Loading ...
Sorry, an error occurred while loading the content.

Re: [taigtools] Removing material fast-- 1/4" or 3/8" bit?

Expand Messages
  • Michael Fagan
    Remember that in machining, power requirements are expressed as horsepower per cubic inch of metal removed. So the larger endmill would remove more material
    Message 1 of 9 , Jan 31, 2010
    • 0 Attachment
      Remember that in machining, power requirements are expressed as horsepower
      per cubic inch of metal removed. So the larger endmill would remove more
      material per pass but need to run slower. Unless you are having chatter
      issues from rigidity of a 1/4" endmill 1.25" down, I would stick with the
      smaller endmill and run it at your current speed.

      On Mon, Feb 1, 2010 at 01:09, rodiponer <matt@...> wrote:

      >
      >
      > Hi Guys,
      >
      > I am new to machine work. I have a Taig mill with a CNC conversion kit from
      > Jeff Birt at Soigeneris, which I am very happy with.
      >
      > I have to make about 218 parts for a weird monstrosity that I am building.
      > Because of the number of parts, I've been spending a lot of time tuning the
      > numerical cutting files to get the milling time down for each one. I am
      > currently spending about 15 minutes per part, which is about 55 hours of
      > total run time.
      >
      > I have been using a 1/4" 3 flute bit, and am wondering if a larger 3/8" bit
      > would allow me to make these parts any faster.
      >
      > I am running the 1/4" 3 flute bit at 30 IPM and 0.1" DOC on a lot of
      > profile cuts that remove about 0.125" of material at a time. The parts are
      > almost entirely made from profile cuts, though in a few places I am removing
      > 0.3125" of material with three 0.125" profile cuts. Some of the lighter
      > profile cuts, which remove 0.0625" of material, can handle a deeper 0.125"
      > DOC at the same 30 IPM. I've experimented between each run and have found
      > that increasing the DOC or IPM any more stalls the motor.
      >
      > Do you think, intuitively, that a larger 3/8" bit would allow me to make
      > these parts any faster? Or does a larger bit require more horsepower, and I
      > probably would not be able to make these parts any faster?
      >
      > I am happy to just do an experiment and see if the larger bit makes these
      > parts faster, but at the 1.25" depth I am milling these bits are $50 each.
      > So I'd appreciate any advice you guys have before I waste money.
      >
      > Thanks.
      >
      > Matt.
      >
      >
      >


      [Non-text portions of this message have been removed]
    • Rick Kernell
      Matt, I am not running CNC yet, but I use 3/8 inch end mills most of the time. I would suggest that you follow the feed and cutting speeds for this size,
      Message 2 of 9 , Feb 1, 2010
      • 0 Attachment
        Matt,

        I am not running CNC yet, but I use 3/8 inch end mills most of the time. I would suggest that you follow the feed and cutting speeds for this size, typically around 1680 for 6061, and you should do well. I have used the two, three and four flute versions, and I prefer the three and four to the two in terms of finish.

        Rick Kernell
        ----- Original Message -----
        From: rodiponer
        To: taigtools@yahoogroups.com
        Sent: Sunday, January 31, 2010 11:09 PM
        Subject: [taigtools] Removing material fast-- 1/4" or 3/8" bit?



        Hi Guys,

        I am new to machine work. I have a Taig mill with a CNC conversion kit from Jeff Birt at Soigeneris, which I am very happy with.

        I have to make about 218 parts for a weird monstrosity that I am building. Because of the number of parts, I've been spending a lot of time tuning the numerical cutting files to get the milling time down for each one. I am currently spending about 15 minutes per part, which is about 55 hours of total run time.

        I have been using a 1/4" 3 flute bit, and am wondering if a larger 3/8" bit would allow me to make these parts any faster.

        I am running the 1/4" 3 flute bit at 30 IPM and 0.1" DOC on a lot of profile cuts that remove about 0.125" of material at a time. The parts are almost entirely made from profile cuts, though in a few places I am removing 0.3125" of material with three 0.125" profile cuts. Some of the lighter profile cuts, which remove 0.0625" of material, can handle a deeper 0.125" DOC at the same 30 IPM. I've experimented between each run and have found that increasing the DOC or IPM any more stalls the motor.

        Do you think, intuitively, that a larger 3/8" bit would allow me to make these parts any faster? Or does a larger bit require more horsepower, and I probably would not be able to make these parts any faster?

        I am happy to just do an experiment and see if the larger bit makes these parts faster, but at the 1.25" depth I am milling these bits are $50 each. So I'd appreciate any advice you guys have before I waste money.

        Thanks.

        Matt.





