Dynamic area mill on P550 material

[SONAVO]

Dear MasterCam User,

 

I want to do a dynamic area mill on P550 material and can't seem to find any samples in the dynamic mill Database.Plan on using a 5/8 5 flute high performance end mill.Any recomendations on step over and speed and feed?

[jeff]

I have no experience with that material.

 

Have a look at http://zero-divide.net/index.php?page=fswizard

I use it for all of my Dynamic paths.

[djstedman]

Haven't worked with that material either .. looked it up .. looks like its gonna be a bit nasty ..

 

Anyhow.. very generic info .. but generally about 10 to 15 % of diameter for stepover maybe a bit less if the material is really bad and depending on depth of cut..

 

I would guess around 225SFM as a starting point.. but since there isnt much to go on on that material I couldn't find anything other than chemical composition.. so thats just an educated guess..

 

Feed would probably be about .002 to .003 per tooth per rev..

 

I think this would be about where I would start but would expect to end up pushing the SFM up by up to 50% from the starting point and IPT might end up as high as .006..

 

Anyhow very hard to say without knowing depth of cut.. and without standing there hearing it cut.. this should serve as a decent guideline to start from though I think

[jeff]

If it's anything like P20,

then a general starting point would be:

S2568

F 74.24 IPM

going with a 5/8", 1-1/4 flute length 38 degree helix angle TiAlN coating

1" d.o.c.

stepover of .02"

 

http://zero-divide.net/index.php?page=fswizard&shell_id=199&load_tool_id=43010

[zero_divide]

Nope it is not like P20

 

P550 is a Very difficult to cut stainless steel

I actually never head of it before.

But it is very close to 17-7 PH stainless. So the SFM should be way below that of P20

I have just added it to the material list

Here is the calculation with correct material

http://zero-divide.n...d_tool_id=43495

 

for 5/8" 5 flute carbide TiAlN coated HPEM 1" doc and 0.020 stepover starting S/F are:

SFM :150

RPM: 900

IPT: 0.004

Feed:18 IPM

 

At this stepover SFM may be increased to 150-170% at a cost of shorter tool life

May i ask you to come back and tell us how it worked. Its an exotic material and not many people ever get to machine it

[mkd]

If it's anything like P20,

then a general starting point would be:

S2568

F 74.24 IPM

going with a 5/8", 1-1/4 flute length 38 degree helix angle TiAlN coating

1" d.o.c.

stepover of .02"

 

http://zero-divide.n...d_tool_id=43010

just from my recent experience i ran a batch of P20 just like the H/T 4340 (IIRC) listed in Rizzo's dynamic database:

5400rpm@140 ipm.

worked great with a SINGLE Guhring 1/2" endmill .06r for roughing!

 

pretty cool throwing chips against the inside of my cnc AND having one endmill last and last.

[zero_divide]

just from my recent experience i ran a batch of P20 just like the H/T 4340 (IIRC) listed in Rizzo's dynamic database:

5400rpm@140 ipm.

worked great with a SINGLE Guhring 1/2" endmill .06r for roughing!

 

pretty cool throwing chips against the inside of my cnc AND having one endmill last and last.

That is quite impressive

 

Was it a 5 flute? how deep per pass?

0.060 per pass is quite agressive.

 

140 IPM at 5400 RPM for even a 5 flute seems to be exceeding manufacturer-recommended chip thickness by 50%

[Scott Lundin Shopware Inc.]

Last week I tried out a calculator for high speed machining that worked very well for one of my training classes. We were working with 1018 steel. Do a google search for gwizard. It is made by CNC cookbook. It seems to have everything covered including how far the tool is sticking out. We started at the lowest of the four aggressive settings and got up to the third most aggressive. We stopped there only because we ran out of time.

 

For Stainless 17-4ph for a 5/8 dia - 5 flute high performance end mill, sticking out 1.75 from the holder, it came up with: .625 doc, .0438 stepover (7%), 3919 rpm and 88.5 ipm (lowest aggressive setting). 4136 rpm and 140 ipm (2nd aggressive setting). At a 10 % stepover it says the tool will deflect more than .001 and will cause chatter.

