Dynamic mill parameters?

[dforsythe]

I’m about to use the dynamic mill for the first time. Anyone have a formula for step over / chip load ect that has been working well for them?

 

info

haas vf-6 hp? rpm 10k

40 taper

3 fl .500 em 1.0 loc ext 1.1 solid holder

mat 6061

 

milling 8 x pockets .800 deep about 6 " x 3" triangle shape.

 

 

Thanks

 

[ 10-28-2009, 01:44 PM: Message edited by: dforsythe ]

[Tony35]

need a bit more info

 

material your cutting?

tool size?

depth of cut?

rigid setup?

40 or 50 taper?

machine?

machine HP?

 

you get the point

[Goldorak]

search "Iscar_Quick_Calculator.xls" on the FTP

 

it'a a excel sheet to calculate thinning factor and others useful formula for HST

[Leigh @ Kodiak]

On our VF6, I would program .800" DOC, .120" WOC, 6050 RPM and 80 IPM

[cunder]

I cannot seem to find the Iscar calculator. Can You be more specific for the location?

[Tony35]

dforsythe

 

i would start at 10000 rpm @300 ipm with a stepover of .03-.06 the full .800 deep and tweak it from there check to see what the max feedrate of the haas is you should be able to rough those fast

 

i run my 3/4 4 flute varimills in alum at 10000 rpm at 465 ipm 1.4 deep with a stepover of .06 nothing but a shower of chips

 

cunder/dforsythe

i have the iscar calc if you want me to email it to ya guys let me know

 

HTH

[cunder]

Please do.

 

[email protected]

 

Thanks Tony

[Leigh @ Kodiak]

Our VF6 only has a 7.5k spindle

[Tony35]

cunder

 

you got mail

[dforsythe]

Thanks for all the info.

tony35 i found it on the ftp.

 

thanks again.

[X-L Engineering Corp]

Tony35,

I was looking for the "iscar calc" to would you mind sending me a copy?

 

thanks

[Tony35]

sure ted

use your profile email?

[dforsythe]

Tony35,

 

what is the internal and external dia? is that the smallest rad you would be traveling around?

[cunder]

The Iscar calculator is not to bad but the ones at http://dapra.com/tech/calculators.htm are the ones I have used in the past.

[Tony35]

quote:

---

what is the internal and external dia? is that the smallest rad you would be traveling around?

---

thats for circle interpolation if i understand you right

[Tony35]

ted you have mail

sent it to the profile email

[Bob W.]

With a Haas VM3 (12k spindle) I have been able to run 3/8" 3 flute end mills at 350 IPM with 12k rpm, .75 LOC, and 25% stepover in an ER collet. Make sure to post a G187 P1 (roughing accuracy) before these toolpaths. The machine will literally run twice as fast. To reset the accuracy simply post another G187 before the next operation.

 

The G187 temporarily overrides setting 191.

[dforsythe]

Thanks for the heads on on the g187.

[Leigh @ Kodiak]

Be careful with G187 set to roughing (P1), It is possible that corners of you part might get clipped off.

[Chris Rizzo]

Try the " helix followed by trochodial medial" in corners feature (on entry motion page). You will have to really adjust it and experiment to get it dialed. It keeps the cutter from getting pinched in those triangular type shapes, and reduces the need to program for worst case corner loading.

 

m2c

 

[ 10-29-2009, 07:08 PM: Message edited by: Chris Rizzo (Italian' stylin') ]

[Bob W.]

quote:

---

Be careful with G187 set to roughing (P1), It is possible that corners of you part might get clipped off.

---

This is true. I did some testing with various settings with dynamic milling in a pocket and it really was very accurate. I machined a pocket to size using a dynamic milling toolpath followed up by a contour toolpath to finish the walls. I then ran the exact same dynamic milling toolpath leaving .005" on the walls while playing with different G187 Px Exxxx values and at 400 IPM with G187 P1 E.2 I was not getting any contact. I was very suprised and it might have something to do with the high speed machining option being turned on in my machine. Do make sure to leave enough material on the walls to you don't overshoot beyond the finishing pass.

 

I think it would be time well spent to see how far you can push it before overshooting becomes a problem.

[ELS44]

One more thing to consider when changing setting #191 to rough is that this multiplies the value in setting #85 max corner rounding by four.

G187 Pm Ennnn sets both the smoothness and max corner rounding value. G187 Pm sets the smoothness

but leaves max corner rounding value at its current value. G187 Ennnn sets the max corner rounding but

leaves smoothness at its current value. G187 by itself cancels the E value and sets smoothness to the default

smoothness specified by Setting 191. G187 will be cancelled whenever “Reset” is pressed, M30 or M02 is

executed, the end of program is reached, or E-stop is pressed.