[FoxCNC1]

As the tittle says I need some help form the experts.
I have broken two AmanaTool 51454.

These are up-cut 1/8" cutters made for metal.
I think this is due to my part moving - at least on the last occurrence.

I have some questions:

1. What makes a tool appropriate for metal? for instance the AmanaTool 51454 versus a wood FREUD 76-100 ? Are they stronger, sharper?

2. I know that when cutting alum. lubrication is recommended due to heat.
I am profiling with a ramping lead in at a pass depth of 1/64" at 60 IPM with 8000 RPM (the slowest my router goes).
I am little confused since I was told once that if you are to run with low feeds, you should up the RPM? For instance I cut MDF at 180 IPM at 16,000 RPM with the FREUD mentioned above.

My settings are giving me good results, but 8000 rpm, should I be running the IPM a little higher in alum, or should I up the rpm to the next speed level (16,000 rpm)

3. Last but not least, this is my biggest challenge.
I have tried to drill alum. with a dremel by hand and it is not very easy. And again acknowledging that alum is harder than MDF, and I know drilling put a great amount of stress on the machine. I am peck drilling with a plunge rate of 2 IPM 1/16" at a time again same 8000 rpm. There is a little amount of chatter but the machine makes the holes.

I see videos of machines cutting and drilling alum, like butter...


The pieces I am trying to make are 1/4" thick.
Again I am looking for some advice on working with this material.

I am using Aspire, and have access to RhinoCAM also.

[FoxCNC1]

I also wanted to add that based on this chart from them:

http://www.toolstoday.com/images/Alu...Speed-Feed.pdf

I should be running at 16 IPM @ 8000 rpm with their 1/8" dia tool. And if I am reading this correcting I should be able to have a cut depth of D1 = 1/8"
does that sound right?

[ger21]

1) They use different geometry that works better with aluminum.

2) You didn't really ask a question here. What exactly are you trying to do? What type of aluminum is it? Some types of aluminum are very difficult to cut. Make sure you climb cut everything. How rigid is your machine?

3) Again, you didn't really ask a question. Are you drilling with a drill bit? What size?

[FoxCNC1]

1) They use different geometry that works better with aluminum.

2) You didn't really ask a question here. What exactly are you trying to do? What type of aluminum is it? Some types of aluminum are very difficult to cut. Make sure you climb cut everything. How rigid is your machine?

3) Again, you didn't really ask a question. Are you drilling with a drill bit? What size?

1- thank you, make sense. =)

2- well what I am asking is if cutting at the speed I am cutting 60 ipm with 8000 rpms sounds good, or am I way off. The machine is pretty rigid with the latest upgrades from the guys at CNCRP and unlike at the begining of the year the machine is pretty accurate and I have learned enough in terms of cutting that I am getting better results. What I still cannot warp my head around is the concept of higher RPM for slower feeds??

3- I am using the same AmanaTool 51454 to first drill some holes and then profile the part out. I am cutting on the outside of my contours so I have found the I get a nicer finish on the part if I go conventional.
The question is what is a good plunge feed rate to drill alum. - the bit is a spiral.

[ger21]

I forgot about the feedrate part.
No, you don't increase rpm as you decrease feedrate. You use the chipload chart to calculate rpm based on feedrate, or calculate feedrate based on rpm.
Their chart is sort of useless, since it doesn't tell you what rpm they're using. Based on the chipload, though, I'm guessing their using 18,000 rpm for their chart.

Based on the chip load, then yes, you should be between 16-32ipm at 8000 rpm. I'm not sure that you have enough rigidity for 1/8" deep cuts. I'd maybe try .03" until you get the hang of it. With deep cuts, any slop in the machine will snap the bit instantly.

I would not try to drill aluminum with a router bit, especially a 1 flute. Use a short 1/8" drill bit instead, you'll get much better results.

[FoxCNC1]

I forgot about the feedrate part.
No, you don't increase rpm as you decrease feedrate. You use the chipload chart to calculate rpm based on feedrate, or calculate feedrate based on rpm.
Their chart is sort of useless, since it doesn't tell you what rpm they're using. Based on the chipload, though, I'm guessing their using 18,000 rpm for their chart.

