First Dynamic Milling attempt

[Justin Beebe at Folsom Tool]

I'm going to machine a pocket and I want to rough it with dynamic mill. Here are the details:

 

Machine: 50 taper Mitsui horizontal

Max RPM: 12,000

Material: 7050 aluminum

Pocket depth: 1.500

Endmill: .500 three flute Viper

 

Question 1:

 

Can I pre drill instead of using helix entry?

 

Question 2:

 

Can I take the entire 1.500 depth in one cut or do I need depth cuts?

 

Question 3:

 

What feed and speed are recommended for this path?

 

Question 4:

 

What should be my settings be for step over, toolpath radius, micro lift distance, and back feedrate?

 

Thanks for the help. I have been putting off using this path and really want to try it out.

[Dave.L]

Justin,

 

I have limited experience with dynamic mill, however, in regard to Q #2, I would not go more than 1 x D. IMO, you should be able to feed a lot faster than 3 x D and it should be fast enough to make up for the 3 extra depth passes.

 

Q #4, I don't think the speed has much to do with the path. I would look up the SFM from your tool manufacture but I would guess it's going to be your max RPM, 12K

 

JM2C

[Justin Beebe at Folsom Tool]

Dave,

 

Thanks for the info. I was hoping I could do it in one depth of cut. I thought the purpose of Dynamic Mill was to take light radial cuts and use the entire flute of the endmill to remove the material. Although 1.500 may be extreme with a .500 endmill. I have to check but I'm pretty sure there is no max RPM for a Viper in aluminum. I'm hoping someone who has been using this path successfully will share some of their settings so I don't have to figure it all out through trial and error.

[Jayson Kramer]

do you have that much flut.if so you can do it.and Like dave said SFM and you can go to a at least .oo5 chip load.

[Dave.L]

Justin, I mean the SFM will be high and therefore probably over the RPM you have, so thats why I say you will probably run this tool at 12k, your max RPM not the tools. Since you have 50 taper, if the geo of the pocket permits, maybe use a bigger tool

[Leigh @ Kodiak]

Definitely utilize the entire flute length. In aluminum, I would try 9500 RPM, .05" WOC and 175 IPM. For Radius, I usally use 30% of cutter dia. .02" lift, and set back feedrate to the max Feed for that machine.

 

Depending on how the look ahead works on your machine, you may want to leave a little more stock for finishing, as the cutter may overshoot at the high feed rates.

[Justin Beebe at Folsom Tool]

I have the flute length so I will try full depth. 9500 RPM at .005 per tooth would be 142 IPM. That sounds fast for that depth of cut. I guess I'm just not used to this type of toolpath. I am going start off a little slower and work my way up. I will run this path in a few days and let you guys know the result.

 

Thanks for all th good advice.

[Rstewart]

I ran a test dynamic mill path in our 7yr old haas VF2.

 

3 FL .5" carb E.M.

1" D.o.c.

22% woc

150 ipm.

7500 RPM (max)

6061 Aluminum

Worked Great!!

[Colin Gilchrist]

Nope, you MUST run a higher feedrate to take advantage of the chip thinning effect.

 

What kind of tool holder? I was going to recommend more like 11,000 RPM and 200 IPM.

 

At .05 stepover on that tool, a .006 Chip load per tooth (.018 per revolution) would equate to more like a .003 thick chip. Even though the standard "Chip Thickness" equation tells you that at 198 IPM @ 11K RPM you would have a .006 chip thickness, this is not correct, due to the chip thinning effect.

 

Your actual chip thickness @ 10% stepover is .003 (half of what you thought it should be).

 

Look at the 2nd to last post on this thread. Great link to an excel spread sheet for chip thickness

[Colin Gilchrist]

You *could* just put a chained point into the toolpath and avoid doing an actual helical entry, but I would caution against this.

 

There really is no reason unless you have the world's fastest toolchanger.

 

There are a ton of different entry options under the entry parameters, not just helical entry. You also have full control over the feed/speed of the entry move, and the option to add a dwell at the bottom while the tool ramps up to the new RPM...

[Justin Beebe at Folsom Tool]

Colin,

 

I was going to hold this tool in a milling chuck or solid holder with a set screw. I will look at the spread sheet tommorrow at work where I have excel.

[Dave.L]

Justin, use the milling chuck.

[Justin Beebe at Folsom Tool]

One other thing worth mentioning is that this part will be mounted on a bridge fixtue with some 1/2-13 screws holding it from the bottom. The stock size is 2.00 X 2.625 X 6.500. The 6.500 will be along the Y-axis. I can post a pic when I get it all drawn up in mastercam. It should be pretty rigid because the fixture is made out of steel.

[Justin Beebe at Folsom Tool]

Dave,

 

Good advice about the milling chuck.

[Leigh @ Kodiak]

As Colin pointed out, the values I suggested were already on the conservative side of things. We only have "general purpose" carbide endmills, so I'm sure your tool will handle those values with no issues.

[Joe788]

Justin, we do 99.99% aluminum, and I've been using dynamic mill on virtually every new job since it was released.

 

You can definitely do the whole depth in one cut if you really want to. Bear in mind, if the bottom of the pocket needs a reasonably flat and/or smooth finish, you'll need another pocket path to smooth it out afterwards. Tools deflect quite a bit at that length of engagement.

 

Depending on how fast/smooth your machine is, here's where I'd start:

 

12,000rpm

240ipm

.750 DOC

.200 stepover

500ipm back feed

no microlift

no retracts

 

Make sure you set the arc filter at 2:1 so that the program size stays reasonable.

 

If you go full depth, you might want to back off the feed a little bit. If you helical entry all the way down 1.5 inches with a .500 tool, you WILL be recutting major chips by the time you get to the bottom, and it will sound like hell and beat up your tool.

 

You don't need to take a super skinny radial cut in aluminum, because you're not worried about heat. .200 works beautifully, and sounds like butter. You'll be amazed the first time you run it.

[Colin Gilchrist]

I don't ever use the actual helix option. I prefer the medial ramp or using a custom chain (ramps the chain). That way you can dial in the speeds and feeds for the light load on the cutter. Some of the cutting forces are also directed up into the spindle in Z, which help to stabilize the cutter in the cut.

[Goldorak]

Question 1:

 

"Can I pre drill instead of using helix entry?"

 

Yes set the entry ramp angle at 90deg ans entry radius at 0.0

check align with entry point and select that point

(this point should be select AFTER the toolpath creation , it looks like a bug for me )

 

Question 2:

 

Can I take the entire 1.500 depth in one cut or do I need depth cuts?

 

i will try 12.5% step over a full depth ans set toolpath radius at 25% to get a smooth toolpath

 

Question 3:

 

What feed and speed are recommended for this path?

 

maximum RPM for sure

 

and using thinning factor your IPT will be near .012 to .015 feed per tooth

 

Question 4:

 

What should be my settings be for step over, toolpath radius, micro lift distance, and back feedrate?

 

a .01 microlift and machine maximum allowable back feedrate will save your tool and considerably cut the machining time but the NC code will be a lot larger

[Justin Beebe at Folsom Tool]

Update:

 

I ran the dynamic mill toolpath today and I must say I was very impressed. I am only milling a small pocket but I roughed it out in under a minute. I started off a little conservative at 8000 RPM and 150 IPM. Tommorrow I am really going to crank it up. I don't know why I didn't start using this toopath sooner. Thanks everyone for your help.

[Leigh @ Kodiak]

quote:

---

I don't know why I didn't start using this toopath sooner.

---

Welcome to the light, my son.