Hello Guest it is September 17, 2019, 09:17:38 AM

Author Topic: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?  (Read 28772 times)

0 Members and 1 Guest are viewing this topic.

Offline Hood

*
  •  25,849 25,849
  • Carnoustie, Scotland
    • View Profile
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #10 on: January 17, 2010, 06:55:16 AM »
Have only ever machined 5083 due to the work I do (marine)  but have always used flood coolant and its fine, bought a mister to try and cut down on the mess but found it a waste of time even when using the same water soluble coolant in it that I was using with the flood.
Hood.
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #11 on: January 17, 2010, 07:28:36 AM »
6061 ranges from T-0 (soft and gooey) to T-651 in this case (tough and gummy) and flood coolant is what we use along with the appropriate speed and feed or cutters are quickly coated with smears of aluminum that attract more aluminum. Although it (6061) is one of the most used aluminum, we try to stay away from it for machined parts on machines without flood coolant, or a constant stream of a light lubricant such as WD40 is needed - smokey! Heavy mist will work but a short period of starved liquid will become a disaster.

7075 can be cut dry in any hardness and it's similar to mild steel in strength.
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #12 on: January 17, 2010, 12:32:13 PM »
Ray ,

2 flute, slow it down , and flood it.
Ed VanEss

Offline simpson36

*
  •  1,374 1,374
    • View Profile
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #13 on: January 17, 2010, 01:10:01 PM »
7075 can be cut dry in any hardness and it's similar to mild steel in strength.

2011 (bar) and 2024 also cut nicely. Like 7075, these very nice to cut after figting with 6061 or 5052 (which is even worse), although that joy comes at twice the price of the 'every day' grades.

2 flute cutters definitely help if you have the power and rigidity to make a big chip.  If you look up cutting speed for aluminum in any text older than a few years you will see what is today a very low number. Aluminum is routinely cut many times faster than that today, and one should get their cutting speeds from the toolmaker and also not forget to multiply that by the appropriate number if using cobalt, carbide or coated tools. You will find an indication for 3x to 10x faster speeds. I  run my 5/16" and 3/8" three and four flute cutters at 7,500 RPM . . . . only because that is as fast as my spindle would go.  My new mill is set up for 8,500.  1/4" cutters are the 'crossover point' below which I go to my die grinder spindle with speed set appropriately up to 28,000 for the really small cutters.

Of course, the faster you go, the more heat problem you have and you start to get into water cooled spindles and stuff like that.
   
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #14 on: January 17, 2010, 01:29:49 PM »
7075 can be cut dry in any hardness and it's similar to mild steel in strength.

2011 (bar) and 2024 also cut nicely. Like 7075, these very nice to cut after figting with 6061 or 5052 (which is even worse), although that joy comes at twice the price of the 'every day' grades.

2 flute cutters definitely help if you have the power and rigidity to make a big chip.  If you look up cutting speed for aluminum in any text older than a few years you will see what is today a very low number. Aluminum is routinely cut many times faster than that today, and one should get their cutting speeds from the toolmaker and also not forget to multiply that by the appropriate number if using cobalt, carbide or coated tools. You will find an indication for 3x to 10x faster speeds. I  run my 5/16" and 3/8" three and four flute cutters at 7,500 RPM . . . . only because that is as fast as my spindle would go.  My new mill is set up for 8,500.  1/4" cutters are the 'crossover point' below which I go to my die grinder spindle with speed set appropriately up to 28,000 for the really small cutters.

Of course, the faster you go, the more heat problem you have and you start to get into water cooled spindles and stuff like that.
   

I was wondering if trying more "high-speed machining" techniques might help.  I find it interesting that small cutters (1/8" and 3/16") seem to work fine, at the same RPM, DOC and feed I normally use, but the 1/2", both HSS and carbide, seem absolutely unforgiving, even at greatly reduced feed and DOC.  I'm tempted to try a 1/2" endmill running max RPM (8200), shallow DOC (maybe 0.050"), and high feed rate (probably 30-50 IPM?).

Regards,
Ray L.
Regards,
Ray L.
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #15 on: January 17, 2010, 05:14:07 PM »
If the chip load per tooth is not exceeded and the cutter is the proper helix for aluminum and lubricated, theoretically there is no top speed.

Offline simpson36

*
  •  1,374 1,374
    • View Profile
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #16 on: January 18, 2010, 05:17:20 AM »
As described, the problem as I see it requires an analysis that is somewhat beyond bobby level, but here it is anyway. For calculating production, you think in terms of the cu.in. of metal removed per minute. Each material has a factor indicating the volume of the material that can be removed per available spindle HP.

