High Speed Programming?

[Rubens]

Hi you guys... Does anyone know if a Mill needs to be compadible or updated to be able to run High Speed Programs? I've been trying the High Speed Toolpaths on Mastercam, and I've been pretty happy with the toolpaths I generate but the Mills (Haas and Mazak) does not seem to be able to run at optimum High Feed.... They run the toolpath program as I programmed it to, but they run slower than what the Feedrate is showing. Not only that but on my Mazak (5x), the toolpaths seem to take short cuts in to my part - causing damage. It seems like the controller can't keep up with the Feedrate - and can't seem to read the program fast enough. What do you guys think? Does anyonw know what is the problem? Do the Mills need to be upgraded to do High Speed Machining?

 

 

Ruben,

[happycat64]

we have a mazak and we had to puchase the high speed , i had the same problem with it cutting corners and the high speed package fixed that.

as for your haas there is a g code that you must use along with a p code.

[Jayson Kramer]

Sounds like you are running into data starvation that your machines do not high speed look ahead option.

[Thee Rickster ™]

One of my hass -none- high speed machines I can only run at 12o IPM. or

it cuts corners on rads.

 

I cut 2 or 3 molds a year on this VF6 for my big molds.

each time I come in the morning, it has what appears to be gouges....on one mold half

 

one owner forgets every time(what I told/showed him the first time it happened)

and cranks the feed up....then says oops....

 

good thing I'm not the senior mold maker or nuthin, what do I know?.....LOL

[JayM]

One issue I have seen with highspeed programming on machines, especially on older controllers, is that because of the sheer volume of arcs being generated there is a chance that the machine and NC code will not agree on the start/end point of the arc. When this happens you get weird moves, one of my customers used to call them "crop circles". We adjusted the "Arc error checks" in his control definition to avoid this issue. It will result in fewer arcs and more code but over all will be safer.

 

One pet peave I have is the term "highspeed machining", I really prefer "Dynamic Machining". The toolpath motion is not necessarily about running faster. It is actually a smoother and better cutting routine that is easier on the tooling. This allows us to speed up the toolpath. I would still run the dynamic toolpaths on a machine without highspeed options.

[John@WMM]

Depending on what you are doing you can use the Arc Filter / Tolerance and set the nc program length to short, doing that should help. Having high speed read ahead would be a big plus as well

[Joe788]

On the Mazak, you need to call G61.1 for the "MAZACC2D" high precision contour control. It's very simple and there are no special rules for calling it. Just put G61.1 on it's own line, anywhere. It's modal, so once you call it, it stays active until you call G64, hit reset, or hit an M30. My post just calls it after the G43 line.

[heavychevy2155]

Joe, do you have to cancel it when drilling or tapping?

[Rubens]

Thanks for all the Great information you guys.... This really helps explain the problem. I kind of figured these would be my issues. So I guess I do not stand alone on this! LOL

 

One last question for you guys. For these "Dynamic Machining Toolpaths", do you guys normally create a Seperate 'FINISH Toolpath' Operation for your Floors and Walls? I was not so happy with my Finish Surfaces so I had to add some Finish Opearations to my part. So it seems that i will only be using these as my Roughing OP. Toolpaths... What do you guys do? Rough ONLY for Dynamic Milling?

 

 

 

Ruben,

[scooke4073]

G61.1 is the answer. NEVER run any dynamic toolpath without it....

 

That said, G61.1 will slow your overall feed rate when it needs to avoid gouging. If you plan on using dynamic milling a lot look into "high smoothing control".

 

Thanks for all the Great information you guys.... This really helps explain the problem. I kind of figured these would be my issues. So I guess I do not stand alone on this! LOL

 

One last question for you guys. For these "Dynamic Machining Toolpaths", do you guys normally create a Seperate 'FINISH Toolpath' Operation for your Floors and Walls? I was not so happy with my Finish Surfaces so I had to add some Finish Opearations to my part. So it seems that i will only be using these as my Roughing OP. Toolpaths... What do you guys do? Rough ONLY for Dynamic Milling?

 

 

 

Ruben,

 

Rough only for dynamic. Unless you like the flowing pattern it creates on the floor

[Guest]

Other than Dynamic contour, the Dynamic toolpaths are roughing only

[Joe788]

Joe, do you have to cancel it when drilling or tapping?

 

You don't have to, but peck cycles will run a little faster with it cancelled.

[Chris Rizzo]

Arc filter, arc filter, arc filter.

 

In my backplot I change the color of arcs to orange, lines to blue (default). Makes is easy to visually see that you've got arcs being output.

[Redfire427]

Running a high-speed machining tool path on a Haas is the equivalent of pushing on a rope. The old Haas controls only had an 8-block lookahead, and even the new VM machines only have something like a 50 block lookahead. To run a highspeed tool path effectively, you need a proper machine that also utilizes a high-speed control. Makino's ( and similar ) have anywhere from 500 to 1000 block lookahead which allow the control time to synchronize the servo motors to achieve high accuracy. On a Haas, setting 85 ( corner rounding ) is essentially a type of tolerance control. The factory default value is .050" which is a joke and the only way a Haas will ever achieve anything even close to the programmed feedrate. If you reduce this value to obtain a higher accuracy, the feedrate will drop like a rock.

 

Having said this, a high-speed tool path WILL RUN on a Haas, which will make for smoother motion for the machine, however, forget about accuracy or speed.

 

 

Carmen

[mkd]

FWIW, G107 is the code for programed accuracy control on Haas. specified in conjunction with E.xxx or P1, P2 etc depending on production era.

high speed is not nearly what the premium brands can attain, due to the small servo motors. .

 

you will see a difference in cycle time for sure, so it is a worthwhile endeavor.

[Redfire427]

It's actually G187, but I hear what you are saying. P1, P2, and P3 simply play around with the tolerances to obtain "some" speed.

 

Carmen

[mkd]

^^^^good catch, my bad^^^

[BrianP.]

Actually the Hass does have a highspeed machining option but you need to purchase it. Makes a world of difference. Look at parameter 315 to see if it is turned on.