End Mills and Feeds n Speeds - Page 3


Page 3 of 4 FirstFirst 1234 LastLast
Results 25 to 36 of 40

Thread: End Mills and Feeds n Speeds

  1. #25
    Registered
    Join Date
    Jan 2011
    Location
    Uk
    Posts
    57
    Downloads
    0
    Uploads
    0

    Default

    I ran another job today which required the use of my new 2mm end mills.

    The first part of my tool (pocketing) using this 3fl 2mm was at 0.75mm cut depth running at 5000rpm with 250 Feed Rate, which worked ok.

    The next part of the tool (pocketing) was at a 0.95mm cut depth, using same feeds and speeds, this then broke. Cutting fluid and air was used.

    I have attached a couple of images to show the successful (square) and failed cut.
    The mill was installed allowing about 6mm out from the collet.

    If I put this data into my GWizard calculator, 2mm, 3 flute, 6mm stickout, 0.95 DOC, 5000rpm then my feed rate is coming out at 250, with an axial engagement of 47.5% well within limits.
    I could drop DOC to 0.5 which would provide 25% engagement.

    Not sure why this is breaking, when the conditions seem to be well within limits.



  2. #26
    Registered
    Join Date
    Sep 2010
    Location
    UK
    Posts
    87
    Downloads
    0
    Uploads
    0

    Default

    Out of interest why the change in DOC for the two jobs if they are basically the same?

    Also don't forget those figures are fine in a straight line but when you get to an inside corner you have much greater engagement.

    edit...no pics showing



  3. #27
    Registered
    Join Date
    Jan 2011
    Location
    Uk
    Posts
    57
    Downloads
    0
    Uploads
    0

    Default

    Hi Rikk,

    The reason for change of DOC is due to two different features, one having depth of 0.75 the other having 0.95 both having one plunge step.

    The 0.75, square feature ran fine, even in the corners, it was the 0.95 straight line cut that caused the mill to break. A 1mm cut width was entered in to the calculator.

    Attached are the missing images.

    Attached Thumbnails Attached Thumbnails End Mills and Feeds n Speeds-imag0808-jpg   End Mills and Feeds n Speeds-imag0809-jpg  


  4. #28
    Gold Member BobWarfield's Avatar
    Join Date
    May 2005
    Location
    USA
    Posts
    2501
    Downloads
    0
    Uploads
    0

    Default

    Hi Simon.

    Seems like all the feeds and speeds calculators agree you're running correct feeds and speeds.



    Next step is to look for other causes of breakage. Here are a few to consider:

    - With small cutters, be wary of runout. I had one day in the shop where I broke 8 small 1/8" diameter EM's. Eventually I thought to check the runout and after fussing about discovered a brand new ER collet was bad. Switched collets and the problem went away. Your pictures of the cuts look awfully rough, so maybe something is going on there. If you can, measure your runout. If not, at least try different collet and chuck.

    - Speaking of collets, you said you are running an ER40. That big collet takes a surprising amount of torque before you get it properly tightened. A quick hand tight on the machine won't get you there. Two hands, a reasonable amount of leverage, and a tightening fixture of some kind will get you much closer. See for example my article on using ER collets here:

    Getting the Best Performance from ER Collet Chucks « « CNCCookbook CNC Blog CNCCookbook CNC Blog

    You may find a smaller chuck is easier to deal with and affords more clearance as well.

    - Take a look at your toolpath options in your CAM program. How are you getting the cutter into and out of the pocket? Gently helixing in is preferred, though ramping is not so bad either. Plunging is the hardest on the cutter and you'll want to make sure you use a much slower plunge feedrate. Also, I sure hope your CAM will do the initial pass at a little slower rate as it is cutting a full slot until it gets things opened up a tad.

    - Take a look at a different cutting fluid. As was mentioned aluminum is sticky. Once it starts welding to the cutter the end is near. Maybe your fluid isn't providing proper lubrication? Easy way to test is turn off your fluid and try some shots of WD-40 from the can.

    - Consider the aluminum itself. Some of it, especially cast aluminum, can be horrible stuff--more like taffy than metal it is so sticky. Even material certified "6061" or whatever can vary quite a bit from one source to the next. Is it possible you've just fallen into some nasty stuff? If so, chip clearance is your paramount considering. Reduce depth of cut and take more passes. Double check your chip clearing--be paranoid about any chips hanging around the cut. Last "secret weapon" for really nasty stickiest aluminum: try a single flute cutter. They sell them largely for the router crowd, but several machinists have advised me they keep some on hand for working with the worst grades of aluminum.

