conventional milling vs. planer mill
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 21
  1. #1
    Join Date
    Oct 2014
    Country
    UNITED STATES
    State/Province
    Maine
    Posts
    873
    Post Thanks / Like
    Likes (Given)
    96
    Likes (Received)
    404

    Default conventional milling vs. planer mill

    The recent posts about stress relieving (via heat or ringing like a bell) of straight edges to reduce movement got me thinking. When I read Moore's Foundations of Mechanical Accuracy, they talked about how castings that were machined with a planer mill showed less movement than castings that were machined with a rotating cutter. I have a few questions about this.

    1) Does anyone know why this is?
    2) Since I don't have a planer mill, are there certain speeds/feeds/DOC that work better with conventional milling to reduce movement?

    Thanks,
    Daniel

  2. #2
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    Quote Originally Posted by DanielG View Post
    The recent posts about stress relieving (via heat or ringing like a bell) of straight edges to reduce movement got me thinking. When I read Moore's Foundations of Mechanical Accuracy, they talked about how castings that were machined with a planer mill showed less movement than castings that were machined with a rotating cutter. I have a few questions about this.

    1) Does anyone know why this is?
    2) Since I don't have a planer mill, are there certain speeds/feeds/DOC that work better with conventional milling to reduce movement?

    Thanks,
    Daniel
    .
    large dia milling cutters can glide over hard spots then sink in a bit on softer spots of metal. milling with smaller diameter cutters is the same as a small width planer cutter in being more stable over hardness variations.
    .
    picture showing the milling cutter cutting deeper at small localized softer areas of metal. literally can measure the over .0005" differences. i later got it down to under .0003" flatness by using a 1" dia rather than 2" dia mill
    Attached Thumbnails Attached Thumbnails ballscrewfacehardspots1_smaller.jpg  

  3. Likes lowCountryCamo liked this post
  4. #3
    Join Date
    Jan 2014
    Location
    Green Lane, Pa.
    Posts
    725
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    431

    Default

    Quote Originally Posted by DanielG View Post
    The recent posts about stress relieving (via heat or ringing like a bell) of straight edges to reduce movement got me thinking. When I read Moore's Foundations of Mechanical Accuracy, they talked about how castings that were machined with a planer mill showed less movement than castings that were machined with a rotating cutter. I have a few questions about this.

    1) Does anyone know why this is?
    2) Since I don't have a planer mill, are there certain speeds/feeds/DOC that work better with conventional milling to reduce movement?

    Thanks,
    Daniel
    When you say planer mill are you referring to the single or double tool when planing or the milling machine for rotary maching on the planer mill? Planer mill has both options, a planer does not.

  5. #4
    Join Date
    Oct 2014
    Country
    UNITED STATES
    State/Province
    Maine
    Posts
    873
    Post Thanks / Like
    Likes (Given)
    96
    Likes (Received)
    404

    Default

    A planer where the tool doesn't rotate. I didn't know there was a distinction between a planer and a planer mill. I've only seen videos of very old ones.

  6. #5
    Join Date
    Jan 2013
    Location
    SE PA
    Posts
    512
    Post Thanks / Like
    Likes (Given)
    474
    Likes (Received)
    388

    Default

    maybe since the metal removal rate is lower for a planer, there is less heat introduced into the part? my wild guess.

  7. #6
    Join Date
    Jan 2014
    Location
    Green Lane, Pa.
    Posts
    725
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    431

    Default

    There is a difference between the 2, we had both with 32 foot tables (Grays) and as far as I know both were used to do the bottoms on the die shoes of very large automotive dies from 50 tons in down. Punch plates, and bolster plates that ranged from 2"-6" thick burned out of hot rolled steel were all planed with dual clapper boxes. Die shoes which are either cast iron or steel castings had their bottoms planed or milled depending on what machine they were on. They could hold .005 over 15 foot. The only time we worried about stress was when a inspection base was to be planed from a steel plate that was burned out. We would machine any side that was burned out as this is where stress would rise from.

  8. #7
    Join Date
    Aug 2007
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    2,077
    Post Thanks / Like
    Likes (Given)
    1111
    Likes (Received)
    943

    Default

    I don't have a planer, someday maybe I will.

    From what I have seen-a planer is much like a surface grinders, and as the tool steps over you really don't get any lines in you part, like you do when milling.

    The chips curl right up and off the part, so all the heat is going away from the part. Not into it. Like hard turning.

    You are only taking a very narrow cut.

    I have a 48" x 120" Busch Precision table that was planed. I can measure it is overall within about .002".

    If you done follow him check out some of this guys posts from Japan on Instagram. He has a huge planer and shows some of the cuts it takes.

    https://instagram.com/daichihira/

    In no way am I claiming to be an expert on planers but these are just my observations.

