Help! What is the best way to mill this part.
Close
Login to Your Account
Results 1 to 19 of 19
  1. #1
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default Help! What is the best way to mill this part.

    Help! What is the best way to mill this part.
    Hello,

    I am a beginner with milling so any help is welcomed.

    I need to make some round moulds in a steel stock.

    I have an old machine with limited memory capacity and that is why I am using 2d pocket strategies to do the roughing.


    My stepdown is 1 mm, I dont dare to use more.

    My issue is that it takes to long to machine the parts.
    Also another big problem is that the tip of my end mills gets destroyed very often.


    So my question is. What is the best strategy to open these pockets?
    Someone suggested to do a pre drill hole. But I dont see how this helps.
    Attached Thumbnails Attached Thumbnails roughing.jpg   2.jpg   1.jpg   6.jpg   5.jpg  


  2. #2
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    366
    Post Thanks / Like
    Likes (Given)
    291
    Likes (Received)
    116

    Default

    You're wearing out the tip of your endmill because that's all you are using with the shallow stepdown. If you go deeper you will get it done faster and get more material removed before trashing your tool.

    What machine and material? Are you plunging in with the endmill or ramping in?

    I would personally use an adaptive roughing strategy with a smaller (cheaper) endmill to clear it, and then finish the floor and walls. 3/8" or 10mm should be much cheaper and they're still plenty strong for good material removal rates. It might be friendlier to your machine too since it sounds like you may have rigidity concerns?

    How much is "limited memory"? Do you have DNC/dripfeed available?
    I run massive programs through my old HAAS with like 80k of memory by using DNC mode. You could also program one pocket, and just call it as a subprogram at different positions to get your array of pockets.

  3. #3
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,455
    Post Thanks / Like
    Likes (Given)
    441
    Likes (Received)
    1746

    Default

    Helical to depth on the centerline with an end mill slightly smaller than the finish width, then one pass around the outside and inside edges.

    Doesn't get any simpler than that part...

  4. #4
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default


  5. #5
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thanks for the feedback.

    Machine is Ares Seiki Tc 619 - Meldas 500 controller.

    Material is a very cheap steel - dont know the exact specifications .

    I use helix ramping.

    I dont have an issue with finishing passes just with roughing.

    Tool size is 14mm and the gap begins at 43.5 mm.


    11.jpg


    I cant use adaptive because it generates a 200 kb or more filesize.

    I have 50k memory available. I dont have dripfeed available.

    The part has a slope so If I use larger stepdowns it leaves some nasty steps that. Also the owner of the machine is afraid to go with larger stepdowns because he fears it will break the tools.

  6. #6
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,455
    Post Thanks / Like
    Likes (Given)
    441
    Likes (Received)
    1746

    Default

    I didn't see the angle on the floor in the first pics.

    You can hemstitch it, but if you don't like the time or you don't have the memory to hold the program, you can use a form tool to finish the floor. Just have the angle put on an end mill, rough it out with steps and finish the floor with the form tool.

  7. #7
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    366
    Post Thanks / Like
    Likes (Given)
    291
    Likes (Received)
    116

    Default

    I ran it through HSM Advisor and it looks like you can do a 6mm depth of cut very safely, at 2150 and 570mm/min

    I made some assumptions about the tool and material, but the worst case cutting conditions at 6mm depth don't even begin to push the limits.

    At 25mm depth and full width of cut you should be safe at 2150RPM, 173mm/min

    At 25mm depth of cut with an adaptive milling strategy, you're safe at 4500RPM, 1.40mm optimal load/WOC, and 3700mm/min.

    Sorry to mix units, HSMadvisor doesn't let me change the material removal rate units.

    With your cutting parameters, you are at .11 cubic inches per minute material removal rate
    With full slotting at a 6mm DOC, you get 3.1 cubic inches per minute.
    With full slotting at full pocket depth strategy using HSMadvisor numbers, you are at 3.7 cubic inches per minute
    With adaptive milling at full pocket depth using HSMadvisor numbers, you are at 7.93 cubic inches per minute as well, but even so chip evacuation will be more favorable and the load on the mill will be lower. Tool torque is lower than full slotting strategy.

    Please ignore the attached screenshot, I cannot delete it. It didn't properly select the material. The numbers above have the correct material selected.
    Attached Thumbnails Attached Thumbnails image-4-.jpg  

  8. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,401
    Post Thanks / Like
    Likes (Given)
    805
    Likes (Received)
    2370

    Default

    Quote Originally Posted by solidjob View Post
    ......I have 50k memory available. I dont have dripfeed available.......
    The machine probably has a method to drip feed. Pretty uncommon for a machine to not be able to.