    Hope that helps!

    Best,

    Bob Warfield

    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html


  5. #29
    Registered
    Join Date
    Jan 2012
    Location
    Australia
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default

    Looking at the photo to the right, the one you see the tool breaks on, it looks like you are cutting a slot. If this is the case you maybe overloading the tool if your speed/feed calculations are based on a 1mm stepover. How is the tool entering the job, ie plunge straight in then start to feed or maybe a ramp to depth. Either way you have a stepover of more than 1mm so feeds need to be calculated to suit. A slot has a tool engagement angle (TEA) of 180deg and a straight plunge 360deg. You will need to adjust feed rates for this part of the cut.

    The best way I have found for entering a cut is helical ramping as this will have a constant step over and allow for chip clearance.

    Looking at the amount of burring on the edge of the cut looks like you are lacking in enough lubrication at the cutting edge causing a built up edge (material welding itself to the cutter) or a soft grade of aluminium. Be sure that the grade is guaranteed what you asked for. 6061 should be in grade t6 (hardness).

    Looking at the photo of the square hole the corners are milled square so you will also get a TEA of 180deg. If your CAM program does not allow a strategy for corners (rounding, slowing the feed rate, corner peeling) you will need to program for the worst case scenario.
    Gary

    When you come to a fork in the road take it


  6. #30
    Registered
    Join Date
    Jan 2012
    Location
    c
    Posts
    173
    Downloads
    0
    Uploads
    0

    Default

    are those pictures of the recent cuts using new cutters and parameters you say to be working or old pictures when you were having problems. I can tell by the buring your aluminum is clearly very soft. The 6061 that machines better is typically the artificially aged to T6 hardness 6061 which mills a lot better.

    The pic on the left look almost unacceptable if done using a flat end mill. It almost looks like something with a ball nose end mill but it could be the perspective of the picture.

    Likes someone said, runout could be an issue too, you should measure it with an indicator. Runout if generally consistent in the say tens of microns range, hurts smaller cutters more than larger cutters in terms of percentage. e.g. one cutting edge takes a really heavy bite than the other. If your runout is poor because the spindle is crapping out then you have to modify your milling parameters to make them less aggressive. Also, the parameters given by manufacturers or calculators are sometimes just suggestions or maximum parameters to minimize machining time. Unless the material work hardens, then the parameters are often not the 'minimum requirement' but rather the suggested or maximum you can push. You will be fine running less aggressive parameters on aluminum than the ones your calculators give you. E.g. try slowing the feed and DOC. For gummy materials you can slow down your RPM also (while maintaining feed) or alternatively increasing feed while maintaining RPM, i.e. you want the cutter to take bigger bites. But I'd definitely start with smaller DOC as the material is gummy and you may have runout issues.



  7. #31
    Registered
    Join Date
    Jan 2011
    Location
    Uk
    Posts
    57
    Downloads
    0
    Uploads
    0

    Default

    @Bob
    Thanks for the advise, I will be looking into runout.
    Even when doing 10mm roughing/finishing I have yet to get a really decent finish, but of course there are other factors I need to consider too.

    When we spoke to the Syil distributor in UK, we sent them image of the types of tools that we wanted to produce and even went and visited a local user, all said our parts were simple and should be no problem. As a complete noob to CNC, we put our trust in Syil and it was them that recommended that ER40 was the best for applications. However, knowing what I know now, ER40 is perhaps not the best solution, more so on the small end mills as we most of our work is going to be using 1.5mm drills and 1, 2, 5mm end mills. Maybe its a bit harsh, but I think we were seen coming.

    For tool paths, we are just using a plunge, at the moment.
    When I started looking at CAM solutions, we wanted something that would integrate into Solidworks. I tried lots of software, open source, free and subscription based too and have a spreadsheet of them all.
    BobCAM are VERY aggressive on sales and dropped their price by over 50% to get the sale. In hind site, was it the best purchase? maybe not. When they did the demo, they used our supplied SW file and it looked a breeze. It wasn't a perfect demonstration in terms of click, click, click done but I wasn't expecting it to be. We used a local training BobCAD trainer, who had a very good training guide, but was just reluctant to teach based on our application. When we did get him to try, he struggled to get some tool paths to create and had no idea why. There were months of going back to him and BobCAM to get support, unfortunately, all BobCAD were interested in were trying to sell us their extended support and training.
    Anyway, they finally gave in and did a live support call and even they had issues getting it too work and this just uses simple pocketing and some drilling routines.
    The expectation that BobCAM could be used straight away on our part was torn apart. We now have to add a bunch of additional planes and boundary sketches to get it to create paths. Luckily for us, we built an awesome app which builds our tools in seconds based on just a couple of dimensions.

