True high speed machining

[brandon b]

Im trying to transition to using the high speed roughing paths the way your supposed to.( 10% stepover and 100% step down).

 

Attached below is a rough sketch of a part im trying to work on.

 

The first toolpath is how ive been doing it. 3/4 rougher .3 stepover .5 stepdown 6 ipm 400 rpm. I can get thru about a part and a half on one cutter.

 

Im using the pct http://www.pctcutters.com/pct_product_M42_4F_CC_Ground_details.aspx?PartNo=T4-CC54212S

 

and the Niagara edp# 68948 http://www.niagaracutter.com/newproducts/vfp.pdf

 

 

 

My question is how do I figure my speeds and feeds for this high speed toolpath??Ive been messing with the iscar tool library slide bar..( 2nd toolpath)

do those values sound right??

 

Material is TI 6 4.

 

running on a fadal VMC 6030 3axis 40 taper 10,000 rpm max.

 

I would like to keep the feed rate below 150.

 

 

 

 

 

 

 

 

TTT.MCX-7

[mkd]

i know about those cutters, but not much experience in 6al 4v.

more experience with corncobb roughers. They work very very well when geometry allows deep and wide cuts.

 

I can get thru about a part and a half on one cutter.

if you're not getting 1 hr of tool life you are doing something wrong/ too fast.

 

a good starting point for HS cutting would be carbide at or under 200 sfm. I've used .040 step over and 80ipm with a fancy 20mm 10 fluter.

 

Rizzo's database has a couple examples

[Chris Rizzo]

Check my database in signature below. .3 Stepover is way more that 10% of a .750 tool. I'd say that is your problem. Tool much heat in cutter. Also I'd increase our min toolpath radius to something like 20% or more. Stepover even less than 10 may be necessary.

 

 

EDIT: I see your second toolpath in that file with the adjusted stepover. That looks better. Still watch the min-radius.

[mkd]

also with the HSS cutters; a chamfer on the tips is critical for tool life.

 

.300 isnt super aggressive, but i might try a little less step over or much more with HSS.

 

I've found running well over center line (70% stepover) adds stability to the cutter, because the semi circle shape. This seemed to work well with 1.25Ø 5 flute corncobbs 6in long probably buried 1 diameter deep channel cutting and old skool pocketing.

[brandon b]

i know about those cutters, but not much experience in 6al 4v.

more experience with corncobb roughers. They work very very well when geometry allows deep and wide cuts.

 

if you're not getting 1 hr of tool life you are doing something wrong/ too fast.

 

a good starting point for HS cutting would be carbide at or under 200 sfm. I've used .040 step over and 80ipm with a fancy 20mm 10 fluter.

 

Rizzo's database has a couple examples

A part and half was like 7 or 8 hours.. tools lasted very well . im just trying to speed up my cycle times by programming the high speed way...

[brandon b]

also with the HSS cutters; a chamfer on the tips is critical for tool life.

 

.300 isnt super aggressive, but i might try a little less step over or much more with HSS.

 

I've found running well over center line (70% stepover) adds stability to the cutter, because the semi circle shape. This seemed to work well with 1.25Ø 5 flute corncobbs 6in long probably buried 1 diameter deep channel cutting and old skool pocketing.

I have .125 corner radius on my roughers.

 

I stared out at .375 step over and I think I had the stepdown a little deeper, but I was breaking tools, so I backed off to .3 stepover .5 deep.

[K2csq7]

I have .125 corner radius on my roughers.

 

^^^That is good.

I actually just finished a volumill seminar this morning. We were cutting 6-4 Ti with some Sandvik Plura (sp?) endmills. See attached screenshot for the specs we ran. It was on a Mazak VCS430 (small vertical).

Volumill slowed the feedrate down in the corners to like 25IPM or so....

MAKE SURE YOU ARE USING GOOD HOLDERS!!!!!

Run-out on the endmill will kill you.

[brandon b]

 

MAKE SURE YOU ARE USING GOOD HOLDERS!!!!!

Run-out on the endmill will kill you.

ya I need to get the old man to buy me some new holders. lol

[brandon b]

http://www.millingadvisor.com/

 

check this calculator out. its a volumill HSM calculator but I assume it would be the same tooling data for mastercams HSM?????

[MotorCityMinion]

Keep in mind that the Volumill defaults average are 7% step over and 45% rounding radius. Their speeds and feeds seem aggressive, but the tool path is also safer. Start with their conservative suggestions and program with those values in mind, things should go smooth.

[brandon b]

here are the values that I get for my part.

[Brewster]

I am currently running 6AL-4V parts. i have an .125 dia em with .02 corner rad (Helical endmills ) running 56 ipm .100 depth of cut. I am getting several hours of run time per endmill.

[brandon b]

Here's another question. Cost wise, is it worth buying .75 cutters ? Looks like a lot of people are running the smaller cutters. A lot of .375 and.5

[K2csq7]

Here's another question. Cost wise, is it worth buying .75 cutters ? Looks like a lot of people are running the smaller cutters. A lot of .375 and.5

I usually base that on the depth I need to go, in Ti I would step up to a 5/8 from a 1/2 if my DOC was more than .75 (1.5xD), also taking part shape into account. If I had a lot of tight corners, I may stick with the .5 EM and get deeper into the corners.

[MWR15]

You can decrease some of your cycle time by changing the back feedreate from 100 to 500. I use .05 for my micro lift.

[Matthew Hajicek - Singularity]

Another calculator:

 

http://hsmadvisor.com/

 

I've been using it in H13 and copper with good results.

[brandon b]

Ok makes sense... I'll use the .75 on this part since its just flat with a boss in the middle . Prolly go full flute length depth and .2 stepup. And start at 7% step over.

[brandon b]

the results are way different between the hsm advisor and the milling advisor...

[mkd]

costwise a prefer 1/2" endmills. it's just a sweet spot in the price/ size ratio. And good for light machines like Haas and Fadal.

 

you might run some numbers: if you can get a 1/2 5 fluter against your 5 flute 3/4, the smaller might win due to more rpm and thus more feed. run the numbers on your part and compare cycle times in MC. then compare cost on the same brand of different sizes.

 

you seem to a very good handle on what you're doing.

[brandon b]

I've only been in the machining field for 3 years. Trying to learn as much as I can while I'm young.

[Matthew Hajicek - Singularity]

the results are way different between the hsm advisor and the milling advisor...

 

In HSM Adviser did you turn on Chip Thinning and HSM? If not it calculates traditionally, though it still limits for flex. What results did they give?

[brandon b]

Ya I hit all those buttons. I'll post a screen shot when I get back from lunch

[brandon b]

left is hsm advisor right is volumills

[MotorCityMinion]

Like I said previously, the Volumill path uses a weeny step over at 7%, a large rounding radius and is obviously biased by the Helical Solutions allegiance. The range between conservative and aggressive estimates is broad. The high end of the Volumill calcs make me nervous. To be fair, I've also snapped tools using FSWizards calcs. Lately, I've been plugging data into both of them and trying to find some middle ground. One thing that does miff me is that the SFM in both of the calcs seems HIGH, but they work.

[zero_divide]

Brandon,in HSMAdvisor you need to choose a HP (Hi-Performance) Entmill tool type.

Othewise it thinks you are using a generic endmill.

Also should specify coating as well.

 

@MotorCityMinion,

FSWizard does not have any of the safety checks that HSMAdvisor has, so however not likely it is possible.

 

Here is milling advisor vs HSMAdvisor side by side.

The specs pretty much match.