"high speed" milling debate

[mkd]

I have read articles in magazines that compare one whittling technique with what seems to me) a slightly different whittling method, all along the author calling one method conventional and one HSM. Maybe I’m a little confused; I’m no mold maker.

Now, I can see the gain pocket milling (with the right mill/cutters) a die cavity from hardened steel would be a good benefit compared to electrode making, EDM plus polishing.

I’ve also heard former co-workers that they are cutting hard cavities at 30,000RPM and 400ipm with a ¼ inch EM, stepping down .011” per pass. Did I forget the 6 minute programmed dwell to warm the spindle in order to hold tenths. Did I mention the double digit cycle time hours?

Maybe someone can enlighten me, but these details sound rather silly to me. Most here probably know with the right method one could bury a 1.0” insert cutter in most if not all tool steels in an annealed state. The chips will pour off the cutter like water coming from a garden hose. There is no way you can tell me a 1/4”EM at .011” DOC is going to get within 10% of “my” insert cuter in terms of cubic inched per minute.

Tell me I’m wrong?

[William Grizwald]

Plunge mill first... then deal with the leftovers.

 

--

Bill

[YoDoug®]

quote:

---

There is no way you can tell me a 1/4”EM at .011” DOC is going to get within 10% of “my” insert cuter in terms of cubic inched per minute.

---

If the work piece geometry would allow use of 1.0 dia mill in annealed state, Why would you use a 1/4 cutter to rough?

 

You need to compare "apples to apples". Look at the material removal rate of a 1.0 dia highfeed insert mill in hardened material vs a 1.0 dia insert cutter in the annealed.

[Guest CNC Apps Guy 1]

Gotta compare apples to apples like Doug says. NOt gonna bury that 1" E/M in 55-60Rc are ya???

[mkd]

apples to apples, gotcha.

 

to refine my basic argument:

 

why would a Mold Shop start from a hardened block?

why not start with an annealed block, bury a rougher and in 20-30 minutes you would have something to harden. only after HT would you Whittle.

i could see it now: a junky fifty taper mill roughing out a basic shape then on to a HS machine.

since i've not done extensive testing with 1.0" insert mill using a HSM method, what kind of CU.IN./MIN can be achived??

[Jerosu]

quote:

---

NOt gonna bury that 1" E/M in 55-60Rc are ya???

---

Not on purpose anyway. But I'm not ruling it out.

[88Matt]

It is overall cycle time and cost. No different than picking out what material to use. We are building many of our gages now out of 440 ss instead of TS because we can skip anodizing. The 440 cost more up front but it is either a break even or cost savings in the end. You also have to look at things such as capacity, machine usage, maint., multiple set-up times, turn around time from heat treat, price of coolant and disposal, etc... There are hundreds of factors that go into it, not just spindle time. .02

[Lightning Larry]

Believe it or not HSM is alot easier on your spindle too. I have done repeat jobs both ways and the end result is that HSM costs about 30% less than conventional methods.

[mkd]

Setup time, heat treat logistics and spindle maintenance are important factors that will effect the outcome of this proposed comparison. But one cannot make a determination without knowing what CU.IN./MIN can be achieved in both instances.

Any guru’s want to break loose with the numbers. I’ll show you mine if you show me yours…

[Guest CNC Apps Guy 1]

So what are the parameters? 1/4" E/M vs a 1" E/M? Same machine using both methods? Different machines? What Taper? What's the Max RPM and horesepower of the spindles? All important variables beofer one can make a comparison.

 

I did some test cuts on a 30 Taper Japanese machine vs. a 40 Taper prominent US machine tool builder. Needless to say the Japanese kicked the $#!+ out of the American hands down. AND, by the time you get the American useful (read added necessary options like tool changer, coolant tank, Floppy Drive/USB Port, etc... prices are comparable. So, lots ov variables/parmeters.

 

Lay it out there for us then we can talk numbers.

[mkd]

Oops, I guess you weren’t reading my mind (maybe a good thing ..haa ha)

 

I’m interested to know what kind of chip removal can be achieved with a 1.0" diameter cutter with a HSM method.

40 taper

20ish horsepower

A2 tool steel annealed with the bury it method vs. 55 Rc (?) A2 with HSM.

Machine tool? Hard to compare apples to apples here. The machine would need to be different to optimize performance of each method. Maybe a linear bearing premium Japanese machine vs. some good box way machine that a forum member knows of. Does this narrow it down enough?

 

I’ve actually taken some pretty big cuts on a Haas VF3 (1997 model). Kinda noisy but it worked and worked. Way, way out of Fadal’s league here of course.

[Matthew Hajicek - Singularity]

I bet those molds need to be done in an absolute minimum of calender time. If you order your hardened stock before you program, it arrives when you're done programming, you cut it overnight, and it's ready to go the next day.

[mkd]

quote:

--------------------------------------------------------------------------------

 

...and it's ready to go the next day.

 

--------------------------------------------------------------------------------

 

that is tough to beat!