    The implementation of a drip feed (DNC) mode is determined by the machine builder, not Mitsubishi. The control can drip feed, but the machine builder has to provide a method for turning on that operation mode. Is there a "TAPE" mode available on the mode selection switch(es)? That is the most common method used. If there is a "TAPE" mode selection then there will be a few parameters to set to match the RS232 parameters used on your PC communication program.

  9. Likes npolanosky liked this post
  10. #9
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,018
    Post Thanks / Like
    Likes (Given)
    13662
    Likes (Received)
    10663

    Default

    790 something RPMs, with a 14mm tool in mild garbage steel..

    I'm thinking you are using a square corner HSS endmill..

    I'm going to go out on a limb, and say its not the tool path... Its the tool.

    False economy, use up qty 5 $20 endmills instead of one $50 endmill, and takes
    3-4 times as long.

    *But the endmills were only $20 each*...

  11. Likes npolanosky, cameraman, solidjob liked this post
  12. #10
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    2,711
    Post Thanks / Like
    Likes (Given)
    3223
    Likes (Received)
    712

    Default

    Just riffing off what BobW says about "IT'S THE TOOL "




    ^^^ Pre-drill + better strategy. Like what folks have already mentioned (peripheral milling) but depends on a minimal rigidity of your machine. .

    Harvi III "Zombie Cutter"...



    ^^^ NOT rigid machine, so when tool is not engaged full depth/length and spindle runout of the machine is not wonderful and significant tool vibration starts to kick in towards the end of the tool in the material (laterally); starts to cause a lot of problems especially with surface finish. So, 'They" push the idea that you can chip the snot out of the tool and it still keeps going and going and going, hence their moniker of 'Zombie" mill …


    Potentially good fit /relevant to smaller less rigid machines.

    Maybe better value for money long term like what BobW is saying.




    ^^^ On the other hand on a rigid fast machine... Just too much fun. (If you have the power and rigidity, gotta admit that DMU 50 3rd gen / Mori Seiki spindle looks pretty awesome.).

    __________________________________________________ ________________________________________________


    @Solidjob on your Cad visualization looks like you have a fillet on the outer wall (bottom wall to floor), but disappears on verification ?


    Did you want a fillet on the other smaller diameter wall / radius, for release / mold ? (no draught angles just straight sides ?).


    Tool like a Harvi* III with a more useful profile (maybe ?)(something with a bit of a radius, doesn't have to be a bull nose end mill, just a thought … especially if your machine can only munch on a few lines of code.

    Corner radius/bull nose end mills

    ^^^

    From the forum one example of bull vs. flat , but coincidently the Harvi III comes in other profiles (even ball end mills) , it's action is along the flute / edge + material processes, ( a lot going on there, I believe Boeing held a competition for a set of requirements that the Harvi III met/ won in a fairly revolutionary way... (I don't know the deeper theory of the tool and they way it breaks chips. )).


    __________________________________________________ ___________

    * No Affiliation but kinda interesting what they get up to in North Carolina... (Kennametal testing facility).

  13. #11
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    2,711
    Post Thanks / Like
    Likes (Given)
    3223
    Likes (Received)
    712

    Default

    Quote Originally Posted by solidjob View Post
    Thanks for the feedback.

    Machine is Ares Seiki Tc 619 - Meldas 500 controller.

    Material is a very cheap steel - dont know the exact specifications .

    I use helix ramping.

    I dont have an issue with finishing passes just with roughing.

    Tool size is 14mm and the gap begins at 43.5 mm.


    11.jpg


    I cant use adaptive because it generates a 200 kb or more filesize.

    I have 50k memory available. I dont have dripfeed available.

    The part has a slope so If I use larger stepdowns it leaves some nasty steps that. Also the owner of the machine is afraid to go with larger stepdowns because he fears it will break the tools.
    Having actually read this...

    OK so your cut (feature) geometry is like 200 mm in diameter run on a reasonably rigid mill tap type machine ,

    I'm not a MACRO B (type) 'Guy".

    Trying to devise a recursive function / nested routine to accomplish that part geometry with minimal code.

    with standard G an M codes you should be able to stay within your 50 KB limit (I don't see an immediate need for trochoidal tool paths and the like ? But shallow sloped long approximated series of arcs shouldn't be that data intensive... ? ) nice if you have it but not mandatory ¯\_(ツ)_/¯

    If you have the time to pull apart an adaptive tool path as posted code from CAD/CAM and then tear into it and attempt to rebuild it as almost hand coded approximation ? So the kinetics match reasonably well but with waaaaay less code ? Pull out some graph paper and start sketching out code on a pad ?