 

Has anyone else tried out this g-wizard calculator and did you like the results? It is free for a 30 day trial. I don't what it costs after that.

[mkd]

That is quite impressive

 

Was it a 5 flute? how deep per pass?

0.060 per pass is quite agressive.

 

140 IPM at 5400 RPM for even a 5 flute seems to be exceeding manufacturer-recommended chip thickness by 50%

the cutter was a Guhring #3079

var helix.

corner radius .062 (not radial engagement)

has about 1.5 flute length with four flutes, firex coated.

3.5 OAL

this cutter is a work of art!

 

i did not exceed 1" axial engagement.

radial engagement was .02-.03 IIRC.

 

attached is a pic of some of the parts i cut with this method/ single cutter. one part with the hourglass shape had a significant amount coming off judging by the raw stock next to it.

P20 is not a big deal to cut it. it's just a prehardened, chemically modified 4140.

thanks to Rizzo for compiling the spreadsheet.

[MotorCityMinion]

Helical Solutions and Volumill have a calculator available as well, with a established material database built in. There is even Material info on the selected materials. This thing is cool. Insane SFM's, or so it seems. Volumill appears to use a larger entry rad ( rounding radius), perhaps a bit smoother toolpath as well, opposed to what your used to seeing now. These numbers should still be in the ball park for MC. I Don't have access to either the tools or Volumill. Check it out at ....

 

http://www.millingadvisor.com/

 

They claim:

 

EX: Stainless PH at 300 HB.

 

5/8 dia., 5 flute at 1.25" ADOC and .044 (7%) RDOC

 

Conservative: SFM = 676, RPM = 4126, IPT = .0047, IPM = 97.63

 

Agressive: SFM = 826, RPM = 5043, IPT = 0058, IPM = 145.85

 

The numbers for P20 are just a little faster.

 

I can't see both of these companies combining R&D, sticking their necks out like this in tandem and generating a bunch of nonsense. It's definitely worth a look.

[zero_divide]

How does that look like?

http://www.zero-divi...d_tool_id=43757

 

For the same 5/8 dia., 5 flute at 1.25" DOC and .044 (7%)

on 17-4PH i get this at 150% chipload (you could call it manufacturer - recommended aggressive level)

 

SFM=794, IPT=0.00589, RPM=4853, FEED=142.93 DOC=1.25, WOC=0.04375 = 7% = 31deg

MRR: 7.8 in^3/min

HP: 9.4

Torque: 121.82 in-lb

Breaking Torque: 231.58 in-lb

Cutting Force: 389.84 lb

Tool Deflection: 0.0021 in

Max Tool Deflection: 0.0025 in

 

Looks close to their tool deflection is a little too close to breaking point than i personally would like, but hey. i am not saying their tool will fail....just might

[jeff]

Last week I tried out a calculator for high speed machining that worked very well for one of my training classes. We were working with 1018 steel. Do a google search for gwizard. It is made by CNC cookbook. It seems to have everything covered including how far the tool is sticking out. We started at the lowest of the four aggressive settings and got up to the third most aggressive. We stopped there only because we ran out of time.

 

For Stainless 17-4ph for a 5/8 dia - 5 flute high performance end mill, sticking out 1.75 from the holder, it came up with: .625 doc, .0438 stepover (7%), 3919 rpm and 88.5 ipm (lowest aggressive setting). 4136 rpm and 140 ipm (2nd aggressive setting). At a 10 % stepover it says the tool will deflect more than .001 and will cause chatter.

 

Has anyone else tried out this g-wizard calculator and did you like the results? It is free for a 30 day trial. I don't what it costs after that.

 

it's $70/year.

Yeah sorry, I'm not buying any software for my speeds and feeds

[SONAVO]

I would like to say thanks a lot for your input. I do appreciate it.

 

Best Regards.

 

SVo