
            use 1 bit diameter max for pass depth
            take the bit diameter / 1/8 = 2
            2 X 60 = 120 ipm adjust down if hard dense material up if soft
            the 2 above would be reduced if majorities of the cut geometries were less than 2 inches long i.e. 1 for a 1" part, etc.

            Toolpath some circles and squares on scraps of the exact material you wish to cut and test using your fingers to feel the chips, a digital caliper to actually measure them, if you wish, and most important, your ears to hear the cutter and router spindle. Vary the feeds up and down, along with the rpms until you can hear "the sweet spot".

            Also cut in both conventional and climb directions. Most plywoods and a good number of solids leave the best finish in conventional direction. You must test to be sure.

            In time this will become second nature to you. Remember the following:
            Always tune for quality, best finish, FIRST! Then increase feeds til quality drops off.
            IF you have a "sweet spot" and raise feed rates by 25% raise rpms by 25% too
            The longest bit life comes from the slowest rpms and fastest feed rates.
            Do not expect to exceed the power of your router/spindle and get good results. You will hear them "bog down" (lower feeds to fix)

            My personal experience showed little advantage in cutting wood over 13,500 rpm and under 240 ipm, but that takes a full size machine & 5hp spindle to accomplish. We have all seen dust. Here is an example of chipload on a custom "louver groover" that I built in the Caribbean:

            1.7kw spindle, 1/4" single flute bit, 240 ipm feed, .26 pass depth @10K rpm. This is an extreme example, but should help you determine if you are getting chips or dust.
            Attached Files
            Gary Campbell
            Servo Control Upgrades
            GCnC411@gmail.com
            https://www.youtube.com/user/Islaww1/videos

            "There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"

            Comment

            • #7

              Excel spreadsheet chipload calculator

              Jim McGrew posted an excel spreadsheet chipload calculator a while back that a lot of people use http://camheads.org/showthread.php?t=287
              Mick Martin
              mickmartin3@comcast.net
              CAMaster Cobra 508 ATC + Recoil + Popup Pins
              Digitize Touch Probe
              Wincnc Handheld Serial Keypad + Wireless Pendant
              Hurricane vacuum
              WinCNC + Aspire 9.5 + PhotoVCarve + EnRoute 5
              www.mickmartinwoodworking.com/

              The search function on the forum is your best friend!

              Comment

              • #8

                Thanks guys. This is great info

                In summary:

                * With wood cutting start with about 15k
                * DO NOT exceed the bit diameter in depth
                *Powder is too fast and breakage is too slow
                * Start with larger bits until comfortable
                * Make some practice cuts to find the "sweet spot"
                *Find the slowest RPM and fastest feed rate (this advise kinda put everything together for me)

                Does everyone agree?

                Gary, you gave me a great info and a great example of what the chips are suppose to look like, but you confused me with your math and other stuff. I didn't understand it.

                "use 1 bit diameter max for pass depth (I got this)
                take the bit diameter / 1/8 = 2 (I did not get x/ 1/8=2)
                2 X 60 = 120 ipm adjust down if hard dense material up if soft ( I have no idea where '2' and '60 'came from)

                the 2 above would be reduced if majorities of the cut geometries were less than 2 inches long i.e. 1 for a 1" part, etc." (I got this)

                IF you have a "sweet spot" and raise feed rates by 25% raise rpms by 25% too (huh?)

                Thanks again everyone this is really good information. Everyone here in this forum is great.
                Stinger I
                1.7 KW (2.27HP) HSD Spindle
                Indexing Lathe
                Digitizing Probe
                Laser Cross
                FTC
                T-Slots
                Aspire 3, Cut 3D, WinCNC

                Comment

                • #9

                  Romeo...
                  Sorry to confuse you. First the math.....

                  Bit diameter (1/4) divide by 1/8 and get 2 (inches per second feed rate)
                  2 ips times 60 = 120 inches per minute federate Hope this helps

                  The chipload calculator posted by Jim and linked by Mick is pretty good. If I put the numbers I gave you in it a .006 chipload is returned. That is a conservative place to start. And if you play some with the numbers, you will see that you will increase chipload by either increasing feed, or decreasing rpm.

                  I do think that the recommended chiploads in the calculator are pretty aggressive for small machines. By almost double for at least the wood products. For example, to reach that .025 chipload in wood with midrange 15000 (router) requires a federate of 750 ipm. Not gonna happen.

