Dynamic milling questions

[MACHINING JIM]

So this is my first attempt at using the dynamic milling toolpaths. I am having trouble getting things to work. I have a plate with 6 seperate pockets in it. The problem is after chaining all the pockets and regening the op. I only get a toolpath for the first pocket. If I use just a regular pocket toolpath it backplots toolpaths for all the pockets as per usual. When using the dynamic milling strategies do I need to create an operation for each pocket or is there a way to link all the geo to one operation? Oh and I am using the dynamic area mill toolpath.

 

I could also use some advice on some settings for milling these pockets. I am using a .500 4 flute kennametal Harvi endmill in 6061 aluminum. I was thinking about a .500-1. inch doc. If I have the horspower. What would be the best stepover amount, would microlift be a good option and if so what would a safe starting point be for approching this job?

 

I am also curious about the first pass in a pocket when dynamic milling. The cutter will be cutting at a 100 percent stepover and a huge depth of cut. This is a foreign concept to the way I have always machined. I am guessing that the trocoidial cutting is how this is overcome?

 

Any advice or explinations would be super since I am pretty new to the dynamic milling thing.

 

Thanks

Jim

[Redfire427]

In X5, you have to create separate toolpaths for each pocket. In X6, you can do everything in one toolpath. Upgrade time..........

 

If you use a helical entry into the pocket, you now have some space between the tool and the remaining stock. The toolpath will then engage the stock in a trochoidal fashion based on your stepover. Horsepower becomes completely irrelevant with these types of toolpaths. The micro-lifts are a nice benefit, but if you have a slow control ( non high-speed machine ) then it might be too much code for your machine to handle efficiently.

 

Carmen

[neurosis]

 

I could also use some advice on some settings for milling these pockets. I am using a .500 4 flute kennametal Harvi endmill in 6061 aluminum. I was thinking about a .500-1. inch doc. If I have the horspower. What would be the best stepover amount, would microlift be a good option and if so what would a safe starting point be for approching this job?

 

 

Thanks

Jim

 

 

I have to ask, why are you using this particular endmill in aluminum? I would think that there are much better cutters for your task. This is assuming that I am looking at the right cutter (Harvi). I am a big fan of SGS S-Carbs but im sure that you could get several opinions on which endmill works the best in Aluminum.

 

Are you pre-drilling the hole or do you plan on helical entry?

 

Im not exactly sure what Redfire means when he say's horsepower becomes irrelevant. Maybe he can explain his thinking. Im not arguing it, maybe I can learn something. I can bring my spindle loads in to the red zone using a 1/2" endmill depending on the machine. I have to run the parameters differently depending on which machine I plan on running the job in due to either lack of power, lack of high speed, or memory. If we use larger diameter endmills I can bring our bigger machines down as well depending on how aggressive I decide to get. Once you get the right combination of depth, axial, speed and feed, you can get your maximum material removal rates for any particular machine.

 

 

Giving you suggestions without knowing the particular machine is kinda difficult. I could stall our old akira seiki with a 1/2" endmill no problem if I got aggressive enough. If you are looking for just a good safe starting point with a light radial cut rather than trying to get your maximum material removal then........

 

What are some specifics on the machine you are going to be running this in? Horse Power, spindle speed, etc. 40 taper? 50 taper?

[Teh Bear without Brains kinda idiot]

I always use depth of cut 90-95 % of flute length and sidestep 0.15-0.2 for small cutters and 0.25-0.3 dia for big ones

For Hanita chatterfree dia 16 I use 11000 rpm if you have more give it more f5000-7000 m/min for my machines sidestep 5 mm depth 30 mm.

HTH

[Rstewart]

Check out the Dynamic Mill Database:

 

https://spreadsheets.google.com/pub?key=0AlMGCRpJJ9GIdG40T2NIZ1F4aS0xOHNGTGd3OTItanc&hl=en&single=true&gid=1&output=html

[MACHINING JIM]

I have to ask, why are you using this particular endmill in aluminum? I would think that there are much better cutters for your task. This is assuming that I am looking at the right cutter (Harvi). I am a big fan of SGS S-Carbs but im sure that you could get several opinions on which endmill works the best in Aluminum.

 

Are you pre-drilling the hole or do you plan on helical entry?