    So, as it stands, we got BobCAM to produce tools paths but had to move to the next stage of making the resultant gcode work through MACH to our Syil
    Reliance/assurance that the default milling parameters in BobCAM we sufficient have also taken a battering.
    I appreciate that I now need to move further and perhaps choose better milling routines like spiralling to reduce stress.

    I certainly learnt that trying to drill 26mm deep in this material with a 1.5mm drill bit in one pass just does not work and pecking at 2mm steps seems to work much better.

    For cutting fluid, I was finding that although it appeared to be working, it was also causing chips to collect after ejecting and without a constant air supply to clear them, it was actually have a negative effect in comparison to running the same job dry (on a 10mm rough)

    As for material, its a face palm moment.
    The decision was made to purchase a bunch of blanks for us to use, from China Although they are specified as T6 6061, in reality they could be anything. The old addage you get what you pay for rings true.
    I have found a new single flute in a box of old bits, so I will certainly give that a go.

    Appreciate your feedback.

    Simon



  8. #32
    Registered
    Join Date
    Jan 2011
    Location
    Uk
    Posts
    57
    Downloads
    0
    Uploads
    0

    Default

    @GazMann

    Yes, you are right, the stepover is set to 50% so a 1mm and thats what the calculations have been based on. Also, the EM supplier were the ones that recommended the F&S.

    I dont believe that my CAM package does have a strategy for corners, its certainly never been mentioned., but I will look into this.

    Many thanks.

    Simon



  9. #33
    Registered
    Join Date
    Sep 2010
    Location
    UK
    Posts
    87
    Downloads
    0
    Uploads
    0

    Default

    Why not buy some 6061 here in the UK, doesn't need to be huge chunks just enough to test out your tool paths/parameters, least then you may know if the material you have now is actually any good.



  10. #34
    Registered
    Join Date
    Jan 2011
    Location
    Uk
    Posts
    57
    Downloads
    0
    Uploads
    0

    Default

    @bebob

    The pictures (square pocket) are the ones that I am having issue with.
    The left picture (pocket) has produced a flat pocket bottom, using a flat end mill.

    More tests are definatley needed with this material and understanding our relationships with DOC etc.

    The Gwizard calculator, does have an option to be aggressive, which I have wound down to be lazy.

    So far from the intial cam settings we were given, machine time has increased from 45min to almost 2 hours. But hey, 2 hours is better if it works than producing crap or constantly breaking mills.

    Simon



  11. #35
    Registered
    Join Date
    Jan 2011
    Location
    Uk
    Posts
    57
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Rikk View Post
    Why not buy some 6061 here in the UK, doesn't need to be huge chunks just enough to test out your tool paths/parameters, least then you may know if the material you have now is actually any good.
    Hey Rik,

    Thats next on my list, along with changing to maybe an ER20 collet system.
    In fact, if we have to change to a smaller collet system and invest in a new shank ans series of collets, then we may just go for an easy change system like the Easy Change System from Coventry Toolholders.

    Do you have any recommendations for ali stock sources in UK?

    Many thanks.

    Simon



  12. #36
    Registered
    Join Date
    Feb 2012
    Location
    United States
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    I have a peck drilling problem (G83); while operating my Cincinnati Milacron Sabre 750 with 2100 Acrimatic controller, the code runs very well till its gets to the line where I have the G83 code and hangs the drill there, just rotating and doesn't feed in the Z-direction;
    Below are the lines of codes I ran on the VMC, the G83 code went rapid to the clearance plane, then stopped there. It did not go further to drill the programmed hole (I.e it didn't feed in the Z-direction as required).
    :100 T15 M6; HSS-Cobalt I (0.272inch diameter drill, 135o point angle)

    N10: G0 z1.0 M08

    N20: G83 X3 Y0.3189 R0Z-1.6563 K0.125 J11 F0.7 S350 M03 W1

    Please any help regarding this will be appreciated.



Page 3 of 4 FirstFirst 1234 LastLast

Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

End Mills and Feeds n Speeds
End Mills and Feeds n Speeds