HST

[malo]

Hi

Can anyone tell me that does the 3D HST is efficiency?

Because it take more time than the conventional surface toolpath on creating and product.

Does anyone work with HST and can tell me how can i use the HST for get better result?

What is the feed rate and max step down on Aluminium and steel material?

Please give me some use full like for watch video and read more about mastercam HST.

Thank you

 

S.M.L

[Odell]

You will have to narrow down some variables.

What type of tooling are you using? What type of aluminum? What type of steel?

[malo]

Hi

Thank you for your reply

ALmgsi1

CK45

 

S.M.L

[Nick Eaton]

What are your "normal" speeds and feeds?

 

I always cringe a little when I see High Speed anything being "sold" in the machining industry.

True "high speed" machining requires a very fast spindle (30,000 rpm minimum........yes I know you can get high speed effects with larger diameter cutters on a slower spindle....but not on say a .375 endmill....and of course we are talking Al here, there are true high speed machining of other materials but this is still pretty R&D)

The idea is that you get the material so hot that it becomes semi fluid. The thermodynamics of the situation start to resemble fluid dynamics more than kinematics.

The main result of this is a fall in tool pressure and cutting forces as the material starts to "flow" around the cutting edge rather than being sheared.The system does not rely so much on rigidity as the forces are reduced. Tool life is also better because of the lower impact forces and once engaged the material is not in the same sort of contact as in "normal" machining.

"High Speed" toolpaths came out of this realm. It is true that they can be very useful toolpaths, I use them all the time, as they have more forgiving entries and cut strategies. But unless your machine has the

rpm/horsepower/rigidity you will not neccessarily see a huge increase in efficiency (i.e. reduced cycletime). It does allow you to take cuts in material/parts for which your machine/setup is not neccessarily designed for. For instance cutting titanium on a Haas.And they are also useful when you are forced into a low rigidity situation. But you will never beat a higher horsepower more rigid machine.

Unless you have a true "high speed" spindle the material removal rate of any machine is most closely a function of horsepower rather than any specific type of toolpath you might use. Some toolpaths might work better under certain circumstances but there is unlikely to be a free lunch.....somethings got to give......

 

Cheers

Nick

[YoDoug®]

If you are referring to the roughing HST toolpaths, then yes they are very in-efficient. I am not even allowed to use them at my job because every single time it has been challenged we were able to save machine time by creating 2d contour and pocket toolpaths at the levels needed. Always more efficient at the machine, however the trade off is sometime I now need to make 10-15 toolpaths to rough my part instead of a few HST rough toolpath.

[Redfire427]

To the above two posters:

I would run circles around anything you could produce with your old way of thinking. Yes, it does take all the elements to make it happen, but it is WAY more efficient. The proper machine, holders, tools, programming, plus many more factors come into play. You have to analize the entire job rather than one single operation.

 

As for the OP's question, we use HST toolpaths almost exclusively. We have 4 Makino 3 axis verticals. We can rough easily at 400 ipm. The guys who downplay the abilities and merits of high speed machining quite frankly have no idea of what is possible.

 

This quote from above "But you will never beat a higher horsepower more rigid machine" is completely inaccurate.

 

Carmen

[Zoober]

I agree with Prosin. I use HS strategies (including peel and trocoidal) at feeds up to 600ipm in aluminum, and 60ipm in 15-5 stainless.

Using these strategies, we have gone to 4 hours of tool life in stainless (vs less than 1 conventionally), much higher efficiencies, and have lowered cycle times dramatically (9hrs roughing is now 1-3).

Also, the tool life is so repeatable now, with life management, we have zero problems running lights out regardless of material.

[YoDoug®]

I should clarify my statement. I am not arguing against high speed machining. I know it works. Our situation here is older machines with slower feeds, slower spindles, and limited controller memory. The HST toolpaths are not efficient in our machines. In a total system as Carmen described, yes HST is the way to go.

