Highfeed Machining

[Zero]

Is anyone using the highfeed toolpath option? If so, are you using the default high feed options or have you custimized them for your machines? How do you get the info needed to custimize the settings?

[mold100]

I primarily do high speed machining,if I backplot my toolpaths for run time without the highfeed option

it always is at least twice as fast so I dont ever use it,most of my feedrates are in the 200-475 ipm in steel and 200-630 ipms in graphite,so I dont really understand what it does maybe someone can fill me

in,I have played with the settings and it still doubles my estimated run time.

[Lucky]

Most newer high speed milling machines will automatically reduce speed during direction changes to maintain a user specified tolerance. This results is an actual cycle time that is longer than the backplot estimate.

 

The highfeed machining function in Mastercam takes care of the feedrate changes within the program. This is especially helpful if your machine does not do this automatically.

[mold100]

Thanks Lucky yhat clears things up alot,our makinos all comp the feedrate at the control.So highfeed doesnt actually change the toolpath.Thus if you are running say a hurco or fadal where the look ahead isnt that good this option compensates for it so you could program at a much higher feeddrate,it may run better at 100 ipms with highfeed than a constant 50 or 75 ipms.

[Zero]

mold100, what settings are you using for cornering acceleration in G's,etc. How did you establish these settings. I've played with it before and it does cut the maching time down considerably, but I'd like to know how to establish the highfeed settings for either of my machines to maximize my speeds and feeds.

 

I'm trying out The Metacut filter for 30 days and it does what sounds like pretty much the same thing that the highfeed option does in mastercam and then refilter the program again to get a better finish on the part. Whether or not it actually works I havn't found out yet due to post communication problems which I hope to have all ironed out after this weekend. I know that metacut tells you to test your machine to see at what feed rate at a given arc you start to get overtravel, then set the filter settings accordingly and it figures out the rest for you putting in decelerations and 'exact stops'. Which brings me to another question, does mastercams highfeed option also insert 'exact stops' or just decelerations( I know that's probably a stupid question but I'm just trying to get all the info I can to help me decide whether or not to push for the purchase of the Metacut filter).

[mold100]

Zero,sorry I can't help you out on this,the controller on our machines does all the work,with the exeption of after each toolchange I have an M250 this tells the controller to use SGI mode (super geometrical intellegence)so the accel/decel is taken care of.If I am roughing or semi finishing or just dont need a super finish I make it M251 this overides it and keeps the feedrate pretty close to what is programmed however it still decels.The controller is a Fanuc 16i Pro A mounted on 2 Makino snc64's and 1 on a makino V55.

[Fred from Université de Sherbrooke]

Zero,

What I would do is print the help file (or .doc file) of highfeed, there's the little test that you're talking about. For the exact stop mode, i'm not sure, but I think it's more of a post thing. Hope it help

[mats_asson]

I think that the default settings for highfeed is for a rather slow machine. If you have a modern makino you need to set acceleration values for your machine. I have tried highfeed for one application in our Deckel Maho DMU 50 eV and it works beautifully when you get the settings right. You have to see it with your own eyes. I think it really is worth the effort.

 

Mats

[Allan]

The highfeed breaks up the code to insert acell and decell moves to acomodate what the machine is capable of. There are no exact stops inserted just more code with smooth flowing feed rates. The default is out to lunch at 20in/min maximum feed rate change per block you will want something more realistic like 2 to 5 in/min

 

Allan

[Zero]

The help file helped out a little in figuring out the cornering acceleration in g's. I've tested one of the machines and got overtravel on a 3" arc at about 65ipm(.00209 g's). Just wondering if anybody else knows what their machine is capable of and if that's any good compared to others. Thanks for the tips Alan and Fred.

[Phil Orenstein]

Just to add my .02 worth, I've played around a little while ago with the HSM option and I observed that it smooths the feed tranisitions from the min to the max values in set intervals. On a paralell finishing pass on a contoured surface I set the max to 250 and the min to around 10 or 20 IPM and it broke the feed rate down and added it to the G01 moves on every line (or every couple of lines on smooth surfaces eg F115. F125. F150 etc...) For sharp angle moves it slowed it down e.g. F50. F30. f25. etc. It doesn't work so well with high speed loops, but rather linear transitions are better. I didn't like the surface finish as compared with flat 60 IPM machining. Fadal has a great option called surface anaylser which does virtually the same thing along with a binary compression. It cuts machining time at least in half. As was mentioned earlier, some modern controls today have feed rate optimization with high look ahead. The Roders is a $1/4 million high speed top-of -the line German machine. Man, what I'd do to work on one of them!

 

Hope some of this input helps!

Phil

[ak762]

Personally to me I think this question need in research from machines producer because they have laboratory and machine application engineers

I asked machine builder from Cincinnati to test Highfeed option vs. acc/deceleration that have Sabre1000

and give a conclusion worth it candle or not. But they keep silence as diver.

[Lucky]

Our machine (Mikron VCP600) is capable of 0.6 g's acceleration. Top of the line high speed machines are doing 1.5 to 2.0 g's. These machines are very scary to watch. Mikron achieves this performance with water cooled motors and leadscrews. Some manufacturers are using linear motors (no leadscrews required).

[Zero]

Alright, after a few tests, I've got some more questions that maybe you guys can help me with. Like Phil said, the highfeed doesn't seem to backplot as fast with arcs as opposed to linear movements( which depends on the machine's cornering acceleration capability which I think I can actually get away with .007 G's with my good machine and have yet to test the old one) and will actually add time to some toolpaths that have had arcs filtered into them(like complex 3D surface contours). So is mastercam acounting for overtravel in the linear path? Is it that much of a difference if your cutting arcs as hundreds of line moves as opposed to true arcs?

[Guest CNC Apps Guy 1]

Personally I'm a fan of SuperGI (Manino's Tweek of Fanuc's HPCC) or HPCC. Basically I program for the maxfeedrate I want, then with some Q Codes (in HPCC) I can alter Acc/Dec according to what tolerance I want to hold.