Tool Life, Step Down and Material

[Lee.]

Hello All,

 

As some of you know i'm not new to this forum and woodworking via cnc however Milling via CNC is a relatively new venture for me.

 

I just ran a job in what I belive to be 4140 material which is fairly common around here.

 

I am using solid carbide 4 fl End Mills, in 3/8" and 1/2" diameters.

 

after running the job I have severe corner rounding on both cutters and wondering what I am doing wrong.

 

3/8" EM, 20 IPM 2000 RPM Depth Cut 0.045"

 

1/2" EM, 13 IPM 1520 RPM Depth Cut 0.055"

 

Coolant for both FLOOD.

 

Any help would be greatly appreciated

 

TIA, Lee

[Dan Skierkiewicz Furnel]

Here are some guildlines to go by.

 

1 Use a coated cutter. TiAlN is good to start with.

 

2 Side mill as much as possible.

 

3 Buy cutters with a radius or chamfer on the corner. Once the corner goes its all downhill from there. Its very common to find this on any new line of tool.

 

4 Dont ramp or helical mill with a sharp corner endmill if you do make shure you ramp at 1 degree or less. By doing so you prevent the center of the tool from cutting.

 

5 Call your local tool supplier and ask about the latest line of tooling. Then contact there support deptment on speeds and feeds. Dont guess at sfm because you can kill the life of the tool. You can find the best spm by experimenting if you have time. Coated tools generally have a higher sfm than the speeds you are using. Taking too little a chip load is just as bad as taking too much or removing it too fast or slow.

 

6 Understand that face milling with and endmill (ie taking the whole diameter or sloting) requires a different speed and feed than side milling. Read seco's article on radial engagement.

 

Hope this helps. I would like to here other feedback as well.

[Lee.]

Hi Dan,

 

Thx for your reply.

 

The cutters are coated with TiAln

 

The corners were sharp.

 

I was using a ramp of 3.0 degrees. ( it was the default setting )

 

The 3/8" cutter is cutting a through slot of 0.436 wide and radial about 95 degrees. material is about 3/8" thick.

 

The 1/2" cutter is cutting a through slot of 3/4 by 1 1/4 and material is about 5/16 thick.

 

Lee

[Dan Skierkiewicz Furnel]

I would say spend the time and drill a start hole first. That way you aviod ramping all together. I think ramping at 3 degrees will definitely reduce cutter life. Usually the angle ground on the bottom of and end mill is 2 deg. You could also try using a .25 em in the small slot and a .375 em on the large slot and tricordial side milling the pockets out and you will never touch the bottom of the cutters.

[Lee.]

Hi Dan,

 

I played around with trochoidial cuts and oh boy does it ever bring my time down.

 

I used an entry point and a 1/4" cutter, seems to work well on the computer.

 

So, will cutting full depth on 3/8 thick not bother the cutter as much as pocketing it out with depth cuts?

 

I guess the corner is the weak link on the cutter?

 

Lee

[Dan Skierkiewicz Furnel]

Lee,

 

Be carefull with tricordial cuts. Make shure to only take a small radial engagement like 2 to 3 percent at first to see how it cuts. Radial engagement is based on the percentage of the tool diameter. A .0025 step over on a .25 end mill would be 1 percent .025 stepover would be 10 percent and so on. You are going to have to play with the speeds and feed alot till you zero in on the right one unless you already have parameters on that tool. Cutting this way should take tons of time off of the job. Depth cuts still can be used if you want.

 

Yes the sharp corner on a tool is the weekest link. You always want to avoid full radial engagement if posible. That is why a cutter squeaks in a corner because of 50 percent radial engagement. Always generate your corners! Look into bull nose endmill and you will never go back I promise. If you need a sharp corner in a pocket you can always chase it will a sharp cutter. Check out iscar chatter free line or seco's solid square end mills you will be glad you did. And no I dont work for any cutter company I am a mold maker and do alot of high speed milling.

[NOTW Programmer]

Are you full slot cutting, if you are the feedrate is too much; if you are side milling there is no reason to go that shallow you can do 1xD and be OK. The SFM is also a bit low, I would bring that up to 300 to 350 and get and RPM of 3000 and a Feed of 20IPM with a .1 WOC and .375DOC. +1 on Dan, if you are helical entry buy chamfered or radius corner EMs; I prefer chamfered. I would check with the manufaturer on the rake angle before making the tool plunge too steep, I have a guhring and that can do 5deg. at 2800RPM and 24IPM a VariMill of course.

[Lee.]

Thanks Guys,

 

I am a total newbie to milling steel via cnc.

 

Grey, Not sure how to get a 0.1 WOC as it is a closed pocket??

 

Pocket is radial at 0.432 wide and full radius at the ends.

 

I understand I need depth of cut increase this will help on time and tool life. so thx for that.

 

Just not sure what the best toolpath is yet.????

 

Lee.

[Lee.]

Dan,

 

I played with Trich toolpath in mastercam but couldn't get it to work unless I went down to 5/16 cutter and even then the other settings had to be reduced to get it to work properly.

 

Thoughts?

 

Lee.

[Chris Rizzo]

.045 doc!? Use the dynamic milling toolpaths and go right to finish depth in one pass. No depth cuts. Also you prob will use a smaller cutter. I'd go 1/4 for the .400 slot.

 

If you want some baseline paramters see the info in my link below. Some good numbers on 4140/4340.

 

If you want send me the file and I can dial in some of the parameters, it can be a bit tricky.

[Lee.]

This probably sounds lame, however where do I find Dynamic Toolpaths?

 

Lee.

[Chris Rizzo]

No worries. All the fun toolpaths are found under 2d High Speed. There are several in there, stick to the "dynamic" ones. They are absolute, total, 100% game-changers for machining, but do take some getting used to. Give You tube a search for dynamic milling and you can see some in action. Here at streamingteacher I've built a lot of videos on the ins and outs and how to use them. The price will pay for it in the first job you run with them!

 

If you like I can help you though your part.