Mass material removal vs. Cutter dia
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 56
  1. #1
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,707
    Post Thanks / Like
    Likes (Given)
    2664
    Likes (Received)
    2354

    Default Mass material removal vs. Cutter dia

    First off...most of the pieces I mfg dont exceed 12" in dia./length, and with that said I have grown accustom to using 3/8-1/2 dia endmills for the majority of my roughing routines.

    When do you step up to 3/4 and such?
    How Do you weight mrr vs corner radius vs tool cost ect?

    I cant seem to get away from the 1/2" endmill and am very interested to see what some of you folks are using for tooling, as well as techniques and tool paths that work well for you.

    Thank you in advance and happy Monday
    This part is 6"x1" and im removing 2/3 of the stock
    image.jpg

  2. #2
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    7,592
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2034

    Default roughing

    Quote Originally Posted by allloutmx View Post
    First off...most of the pieces I mfg dont exceed 12" in dia./length, and with that said I have grown accustom to using 3/8-1/2 dia endmills for the majority of my roughing routines.

    When do you step up to 3/4 and such?
    How Do you weight mrr vs corner radius vs tool cost ect?

    I cant seem to get away from the 1/2" endmill and am very interested to see what some of you folks are using for tooling, as well as techniques and tool paths that work well for you.

    Thank you in advance and happy Monday
    This part is 6"x1" and im removing 2/3 of the stock
    image.jpg
    .
    we use 5" facemills at 0.150" depth of cut going 30 inches per minute to remove material fast
    4" facemills at 0.150" depth of cut and 3" width of cut at 35-40 ipm
    2" carbide insert end mill at 0.3" DOC and up to 1.5" WOC at 850 sfpm and about 30 ipm. a 2" diameter carbide insert end mill can often take 1" depth of cut if width of cut is 0.1" or less at 20-30 ipm at 850 sfpm for 1018 steel.
    .
    for slotting (full width cutting) i normally take less depth of cut to avoid chatter. end mills slotting if end mill if 3 or more diameters long sticking out we normally slow down to 300 sfpm. Facemilling (less than full cutter width) even with a carbide insert end mill normally we double sfpm compared to slotting with longer cutter.
    .
    the biggest advantage with 2" carbide insert end mill is length of cutter is 3 to 6" depending on tool. we use 3 different lengths of carbide insert end mills.
    ....... the other thing is ability to hold the part and part being thick enough or rigid enough to with stand cutting forces. trying to cut material less than 0.1" thick and part vibration can destroy a cutter. i would not use a 1/2" roughing cutter if i needed a 2" or more depth of cut or tool stick out. a end mill sticking out that much will vibrate too much.

  3. #3
    Join Date
    Aug 2013
    Location
    upper michigan
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    112
    Likes (Received)
    314

    Default

    you may want to give some more information on your machine types that you have and types of material you cut. It will do you no good to tell you to use a 6" face mill .250 deep if you only have a R-8 spindle.

  4. Likes Big B liked this post
  5. #4
    Join Date
    May 2003
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    9,529
    Post Thanks / Like
    Likes (Given)
    2729
    Likes (Received)
    3374

    Default

    It would sure be nice to work on itsy bitsy parts like that.

    Do you do any machining with inserts now? Who's your tooling and insert supplier?

    It's almost like chocolate and vanilla, everybody has a preference. We used to be a KM shop and now I don't think that they have 25%. Lots of SECO, Sandvik, ISCAR, and Mitsubishi. If we get a new product design or some exotic material, we'll have a supplier take a look and give us a recommendation. Most machines, we look at the tool change capacity and the HP available. We've got one application where we face mill a 16*36" casting face. Try that in a super duplex stainless.

    A couple of the guys I know just love these: Harroun Enterprises HIBF Mold Masher 1.00 Inserts, Accessories

    I've got one of these for my home BP, just awsome. Turbo 10 - Seco Tools
    JR

  6. #5
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,707
    Post Thanks / Like
    Likes (Given)
    2664
    Likes (Received)
    2354

    Default

    Quote Originally Posted by upnorth5axis View Post
    you may want to give some more information on your machine types that you have and types of material you cut. It will do you no good to tell you to use a 6" face mill .250 deep if you only have a R-8 spindle.
    Right now im on a 12k rpm 25hp mazak

  7. #6
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,707
    Post Thanks / Like
    Likes (Given)
    2664
    Likes (Received)
    2354

    Default

    Quote Originally Posted by JRIowa View Post
    It would sure be nice to work on itsy bitsy parts like that.

