How long do your bits live?

New Home Forum Mostly Printed CNC – MPCNC Advice – MPCNC How long do your bits live?

This topic contains 22 replies, has 6 voices, and was last updated by  Jethro 2 months, 4 weeks ago.

Viewing 23 posts - 1 through 23 (of 23 total)
  • Author
    Posts
  • #103614

    grishien
    Participant

    Hello all,

    I would like to initiate experience sharing about:

    1. How long specific bits live, depending on material and nuances;
    2. Where to buy ones that live long;
    3. Any advise to save longer life for them.

     

    So far I have some experience with roughing 6mm flat end (aliexpress.com/item/32819837274.html).

    Mine survived for 25 hours of working. Stepover 40%, 2mm stepdown, 650mm/min, 12000RPM, hard wood (ash-tree). After 25 hours it started to work like you can see attached photo. Actually, I expected it to live 10X times longer and this frustrates me.

    Attachments:
    #103646

    Tim
    Participant

    I think expecting a $5 endmill to last 250 hours of cutting is very optimistic.

    I also have doubts about a $5 endmill actually being carbide as that one is advertised.

    #103668

    Ryan
    Keymaster

    Lots to consider. If you only use the bottom 0.5mm it, coatings on wood are not needed, quality of the metal, and use. That said, I have had some last 2 hours and some 30+ for me in MDF, in regular not glued wood I would think they would last a crazy long time if you are not over heating and using a majority of the cutting edge.

    #103696

    grishien
    Participant

    Lots to consider. If you only use the bottom 0.5mm it, coatings on wood are not needed, quality of the metal, and use. That said, I have had some last 2 hours and some 30+ for me in MDF, in regular not glued wood I would think they would last a crazy long time if you are not over heating and using a majority of the cutting edge.

    Ryan, thanks. Would you please explain what is meant by “using a majority of the cutting edge”? More stepover, deeper cut?

    Which ones to you use? I mean can you post a link to shop page?

    Do you mean that on MDF they last shorter? But MDF is a carton, they theoretically should last longer on it.

    If you only use the bottom 0.5mm it

    Do you mean 0.5mm stepdown?

    #103697

    grishien
    Participant

    I think expecting a $5 endmill to last 250 hours of cutting is very optimistic.

    I also have doubts about a $5 endmill actually being carbide as that one is advertised.

    Tim, thanks. Any info about yours?

    #103712

    Barry
    Participant

    Lots to consider. If you only use the bottom 0.5mm it, coatings on wood are not needed, quality of the metal, and use. That said, I have had some last 2 hours and some 30+ for me in MDF, in regular not glued wood I would think they would last a crazy long time if you are not over heating and using a majority of the cutting edge.

    Ryan, thanks. Would you please explain what is meant by “using a majority of the cutting edge”? More stepover, deeper cut?

    Which ones to you use? I mean can you post a link to shop page?

    Do you mean that on MDF they last shorter? But MDF is a carton, they theoretically should last longer on it.

    If you only use the bottom 0.5mm it

    Do you mean 0.5mm stepdown?

    MDF is full of glue, which kills endmills pretty quick.  Same with plywood.  Ignoring metals, plywood will kill your endmills the fastest. The stepdown is what Ryan is talking about.  If all you ever cut is .5mm, then that’s really all that is being used on your endmill.  It will dull and the rest of the cutting edge will still be sharp, but you won’t be able to use it.

     

    I’m basically using the same endmills Ryan sells in the shop, which I think are Kyocera.  1/8″, 1/16″ Single flute and double flute.  I also have a couple 1/4″ double flute that I use on the lowrider, and a 1″ surfacing bit I got from amana tools.

    2 users thanked author for this post.
    #103774

    grishien
    Participant

    The stepdown is what Ryan is talking about. If all you ever cut is .5mm, then that’s really all that is being used on your endmill. It will dull and the rest of the cutting edge will still be sharp, but you won’t be able to use it.

    Ok, got it. I actually used 2mm stepdown. I’m thinking, maybe I used wrong stepover and/or fast feedrate that has led to fast wearout?

    #103775

    Aaron
    Participant

    Lots to consider. If you only use the bottom 0.5mm it, coatings on wood are not needed, quality of the metal, and use. That said, I have had some last 2 hours and some 30+ for me in MDF, in regular not glued wood I would think they would last a crazy long time if you are not over heating and using a majority of the cutting edge.

    Ryan, thanks. Would you please explain what is meant by “using a majority of the cutting edge”? More stepover, deeper cut?

    Which ones to you use? I mean can you post a link to shop page?