[Nick Eaton]

Hi Carmen,

 

Well I rough regularly at 650 ipm with or without HST. Material removal rate is not only a function of feedrate it also depends on cutter engagement. I have run .75 cutters with a 1.25 axial engagement and a 75% radial engagement at 350 ipm......do you manage that with your Makinos? Of course I had a 50T 15k spindle with 40 true horsepower.

As I said the HST toolpaths ARE useful(as I said I use them all the time), but they won't turn a Haas into a Makino.....

Even the more advanced products like volumil can only get you so far. If you look at the material removal rates in the region of 4 cubes/min in Ti.

I have moved 15 cubes/min on a good day and 10 -13 is feet up on the couch machining.

With Al its basically 4x your horsepower will be your maximum material removal rate.....without a true high speed effect going on the laws of physics and conservation of energy are somewhat stacked against you.....it takes x amount of energy to move y amount of material.

So I guess it really depends on how you define "efficiency". As I said I use HST regularly on our 20k spindles because of the entries exits and transitions are designed to stop rapid direction changes putting unneccessary strain on ball screws and spindles....and these are of course good things, even on machines without a 15k+ spindle using fast feedrates.

But from a strictly machining standpoint I'm not sure they are neccessarily more efficient.

What spindle speeds are you running on your Makinos? If you don't have 30k spindles you are not doing true high speed machining.....you are using high speed programming techniques.

As an example we once did a test(50T mori horizontal with 40HP and a 15k spindle as mentioned above). We chucked up a Dapra facemill (I can't remember if it was 3 or 4 inch). As we cranked it up and got near the 15k you could definitely start to notice the drop off in spindle load......to get a .5 inch or even a .75 endmill into this effect you have to have the extra rpms.

Cheers

Nick

[gcode]

quote:

---

Our situation here is older machines with slower feeds, slower spindles, and limited controller memory

---

Yup.. I contract for a guy who has a couple of 10 year old HAAS VMC's.. They choke on the HST toolpaths..they slow to a crawl and stutter and jerk through the lead-in/out moves..

If we dial up the look ahead so the lead-in/lead out's are smooth, the toolpaths are too inaccurate to be trusted.

[Zoober]

What's this Haas thing you speak of?

Personally, I think High speed is not necessarily the right term for what I try to accomplish.

High feed is what I'm after. Not too often do I get over 6K in stainless. Moot point.

What I'm after, is .04+ chip load, thru chip thinning (whether radially, angular, or axially).

I can pull more cubes with a 1/2 or 3/8 5 flt em (1.5xd axial depth) with trocoidal than any old 50 tapercorncobslowmoheavy HP1-1/2diaendmill machining. And do it on a fairly old mazak with drip.

Here is a link to an SME artical on High Efficiency Machining:

Linkage

quote:

---

High-speed cutting means machining with high cutting speeds and low feed rates per tooth. But in many cases, the use of high cutting speeds is not advantageous. In high-efficiency machining of aluminum alloys, the highest material removal rates (up to 5000 cm3/mm) are reached at rotational frequencies no higher than 18,000 rpm.

---

[Nick Eaton]

Hi Zoober,

You are absolutely right. It is high feed machining not high speed machining. This is why I always cringe when I see the High Speed term bandied about....because the chances are its not high speed.

I think this is a marketing ploy from different interests that want you to believe that there is some magic wand to move more material faster all you need to do is buy their product......what ever it may be.

I would hardly call a 50T Mori with a 40 HP dual winding motor and 15000 rpm (made in 2001)a 50 tapercorncobslowmoheavy machine. Can you move 160 cubes with your machine? That was our benchmark.....if you weren't running that quick someone would want to know why....and there might well be good reasons. Sounds to me like you are more in the 60-90 cube range which is fine for a 20-25HP 40T machine.

The fact of the matter is material removal rate is a function of horsepower until you get fast enough to "soften" the material.

How you use the energy from your machine will depend on the HP/Spindle speed/feedrate/rigidity combination you have.

