Milling D2 Tool Steel Annealed

[Chance22]

Looking for some insight on feeds and speeds on milling D2 tool steel.  I am using a 3/4"  4 flute carbide flat end mill, dynamic mill taking a depth of .300 and about .025 per pass at 3000 rpm and 40ipm and tools are not lasting.  

[#Rekd™]

What make is the tool? Most companies have suggested speeds and feeds charts. How are you holding it? Cat 40 or 50? How far is it sticking out of the holder?

I would say your speed seems high, about 1400 RPM.

If you use Helical Solutions end mills they have a great advisor for speeds and feeds.

https://www.harveyperformance.com/machining-advisor-pro/

 

[crazy^millman]

On 6/19/2020 at 11:25 AM, Chance22 said:

Looking for some insight on feeds and speeds on milling D2 tool steel.  I am using a 3/4"  4 flute carbide flat end mill, dynamic mill taking a depth of .300 and about .025 per pass at 3000 rpm and 40ipm and tools are not lasting.  

Slow it down way to fast for that material. Need to increase the depth of cut to .75 at least. Here is what what HSMAdvisor came up with from the Helical Website's speeds and feeds for this tool. Here is a good link from their website about how to know what a tool is doing. 8 Ways you're killing your endmill

 

 

[Guest]

11 minutes ago, crazy^millman said:

Slow it down way to fast for that material. Need to increase the depth of cut to .75 at least. Here is what what HSMAdvisor came up with from the Helical Website's speeds and feeds for this tool. Here is a good link from their website about how to know what a tool is doing. 8 Ways you're killing your endmill

Nailed it,

 

1 hour ago, Chance22 said:

am using a 3/4"  4 flute carbide flat end mill, dynamic mill taking a depth of .300 and about .025 per pass at 3000 rpm and 40ipm and tools are not lasting.  

what toolpath are you using? I hope you are not plunging into the Material, you should be using ramp entry and 2d dynamic mill for pockets, or area mill with profile ramp at least..

[JParis]

Just now, byte me said:

you should be using ramp entry and 2d dynamic mill for pockets, or area mill with profile ramp at least..

Even a ramp entry on that stuff can be brutal on the tool...

Harder materials are the one place I'll still use a start hole is necessary

[Guest]

8 minutes ago, JParis said:

Harder materials are the one place I'll still use a start hole is necessary

^ Yeah that's not a bad idea, I find if i do my ramp with .002 doc or something really light with a well calculated feed and speed, it's not too bad on the tool..

A nice bullnose rougher should be able to do it, but actually i'd lean toward the drill hole idea providing its not a small deep hole where the chips clog and burn the tool.

[JParis]

4 minutes ago, byte me said:

I find if i do my ramp with .002 doc or something really light with a well calculated feed and speed, it's not too bad on the tool..

Just gotta be careful that with that light a cut you don't work harden the material... 

[Guest]

1 minute ago, JParis said:

Just gotta be careful that with that light a cut you don't work harden the material... 

Very true, that is where feeds speeds and correct tooling come into play, work hardening could equally occur while drilling o course :p.

I like to do a couple of test cuts and ensure no heat is being generated.

[pro grammer]

Get this:

https://www.imcousa.com/parts/65085

Adoc .3

Rdoc 5%

SFPM 390

IPT .0065

 

Just make sure some genius did not flame cut your stock.

 

[crazy^millman]

15 minutes ago, pro grammer said:

Get this:

https://www.imcousa.com/parts/65085

Adoc .3

Rdoc 5%

SFPM 390

IPT .0065

 

Just make sure some genius did not flame cut your stock.

 

not trying to nit pick, but he is using a 3/4 tool any reason why you called out a 3/8?

[pro grammer]

On 6/19/2020 at 4:04 PM, crazy^millman said:

not trying to nit pick, but he is using a 3/4 tool any reason why you called out a 3/8?

Yup. He says he is milling .3doc. He does not say if he is actually going deeper than .3. Many people think using a bigger endmill miraculously gives them better performance. It does not. It just costs a lot more. If I was only going .3 deep I would choose 1/4 - 3/8 endmill. 1/4 would actually do just fine. I assume he is only cutting .3 deep because nobody in there right mind would only use .3" of flute on a .75 endmill. Dynamilling with a .75dia endmill should be upto 3xD in D2 material with these tools.

[crazy^millman]

1 hour ago, pro grammer said:

Yup. He says he is milling .3doc. He does not say if he is actually going deeper than .3. Many people think using a bigger endmill miraculously gives them better performance. It does not. It just costs a lot more. If I was only going .3 deep I would choose 1/4 - 3/8 endmill. 1/4 would actually do just fine. I assume he is only cutting .3 deep because nobody in there right mind would only use .3" of flute on a .75 endmill. Dynamilling with a .75dia endmill should be upto 3xD in D2 material with these tools.

Good point I didn't think about yes he was only going .300 deep for a reason.

[pro grammer]

1 hour ago, pro grammer said:

Yup. He says he is milling .3doc. He does not say if he is actually going deeper than .3. Many people think using a bigger endmill miraculously gives them better performance. It does not. It just costs a lot more. If I was only going .3 deep I would choose 1/4 - 3/8 endmill. 1/4 would actually do just fine. I assume he is only cutting .3 deep because nobody in there right mind would only use .3" of flute on a .75 endmill. Dynamilling with a .75dia endmill should be upto 3xD in D2 material with these tools.

There should be their.

[crazy^millman]

9 minutes ago, pro grammer said:

There should be their.

I know we have some grammar police on this forum, but I am not one of them.

[pro grammer]

23 minutes ago, crazy^millman said:

I know we have some grammar police on this forum, but I am not one of them.

Yeah, the problem is I am a grammar cop.

[Goldorak]

Why just .3 deep? 

i'd go full dept, 12% stepover .05 step up 

first of all, try to get a variable pitch endmill, they are way much stable, and perform better than a regular 4 flutes, yes they cost more but the payback will be in time and problems savings

 

you can start

around 1500-2000 RPM 

AS much coolant as possible 

feed + or - 80ipm 

All theese are for a good rigid machine and setup 

[nickbe10]

I have machined a fair number of swaging dies in this and S7.

250 sfm. - 600 sfm (high feed)

I will program for a typical chip load for the cutter diameter and use Mastercam's  RCTF. 

1.5 dia depth is usual but 2 dia isn't usually a problem with a little less energy (hence the 250 sfm which is on the low), but tool life is excellent.

We use Imco and Helical

It's important to calculate effective surface footage and chip load if you do any surfacing or you will rub your cutter to death quickly.