    Do you mean that on MDF they last shorter? But MDF is a carton, they theoretically should last longer on it.

    If you only use the bottom 0.5mm it

    Do you mean 0.5mm stepdown?

    MDF is full of glue, which kills endmills pretty quick. Same with plywood. Ignoring metals, plywood will kill your endmills the fastest. The stepdown is what Ryan is talking about. If all you ever cut is .5mm, then that’s really all that is being used on your endmill. It will dull and the rest of the cutting edge will still be sharp, but you won’t be able to use it.

    I’m basically using the same endmills Ryan sells in the shop, which I think are Kyocera. 1/8″, 1/16″ Single flute and double flute. I also have a couple 1/4″ double flute that I use on the lowrider, and a 1″ surfacing bit I got from amana tools.

    Agree on the glue in MDF. Additionally, the most common routers used for the mpcnc/lowrider spin too fast to make anything other than dust in mdf (since they can’t reach the appropriate feed rate), so you make a lot of dust instead of chips. That is in general for MDF though, Even the Shopbot Buddy we have just makes dust. Dust means heat, heat kills endmills.

    #103780

    grishien
    Participant

    so you make a lot of dust instead of chips

    I have just read same 30 seconds ago in another local forum 🙂 From 2 separate sources I interpolate that with feed of 1 m/min I should reduce RPM to 4800-5000 (while so far I did 12000 and I witnessed dust).

    However, which size of particle is dust and which one is chip?

    #103790

    Aaron
    Participant

    cxhips-onsrud

    While I can’t quantify what size makes a “chip”, maybe this graphic will help. The reason it’s more difficult to get chips when cutting MDF  (for most hobby routers) is because it’s literally dust and glue.

    Attachments:
    #103801

    grishien
    Participant

    Yes, I definitely didn’t see such a big particles in my dust…

    #103802

    Aaron
    Participant

    To be fair those aren’t MDF chips/shavings, but I believe you get the idea.

    #103845

    grishien
    Participant

    I got dug into other forums and bits selling websites. They say how to calculate parameters.

    Here is data for flat end spiral bits: say, 2 flute bit. 1 flute should cut a chip of 0.05-0.15mm thick. Therefore 1 turn of a bit should cut 0.1-0.3mm of material. Therefore if you spin 12000 RPM then your feed rate should be [0.1-0.3]*12000 => 1200 – 3600 mm/min. If you make your bit cut less per revolution – then it’s not cutting but tearing material, so heating and fast wear out.

    Of course MPCNC cannot afford 3.6 m/min. But 1.2 m/min is affordable and also spindle can be slowed down a little.

     

    1 user thanked author for this post.
    #103872

    grishien
    Participant

    Also should take this into account. When stepover less than 50% then a single cut that a flute makes is thinner than theoretical. So above stated formula should be adjusted correspondingly.

    Attachments:
    #104207

    grishien
    Participant

    I was wrong. MPCNC can handle way more than 1.2m/min of feedrate. I tried 9KRMP with 2.16 m/min, 20% stepover and 3mm stepdown it worked just fine (oak). I assume it’s not the limit but I was close because that chinese spindle apparently can be only 10.5KRPM as per my laser tachometer.

    Of course, central node should be stiff and without backlashes to afford minimal deviation of the bit.

    Gonna push feedrate to the limit and see what happens.

    #104239

    Ryan
    Keymaster

    I suggest pushing the depth before the speed. That saves time, endmills, and the steppers retain more power at slower speeds.

    #104403

    grishien
    Participant

    So. I tried the following with OK result:

    10500 RPM – 30% stepover – 2mm stepdown – 3m/min

    10500 RPM – 30% stepover – 3mm stepdown – 3m/min

    10500 RPM – 30% stepover – 2mm stepdown – 4.063m/min

    10500 RPM – 30% stepover – 3mm stepdown – 4.063m/min

    and Fusion 360’s algorythm where it first cuts with 6mm depth and then refines by 2mm stepover where material is left in order to finalize roughing. Also 10500RPM – 30% stepover and 4.063m/min.

    Thus I successfully achieved 0.3mm material removal per revolution of a 6mm flat end 2 flute bit, just as per recomendations.

    I can say that MPCNC is capable of doing this intencity. Maybe it’s because I reinforced it. However, on 4m/min the moving trajectory under load is not always smooth and some inertion (asumingly) vibration is noticed on head node. Maybe better to slow down spindle and feed rate. Or maybe should use stronger and shorter pipes (this also will be tested in my second hybrid MPCNC).