 

Im not exactly sure what Redfire means when he say's horsepower becomes irrelevant. Maybe he can explain his thinking. Im not arguing it, maybe I can learn something. I can bring my spindle loads in to the red zone using a 1/2" endmill depending on the machine. I have to run the parameters differently depending on which machine I plan on running the job in due to either lack of power, lack of high speed, or memory. If we use larger diameter endmills I can bring our bigger machines down as well depending on how aggressive I decide to get. Once you get the right combination of depth, axial, speed and feed, you can get your maximum material removal rates for any particular machine.

 

 

Giving you suggestions without knowing the particular machine is kinda difficult. I could stall our old akira seiki with a 1/2" endmill no problem if I got aggressive enough. If you are looking for just a good safe starting point with a light radial cut rather than trying to get your maximum material removal then........

 

What are some specifics on the machine you are going to be running this in? Horse Power, spindle speed, etc. 40 taper? 50 taper?

 

 

 

My machine is a lightweight when it comes to machines. Its a HAAS TM-3 40 taper with only 7.5hp and 4000rpm. Pretty basic machine but I manage.

As far as the endmill goes thats all I have. We are a small job shop and I have limited resources. I am not even 100 percent sure these toolpaths would be effective on my machine perhaps they would be slower. I guess thats why I am posting these question. I know I have run some pretty large files in the past and my control definitly has a hard time keeping up. I says its outputting 100-200 ipm when chewing through g code but it definitly isnt.

Like I said perhaps Dynamic milling would be a total waste of time?

 

Thanks again

Jim

[MACHINING JIM]

Check out the Dynamic Mill Database:

 

https://spreadsheets.google.com/pub?key=0AlMGCRpJJ9GIdG40T2NIZ1F4aS0xOHNGTGd3OTItanc&hl=en&single=true&gid=1&output=html

 

 

Sweet thanks

[K2csq7]

Like I said perhaps Dynamic milling would be a total waste of time?

Absolutely not.... I have used these toolpaths on everything from .06 dia. EM's picking out small corners to Hogging massive amounts of material away with a 2" HSS rougher at like 200 RPM and 3 IPM.

You just need to find what works for you... at the very least you will get the best tool life you've ever seen.

[Tony35]

Absolutely not.... I have used these toolpaths on everything from .06 dia. EM's picking out small corners to Hogging massive amounts of material away with a 2" HSS rougher at like 200 RPM and 3 IPM.You just need to find what works for you... at the very least you will get the best tool life you've ever seen.

 

+100

 

i use the 2D HSM paths all the time

they are worth taking the time to learn how to use them rather you have a HS machine or not

[neurosis]

I think that the dynamic tool paths will probably still work for you but you may have to change your strategy a little.

 

If the machine is having a hard time keeping up with code then a deep axial and light radial cut may not be the right solution for you. You are also limited by your RPM unfortunately so light and fast is pretty much out of the question anyway. You may have to take a shallower cut with a larger radial to get a good combination of material removal rate and not overwhelm the machine with code.

 

Are these pockets a basic shape or do they have odd contours? If they are basic shapes, the tool is not having to cut in to tight areas, and you take advantage of the arc filter, you may be able to get a program that doesnt have a ton of code.

 

Dynamic paths will probably work better for that particular endmill than the standard pocketing routines. The standard pocketing paths bury the endmill. I am sure that endmill will be much better than a standard 4 flute cutting aluminum but its not optimal. The dynamic paths keep the tool from burying itself in the material, always climb cuts (except in x6 where you have an option to zig-zag now), and has smooth transitions in to the cut.

[Teh Bear without Brains kinda idiot]

You are also limited by your RPM unfortunately so light and fast is pretty much out of the question anyway.

~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

I am not sure

If someone worked once on conventional mill he knows that on conventional mill you always prefer to work with doc full length of flute

Dynamic operations in HST optimized for the full length of flute work .

Even with HSS mills I would prefer to use them .

Less spindel load ,faster work and longer tool life .

I checked it on every Machine we run and most of them are not high end

Some have 6000 rpm max still it worth to use dynamic operations

The only limit I see if the machine has limitied memory and small DNC baud rate.

HSt not able to produce subroutines this problem was raised by my request

by my dealer.

