ROUGHING STRATEGY FOR LARGE AEROSPACE AL PARTS

[lowcountrycamo]

I have been programming for an aerospace job shop for several years.  Up until now I have only work on small to medium sized 3, 4, and 5x mills.  On these I mostly rough with dynamic paths. I am now working on a panel that will run on a large SNK HEAD/HEAD horizontal profiler with travels of 48" x 120" cat 50 20,000rpm  Fanuc 31i.  So my question is: considering the size and acceleration of a large machine, what type of roughing should I be focused on:  modern dynamic roughing or old style roughing .5D axial and .5D radial step over?  On the smaller machines the dynamic is generally faster and more reliable.  I am not sure if this is true for larger machines.  Do any of you have experience with larger profilers like this?  Do you have any other advice that would be helpful here?

Thanks,

Steve Austin

 

[Leon82]

You probably have the horsepower to go .5 x .5 or 1x deep and still go pretty fast.

 

I personally before dynamic I would go with a 3/4 accupro 3 flute .375 radial by .375 deep 20k rpm 600 ipm. On a 40 taper. The piece was screwed down, so it could go flying from a vise

[gcode]

If your machine can handle it, 6" Ingersoll hi feeds work very well in steel and stainless steel

In aluminum I'd run a 4" shear mill at 50% step over, .25 DOC dynamic path running as fast as the machine can go

[motor-vater]

2 hours ago, gcode said:

If your machine can handle it, 6" Ingersoll hi feeds work very well in steel and stainless steel

In aluminum I'd run a 4" shear mill at 50% step over, .25 DOC dynamic path running as fast as the machine can go

Agreed, but it depends on the feature... On our big Cat50 Hori's on aluminum parts I try to use the 3 inch 4 insert iscar cutter. Have it on a 10 inch long holder and can still rip material out at ridiculous feeds and speeds it will ramp, pocket, face, what ever I need it to do, only problem is it fills the chip bin to dam fast! here is a photo snagged from the inteweb!

[nickbe10]

Aluminum like Titanium is a heat resistant material. There are two considerations

 Keep you chip load up to make sure you get as much heat into the chip as possible to avoid thermal distortion (induced thermal stress).

For parts above 18" or so the number of cutter impacts can become a factor (induces kinetic stress).

Now its a question of balancing your horse power and the rigidity of your set up.

I will quite often use more traditional step overs (i.e. larger)  to keep the number of impacts down but use the HF toolpaths for "smoothness" if I have the HP available.

The larger the part the more horse power and rigidity are your friend, that's not to say you can't do it with less, it can be just more work.

Conveniently enough keeping your chip load up and you impacts to a minimum = shortest possible run time.

Until finally the parts get so big its time to go true high speed.

There are a lot of efficient high sheer insert mills out there to choose from these days, I have always used Dapra if I don't need to ramp, it's still one of the most free cutting.

[lowcountrycamo]

We have a Mits AXD 2.0" that I use when I can but on this part the pockets are too small.  So I will go for the more traditional milling on this one.  I will try a ZIG ZAG path to get up to speed on as much as possible.

Thanks,

Steve

[Newbeeee™]

15 hours ago, lowcountrycamo said:

... cat 50 20,000rpm ...

 

Ooohhh... I bet it's quite draughty stood next to that when she's running

[nickbe10]

16 hours ago, lowcountrycamo said:

cat 50 20,000rpm

If you can run this rpm with a 2" - 3" insert mill you will probably be just nudging into high speed territory. You might be able to make this work for you under some circumstances, not this one by the sounds of things.

You won't be fast enough (sf wise) with smaller cutters, you really need a min 30,000 spindle.

[JB7280]

14 hours ago, motor-vater said:

Agreed, but it depends on the feature... On our big Cat50 Hori's on aluminum parts I try to use the 3 inch 4 insert iscar cutter. Have it on a 10 inch long holder and can still rip material out at ridiculous feeds and speeds it will ramp, pocket, face, what ever I need it to do, only problem is it fills the chip bin to dam fast! here is a photo snagged from the inteweb!

looks similar to an Ingersoll Roughair tool.  Really an amazing tool for roughing aluminum.

[crazy^millman]

8 minutes ago, JB7280 said:

looks similar to an Ingersoll Roughair tool.  Really an amazing tool for roughing aluminum.

The big difference is the ramping ability of the Iscar tools verses the Ingersoll one. I have used the Iscar 2" one at 1200 IPM, 24K running a .125 DOC with a 60% ROC achieving 180 Cubes a minutes. I am looking to go the other direction in the near future using a full inserted body style to see if 100% DOC with 20% ROC is possible on the 2" diameter cutters. I figured if I can hit the 5 Cubes per horsepower mark Ingersoll says is supported with  there tools on a 100 HP spindle I shouldn't have any problem hitting at least 280 to 350 cubes. 180  cubes was the best I have done' but that is not good enough and we must push harder and faster to see what we can achieve.  

[David Colin]

Stellram 5720 (now Kennametal) is a nice tool to give a try.

Kennametal says its 2" 4fl can remove 527 cubes per min at 24k.   

[huskermcdoogle]

6 hours ago, 5th Axis CGI said:

figured if I can hit the 5 Cubes per horsepower mark Ingersoll says is supported with  there tools on a 100 HP spindle I shouldn't have any problem hitting at least 280 to 350 cubes.

And I'm doing amazing if I can get over 15 cubes cutting Ti....  Horsepower and Torque are not my limiting factors.  Previous to this project 50 taper spindles have treated me well.  My opinion of them has changed greatly. 

Wishing I had an aluminum project to work on with some hogging on it.  Given you are cutting aluminum you shouldn't have to worry too much about bending moment at the spindle connection.  But do pay attention to it, you don't want to exceed it's capability.  Long gage lengths creep up on you, and all of a sudden you are scratching your head as to why your holders are fretting.

For reference, a CAT 50 connection has a bending moment capability of 940Lb-ft.  HSK-100A is 1105, HSK125 2139.  If you need more, which in the world of high strength materials, is absolutely necessary, then you option for more connection strength is to go KM4X100 @ 3540Lb-ft, and KM4X125 @ 5310 LB-ft.

As far as strategy on a large format machine, whatever keeps the cutter in material the most will typically be the best strategy.  You should have the rigidity to deal with heavy radial cuts, so you shouldn't need to worry about radial engagement so much, meaning don't worry about using adaptive paths, just good ol fashioned efficient tool path.  Depending on feature depth and shape, make the best call on whether to go solid or inserted.   I can easily see a 1" KOR5 doing 300 cubes.  Biggest limiting factors to achieving that is feedrate and horsepower.  To give you an idea that would roughly be 500IPM feed sucking down 100HP or so.

Have fun.