    Do you do any machining with inserts now? Who's your tooling and insert supplier?

    It's almost like chocolate and vanilla, everybody has a preference. We used to be a KM shop and now I don't think that they have 25%. Lots of SECO, Sandvik, ISCAR, and Mitsubishi. If we get a new product design or some exotic material, we'll have a supplier take a look and give us a recommendation. Most machines, we look at the tool change capacity and the HP available. We've got one application where we face mill a 16*36" casting face. Try that in a super duplex stainless.

    A couple of the guys I know just love these: Harroun Enterprises HIBF Mold Masher 1.00 Inserts, Accessories

    I've got one of these for my home BP, just awsome. Turbo 10 - Seco Tools
    JR
    Most used insert cutter is my 2" sandvik face mill
    I bought 3/4" sumitomo wex mill a while back but havent been able to utilize it to the capacity i get out of my 1/2" 4 flute endmills.

  8. #7
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    10,383
    Post Thanks / Like
    Likes (Given)
    31
    Likes (Received)
    7714

    Default

    Quote Originally Posted by allloutmx View Post
    Most used insert cutter is my 2" sandvik face mill
    I bought 3/4" sumitomo wex mill a while back but havent been able to utilize it to the capacity i get out of my 1/2" 4 flute endmills.
    And you never will. Insert cutters can work in you have a long reach situation, or a really deep pocket. For bread and butter, a 1/2 or 5/8 end mill should be able to beat it.

    I was at the Emuge booth at IMTS and they were running a 5 axis Hermle at 125% of spindle load with a 12mm end mill. It's unbelievable what these tools can do if you program them correctly.

    I personally find that 5/8 solid to 2" indexable is a total no man's land where nothing really works very well. I skip right over it. There are exceptions, such as aluminum, where I have a 1" indexable mill that really works well. But, for steel, or general shop stuff, forget it.

  9. Likes Bobw, Jorgo, Big B liked this post
  10. #8
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    7,940
    Post Thanks / Like
    Likes (Given)
    10203
    Likes (Received)
    8644

    Default

    My goto tool is the 1/2".

    Programmed right, it will peg your load meter, and stay there for a very long time.
    Anything bigger in solids and the dollar amount goes up sharply, and for the metal removal,
    generally, though not always, not worth it.

    Like, Ewsley, indexables for facing and long reach stuff.

    Aluminum is a bit different, its not that hard to pack up the flutes on 1/2" tool. In that case I like a 5/8 or 3/4, but they
    last for fricken ever so... its worth it.

  11. #9
    Join Date
    May 2013
    Location
    Austin, Texas
    Posts
    278
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    268

    Default

    In reference to the Load meter, Ideally what are you shooting for on it?

  12. #10
    Join Date
    Dec 2010
    Location
    Kansas City KS
    Posts
    387
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    98

    Default

    Quote Originally Posted by Whatley View Post
    In reference to the Load meter, Ideally what are you shooting for on it?

    I think it would depend on the machine again, wouldn't it?

    I could have sworn that I read somewhere in the manual that a particular mazak was rated for 100% duty cycle @100% but another was rated at 80% for 100% cycle.

  13. #11
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,707
    Post Thanks / Like
    Likes (Given)
    2664
    Likes (Received)
    2354

    Default

    Quote Originally Posted by Whatley View Post
    In reference to the Load meter, Ideally what are you shooting for on it?
    Im not sure how to answer that... I have no particular number in mind, just optimal mrr and tool life without inducing mass amounts of stress into the work piece.

  14. #12
    Join Date
    May 2013
    Location
    Austin, Texas
    Posts
    278
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    268

    Default

    Quote Originally Posted by Mike_ View Post
    I think it would depend on the machine again, wouldn't it?

    I could have sworn that I read somewhere in the manual that a particular mazak was rated for 100% duty cycle @100% but another was rated at 80% for 100% cycle.
    I mean that would make sense, I just did a quick scan through the operational manual for the FH-4800 I work on, I found the page for figuring out where to read the Spindle Load Graph, but no mention as to recommended rating. I wonder where that information is kept.


    I was talking to a Tech the other day who was repairing the ATC on our DMF 360 Linear, and he was saying that of course running the machine at 100% rapid and 100+% Spindle Load is going to take a heavy toll on the machine. So I've been trying to delve up more information on how to effectively run a machine in a way that will have it lasting for years and years ( barring crashes of course :P )

    I do imagine that your end mill will probably be the weakest link in an equation, unless your parts are small. So you probably won't hit a high Spindle load with it.