Here is an important consideration to keep in mind when deciding on your parameters; SFPM can be all over the map and will effect surface finish and production time, but there is a very wide range that you can use successfully. The same is not true for chip load per tooth. There is a definite 'sweet spot' where the heat goes overboard and the cutter runs smoothly. This is a very narrow range and you will have no success on either side of it. The beauty of CNC is that you don't need to go thru a ton of calculations to arrive at the proper IPM. You just set your feedrate in terms of feed per rev based on the chip load and number of flutes and then run the spindle as fast as your machine will allow (for aluminum). The IPM will automatically be optimized for ANY spindle speed.

Moving on the the analysis; in general terms it goes something like this; lets say you have 'X' spindle power available. You can remove 'X' volume of 6061-T6 per minute.  SFPM of the cutting tool indicates a max RPM of 'X'. With that, you calculate the chip load per tooth required to remove the prescribed volume of metal per time. DOC obviously dictates the VOLUME of the chip at the same per tooth feed, and a 4flute cutter can run at twice IPM of a 2 flute for the same tooth load . . . . BUT, that requires a lot more power and if you don't have the available power (or rigidity), then the solution is not to lower the IPM, which I think most hobbyist's tend to do, which will make the chip too thin, but to use less flutes (for the same DOC), or less DOC so that you can maintain the proper chip load.

Quick word about DOC; the deeper the cut, the more of the tool edge you use and therefor the longer it will last per cu.in. of material removed, but reducing the feedrate to get more depth is not a good trade off if it reduces the chip load beyond the 'sweet spot'.

That being said, it should be simple to combine these factors into 'volume per tooth' thinking. This is the basic idea behind roughing cutters. Obviously a 1/2" cutter is going to make a very much larger volume chip that a 1/4" cutter at the same feed per tooth, the effect of which is what is being observed, methinks. In practical terms, on my little X2 I could not drive a 3/8" cutter at a feedrate (per tooth) that was acceptable, so I went to a roughing cutter in that size.
 
Just my 2 cent's worth . . .

Offline piv

*
  •  91 91
    • View Profile
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #17 on: January 18, 2010, 08:51:13 AM »
Heres what we use 10 hours a day, cutters last months.
Okuma 4VA, big ridgid tool making cnc.
6000 rpm, thats as fast as it goes. Always climb milling.
Ultra synthet (with water) lubricant, we used to use soluble oil/water emulsion.  Always flood coolant.
Nearly always solid carbide uncoated tools. Sometimes brazed carbide router bits for special profiles.
Roughing with 16mm rmr, three flute, Sandvick, tagutec,  or hanita, stelram. feed 2500mmpm, cut about 8mm deep, full width.
Facing with sandvick 8 tip, dia 125mm, aluminium wiper inserts, 2500rpm, 2500mmpm.
Finish with 2 flute carbide end mill, 6000rpm, 1000mmpm (40ipm), 0.2mm  stock finish cut, 5mm step depth for profiling.
Some cutters seem to work better than others.  We find 6061-T6 or 6061-T651 to machine quite well.  5005 is horible, 5083 OK and 7075 good.
HSS tools do work at 1/3 of the rpm of carbide but need to be short to be stiff enough.
We always use the shortest tools practical and on deep parts we often use a short tool then a long one for the deep parts at lower feed rate and depth of cut.

Good luck.
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #18 on: January 18, 2010, 09:08:39 AM »
Simpson,

You're absoutely correct.  My mistake seems to have been in mis-interpreting the tool manufacturers chipload recommendations.  My assumption was they provide recommended chiploads, but I now think they are more like minimums, and you need to go up from there, and see what you can get away with.  I have been running for a long time on values derived by calculating RPM based on SFPM, using the manufacturers chipload to calculate feed rate, then testing to see how deep I could go.  But yesterday I instead started with a shallow cut, and greatly increased chipload.  I found running MUCH higher feedrate did the trick with the icky material. I can run the same DOC (0.175"), but at a 30-50 IPM feedrate, and get an acceptable result, even without coolant.  I need to do more experimentation to come up with optimal values.

Regards,
Ray L.
Regards,
Ray L.
Re: Anyone Here Have Experience Milling 6061-T651 Wrought Plate?
« Reply #19 on: January 18, 2010, 11:58:23 AM »
I must be on the ignore list...