    I estimate that I increased bit’s life by at least 5 times by a factor of feedrate which is still not too long. I hope that it’s will also be increased by a factor of cutting instead of tearing material. A good hope is supported by comment of one of sellers that such bits life for very long time and are being broken more often (on strong machines) than become dull.

    I suggest pushing the depth before the speed. That saves time, endmills, and the steppers retain more power at slower speeds.

    Yes. However, this only should be possible if you can handle such depth (1*D of bit for oak) with recommended combination of feedrate and spindle RPM. Luckily I proved that it’s possible. And, 2X longer life time because of depth factor, s0 at least 10X now, not bad.

    #104439

    Ryan
    Keymaster

    They use 1*D as a standard for easy reference, if you are using a single flute or other large fluted endmill and get good chip evacuation I can easily pocket wood and plastic at 4*D, Slotting is 1-3*D for me.

    The speeds we use might make a lot more sens if you use mm/s. You have 3m/min and 4.063m/min which does not sound all that different and even wondering why the .063 is in there until you realize, that is 50mm/s (much faster than I even rapid) and 67.72mm/s. Those speeds are pretty nuts for this machine and could be the cause of your movement issues, the junction deviation calcs do take time to process, and on small cuts the accels will not let you get anywhere near that so you could very well not actually be changing your speeds. I really suggest 8-15mm/s and deeper. If you think about it that way your 1*[email protected]/s is the same as the recommended 4*[email protected]/s with the exception of making your endmill last 4X as long and the machine moving smoother and the steppers having at least 2X the torque. If you do want to keep cutting fast I suggest larger pulleys to slow down the steppers.

    #104484

    grishien
    Participant

    get good chip evacuation

    Yes, here comes the problem. My dust removal system seems to be quite powerful. However, it can’t evacuate chips well even from 1*D slots. Or, if you meant bit’s structure designed to evacuate chips well, mine also don’t.

    I really suggest 8-15mm/s and deeper

    Yes but:

    1. Spindle should do only 2400-4800 which is ok on a high margin. But will decrease sppindle’s power from 500W to 100-200W;

    2. I am 3D milling, not cutting. So anything deeper than 1*D doesn’t make sence in my case.

    3. But I will try to simulate in Fusion360, maybe it makes sence.

    If you do want to keep cutting fast I suggest larger pulleys to slow down the steppers

    But what is the point to that considering that larger pulleys apply greater lever..?

    #104522

    Ryan
    Keymaster

    But what is the point to that considering that larger pulleys apply greater lever..?

    Steppers have a rapid decrease in torque with RPM, a larger pulley will keep the RPM down. There is a balance point and at the speeds you are going I am sure a larger pulley would result in a net return on torque. I don’t have 12V specs for our steppers but you are running at 93rpms and the torque starts to fall of sooner than 50 @12V (They seem to be peak at 30 from the looks of a generic stepper plot).

     

    It is not a big deal just a good exercise in double checking all my calcs from a few years ago.

    1 user thanked author for this post.
    #104546

    grishien
    Participant

    Thanks Ryan, I will give it a try.

    #105449

    grishien
    Participant

    Hi.

    I tried different depths. At 10 mm new very sharp bit worked fine. Hovever a bit quickly loses a little of sharpness (but stays sharp enough to work yet). In such state 10mm (6mm flat end bit) is too much – it can suck into material and force MPCNC to skip steps.

    What I found ok is 1.25D with 30% stepover, 9K RPM, 2000 mm/min feed rate (62.5 RPM on NEMA17). This way the work is stable and quality is acceptable.

    #106578

    Jethro
    Participant

    I’m pretty new to all this stuff, but you’ll see ahead before the bit is giving completely up.
    I took it pretty much to the edge this afternoon, had to change the bit on my last part for the MP3DP.
    The one I used is a dirt cheap 1/8″ bit from Aliexpress, for ~12$ / 10 pcs.
    https://www.aliexpress.com/item/32888641325.html?spm=a2g0s.9042311.0.0.b1824c4dJ2tf3X
    The time I ordered them I didn’t know that it would be better to use a single flute, furthermore the usable length was 12mm, as the multiplex was 12mm as well, I decided to go in 2 passes.
    On the picture you can see quite clearly where I changed the bit, the sawdust turns a lot darker on the last hour of the bit too, so that should clearly tell you when it’s time to change.

    • This reply was modified 2 months, 4 weeks ago by  Jethro.
    Attachments:
Viewing 23 posts - 1 through 23 (of 23 total)

You must be logged in to reply to this topic.