    I was about to say that you could use the Spindle Load to raise your DOC/Speed/Feed if you feel like it can take more. But then I realized y'all probably use that handy calculator thing that I need to buy to come up with all of that anyways.

  15. #13
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,707
    Post Thanks / Like
    Likes (Given)
    2664
    Likes (Received)
    2354

    Default

    Quote Originally Posted by ewlsey View Post
    And you never will. Insert cutters can work in you have a long reach situation, or a really deep pocket. For bread and butter, a 1/2 or 5/8 end mill should be able to beat it.

    I was at the Emuge booth at IMTS and they were running a 5 axis Hermle at 125% of spindle load with a 12mm end mill. It's unbelievable what these tools can do if you program them correctly.

    I personally find that 5/8 solid to 2" indexable is a total no man's land where nothing really works very well. I skip right over it. There are exceptions, such as aluminum, where I have a 1" indexable mill that really works well. But, for steel, or general shop stuff, forget it.
    My favorite machining video hands down is on the emuge website. They do make some pretty impressive tools.

  16. #14
    Join Date
    Dec 2010
    Location
    Kansas City KS
    Posts
    387
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    98

    Default

    Quote Originally Posted by Whatley View Post
    I mean that would make sense, I just did a quick scan through the operational manual for the FH-4800 I work on, I found the page for figuring out where to read the Spindle Load Graph, but no mention as to recommended rating. I wonder where that information is kept.


    I was talking to a Tech the other day who was repairing the ATC on our DMF 360 Linear, and he was saying that of course running the machine at 100% rapid and 100+% Spindle Load is going to take a heavy toll on the machine. So I've been trying to delve up more information on how to effectively run a machine in a way that will have it lasting for years and years ( barring crashes of course :P )

    I do imagine that your end mill will probably be the weakest link in an equation, unless your parts are small. So you probably won't hit a high Spindle load with it.

    I was about to say that you could use the Spindle Load to raise your DOC/Speed/Feed if you feel like it can take more. But then I realized y'all probably use that handy calculator thing that I need to buy to come up with all of that anyways.
    On our Mazaks we can limit the rapid to a percentage of maximum, so any of our mills are likely only running 75-80% at "100%" rapids. Not too often we max the load meters, but I won't go much higher than 80%. Course I'm not doing production usually, so it's all good.

    I've only replaced one set of thrust bearings from wear in a little over 4 years, never a motor or servo drive (unless it was crashed!)

    The damn ATCs though... Always fighting those, the pullstud fingers, belleville washers, turret fingers...

  17. #15
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,707
    Post Thanks / Like
    Likes (Given)
    2664
    Likes (Received)
    2354

    Default

    Quote Originally Posted by Whatley View Post
    I mean that would make sense, I just did a quick scan through the operational manual for the FH-4800 I work on, I found the page for figuring out where to read the Spindle Load Graph, but no mention as to recommended rating. I wonder where that information is kept.


    I was talking to a Tech the other day who was repairing the ATC on our DMF 360 Linear, and he was saying that of course running the machine at 100% rapid and 100+% Spindle Load is going to take a heavy toll on the machine. So I've been trying to delve up more information on how to effectively run a machine in a way that will have it lasting for years and years ( barring crashes of course :P )

    I do imagine that your end mill will probably be the weakest link in an equation, unless your parts are small. So you probably won't hit a high Spindle load with it.

    I was about to say that you could use the Spindle Load to raise your DOC/Speed/Feed if you feel like it can take more. But then I realized y'all probably use that handy calculator thing that I need to buy to come up with all of that anyways.
    Have you tried the hsmadvisor.com calculator yet? Free 30 day trial...and worth every penny after. Definity changed the way I program.

  18. #16
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,707
    Post Thanks / Like
    Likes (Given)
    2664
    Likes (Received)
    2354

    Default

    Quote Originally Posted by Mike_ View Post
    On our Mazaks we can limit the rapid to a percentage of maximum, so any of our mills are likely only running 75-80% at "100%" rapids. Not too often we max the load meters, but I won't go much higher than 80%. Course I'm not doing production usually, so it's all good.

    I've only replaced one set of thrust bearings from wear in a little over 4 years, never a motor or servo drive (unless it was crashed!)

    The damn ATCs though... Always fighting those, the pullstud fingers, belleville washers, turret fingers...
    Im new to the yamazaki. I miss the simplicity of the haas..but thats about it so far

  19. #17
    Join Date
    May 2013
    Location
    Austin, Texas
    Posts
    278
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    268

    Default

    Quote Originally Posted by Mike_ View Post
    On our Mazaks we can limit the rapid to a percentage of maximum, so any of our mills are likely only running 75-80% at "100%" rapids. Not too often we max the load meters, but I won't go much higher than 80%. Course I'm not doing production usually, so it's all good.