    Here is an old video I took at Busch Precision when we were doing some testing.

    https://www.youtube.com/watch?v=nCRYiMzOYaM

  9. #8
    Join Date
    Dec 2011
    Location
    Washington State, USA
    Posts
    208
    Post Thanks / Like
    Likes (Given)
    62
    Likes (Received)
    100

    Default

    Stress appears to be less if the tool puts pressure into the scrap, like a planer or face mill would. A horizontal mill's side cutter or the periphery of an endmill puts the pressure into the work, where the stresses will now live. My take on things.

  10. Likes stephen thomas liked this post
  11. #9
    Join Date
    Apr 2013
    Location
    Damascus, MD
    Posts
    1,433
    Post Thanks / Like
    Likes (Given)
    4136
    Likes (Received)
    808

    Default

    A big difference (and I believe it was explained also in the Moore's book) is that, with shapers and planers each cutter makes a continuous cut end-to-end, whereas each cutting surface of a milling cutter cuts just a small portion, impacting the surface when entering the cut. Each impact produces stress.

    In these regards, a face-mill should be the least offending of the rotary cutters.

    Paolo

  12. Likes ironsmith89 liked this post
  13. #10
    Join Date
    Oct 2014
    Country
    UNITED STATES
    State/Province
    Maine
    Posts
    873
    Post Thanks / Like
    Likes (Given)
    96
    Likes (Received)
    404

    Default

    Thanks for all the replies. It's been a while since I read Moore's book.

    Since I don't have a planer, just a knee mill, it sounds like the best option for a low stress part would be fly cutter. Does that sound reasonable?

  14. #11
    Join Date
    Mar 2007
    Location
    Milwaukee
    Posts
    420
    Post Thanks / Like
    Likes (Given)
    345
    Likes (Received)
    188

    Default

    Quote Originally Posted by DanielG View Post
    Thanks for all the replies. It's been a while since I read Moore's book.

    Since I don't have a planer, just a knee mill, it sounds like the best option for a low stress part would be fly cutter. Does that sound reasonable?
    I cut all of my precision tooling with a 3 flute 1/2 carbide endmill. The ones with a small corner radius stay sharper longer and have better cut engagement. A fly cutter will get dull by the time you finish a cut. The nice thing about an endmilll is that is always engaged into the cut. I feel that banging cutting teeth into a part will induce some level of stress into the surface you are going to scrape.
    I avoid the temptation of using a large diameter face mill and 1/8 depth of cut. With the endmill you do not need a lot of clamping force to hold your work.
    Yes it may be a bit slower, but it will be a small percentage of time you spend making the tool straight.

    I read the same thing about planning in the Moore book myself. I would like to think they were comparing against a slow SFM large dia. milling cutter banging into the workpiece. If Moore went through the trouble of writing it, they must have done a study. I believe Moore.

    One of my boatbuilding mentors worked at a printing press manufacture that rebuild machine tools in WW2. He swore a planed surface such as a gib stayed straight due to the cutting forces going in one direction.
    Doubtful that I will ever get a chance to test the theory. I'll stick with and endmill

  15. #12
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    i cut machine slide sections to .0005" flatness, straightness, perpendicularity tolerances over distance over 40" every day with milling equipment.
    .
    of course it requires at least 2 finish cuts (often 3 or 4) and care in supporting part and rechucking before finish cuts as a warm part expands and flat milled surface can bend into a curve easily when cooled to room temperature.
    .
    more depends on how a part is supported, torque used to clamp in position, temperatures when part machined, how much is being removed at a time (width and depth of cut and speed)
    .
    i can easily see a slower metal removal process being thought of as more precise when it is more a slower process makes less heat changes and less metal removal rate creates less part flexing from cutting forces which helps create more precise surfaces .
    .
    you can go as slow as you want milling. taking .0005" depth cuts i do all the time especially if error is less than .0005" , like i said if metal has hardness variations and part flexing in fixture as cutter goes past hard spots and then sinks in further in softer areas a small diameter milling cutter is used similar to using a narrower or small radius planer tool. think of it as trying to hand file a hard steel part and file feels like it is not digging in or just sliding over rather than cutting. it you have a part only hardened on the end as you file it you can feel it cutting more on the softer end compared to the harder end
    .
    you cannot easily make 6" wide milling passes flat to less than .0003" usually. i often have to use a smaller diameter milling cutters the tighter the tolerance is

  16. Likes CBlair liked this post
  17. #13
    Join Date
    Jan 2012
    Location
    Savannah, Georgia, USA
    Posts
    1,657
    Post Thanks / Like
    Likes (Given)
    2625
    Likes (Received)
    631

