Improving cutting efficency

[John T.]

This topic came up at our weekly shop meeting. One is improving overall efficency (feed rates mostly) in cutting aluminum molds. We are using Fadal machines, tops about 10K rpm. Right now, we are using hi-helix carbides as our main rougher, and some guys aren't using them right (slow ipm, about 80-100ipm). I've been running about 120, and its been suggested trying 180-200ipm with cutter lengths up to 2.5", and experimenting with higher feeds with longer cutters. We used to use mini-cuts, but have since switched to 99% hi-helix. the speed/feed tables from the cutter manufacturers are too conservative.

 

Another material is syntac,which we use for plugs. This came up because of a deep mold and the plug it needed. Syntac is not friendly to HSS, and long carbide cutters (in this case, the cutter was a HSS 6", 5 degree ball end mill. A carbide would have been very expensive). It was brought up that trying inserted cutters might help, if they can replace the tapered bem's where we use them in 3D toolpaths. We'd also like to look at 0 degree endmills equally long for roughing.

 

Any thoughts, ideas, or experience out there?

 

John

[Rekd™]

You likely won't have accuracy running that fast on a Fadal. Have you tried MC's High Feed options??

 

'Rekd

 

[ 01-14-2004, 05:36 PM: Message edited by: Rekd ]

[chip]

I believe we are on the verge of maximum efficency, everyone always wants more........I just got a sample cutter that I used this morning. .500 1/2 in. high helix (deg.?). I was cutting a pocket 18.00 * 2.500 *1.500 dp. running 7000 (7500 max) at 105. ipm. when it was finished the pocket looked like S@#T! I still had to go in there and leave a decent finish so the part won't stick. I don't think you could give any more any faster!

 

Reality, a $1,000,000.00 Makino with 20,000 rpm spindle.........

 

Good luck! let me know if you do much better than you already are!

[Guest CNC Apps Guy 1]

Horsepower is going to be your main limitation in roughing. We've been using Duramill Roughers in our 20 HP Cinci's @ 180-220 IPM and 75-100% DOC for .500 Dia. and up. WOC averages around 40-75%

These are 100% load cuts but we've been doing it that way for a while.

 

HTH

[TheePres]

Chip,

Am I reading this correctly??

Are you cutting 1.500" deep at 105" IPM?

[chip]

Well.............

[chip]

My bad! One of these days I will figure out how to post a pic.

[crazy^millman]

Wel here coem the relaity of your problem. I hate to say this but you are at the best for the machien you are going to get. The Fadals will feed at those feedrates but they dont like it. I got 2 Haas SS machines and was able to improve to 400 ipm to 600 ipm on cutting alum on our parts. I can see a reduction of 60% to 80% on cycle times with havign these new machines. I have soem parts that we can finish no better than 40 ipm on the Fadals we can do 200 ipm on the HAAS machines. I am payign $2300 a month in Payments on these machine. I have incresed our output by $15,000 to $30,000 a month with the addition of these 2 machines. I also just added another machine and at this poitn ni the month have picked up $22,000 worth of work for that Machine which is a Thremwood Router. Yeah I know the Fadal faitfull will be on me for the converstion here oh well. We wonder why our work keeps going to China be more productive mean more money which mean cheaper prices which mean more work which means China can kiss my But.

 

Crazy Millman

[John T.]

just to be clear, the high feedrates I'm talking about are for roughing passes. we leave about .02 for semi-finish (leave .005) then finish.

When it comes to cavities, you wanna get rid of the unwanted material fast.

 

 

There is a group here at work looking into a hi speed machine, but I don't know whats going on with it.

[crazy^millman]

John there is a thing called the AFF advanced feed foward that might help you be able to feed at the 200 ipm and allow you to keep the machine in the tolerance you need. Here is the link to what I am talking about: Advance Feed Foward for Fadals PDF

 

Here is what you can do to put this in your post to post automatically. Yuo get this done ni the Misc Real and Mi7 to turn it on. This is written to support different tools for roughing and finishing and not using all the same tool. Here is the post code for a MPMASTER_FADAL post:

code:

---

fmt  R1+2   mr7         #Acceleration Value 

fmt P 2 mr8 #Decceleration Value

fmt Q 3 mr9 #Detail Value

.

.

ptlchg_com #Tool change common blocks

pcom_moveb

c_mmlt #Multiple tool subprogram call

#ptoolcomment

comment

if mi7 = 1,

[

pbld, n, "G94.2", *mr7, *mr8, *mr9, e

]

pcan

if plane < 0, plane = 0

if stagetool >= zero, pbld, n, *t, "M6", ptoolcomm, e

spaces=0

if output_z = yes,

[

preadbuf5

if (opcode > 0 & opcode < 16) | opcode = 19,

[

n, pspc, "(", "MAX | ", *max_depth, ")", e

n, pspc, "(", "MIN | ", *min_depth, ")", e

]

]

spaces=sav_spc

.