    I've only replaced one set of thrust bearings from wear in a little over 4 years, never a motor or servo drive (unless it was crashed!)

    The damn ATCs though... Always fighting those, the pullstud fingers, belleville washers, turret fingers...
    Ours got real weird... Somehow the magazine rearranged/forgot the locations of pockets, so the loader would go to random pockets... in between pockets, attempt to travel 4 feet through the wall... You know, just lots of fun stuff. Besides trying to figure out the last time lightning struck a power line, we decided that the box probably overheated, as the filter to the fan was just caked full of dirty coolant and sucking no air in.

    We run most of the MAzak's at 25%, it's fast enough and we do very short run job stuff so it doesn't really make sense to kick it up past that. But everytime you turn the machine off and on. It defaults to 100%, and sometimes I forget so I'll load a program and it will just haul significant ass to the part. Scares the hell out of me everytime It's like it's testing how fast I can hit feed hold

    Quote Originally Posted by allloutmx View Post
    Have you tried the hsmadvisor.com calculator yet? Free 30 day trial...and worth every penny after. Definity changed the way I program.
    That's the one I was talking about! Heard you talk about enough times on here that I'd buy it even without a trial. I'm not at a point where I do consistent programming, just minor fixes and such. So I was gonna wait until that happens to get a copy. But getting a copy is definitely something that will be happening.

  20. #18
    Join Date
    Oct 2012
    Location
    Oklahoma, United States
    Posts
    28
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    5

    Default

    I machine a lot of 6061 Aluminum on a Daewoo DMV 3016. It only has 8000 RPM's, and 15 HP. So like you have already mentioned got the HSM calculator and dove head first into HSM. I actually took a block of 6061 that we used to face all 6 sides at about 10 min. a side, and with HSM I am running a 4in. Face mill. 175 DOC, .800 Radial or 20% at 500 IPM. As well as profiling with E.M. instead of Flipping part for next side. I use as big of an E.M. i can that's reasonable. Which is a 1.25 ALTIN coated carbide e.m. from Detroit Industrial and i take 1 in. DOC, .05 radial, and fees about 250 IPM. So i cut run time down from 10 min a side (6 sides) so 1 hour start to finish. To 12 min. Start to finish. This HSM has opened my eyes to a whole other world.

  21. #19
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,075
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    397

    Default

    We are machining a lot of Aluminum here.
    Recently i fell in love with SGS Aluminum-Specific endmills.
    Switf-Carb or something.
    So i am taking a 1.5" deep cut at 0.25" radial at 7000RPM and 170 IPM and hitting a friggin strap clamp with the end of the tool.
    Before i could hit a feedhold HAAS's Torque Limit kicks in at 120% and shuts it down WITHOUT breaking the endmill!
    A the tool almost made it through case hardened clamp 3/4" deep at fill slot and only one flute got little chipped.
    Still using the same tool. Works fine.

    So for aluminum SGS SwiftCarb 3/4" Dia Can really haul more material than our puny conveyor can remove.
    Still a 2" APKT16 Face Mill Easily removes 50in^3/min even when 5" long.

  22. Likes allloutmx liked this post
  23. #20
    Join Date
    Oct 2012
    Location
    Oklahoma, United States
    Posts
    28
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    5

    Default

    Quote Originally Posted by zero_divide View Post
    We are machining a lot of Aluminum here.
    Recently i fell in love with SGS Aluminum-Specific endmills.
    Switf-Carb or something.
    So i am taking a 1.5" deep cut at 0.25" radial at 7000RPM and 170 IPM and hitting a friggin strap clamp with the end of the tool.
    Before i could hit a feedhold HAAS's Torque Limit kicks in at 120% and shuts it down WITHOUT breaking the endmill!
    A the tool almost made it through case hardened clamp 3/4" deep at fill slot and only one flute got little chipped.
    Still using the same tool. Works fine.

    So for aluminum SGS SwiftCarb 3/4" Dia Can really haul more material than our puny conveyor can remove.
    Still a 2" APKT16 Face Mill Easily removes 50in^3/min even when 5" long.

    Damn, getting after it pretty freaking hard there zero_Divide. I will have to remember that brand. Sounds like i would max out my machine before I max out tool.


Bookmarks

Posting Permissions

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