    Default

    Quote Originally Posted by DMF_TomB View Post
    i cut machine slide sections to .0005" flatness, straightness, perpendicularity tolerances over distance over 40" every day with milling equipment.
    .
    of course it requires at least 2 finish cuts (often 3 or 4) and care in supporting part and rechucking before finish cuts as a warm part expands and flat milled surface can bend into a curve easily when cooled to room temperature.
    .
    more depends on how a part is supported, torque used to clamp in position, temperatures when part machined, how much is being removed at a time (width and depth of cut and speed)
    .
    i can easily see a slower metal removal process being thought of as more precise when it is more a slower process makes less heat changes and less metal removal rate creates less part flexing from cutting forces which helps create more precise surfaces .
    .
    you can go as slow as you want milling. taking .0005" depth cuts i do all the time especially if error is less than .0005" , like i said if metal has hardness variations and part flexing in fixture as cutter goes past hard spots and then sinks in further in softer areas a small diameter milling cutter is used similar to using a narrower or small radius planer tool. think of it as trying to hand file a hard steel part and file feels like it is not digging in or just sliding over rather than cutting. it you have a part only hardened on the end as you file it you can feel it cutting more on the softer end compared to the harder end
    .
    you cannot easily make 6" wide milling passes flat to less than .0003" usually. i often have to use a smaller diameter milling cutters the tighter the tolerance is
    What type of insert tooling do you use? Double positive, neg-pos,up sharp, t-land, coatings, etc. or large endmills? Thanks Tom I value your experience.

  18. #14
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    Quote Originally Posted by lowCountryCamo View Post
    What type of insert tooling do you use? Double positive, neg-pos,up sharp, t-land, coatings, etc. or large endmills? Thanks Tom I value your experience.
    .
    i have no ideal the exact tooling i use i do not think we use any negative inserts flat top surface inserts almost all have shaped or grooves that give a positive edge. we use no simple flat inserts all we use have chipbreaker shapes on top. some insert cutters have 1 wiper insert and 6 regular inserts. the wiper insert smooths out finish. or other cutters have a small wiper area on the insert corner.
    .
    basically we use roughing inserts better at higher metal removal rates and we use finishing cutters made for better finishing and do not work well at roughing. we avoid general purpose stuff.
    .
    end mills we use are nothing special, corner radius .008 to .020" 2 to 6 flute carbide coated to last longer but when resharpened obviously coating is missing on side reground. finish cutters are used less than 80 minutes and surface finish gets below spec when cutter going dull. when we want the best finish and the most precise we use fresh inserts
    .
    usually when i cut parts over 40" long flat, straight, perpendicular to less than .0005" things most important are
    .
    1) servo oscillation or steadiness of machine to hold a position. often servos need tuning or programmed delays to give it time to steady position
    .
    2)part supported on airy points which if you have to ask is maybe why some have trouble cutting flat shapes. basically parts can sag by their own weight by how they are supported or held
    .
    3) taking multiple finish cuts so final cuts push and or deflect part or tool very little. probably the most important thing. finish cutter size often has a maximum size to get a higher precision flat surface. smaller cutters have less cutting forces
    .
    4) machine calibration or some machines like a double column gantry mill you can fine adjust height difference between columns so machine cuts perpendicular. just saying some machines are far faster to calibrate precise cutting than others by their design.

  19. #15
    Join Date
    Jun 2001
    Location
    downhill from Twain\'s study outside Elmira, NY
    Posts
    11,050
    Post Thanks / Like
    Likes (Given)
    4131
    Likes (Received)
    3867

    Default

    When I first started selling straight edge castings i did not have a planer, and built a face mill to surface them. I built the face mill to take APKT inserts (Pos) with a neg setting in the tool body. This cutter worked very well and is very free cutting.







    I milled the angles with a fixture, and also the square edge, then sent them out for heat treat/thermal stabilization.
    The customer did any finish milling or plaing. I was able to scrape them without further machining after heat treat, but the error (curve) was sometimes in the range of .010. Kind of on the boarder where "does it actually save any time to set up and plane again, vs just going at it with the biax?"

    When I got a planer, they could be done 2 at a time.







    Here's a one-time set up to plane a 5' SE on edge. My planer is a little bit more true side-to-side/tool planing down, than it is cutting with the surface horizontal. The ends kick up on the table in a long cut. This is minor for parts under 4' long, but increases after that.