When CNC software will solve it it will help to use yhem on the machines with limitied memory

[neurosis]

You are also limited by your RPM unfortunately so light and fast is pretty much out of the question anyway.

~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

I am not sure

If someone worked once on conventional mill he knows that on conventional mill you always prefer to work with doc full length of flute

Dynamic operations in HST optimized for the full length of flute work .

Even with HSS mills I would prefer to use them .

Less spindle load ,faster work and longer tool life .

I checked it on every Machine we run and most of them are not high end

Some have 6000 rpm max still it worth to use dynamic operations

The only limit I see if the machine has limitied memory and small DNC baud rate.

HSt not able to produce subroutines this problem was raised by my request

by my dealer.

When CNC software will solve it it will help to use yhem on the machines with limitied memory

 

You left out the

You may have to take a shallower cut with a larger radial to get a good combination of material removal rate and not overwhelm the machine with code.

 

Edit:

I agree with what you are saying, I am just considering his options and his limitations. I should have emphasized the FAST. If his machine is already having a hard time chewing through code, the faster his feed, the more it will struggle. With a lighter depth and larger radial, he can keep the same material removal rate, not have to push his feed rates, and have far less code for the machine to deal with. I am sure that on your conventional machine you never had to worry about the machine stuttering on code. Im still not sure what feed rates his machine can handle before it becomes a problem and whether the pockets have tight areas to get in to or if they are basic wide open shapes which all makes a big difference.

 

If I have to run a 1/2 diameter endmill in a machine with a low rpm, little horse power, no high speed look ahead or contour control, I am probably not going to run it the same as I would in a machine with a much higher rpm, more horse power, more memory, high speed look ahead etc. I can achieve very high material removal rates on our akira seiki by taking a full depth of cut and a light radial, but I have to take advantage of the spindle speed in order to do that. If I run the same program on our 6000 rpm machine, I am going to have to significantly reduce the feed rate and so reduce my material removal rate which makes me change my strategy. Keep in mind that I do not have a 7.5 HP limitation either so my strategies significantly change between our high and low rpm machines which in includes the type of tools that we use.

 

 

That is just my thinking anyway.

[K2csq7]

I just looked into one of my older dynamic paths. Material is a Stainless alloy. Machine is a big 'ol Daewoo B130. Max RPM for us is 4K (spindle grows with thermal expansion up to .015 with any RPM higher than 1200 so we keep it slow).

2.0" Kennametal inserted rougher.

 

4.0 IPM

260 RPM2.2" DOC

climb milling

30 IPM backfeed rate

.3125 stepover

.250 toolpath radius

Filter 1:1

filter & cut tolerances at .003

total tolerance = .006

create arcs in X & Y

 

Inserts last at least 3X as long as convention machining methods.

[MACHINING JIM]

Ok so here is my part. The bumps on the outside have a radius of about .375. I also found a 3 flute .375 Hanita endmill that looks like a much better choice for aluminum. Now that everyone knows my parameters where should I start for settings? Normally on a pocket routine I dont go much over 50ipm and around .150" doc so with dynamic milling what would be a conservitive start point.

OSCILLATING SPROCKET.MCX-5

[MACHINING JIM]

Oh and thanks again for all the imput!

[neurosis]

I would definitely go full depth on that. And definitely use the dynamic tool path.

[neurosis]

Ok so here is my part. The bumps on the outside have a radius of about .375. I also found a 3 flute .375 Hanita endmill that looks like a much better choice for aluminum. Now that everyone knows my parameters where should I start for settings? Normally on a pocket routine I dont go much over 50ipm and around .150" doc so with dynamic milling what would be a conservitive start point.

 

 

Will you be pre-drilling the start holes or do you plan on helical entry down to depth? Your four flute should work fine but im not sure how well it will like the helical entry 1" deep. Ive never tried that. I pre-drill our entry holes in steel and as stated above, we use s-carb for aluminum. You can literally drill the start hole with the endmill.

 

Not being familiar with your machine I wouldnt want to mislead you, but if it were me on one of my lighter duty machines, I would start at 1" depth and .15 Radial. I would think that you should be able to get away with around 100ipm. no problem. If you plan on helical entering the material I would keep your plunge angle fairly shallow for that 4 flute endmill to be safe. Maybe 2deg and 50ipm?

