Need help with settings

New Home Forum Mostly Printed CNC – MPCNC Advice – MPCNC Need help with settings

This topic contains 10 replies, has 5 voices, and was last updated by Profile photo of P3DCNC P3DCNC 2 weeks ago.

Viewing 11 posts - 1 through 11 (of 11 total)
  • Author
    Posts
  • #19157
    Profile photo of Mike
    Mike
    Participant

    Hi,

    I’m trying to mill out 3d shapes from planks of pine using Fusion 360, however I’m really unsure what speeds I should be using for things.

    All of the formulas I’ve seen online require you to know what RPM you’re using first. How do you decide what RPM to use? My Kress 800 FME doesn’t have a digital RPM display (it just has a dial) so I can only really guess what RPM I have. Is that accurate enough?

    I’m using an 8mm flat carbide end mill and my spindle does between 10,000 RPM and 29,000 RPM. What would be the best settings for me to use to do pine?

    I’m getting confused because the terminology in fusion is a bit different from estlcam. In fusion I have the following fields:

    Spindle speed (RPM)
    Surface speed
    Cutting feedrate
    Lead-In feedrate
    Lead-out feedrate
    Ramp feedrate
    Feed per tooth
    Plunge feedrate
    Feed per revolution

    A lot of the guides I’ve seen online say things like “Make sure you use a conservative/sensible value”, but nobody says what a sensible value is 😉

    Any advice would be hugely appreciated

    #19186
    Profile photo of P3DCNC
    P3DCNC
    Participant

    I’m in a similar boat. I’ve looked up the bits that I have for the required feedrates, chip load, etc.

    As an example:

    – Onsrud (40-100 series) 1/8″(3mm) upcut 2 flute bit,
    – Cut depth same as bit diameter (3mm),
    – Chip load for softwood .005-.007 (use .006),
    – My router is 20-24krpm (use 20krpm),
    – (Feed rate) Inches Per Minute (IPM) = RPM x # of cutting edges x chip load = 20000 x 2 x .006 = 240 IPM
    – 240 IPM x 0.423333 = 101.6 mm/s

    At .005 chip load this would work out to 84.67 mm/s and at the high end of .007 it would be 118.53 mm/s.

    I’ve tried it and it’s very fast. Are people following manufacturer specs for bits or are they slowing things down intentionally? What is recommended?

    #19188
    Profile photo of vicious1
    vicious1
    Admin

    If you are unsure you should follow the estlcam guide. It is free, and simple. Fusion is not for beginners. If you follow my guides you will see the numbers I use, or others on their videos. When you get the hang of it and have a sense of things then try out fusion.

    I would start with a much smaller bit, 3mm is good to learn with and very forgiving. 8mm is more of a roughing bit.

    You will see for all my cuts I use between 12-20mm/s on a 1/8″ bit and vary the depth of cut and spindle speed depending on material. If you are really new to this a single flute bit is even more forgiving and more suited to our high spindle speeds and machine rigidity

    #19189
    Profile photo of vicious1
    vicious1
    Admin

    You are going too slow if your material is melting or burning, too fast if your cut is ugly or you break something. Start with a 2D pen drawing, then mill some foam, then soft stuff like pine. By then you will probably have a good sense of what it should sound and look like while it is cutting. Experience is key, Hard numbers are not given by many because every machine will require something different.

    #19207
    Profile photo of wichitapilot
    wichitapilot
    Participant

    I second Ryan’s advice on this. Experience and testing are key factors. Once you have done some testing you will know what a good cut sounds like. Personally I do not follow the suggested equations for the tools just for the fact that I am not comfortable with my machine moving that fast. I use Fusion 360 a lot and really like it. There are some settings that are mentioned in the first post that either don’t matter (Spindle RPM) or they are calculated based on some of the other inputs. I would only worry about:
    Cutting feedrate
    Lead-In feedrate
    Lead-out feedrate
    Ramp feedrate
    Plunge feedrate
    Here is what I do for Pine:
    1/8″ Up or Down cut 2 Flute End Mill
    Depth of Cut: .1
    Cutting Feedrate: 35 in/min
    Lead in and out feedrate: 13 in/min
    Ramp and Plunge feedrate: 13 in/min
    I have a Dewalt 660 and a speed controller and I am guessing that I am running it at about 16k – 18k.

    Let me know if I can offer any advice for Fusion 360.

    #19246
    Profile photo of Mike
    Mike
    Participant

    Great, thanks for the advice.

    After 12 hours of messing around with trial and error in Fusion 360 I seem to have found my machines limits for the wood I’m using, although I’m still struggling to judge how to balance the relationship between “depth of cut” and “cutting feedrate”. Is it better to do for deeper cuts at a slower speed or shallow cuts at a faster speed? 🙂

    As for Fusion – I’m loving it so far. A few dodgy tutorials on YouTube sent me down a bad direction to start with, but I’m starting to understand it much better now. I love being able to define various strategies for different parts of the model.

    Unfortunately, my better half has banned me from playing with it until I get the dust issue sorted, so I guess everything is on hold for a while 🙂

    #19247
    Profile photo of Barry
    Barry
    Participant

    You need a dust shoe.

    #19261
    Profile photo of Mike
    Mike
    Participant

    Yup! Working on one now. 🙂

    #24364
    Profile photo of P3DCNC
    P3DCNC
    Participant

    Hey gang.