    These also went out for thermal treatment to Elmira Heat Treating after planing.

    smt

  20. Likes Paolo_MD, cash liked this post
  21. #16
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    finish machining after warping from heat treatment or even rechucking multiple times so parts warps if it wants to, then finish machining machines it straight again is basic method of machining precision surfaces.
    .
    obviously if poorly designed fixture and you force a warped part straight it will when removed from fixture warp again. often the trick is how to hold a part and not be putting force on it that can cause it to bend from the clamping force. this usually means part is rarely clamped directly to a table
    .
    mounting a part at its airy points so it is free to warp after roughing and can easily be finish machined usually require careful thought on where and how a part is held. fixture design and or part holding often is 99% of the job machining precise surfaces
    .
    picture of a machine i run machining parts in the 1 to 10 ton range and the parts are torqued often to 10 foot lbs or even less than 3 foot lbs to minimize part bending from clamping forces. i often use a .00005" or .0001" indicator to measure part moving when torquing or clamping in a fixture. i often see .0005" movement or more when clamping. a poorly designed fixture and part can warp easily over .001" just from clamping forces
    .
    i often normally align a side surface or proof edge to within .0001" so i can get part bottom edges in alignment to edges i will cut on the top side. fixture at best will get part too .0005" over 40" distances. fine adjustments is needed 90% of the time if i want to get part to within .0001" over 40" distances. this often requires using pusher screws and over travel a bit then remove pusher screw pressure and see what part reads with little pressure on it. there are some parts literally only hand finger tightened of clamping bolts to minimize part distortion
    .
    also we have a climate controlled building and even our coolant temperature is controlled. obviously if using coolant 5 degrees hotter or colder than part, warpage can and often does occur
    Attached Thumbnails Attached Thumbnails bn25a_partsnearby_smaller.jpg  

  22. #17
    Join Date
    Jun 2013
    Location
    england-newcastle upon tyne
    Posts
    713
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    154

    Default

    I normally rough long jobs at slower speed ease the clamps off and chalk the surface and take a "spring cut" normally works but not unusual to have to "flip" the job over more than once depends how flat and the tolerance on the job

  23. #18
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    Quote Originally Posted by onecut View Post
    I normally rough long jobs at slower speed ease the clamps off and chalk the surface and take a "spring cut" normally works but not unusual to have to "flip" the job over more than once depends how flat and the tolerance on the job
    .
    typically i
    rough and semi finish 1st side leaving .020"
    rough and semi finish then final finish 2nd side
    flip and final finish 1st side
    .
    rare but sometimes have to flip again to finish 2nd side again but normally not needed

  24. #19
    Join Date
    Sep 2009
    Location
    washington
    Posts
    260
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    46

    Default

    Hi All,

    I've been to Moore's factory. It's a wonderful place. They use a very large planer ,
    essentially a one or more clapper planer with a very large bed. They rebuild
    them every 3 months.

    If you think about it in engineering terms it is easy to understand why they
    use a planer instead of a face milling cutter, but it's a very slow process.
    In simple terms, the planer process is 100's of times slower than using a face
    milling cutter, and since you are cutting the same amount of material, at the
    same feed rate - you are essentially putting 100 times more energy and heat into
    the material, thus causing it to warp.

    If you want to calculate the real heat difference: calculate the amount of material
    removed per minute, for each process. Figure 1 Horse power(HP) per cubic inch per minute - 746 watts/HP.

    I hope I didn't put you all to sleep, but it becomes obvious why use a planer.

  25. #20
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,212
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2651

    Default

    Quote Originally Posted by toolnuts View Post
    Hi All,

    I've been to Moore's factory. It's a wonderful place. They use a very large planer ,
    essentially a one or more clapper planer with a very large bed. They rebuild
    them every 3 months.

    If you think about it in engineering terms it is easy to understand why they
    use a planer instead of a face milling cutter, but it's a very slow process.
    In simple terms, the planer process is 100's of times slower than using a face
    milling cutter, and since you are cutting the same amount of material, at the
    same feed rate - you are essentially putting 100 times more energy and heat into
    the material, thus causing it to warp.

    If you want to calculate the real heat difference: calculate the amount of material
    removed per minute, for each process. Figure 1 Horse power(HP) per cubic inch per minute - 746 watts/HP.

    I hope I didn't put you all to sleep, but it becomes obvious why use a planer.
    .
    facemill finish recuts are typically .001" or .0005" depth
    .
    smaller diameter mills are used if metal hardness variations cause cutter and part deflection variations causing wavy surface. smaller diameters and the waves are less than .0003" much more often
    .
    i cut everyday less than .0005" flatness variations over distances over 40", flatness and edge straightness of less than .0003" per 40" is possible. easier with some lots of castings, other lots of castings with hardness variations are more difficult to meet .0003" tolerance. not all castings are the same consistent metal throughout the casting, there can be definite variations in metal hardness


Tags for this Thread

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
  •