.

ptlchg #Tool change

pcuttype

toolchng = one

toolcount = toolcount + 1

if toolcountn <= tooltotal, nexttool = rbuf(4,toolcountn)

else, nexttool = first_tool

if wcstype = one, #Work coordinate system

[

pfbld, n, "G28", "X0.", "Y0.", e

pfbld, n, "G92", *xh, *yh, *zh, e

]

if mi7 = 1,

[

pbld, n, "G94.2", *mr7, *mr8, *mr9, e

]

 

pbld, n, *sm01, e

if mi10=one, n, *sm00, e

ptlchg_com

.

.

peof #End of file for non-zero tool

pretract

if mi7 = 1,

[

pbld, n, "G95.2", e

pbld, n, "G91", e

]

#pbld, n, "X0", "Y0", "Z0", "E0", "H0", e #(This line is not needed on Fadals)

#pbld, n, "G28", "X0.", "Y0.", protretinc, e

comment

#Remove pound character to output first tool with staged tools

#if stagetool = one, pbld, n, *first_tool, e

#n, *sg90, e #(This is not needed on Fadals)

n, "M02", e #(This was changed to M02)

mergesub

clearsub

mergeaux

clearaux

#"%", e #(This is not needed for Fadals)

"%", e

---

Here is what you change in the TXT file for the MPMASTER_FADAL:

code:

---

[post menu]

menu 1 {

"Post Processor: Fadal",

"&Change",

"&Run",

"",

"",

"",

"",

"",

"",

"",

""}

 

[canned text]

1. "Stop - M0"

2. "Op Stop - M1"

3. "Bld on"

4. "Bld off"

5. "Dwell - G4 P1"

6. ""

7. "AFF [0=Off,1=On]"

8. ""

9. ""

10. ""

 

[misc reals]

1. ""

2. ""

3. ""

4. ""

5. ""

6. ""

7. "Decceleration Amount"

8. "Acceleration Amount"

9. "Detail Vaule For Stock"

10. ""

---

I hope that helps.

 

Crazy Millman

 

[ 01-14-2004, 11:37 PM: Message edited by: Millman^Crazy ]

[Saultspics]

John T,

What depth are you cutting and how much material do you have to remove? We use a 1.25 inch aluminum cavity end mill for roughing from seco carboloy. It leaves a good finish on flat surfaces. It can plunge or helix in to parts. I am at home and I don't have the number of the cutter, but I think it will cut about 3/8" deep. It is similar to a face mill. We run it about 10,000 rpm. Up to 250-300 inches a minute. The biggest problem with roughing is horse power. The other mill we have can only rough at 5K rpm with a depth of cut of .15-.2 with a feed of about 100-150 inches a minute. Anything heavier will stall the machine. I will try to look up this cutter if you are interested. Let me know.

Hope this helps.

Stephen

[Hacsta]

quote:

---

I got 2 Haas SS machines and was able to improve to 400 ipm to 600 ipm on cutting alum on our parts.

---

what kind of cutter are using to go this fast ?

[crazy^millman]

Well I use carbide endmills and Inserted tooling the Tialn coatings really help when feedign this high of feed rates. We also do alot fo different Materials that allow this. We are doing soem Aluminum parts right now at 400 ipm at 12000 rpms and .15 doc no problem. I use 4 flute endmills when feeding this high.

 

Crazy Millman

[specv]

ssaults

the seco cutter is a great endmill, we run that same cutter at 14,000rpm 1.25 dia .390 doc at about 196 ipm it can remove a lot of material i a hurry, although i must say i just got done testing a .625 3fl em an i was hitting 441 ipm with it this week and its not even a high helix endmill.

Pete

[Saultspics]

specv,

what cutter was it?

 

John T,

We got the rep from seco to come out .He look at what we was doing then he suggested this cutter. He let us try it out for about a week.

[Hacsta]

crazy

whats is the max rpm on them Haas ss 's you have?

[specv]

its called a high-productivity routing cutter(copymill)

funny thing is that i cant find it in any of their books, i just have a small booklet on it

what is nice is that if you have the horsepower you can pull it through at about .01 per insert full width of cut and max rpm of 40,000 on the 1.25 dia em

[Hacsta]

wow

 

[ 01-16-2004, 05:51 PM: Message edited by: Hacsta ]

[crazy^millman]

12000 rpm 30 hp spindles on the HAAS SS machines we got. I wish they had a 50,000 rpm spindle with 30 hp I would get that.

 

Crazy Millman

 

[ 01-17-2004, 05:11 PM: Message edited by: Millman^Crazy ]

[Midwest]

Just wanted to share an article about HSM. Go to site and look at the Nov. 2003 magazine article and read the article called "Cutting Tool Selection Impacts the Outcome of Hard Metal Machining"