Based on the chip load, then yes, you should be between 16-32ipm at 8000 rpm. I'm not sure that you have enough rigidity for 1/8" deep cuts. I'd maybe try .03" until you get the hang of it. With deep cuts, any slop in the machine will snap the bit instantly.

I would not try to drill aluminum with a router bit, especially a 1 flute. Use a short 1/8" drill bit instead, you'll get much better results.

I just went to this page from toolstoday.com and it says:
Solid Carbide Spiral 'O' Flute, Aluminum Cutting Inch & Metric Router Bits -Toolstoday.com- Industrial Quality Router Bits

Please Note: For aluminum cutting please lubricate.
Please Note: The recommended feed rate for Aluminum is 3 M/min or 120 inch/min at 18,000 RPM.

Maximum RPM: 35,000

This must be at very shallow depths or with an industrial type machine.

What I would like to know is how to figure out the plunge speed for a peck drill.. it is best to plung fast 80-120 ipm. or in something like alun do you want to go 10-20 ipm

[ger21]

recommended feedrate will vary with tool diameter. don't pay any attention to general statements like that, as you have no idea what they apply to.
If you use a lubricant, then you'll get better cuts, and your bits will last longer. Some types of aluminum may be almost impossible to cut dry.

Chip loads are calculated to maximize tool life. they don't care what kind of machine you have when they determine chip load. But in most cases, homebuilt routers are usually not rigid or powerful enough to achieve recommended chip loads. You need to do some trial and error testing to find out what works best for your particular setup.

There are formulas to calculate speeds for all types of cutting tools. There's also a learning curve that takes time and practice.
Drilling aluminum on a machine designed to cut wood is not the same as drilling aluminum on a mill.

[FoxCNC1]

I guess what you are saying is that at first you just have to make a cut and evaluate the results until you get familiar with the material and tool.
you last post was very helpful.

[awerby]

If you're profiling and want to use the same bit for drilling, I'd say a drill-point endmill would work better for you. See: http://www.endmill.com/software/Meli...nd%20Mills.pdf (the HSS/Cobalt ones will be less brittle). Even a center-cutting endmill doesn't drill very well. And like Ger says, doing this on a router, where everything is shaky, isn't going to help. Use as fat a tool as you can get away with, since the lack of rigidity is going to be hard on your skinny bits, snapping them off as soon as they're well engaged in the cut. Any run-out in your router spindle (which typically aren't noted for precision) won't help either.

[inventor83]

The run-out on a typical router with standard collets is pretty terrible. I cut T6061 with 1/4 and 1/8th inch endmills at 0.5mm depth 9,000rpms @ 50 IPM. I use the 'stardust' bits from PCT carbide. Use isopropyl or kerosene as lubricant, even WD40 works too.

Happy cutting.

[FoxCNC1]

thank you guys.
What software you "Aluminum cutter guys" using? I am using aspire for profiling, but somehow I feel that rhinocam may be the right tool for metal etc.

[m4bushy]

When cutting 3/16 or 1/4 we step the dia over .020 with every pass. So say you are cutting a 6" x 6" square out of 3/16 6061-t6. Your first pass at z-.06 would leave the square at 6.06 x 6.06 the next pass at z-.12 would leave the square at 6.04 x 6.04 etc. this leaves chip clearance and greatly reduces chip welding.

[FoxCNC1]

thanks, where did you get the 0.020 constant?

[m4bushy]

It is just something I have always done on thicker material. I do use more 3/16 bits so you might need to reduce the step over a bit so not to over stress the tool at full depth.

[jimmyjames1981]

1/8" deep with an 1/8" endmill? Good luck with that, thats not going to happen.

[FoxCNC1]

^ Y not? can you elaborate or then offer some help?

[jimmyjames1981]

9,000rpm and 50 ipm? Where did you come up with those feed rates? if its a 2 flute thats .003 chipload.... it should be between .0005 and .001 for an 1/8" cutter. I guess at only .02 depth of cut you shouldnt have a problem.

[FoxCNC1]

I see what you are saying. thank you