    Wondering about more unusual tool profiles... (an additional roughing tool) That shallow slope at the bottom of the large shallow doughnut … Maybe for roughing something not straight sided/ square + improved tool life (like what folks have been saying).


    Not sure how you program "Rest" machining lol, but you said you have no trouble with finish passes.

    __________________________________________________ __________________________________________________ _______

  14. #12
    Join Date
    Oct 2014
    Country
    CANADA
    State/Province
    Ontario
    Posts
    136
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    54

    Default

    I'd look at using an indexable high feed mill, as long as you have the money for one. Judging by the part, a .75" tool would be a good size and would get you most of the way down the taper on the floor.

  15. #13
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thanks for the reply.

    I am afraid I dont understand what hemstitching in milling means!?

  16. #14
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    I am using nc lite to transfer the nc program.

    I have tried with other dnc software to configure the dripfeed but to no avail.

    I am using hsmworks and I am transfering the program piece by piece. The roughing operation than the finish.

  17. #15
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thank you for reading and replying.

    I dont have much experience with writing g code.

    My operations list is as follows.

    Roughing

    1. I do 3d pocket operation for roughing with 14 mm flat end mill Hss.

    2. 3d pocket with 6mm flat endmill - for the bottom where the 14mm cannot reach

    Finish

    3. 3d contour with - 8 mm ball endmill - for the outer face

    4. 2d contour for the inner straight face

  18. #16
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Hello.

    What do you propose?

    Should I use indexable endmills?

    Higher quality flat endmills?

    Or maybe bull nose endmills?

  19. #17
    Join Date
    Jun 2019
    Country
    MACEDONIA, THE FORMER YUGOSLAV REPUBLIC OF
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Quote Originally Posted by npolanosky View Post
    I ran it through HSM Advisor and it looks like you can do a 6mm depth of cut very safely, at 2150 and 570mm/min

    I made some assumptions about the tool and material, but the worst case cutting conditions at 6mm depth don't even begin to push the limits.

    At 25mm depth and full width of cut you should be safe at 2150RPM, 173mm/min

    At 25mm depth of cut with an adaptive milling strategy, you're safe at 4500RPM, 1.40mm optimal load/WOC, and 3700mm/min.

    Sorry to mix units, HSMadvisor doesn't let me change the material removal rate units.

    With your cutting parameters, you are at .11 cubic inches per minute material removal rate
    With full slotting at a 6mm DOC, you get 3.1 cubic inches per minute.
    With full slotting at full pocket depth strategy using HSMadvisor numbers, you are at 3.7 cubic inches per minute
    With adaptive milling at full pocket depth using HSMadvisor numbers, you are at 7.93 cubic inches per minute as well, but even so chip evacuation will be more favorable and the load on the mill will be lower. Tool torque is lower than full slotting strategy.

    Please ignore the attached screenshot, I cannot delete it. It didn't properly select the material. The numbers above have the correct material selected.


    Thanks for the reply.

    The adaptive tool strategy is not an option for now - because the file size gets to high. I have a limit of 54 kb.

    I have a couple of options:

    1. To configure drip feed - but this is highly unlikely because the owner of the machine doesn't want to experiment.

    2. Maybe I can use and indexable endmill and just do plunge milling. Like so: YouTube

  20. #18
    Join Date
    May 2019
    Country
    FRANCE
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Quote Originally Posted by solidjob View Post
    Thanks for the reply.

    The adaptive tool strategy is not an option for now - because the file size gets to high. I have a limit of 54 kb.

    I have a couple of options:

    1. To configure drip feed - but this is highly unlikely because the owner of the machine doesn't want to experiment.

    2. Maybe I can use and indexable endmill and just do plunge milling. Like so: YouTube
    If you have macro capability you could program an adaptive strategy with a very short program since your geometry is really quite simple.

  21. Likes cameraman liked this post
  22. #19
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    778
    Post Thanks / Like
    Likes (Given)
    59
    Likes (Received)
    294

    Default

    I don't have any input on your toolpaths.

    However, there is nothing stopping you from having a huge program (whether that is high speed machining or anything really) and just break the program up into several programs.

    It would be slow. And when it completes one segment, you'd have to upload another program to the machine. But you CAN do it.


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
  •