 

One caveat to this strategy. If your machine has trouble handling that feed rate, you can always keep your toolpath radius a little higher to keep the tool out of those tight areas and then come back with either a dynamic rest at a lower feed, or a different strategy all together to rough out the tighter areas without worrying about overshooting and gouging the part.

[Tony35]

and dont forget once you get your feet wet with these toolpaths/your machine, then start applying chip thinning and watch the feedrates go UP

[MACHINING JIM]

Will you be pre-drilling the start holes or do you plan on helical entry down to depth? Your four flute should work fine but im not sure how well it will like the helical entry 1" deep. Ive never tried that. I pre-drill our entry holes in steel and as stated above, we use s-carb for aluminum. You can literally drill the start hole with the endmill.

 

Not being familiar with your machine I wouldnt want to mislead you, but if it were me on one of my lighter duty machines, I would start at 1" depth and .15 Radial. I would think that you should be able to get away with around 100ipm. no problem. If you plan on helical entering the material I would keep your plunge angle fairly shallow for that 4 flute endmill to be safe. Maybe 2deg and 50ipm?

 

One caveat to this strategy. If your machine has trouble handling that feed rate, you can always keep your toolpath radius a little higher to keep the tool out of those tight areas and then come back with either a dynamic rest at a lower feed, or a different strategy all together to rough out the tighter areas without worrying about overshooting and gouging the part.

 

 

Yes I was going to use a helical entry. I use this type entry usually. I do not have an enclosure on my machine so I tend to use my blowgun to get in there with my blow the chips clear. I was going to start with a .100 radial cut and run 50ipm just to see how things react and step up from there. Looks like I am going to have to use a .500 3 flute cutter as well since the .375 isnt quite long enough.

[MACHINING JIM]

On the helical entry should I only use this or one of the other options in the drop down menu. Not sure if I see any reason to use trochodial cuts but perhaps I.m way off base with that thinking?

[neurosis]

Regular helical is fine. If you use a rad larger than 1/2 your endmill diameter it will leave a pole in the center so keep that in mind.

[MACHINING JIM]

Regular helical is fine. If you use a rad larger than 1/2 your endmill diameter it will leave a pole in the center so keep that in mind.

 

 

Yes true. I never usually use more than 50% so this shouldnt be an issue.

 

What exactly makes this toolpath more effective in this case? Why couldnt I use a regular pocket toolpath in the same manner. Cutting full depth and just turning the roughing stepover down to the same values as the dynamic path. With the regular pocket at least if would run a finish pass around the pocket. I dunno just trying to wrap my head around this stuff.

[Guest]

What exactly makes this toolpath more effective in this case? Why couldnt I use a regular pocket toolpath in the same manner. Cutting full depth and just turning the roughing stepover down to the same values as the dynamic path. With the regular pocket at least if would run a finish pass around the pocket. I dunno just trying to wrap my head around this stuff.

 

With 2D Pocketing, your tool "could" still engage far beyond the step over values plugged in. Watch it sometime when it has to plow into a 100% engagement. So with pocketing, you're almost always programming for your worst case cutting scenario.

 

With the 2D highspeed paths, you can program for your best case cutting scenario. This allows a greater MRR while saving your tools with better cutting life and money based on using generally 1 smaller tool.

[Chris Rizzo]

Program with your conservative/safe numbers, and use feed overide to "tune" and figure out how fast you can go. I'll bet you will be at 200-300% on the feed overide wheel. Whatever the first cut sounds like, it will be that way through the entire toolpath. NO surprises of it burying itself in a corner anywhere in the toolpath.

 

Make sure you turn the filter on also.

 

Pull some numbers out of the database. They all are pretty darn solid.

[MACHINING JIM]

Program with your conservative/safe numbers, and use feed overide to "tune" and figure out how fast you can go. I'll bet you will be at 200-300% on the feed overide wheel. Whatever the first cut sounds like, it will be that way through the entire toolpath. NO surprises of it burying itself in a corner anywhere in the toolpath.

 

Make sure you turn the filter on also.

 

Pull some numbers out of the database. They all are pretty darn solid.

 

Aww! that make loads of sense. Sometimes when machining pockets with a smaller dia tool in the past I have broke tools in sharp corners. Its all starting to become clearer now.