        [Non-text portions of this message have been removed]
      • Ken Cline
        Matt, Start by asking yourself if you will need to remove more material if you choose a longer end mill. If so, expect it to take longer. As a rule, I find I
        Message 3 of 9 , Feb 1, 2010
        • 0 Attachment
          Matt,

          Start by asking yourself if you will need to remove more material if you choose a longer end mill. If so, expect it to take longer.

          As a rule, I find I have better luck with smaller end mills on the Taig.

          You may be over paying for your end mills. I have been sourcing end mills from Cutting Edge Tool Supply in Colorado [http://cetsonline.com]. Their ebay store currently has 3/8" end mills for as low as 2 for $20, double ended 2-flute M-42 cobalt steel from Hertel. They also have five packs of 3-flute Monster (also US made) carbide end mills for $55. Individual 3/8" end mills are around $15-20.
        • rodiponer
          Thank you everyone for your help. I am going to stick with going fast with the 1/4 bits, though they do wobble a bit at the 1.25 depth, so I am doing extra
          Message 4 of 9 , Feb 2, 2010
          • 0 Attachment
            Thank you everyone for your help.

            I am going to stick with going fast with the 1/4" bits, though they do wobble a bit at the 1.25" depth, so I am doing extra finish passes on the parts where close tolerances are important.

            I never thought of horsepower as a function of metal removal rate. I am going to look for some kind of math to add to my speed and feed spreadsheet, so that I can take that into account. It would be nice to be able to figure this out scientifically rather than stalling the motor and risk breaking a bit.

            I was able to halve the time for one of the parts by making it ever so slightly smaller, so that it could be cut from 1" square stock instead of 1.25".

            I've been buying bits from MSC, and will look more carefully at other suppliers. Thank you for the heads up.

            Matt.


            --- In taigtools@yahoogroups.com, Ken Cline <cline@...> wrote:
            >
            > Matt,
            >
            > Start by asking yourself if you will need to remove more material if you choose a longer end mill. If so, expect it to take longer.
            >
            > As a rule, I find I have better luck with smaller end mills on the Taig.
            >
            > You may be over paying for your end mills. I have been sourcing end mills from Cutting Edge Tool Supply in Colorado [http://cetsonline.com]. Their ebay store currently has 3/8" end mills for as low as 2 for $20, double ended 2-flute M-42 cobalt steel from Hertel. They also have five packs of 3-flute Monster (also US made) carbide end mills for $55. Individual 3/8" end mills are around $15-20.
            >
          • Will Schmit
            Another concern which hasn t been addressed -- Do you have an ER-16 spindle? A normal Taig spindle won t take 3/8 collets.   Look at the old posts -- look
            Message 5 of 9 , Feb 2, 2010
            • 0 Attachment
              Another concern which hasn't been addressed -- Do you have an ER-16 spindle?
              A normal Taig spindle won't take 3/8" collets.

               
              Look at the old posts -- look for Steve Blackmore
              He has a chart or spreadsheet -- maybe he would share it with you.


              ________________________________
              From: rodiponer <matt@...>
              To: taigtools@yahoogroups.com
              Sent: Tue, February 2, 2010 10:20:44 AM
              Subject: [taigtools] Re: Removing material fast-- 1/4" or 3/8" bit?

               
              Thank you everyone for your help.

              I am going to stick with going fast with the 1/4" bits, though they do wobble a bit at the 1.25" depth, so I am doing extra finish passes on the parts where close tolerances are important.

              I never thought of horsepower as a function of metal removal rate. I am going to look for some kind of math to add to my speed and feed spreadsheet, so that I can take that into account. It would be nice to be able to figure this out scientifically rather than stalling the motor and risk breaking a bit.

              I was able to halve the time for one of the parts by making it ever so slightly smaller, so that it could be cut from 1" square stock instead of 1.25".

              I've been buying bits from MSC, and will look more carefully at other suppliers. Thank you for the heads up.

              Matt.

              --- In taigtools@yahoogrou ps.com, Ken Cline <cline@...> wrote:
              >
              > Matt,
              >
              > Start by asking yourself if you will need to remove more material if you choose a longer end mill. If so, expect it to take longer.
              >
              > As a rule, I find I have better luck with smaller end mills on the Taig.
              >
              > You may be over paying for your end mills. I have been sourcing end mills from Cutting Edge Tool Supply in Colorado [http://cetsonline. com]. Their ebay store currently has 3/8" end mills for as low as 2 for $20, double ended 2-flute M-42 cobalt steel from Hertel. They also have five packs of 3-flute Monster (also US made) carbide end mills for $55. Individual 3/8" end mills are around $15-20.
              >




              [Non-text portions of this message have been removed]
            • Ken Cline
              ... Machinery s handbook gives the following formula for power: Pc =Kp * C * Q * W where Pc is the power at the cutting tool Kp is the power constant for the
              Message 6 of 9 , Feb 2, 2010
              • 0 Attachment
                On 2 Feb 2010, at 10:20 AM, rodiponer wrote:

                > I never thought of horsepower as a function of metal removal rate. I am going to look for some kind of math to add to my speed and feed spreadsheet, so that I can take that into account. It would be nice to be able to figure this out scientifically rather than stalling the motor and risk breaking a bit.

