DYNAMIC AREA MILL FEEDS AND SPEEDS ??

[FTI2007]

Im looking for suggestions for feeds and speeds for a general purpose garr 1/2 carbide endmill in P20 steel. I was going to try to rough out a pocket that is .800 deep. I looked at the database but everything there is coated carbide. I was going to try 3056 rpm and feed of 81. with a 10% stepover and full depth. Am I close with these numbers?? Thanks in advance.

[LA CAMmer]

All things being equal I think you are good with your speed. For me your feed is a little high. I run 10% stepover at .0045 fpt (with an IMCO General Purpose AlTiN coated endmill), which in your case would be 55 ipm. Once I get above about 450 SFM and .005 ftp I start tearing up endmills.

 

If you can run at what you have stated you will try, great! Let us know.

[Machineguy]

From the database, thats to fast for a uncoated Garr standard endmill. Im running a VRX .500 in A36 steel ,.375 deep. 3600rpm at 24ipm, 10% stepover, it works. part is run dry. If I run at the full #'s the tool wont last long.

 

Machineguy

[FTI2007]

I played with the numbers and I dont think there is an efficent way to do it with an uncoated standard endmill. I ended up switching it out for a 1.00 AJX feed mill to do the pocket. I had a pretty good idea this was going to happen but wanted to try it. Thanks guys.

[jeff]

Uncoated = ewww

[Chris Rizzo]

We've machined D2 with an el-cheapo.250 uncoated garr, .500 doc. 100ipm Cycle time about 20 min, tool looked new, part looked beautiful.

 

I've found inexpensive tools to work very well with the dynamic paths. (Not to say coated or more spendy tools might be run at higher sfm, thus higher feed rate too.)

[Guest CNC Apps Guy 1]

I'll 2nd that. You can often do okl with cheap e/m's using the HSM toolpaths. You can do AMAZING if you spend some money.

[zero_divide]

I am getting something like that at mediocre aggressiveness:

Material: P20 Tool Steel 330 HB

Tool: 0.500in 4FL Carbide Solid End Mill

Speed: 525.0 SFM/ 4012.7 RPM

Feed: 0.0029 ipt/ 0.0115 ipr/ 46.23 ipm

Chip Thickness: 0.0017 in

Reference Chipload: 0.0012 in

Engagement: DOC=0.800 in WOC=0.050 in

 

and really aggressive:

Material: P20 Tool Steel 330 HB

Tool: 0.500in 4FL Carbide Solid End Mill

Speed: 525.0 SFM/ 4012.7 RPM

Feed: 0.0043 ipt/ 0.0173 ipr/ 69.34 ipm

Chip Thickness: 0.0026 in

Reference Chipload: 0.0012 in

Engagement: DOC=0.800 in WOC=0.050 in

 

Info from here: http://zero-divide.net/index.php?page=fswizard&shell_id=199&load_tool_id=48655

[Chris Rizzo]

Don't forget regular chip thickness calculators are no good, because of radial chip thinning with the reduced stepovers.

 

Also, if you don't mind, when you find some good results, enter them in the dyanamic milling database (in my sig below).

[zero_divide]

Yep i have chip thinning enabled on my own calculator

I tied putting good calculations into my DB but then found out that 90% percent of them are almost dead-on at 150% feed override anyway.

I still save data for different tools though- save me a lot of typing.

 

check it out, both the online and slightly reduced standalone versions are free, might even like it

 

BTW do you mind if i include data from your library into my online calculator?

[Chris Rizzo]

BTW do you mind if i include data from your library into my online calculator

 

Go right ahead.

 

You've really got ALOT of functionality into your site there. Nice.

 

150% feed override anyway

 

Yes the headroom on those toolpaths seem near limitless at times. Frequently dictated by machine's dynamics and capability alone..

[Matthew Hajicek - Singularity]

Looks great Zero. I did notice that the downloaded version doesn't seem to be adjusting SFM and RPM with the HSM option the way the online version does. Is that what you meant by "slightly reduced"?

[zero_divide]

Nope. My goal is to make them give the same results.

Standalone is reduced in a way that it lacks the tool database. But it has safety limits on main things like HP, torque and such. That may be the reason results are slightly different. I will check it again and report back. Thanks for telling.

[zero_divide]

Followup. yeah i just checked it.

 

online version increases sfm as well as chipload when using hsm option.

 

but that feature was introduced AFTER v0.014 release and thus is yet not supported in standalone version.

 

it however is included into the next release being tested right now. Along with some other features none else has.

 

[Newbeeee™]

Yes the headroom on those toolpaths seem near limitless at times. Frequently dictated by machine's dynamics and capability alone..

This is the big thing IMO. If you have a Matsuura/Robodrill (probably Makino etc) the machine is more than likely configured for the high feeds.

If it's budget (read cheap like our Chevalier's), then it's not set up and will blow the machine's thrust bearings/ball screws in very little time becuase of the mechanical shock from direction changes at such high feeds.

But spend some time and get the machine sweet and you can have BIG rewards.

Or spend some cash and buy a Matsuura...