DYNAMIC MILL VS 2D POCKET

[stevieboy]

Hello

 

From what my program shows in my 2D Pocket program is at least 2x faster than my Dynamic mill program..

Material is 7075 T6

Pocket depth is 1.25

8 pockets to machine

2D Pocket parameters..

1" fem cobolt, fr. 45, ss.8500

stepover 65%, helix entry, cut depth .5

cycle time 15 mins. for all 8 pockets

 

Dynamic Mill

same tool, fr. 200 ss. 8000

stepover 8%, toolpath radius 36%,

helix entry, cut depth 1.25

cycle time for (2)of the 8 pockets 9 mins

 

any suggestions

 

thanks again

[jeff]

how big are the pockets?

[stevieboy]

4 pockets are about 9 1/2 x 3 5/8 and the other 4 are about 4 1/2 x 4 1/2

[BenK]

Are you using the depth cuts with the dynamic? With the dynamic path I would go full depth ans around 20-30% step over. Also make sure you are using chip thinning.

[stevieboy]

Full depth with Dynamic, I'll change my stepover to 25% and see what I get, Chip thinning I'm not sure, I'll check.. chip thinning?

[stevieboy]

My stepover change to 25% cut my cycle time to 3 1/2 mins.

Still checking into chip thinning

[Tony35]

check into a nice carbide endmill and let her eat

i use a varimill with TSC on @ ss10000(machine max) feed 469ipm with a .08 stepover 1.5 DOC cuts it like butter

[stevieboy]

Company won't spring for the carbide, we use 1" 3 flute cobalt, that seems to do ok, we mill a lot of T6, some with thin walls.

The 25% step over seems a bit much to me at 200 ipm, This is my first time doing Dynamic milling

and it's got to be right.

Still not sure about the chip thinning yet.

[jeff]

quote:

---

Company won't spring for the carbide, we use 1" 3 flute cobalt, that seems to do ok, we mill a lot of T6,

---

WOW, just... wow.

Sounds to me like your boss has the old school toolmaker mentality.

Does he know that the money spent on 1 carbide endmill alone will pay for itself most likely on the very first job? He wil spring for Mastercam, but won't buy carbide.

wtf?

[Goldorak]

quote:

---

Company won't spring for the carbide

---

there is your problem

 

for the thinning factor search for Iscar_Quick_Calculator.xls on the FTP

 

in 7075 i can easily go up to 33% step over on our CAT50 Okuma and still feed a 350 ipm

[stevieboy]

Well, let me rephrase, If I could show justification for the carbide they just might.

Show me the speeds and feeds for the carbide EM

so I can compare.

See what I first posted

[stevieboy]

we use cat 40

[Tony35]

check out this link for dynamic milling from emastercam users

once you go dynamic you never go back

 

Dynamic Feeds And Speeds

[Goldorak]

ok so

 

for a Niagara AR340 series that we use

 

RPM=4500 (moderate for the application you can boost it up to 6000 if the machine can handle it)

 

step over 25%

 

IPT .034 (.03 recommended by Niagara boost to .034 using chip thinning factor)

 

 

so in fact at 6000 rpm you can feed up to 612IPM if your machine can handle those feedrates

 

and i know that Hanita Varimill can easily go faster than this but i never run them here

 

so for a 9 x 4 pocket, Dynamic mill in mastercam gives me a 22 seconds running time par pockets

[BenK]

I just got done doing a test with 6061 and a .5 3 flute carbide endmill going 1" deep and stepping over .1 at 14000rpm and 370ipm in a 40 taper. The only thing I think I will change the next time I do that is move my step over to .15.

[stevieboy]

Tony

What about toolpath rauius, micro lift, and back feedrate. (Dynamic Mill)

Can you give some more details on them?

[Goldorak]

microlift , simply lift the tool by X amount to clear the back feedrate that i set at maximum machine feedrate

 

and force dynamic to keep the tool down, this generate a faster cycle time

[jeff]

quote:

---

If I could show justification for the carbide they just might.

---

Speeds and Feeds are SIGNIFICANTLY faster with carbide.

 

Just plain 2D milling, slotting, and everyday work with a 1/2" OSG Blizzard the recommended values are:

S7900 F199. IPM (I found that increasing the rpm's to 10k work much better.

Apply that tool to Dynamic milling or any HST and you can go way faster.

And the cost isn't that much, you can get them for approx $50,and they last quite a long time if used properly.

You're missing out on all of the fun of hogging aluminum and having chips fly! lol

[Tony35]

quote:

---

Tony

What about toolpath rauius, micro lift, and back feedrate. (Dynamic Mill)

Can you give some more details on them?

---

quote:

---

microlift , simply lift the tool by X amount to clear the back feedrate that i set at maximum machine feedrate

---

i set this the same as goldorak when i start i will use a .01 micro lift in a .01 distance and start with a 50% rad and tweak it from there i try to keep the machine at the highest possible feed so if you have a tighter rad its slows down have a bigger rad and it can keep the feed up and i set keep to tool down and clear for boundary only

[stevieboy]

Thank for all the help!

[stevieboy]

Thanks again,, This going to be fun!

[Tony35]

quote:

---

Thanks again,, This going to be fun! [big Grin]

---

nothing better then a shower of chips flying and the machine moving in a blur

enjoy

[Chris Rizzo]

Here's my little dynamic database we've all been contributing to and building.

 

dynamic database

[jhjr]

Wow I thought my employer was cheap but no carbide cutters that's f'n ridiculous. Do you machine anything besides alum? I couldn't imagine cutting steel or anything else at hss/co speeds all the time. I'd be like watchin paint dry. Lol.

When i ask for a $2k 12'' facemill then i'd have problems but not with an endmill! Good luck.

[stevieboy]

jhjr

 

I WAS referring to 1" 3 flute carbide, we still use carbide endmills! Our experience with the Brubaker truncated 3 flute 1 inch rougher has been all good, and they will resharpen them for us.

We do not do a lot of production jobs, and almost all the macine time is spent on finishing operations and not roughing operations.

90% Aluminum parts

 

thanks again for your comments.