                  The chart returned a .024 chipload number for my louver chips in the pic. The actually measured at or just under .020. Which lets me know that I was not attaining full feed during the geometry. Feed was lowered to 120 and it returned .011 to .015 chips that didn't tear out the surface as much.

                  The speed vs feed percentage means that to keep the same chipload (stay in the sweet spot) if you speed up feeds, like for a large part, increase the rpm by the same percentage. Download Jims chart and change a few numbers. It may become clearer.
                  Last edited by Gary Campbell; 12-29-2013, 09:05 AM.
                  Gary Campbell
                  Servo Control Upgrades
                  GCnC411@gmail.com
                  https://www.youtube.com/user/Islaww1/videos

                  "There are 10 kinds of people in the world. Those that understand binary logic, and those who don't"

                  Comment

                  • #10

                    Thanks everyone.

                    Seeing that a spindle would be more beneficial to me rather than a router, I called Camaster and upgraded to a 1.7kw Spindle w/ counterweight.

                    I'm excited and reorganized my portable shop, awaiting the Stingers arrival.
                    Stinger I
                    1.7 KW (2.27HP) HSD Spindle
                    Indexing Lathe
                    Digitizing Probe
                    Laser Cross
                    FTC
                    T-Slots
                    Aspire 3, Cut 3D, WinCNC

                    Comment

                    • #11

                      Good call on the spindle, Romeo! That's what I have and I love it. It's powerful and quiet at the same time.

                      I would try some simple profile cuts first (cut out some circles and squares) with a cheap 1/4" bit and try doing 1/2 the diameter depth (1/8" deep) just to get a feel for the speed and sound. Set your feed speed and rpms in the program but be aware that you can adjust them on the machine as you are running so you can fine tune your chips a bit. The spindle has a little control panel with a rheostat for speed (rpm). I mounted mine in a little easier to see position in front of my keyboard. In WinCNC, you will see a panel at the middle left (I'll find a screen shot for you) with X, Y, Z and A and a slider on the right of them. It says 100% above the slider when you start the machine and you can adjust it up and down.

                      We are all here to help you so don't be afraid to ask us anything at all!

                      Mike
                      Attached Files
                      Mike Schnorr
                      Stinger 1 with Spindle and Recoil
                      Win CNC - Aspire 10.0
                      Sidewinder Back Knife Rotary
                      www.artcentergraphics.com
                      www.baconwood.com

                      Comment

                      • #12

                        Gary, can you post your chip load calculator?
                        Big Papi (John Smith)
                        Camaster 508 ATC / WINCNC / Aspire

                        Comment

                        • #13

                          Like many folks I played with feeds and speeds and my summary...

                          A: the stinger only goes so fast. I've tried to measure mine and it doesn't do much more than 200 IPM so you can forget about faster speeds. When cutting arcs and reversing directions it's even slower.

                          B: The chip load is a function of the number of flutes on a spiral bit so don't get more than 2. You can't go fast enough. I use 4 on carving bits for strength but they're not chiploaded.

                          C: Speed can depend on how you're cutting and what wood. I cut hickory way slower than mahogany - so 'hardwood' isn't enough info. I also finish carve 3d at full speed since the stopover and depth are so small.

                          D: wincnc has this great slider to let you change feed speed on the fly. I usually rev it up and down until the bit sounds 'happy'.

                          Most of the bit makers provide feed info for their bits. Since flutes are cut differently that's horses mouth and good info.

                          Just my 2 cents
                          Mark Z
                          ____________________________
                          Stinger II 3x4 with recoil and Z+
                          Chapel Hill, NC

                          Comment

                          • #14

                            According to the CAMaster website here is the info on the speeds.


                            Stinger 1
                            Rapid Speeds (X,Y,Z) 600,600,400 ipm
                            Cut Speeds (X,Y,Z) 350,350,250 ipm


                            Stinger 2
                            Rapid Speeds (X,Y,Z) 800,850,400 ipm
                            Cut Speeds (X,Y,Z) 500,500,300 ipm


                            Stinger 3
                            Rapid Speeds (X,Y,Z) 800,850,400 ipm
                            Cut Speeds (X,Y,Z) 500,500,300 ipm



                            If you’re not able to do these then you may want / need to adjust your ini file.

                            Michael
                            Michael Mezalick
                            Cobra, WINCNC

                            3-D Modeling
                            https://carveddetails.com

                            mm@mezalick.com

                            Comment

                            Working...
                            X