                Machinery's handbook gives the following formula for power:

                Pc =Kp * C * Q * W

                where

                Pc is the power at the cutting tool
                Kp is the power constant for the material being cut
                C is the feed factor, which increases for shallow cuts (e.g. at 0.012" feed/tooth, c=1; at 0.001" feed, c=1.6)
                Q is the rate of removal
                W is the tool wear factor (another constant)

                As you now know, the rate of removal of material is the main factor. The other factor you have control of is feed, where the theory says an aggressive feed (a few thousandths, if you can get away with it) with shallow depth of cut is more efficient than a deeper cut and slow feed.

                Don't forget god lubrication. I'm sure these power calculations assume it.





                [Non-text portions of this message have been removed]
              • Michael Fagan
                http://met.spsu.edu/dhorton/MET4342/Metal%20Cutting%20Mechanics/Determining%20Power%20Rqmts%20in%20Machining.pdf
                Message 7 of 9 , Feb 2, 2010
                • 0 Attachment
                  http://met.spsu.edu/dhorton/MET4342/Metal%20Cutting%20Mechanics/Determining%20Power%20Rqmts%20in%20Machining.pdf
                  <http://met.spsu.edu/dhorton/MET4342/Metal%20Cutting%20Mechanics/Determining%20Power%20Rqmts%20in%20Machining.pdf>I
                  also have a couple spreadsheets I made for the WPI students taking our intro
                  to manufacturing class when I was a TA.

                  On Tue, Feb 2, 2010 at 12:20, rodiponer <matt@...> wrote:

                  >
                  >
                  > Thank you everyone for your help.
                  >
                  > I am going to stick with going fast with the 1/4" bits, though they do
                  > wobble a bit at the 1.25" depth, so I am doing extra finish passes on the
                  > parts where close tolerances are important.
                  >
                  > I never thought of horsepower as a function of metal removal rate. I am
                  > going to look for some kind of math to add to my speed and feed spreadsheet,
                  > so that I can take that into account. It would be nice to be able to figure
                  > this out scientifically rather than stalling the motor and risk breaking a
                  > bit.
                  >
                  > I was able to halve the time for one of the parts by making it ever so
                  > slightly smaller, so that it could be cut from 1" square stock instead of
                  > 1.25".
                  >
                  > I've been buying bits from MSC, and will look more carefully at other
                  > suppliers. Thank you for the heads up.
                  >
                  > Matt.
                  >
                  >
                  > --- In taigtools@yahoogroups.com <taigtools%40yahoogroups.com>, Ken Cline
                  > <cline@...> wrote:
                  > >
                  > > Matt,
                  > >
                  > > Start by asking yourself if you will need to remove more material if you
                  > choose a longer end mill. If so, expect it to take longer.
                  > >
                  > > As a rule, I find I have better luck with smaller end mills on the Taig.
                  > >
                  > > You may be over paying for your end mills. I have been sourcing end mills
                  > from Cutting Edge Tool Supply in Colorado [http://cetsonline.com]. Their
                  > ebay store currently has 3/8" end mills for as low as 2 for $20, double
                  > ended 2-flute M-42 cobalt steel from Hertel. They also have five packs of
                  > 3-flute Monster (also US made) carbide end mills for $55. Individual 3/8"
                  > end mills are around $15-20.
                  > >
                  >
                  >
                  >


                  [Non-text portions of this message have been removed]
                • mrehmus
                  ... If the quarter-inch end mills are bending, go to carbide which is much stiffer for your final passes.
                  Message 8 of 9 , Feb 3, 2010
                  • 0 Attachment
                    --- In taigtools@yahoogroups.com, Michael Fagan <woodworker88@...> wrote:

                    > > Thank you everyone for your help.
                    > >
                    > > I am going to stick with going fast with the 1/4" bits, though they do
                    > > wobble a bit at the 1.25" depth, so I am doing extra finish passes on the
                    > > parts where close tolerances are important.

                    If the quarter-inch end mills are bending, go to carbide which is much stiffer for your final passes.
                  Your message has been successfully submitted and would be delivered to recipients shortly.