    I’m back at trying to figuring out cutting speeds. My primary goal is to cut MDF and plywood panels for different projects. I am using a Rigid R2400 router which has a 1/4″ shank on it. So my preferred bit to cut 1/2″ to 3/4″ material is a 1/4″ double flute cutting small amounts at high speed to keep the bit cool and get good chips off of it.

    Based on the settings recommended by the bit manufacturer, these are the speeds they recommend for this bit:
    (federate (IPM) = RPM x Flutes x chip size)
    (mm/s = IPM x.423333)
    (mm/min = mm/s x 60)
    for .005 = 20,000 x 2 flutes x .005 = 200 IPM * .423333 = 84.6666 mm/s * 60 = 5079.996 mm/s
    for .006 = 20,000 x 2 flutes x .006 = 240 IPM * .423333 = 101.59992 mm/s * 60 = 6095.9952 mm/s
    for .007 = 20,000 x 2 flutes x .007 = 280 IPM * .423333 = 118.53324 mm/s * 60 = 7111.9944 mm/s

    Now the MPCNC cannot push these rates in a single cut, but I used a 1mm cutting depth and that seems fine for the machine.

    Sort of… read on… here are some issues I’ve come across..

      Super slow router movements (I mean you can count the stepper steps it’s sooo slow) initially when using Fusion 360 CAM and Repetier:

    This I found was due to a mismatch in the units being used in Fusion 360 CAM workspace (inches) and what Repetier was using (mm). To fix this, look for the units entry in the tree when you are in Fusion 360 CAM workspace. I changed it to mm. This does not affect the units you use in the Design workspace btw.

      Loose Belts (cutting chatter):

    I noticed is that my belts were no where near tight enough. To fix this, I used new zip ties and really made sure there was no slack in the belts when done. When the machine moves, the belts are stationary (they don’t sag or otherwise move at all).

      Height of MPCNC frame above cutting surface:

    My frame is designed around a cutting surface of 25″x49″x6″ so it’s big but I am using stainless 1″ tube. I found that at this height, the router mounting on the Toolmount was so far from the cross bars that it caused a fair bit of movement at the bit. So I shortened the corner tubes by cutting them to 4″ in length (I may even go further since I only cut sheets of material). This accomplished 2 things. The frame is more sturdy since it is not perched as high, and the distance between the bit and the cross bars is much closer so the Z assembly is far stiffer. This change alone meant a major change in stiffness, and as a result, much cleaner and faster cut (you can hear how much happier the bit is).

      Cut depth of 1/4″ 2-flute Up-cut:

    At these speeds, which makes the bit happy, you have an issue with it wandering (chatter or worse) based on 2 things. First, any flex in the machine will allow the bit to wander. This can cause a change in the line the bit takes through the material. You especially notice it when the load on the bit changes, for instance when it goes from complete load in full material to as it exits the material at an edge. The bit will release it’s lateral tension and leave an angle on the piece at that point. Secondly, the steppers can only take so much. So if there is too much pressure trying to push the bit through the material, it causes the steppers to miss steps. Nastiness ensues when that happens. So I used a 1mm cutting depth to get through 3/4″ of material. Faster thinner cuts produces good chip out keeping the bit sharp and cool. Slower thicker cuts heat the bit up, smells like burning wood, and in the end is slower. I’ve tried the really slow speeds like 12-20 mm/s. On a 1/4″ bit, this does not produce a clean cut at all and only causes the bit to heat up, burn material, get glued up and dull, making it worse as it continues to cut.

      So my strategy for cutting sheet material is as follows:

    – (1) Make the machine as stiff as possible (tight belts, minimize the Z height),
    – (2) Cut the material at the speeds the bit wants (or pretty close),
    – (3) Set the cut depth that allows for the proper speeds for the material you are cutting.

    Hope this helps,
    Phil

    #24368
    Profile photo of vicious1
    vicious1
    Admin

    As I sell/recommend them the mpcnc’s have a firmware max speeds of 190mm/s with the torque being max at 30mm/s or lower.

    Have you seen this, http://www.vicious1.com/software-updates/
    Make sure you are using the new post processor.

    You can easily over tighten the belts.

    Shorter is better 4″ is still really tall, and you have a large machine in general 49″ is more than 2 times the recommended, are you using midspan supports?

    1/4″ bits put a lot more torque on the frame, this is why we use 1/8″. You also get a nice bump in detail and speed.

    If you want to continue using that router, Try slowing it down. Does it have a speed control? If not there are a few ways to make or buy one.

    I use .5-4mm cut depth, never more.

    #24374
    Profile photo of P3DCNC
    P3DCNC
    Participant

    I’m pretty sure it is the newer post processor. Will check tonight.

    I think the belts are good now. They were bowing and moving a lot as the machine changed directions. This is eliminated now. Improved things quite a bit. Not sure if that’s too tight.

    Ya, may go even shorter as mentioned. Was definitely too tall before. No mid span supports…yet.

    I can see the advantage to going to 1/8″ bit. To get good chip out, you need less feedrate than a 1/4″. I happen to have this router around which is why I was trying to use it. It would need a PID to go below 20000 RPM as that’s it’s lowest speed. Plus the 1/8″ bit I have are 1/4″ shank, meaning the flutes won’t go through 3/4″ material as the flutes flare from 1/8″ to 1/4″ as they near the shank.

    I do have a 1/8″ largish rotozip somewhere… perhaps I’ll repurpose it..

    Will try some of this and report back.
    Phil

Viewing 11 posts - 1 through 11 (of 11 total)

You must be logged in to reply to this topic.