[Redfire427]

mkd,

 

To answer this question properly, you must first understand that high speed machining in the hardened state takes quite a few ingredients to achieve the final goal. You must have all the ingredients or you will not succeed. Makino looks at it as a total process time. If you add up all the time to program in the soft state, set-up, machine, send for heat treat, program again, set-up again, machine again versus just setting it up once and cutting it to size, you will be surprised with the results. To address your issue of metal removal rate, yes you can acheive the same rate as in the old fashioned hogging mode. The biggest differnce will be that if you were to hog out a large 3D model with a large step down, you would end up with large stair heights between passes and a variable amount of stock all over the part. With the high speed approach, your part will be cut much closer to the final net shape and require less reroughing or pick out. Typically you also use smaller cutter diameters using the high speed approach which also leave less material behind. The old ways of cutting also generate huge amounts of heat build-up in the part, where it is completely eliminated using the high speed approach. To have any success with HSM you must have a great machine, control, tools, holders, etc. These are all the magic ingredients that make it all happen. Overall savings in time of 40% are not uncommon using HSM versus the old fashioned method. I have some spread sheets that I got from Makino a number of years ago that clearly illustrate the two different approaches to machining. I was a little sceptical at first, but after almost 4 years of using the new techniques, I can absolutely verify that their figures are accurate.

 

[ 08-09-2007, 10:38 PM: Message edited by: Prosin Molds ]

[peon]

I recently applied the methods described in the two books authored by Dale Mickelson. I'm still in the testing stages, but I really like the results at this point. These books are a MUST HAVE for those new to Hard Milling like myself.

[mkd]

i'm an outsider looking in on this subject, thanks for the excellent insight!

i'd love to know what cutting parameters you gurus can get away with using HSM on hard A2.

1.0" insert mill of your choice

rpm_________?

feed_________?

Axial DOC_______?

radial DOC________?

 

i guess i'd better buy that book.

Seems like setup time could very minimal (20 minutes to clamp the block and set offsets) for a mold shop setup efficiently.

programming time is a wash, you still have to do it start to finish for either choosen method.

 

One could also use a parallel-steep toolpath to knock down those steps prior to heat treat..just thinking out loud

thanks

[mold100]

I am a huge fan of hard milling, I started into about 6 years ago, start to finish time with one set up smokes the OLD lets rough that before heat treat thinking. First and I have done both ways in mold shops for lotsa years.

 

Old way -

Set up, rough / semi leaving .02 for heatreat movement, re rough some of the area because of distortion and then finish.

 

New way I can take a half in diameter, cheap 2flute tialn coated garr (mind you thats not a cutter of choice for this but I have done this) 11,800 rpms 155.imp with a .035 step down and .187 step over leaving .008 to finish without stressing the block and is already at semi finish state with 1 tool path in 58-60 rc H-13

 

Even if that path takes longer to actually run as going from a 1" rougher , to a 3/4 to a half incher, plus to set up times, and 4 times the tool paths ??????????????? just an example

[kinglouie V]

if you want to disect HSM to a scientific process (no kidding) I found this link in a search on this forum. I have found that these toolpaths are great. Although it may be extrememly necessary to linearize your arcs if you haven't done so already as a general rule. (that one bit me a little). anyway....

 

http://highspeedmachining.mae.ufl.edu/html.../tutorials.html

[mkd]

To whom was I supposed to send my MC FORUM subscription fee to?

true: over all process time start to finish is the bottom line.

you guy have balls setting up a new program then going home, or great confidence in mastercam.

[mold100]

Lights out running +1000.

[Guest CNC Apps Guy 1]

quote:

---

...you guy have balls setting up a new program then going home, or great confidence in mastercam...

---

Both. Been leaving programs running and going home for over 10 years now. Once, I started a part on Friday @ 5:30pm, turned the lights out went home for the weekend, came in Monday morning just in time to hear it turn off. It's nothing. Besides machines are so fast now that even if you're right next to them you can't react fast enough to stop bad things from hapening.

 

Lights out and Quality will be the ony thing that keeps the US competitive.

[Rick Henrickson 65]

+1000 James!!!!!!!!!

that is what will keep us competitive, verification software will help people improve there confidence to.

Horizontal cells often run all weekend without intervention.

[mkd]

I've not left a machine running an unproven program overnight in almost ten years...guess I’ve grown into a chicken. ha

 

To sum up what I’ve learned from this thread:

1. HSM most likely is not capable of matching the OLD method in terms of outright metal removal. Annealed H13 cuts like butter: 23+ipm at .3-.4 DOC channel cutting in my sleep.

2. Point #1 doesn’t matter when taking into account the total volume of chips of the typical mold.

3. There may be good reason to use the OLD method if the volume is great.

 

Thanks for the mentoring guys.

[Guest]

quote:

---

Horizontal cells often run all weekend without intervention.

---

It's amazing to me how this thought process has just not made it in a big way on the east coast.

 

People in this part of the country just don't seem to get this.

 

They see it as a big dollar investment and can not see the pay back beyond that.

 

Seems there are so few shops that even have a horizontal, there are some but doesn't seem to me from all the shops I have been in that many get it.

 

Too bad really.

 

Lot's of mom and pop down and dirty jobs shops are mostly all that's left in the northeast.

[crazy^millman]

I will join this club as well. I have had 120 hour runs with no problem. I have done 30/40 hour runs again no problem.