And of course you want to run as high a chipload as possible in heat resistant materials (e.g. Al and Ti). And this is also helped by the larger machines......012- .015 (thats true effective chipload with thinning taken into account) chiploads are no problem, and thats with an ordinary carbide endmill.....not a feedmill.

This is not to say that the big machines are the only way to get the job done. As I said there is no free lunch. They are more expensive both upfront costs and running costs. And the footprint is huge. Everything needs to be overengineered as you are moving alot of mass around quickly along with rapid accel/decel etc.....and I have seen some pretty horrific crashes.You could probably fit 4 typical 40T 3 ax machines in the same space.....then you have the 8-12 inch floor pad to pour.....the list goes on.

Just as a matter of curiosity what surface footage are you running your 15-5 at. I started running 700 SFM with an airblast about 10 years ago.......it was astounding, faster and as you say way more tool life.....trying to convince people that it worked was the main problem.

And I guess the orignal point was that simply running HST paths on a machine that can't take advantage of them is not going to make you faster...

Cheers

Nick

 

[ 05-06-2010, 06:19 PM: Message edited by: Nick Eaton ]

[Redfire427]

Nick,

 

Our Makino's are:

S56 13K spindle

S56 20K spindle

(2) V56 30K spindle

 

Yes, we do utilize high speed machining.

 

Without getting into a pissing contest, I believe some of the info you posted above is purely imaginary. I will leave it at that.

 

Makino was the pioneer in the development of high speed machining and technology. I have "graduated" from their intensive weeklong training in Michigan. To truly understand and apply the techniques requires an open mind and willingness to learn. To see their lab and time studies is simply mind-blowing. I too came from a 50 taper background. In fact, almost 20 years running Okumas. Once I was introduced to this new concept and was shown the proper way, there was no turning back. I now have 6 years of nothing but highspeed machining for experience. Now that I have that experience from both backgrounds, I can say with confidence, forget about the old ways.

 

Again, I will repeat. You have to have "ALL" of the ingredients to make it work. Honestly, buying the machine is the easiest part of all. I use the example of baking a cake. ( simply analagy ). There are many ingredients that go into the recipe, however, if you miss one of them, or, replace it with a substitute, the cake will be a fail.

 

I would guess you are in the aerospace industry based on some of your examples. Sure, a 50 taper machine has its place. I come from a mold-making background. I can't even recall the last time I saw someone buy a 50 taper machine.

 

Mastercam's highspeed toolpaths are a fantastic addition to the software. They are still fairly crude compared to some of the other systems out there, but for most users, they work great. To truly see a high-speed machine "dance" requires a much higher level system.

[Zoober]

I am along the same lines as you prosin. Although we do not do molds, we do valve bodies, which in many instances have the same "type" of complex surfacing requirements. We make these on Toyoda 15K 40T horizontals and 20K Matsuura Mam's. You just can't push the big machines as fast as these. It's a physics thing. I don't care how much HP I have, I will beat ANY big 50T machine making these parts.

 

I lived in the huge 50T world, doing parts that would not fit in that little Mori. !00" parts were the norm. 6K max rpm, 100HP. With that configuration, it was push hard, max chip load. But the work I do now, is more "finess" type machining utilizing HS machining strategies. Which was better? Depends on the work, but my little race cars and machining strategies are far faster for these types of parts I make now.

In the past, I was an apps engineer for a Makino dealer, and Prosin is very correct. They know fast! They have better education for HS machining than anyone.

[Joe788]

quote:

---

With Al its basically 4x your horsepower will be your maximum material removal rate....

---

quote:

---

I have run .75 cutters with a 1.25 axial engagement and a 75% radial engagement at 350 ipm....I had a 50T 15k spindle with 40 true horsepower.

---

.75x1.25x75%x350 = 246cim

 

246/40hp = 6cim per hp

 

quote:

---

With Al its basically

4x your horsepower

will be your maximum material removal rate....

---

[Redfire427]

The above is exactly what I was referring to about "imaginary" results.