What's new
What's new

2019 next gen, cutting holes

jm0502

Plastic
Joined
Oct 10, 2017
I have a new vf9, trying to bore some smaller holes to size (.625) using a 3/8 endmill. With default smoothness at medium, lets say I try to open it up .001 total at 45 ipm .1 ramp, it won't cut anything off the wall but if I drop the feed rate to 35 ipm it will start pulling a bunch off the wall.

In the past on a older vf9 we could bore holes at that default smoothness and feed rate and not have a problem aslong as we were under roughly 60 ipm.

Did they change this controller that much? The safety features on the new machines are horrible. We have a 2017 mill and it's useable, but on this new one you can't even turn the spindle on at all with the door open. So if you are using a wiggler you are SOL unless you override the door locks.
 
So if I understand you are not really boring but doing a contour finish cut to the wall of the hole.
If that is the case don't feed down with a ramp but go all the way down to the bottom and finish cut from there. (am I reading you right?)

So you have a 2017 machine and this one is newer. Could you expand on what differences you see to the control and safety systems
Thanks,
Gary
 
I have a new vf9, trying to bore some smaller holes to size (.625) using a 3/8 endmill. With default smoothness at medium, lets say I try to open it up .001 total at 45 ipm .1 ramp, it won't cut anything off the wall but if I drop the feed rate to 35 ipm it will start pulling a bunch off the wall.

In the past on a older vf9 we could bore holes at that default smoothness and feed rate and not have a problem aslong as we were under roughly 60 ipm.

Did they change this controller that much? The safety features on the new machines are horrible. We have a 2017 mill and it's useable, but on this new one you can't even turn the spindle on at all with the door open. So if you are using a wiggler you are SOL unless you override the door locks.

First, you need to clarify "a bunch" - .002" .005" ??

Second, a 3/8" endmill in a .625 hole at 45 ipm sounds way too fast, even in aluminum. Is it possible the old machine (or cam program) had a setting turned on to adjust feed rate on arcs? Also, all new machines (Haas or otherwise) have crazy 'safety' features, but you will get used to them, I promise. ;)
 
So if I understand you are not really boring but doing a contour finish cut to the wall of the hole.
If that is the case don't feed down with a ramp but go all the way down to the bottom and finish cut from there. (am I reading you right?)

So you have a 2017 machine and this one is newer. Could you expand on what differences you see to the control and safety systems
Thanks,
Gary

We have a

2003 VF3
2017 VF2
2019 VF9

In the past Ive always had better luck it seems doing a large ramp to bottom finishing holes. like you said contouring. I changed the default smoothness to Finish and the issue is still there. I also did as you mentioned and dropped to the bottom of the hole and made a few passes, If im at at mid 30's for feed rate it wont cut it near size, if that makes sense. So at 40IPM it will cut a .623 hole and at 35 IPM it will cut a .625 hole.


Safety is so overrated..:leaving:

I have no problem with Safety on the machines in general. But with the newest year they made a lot of changes. You can no longer have the spindle on at all with the doors open. In the past it was limited to 750 RPM, that was fine you could still use a edge finder, wiggler or coax if needed.

Chip auger can not be on with the door open. This isnt that bad, just use to the way the older machine were.

cant open the door if coolant is on, you need to shut it off at the control before the door will unlock. The 2017 mill I have will shut the coolant off if you open the door.

Shuttle jog doent work if the door is open on the remote pendant. which kinda defeats the purpose of the remote jog.

I knew I would get crap for it, but some of the added features are over the top and make setting some jobs up almost impossible.
 
What's the actual feedrate you would like to use for the finish pass? The reason I ask is because milling inside bores requires calculating the feedrate at the tool's outer edge which will need to be slower than the programmed feedrate at the center of the tool. (inversely, when milling around the outside of a boss, you can increase the programmed feedrate in the same way)

There's a formula for it:
Linear feedrate X (inside radius - cutter radius)
all divided by inner radius

For example:
(50 IPM X (0.3125" - 0.1875")) / 0.1875"
This example would yield 33.3 IPM for those parameters.

I can't speak to the different smoothness settings for that, but I just wanted to mention that slowing the feedrate may be a good starting point to experiment further..
 
I think the older machines were OK because of slower processors and slower acceleration / ramp rates on the servos. The machine never really got over 30 ipm. Ive also notced that 30ipm is about the point where it shows. Newer mills seem to have a more aggressive servo tune I have also noticed what you speak of. I have a 2004 TM1, 2016 VM3, and 2018 DT2. This issue shows up a little on the VM. Really in the cases when I'm doing a bore that is 2x tool dia. Or less. The DT machine really amplifies the effect. The old turd TM1 never shows an issue because it just can't match modern acceleration. You can visually see it. I would suggest just programming a slower feed. I know it sucks but that's the best I've got.
 
If I was setting this up first time I would program center plunge to the bottom..10ipm and measure hole with a pin. Also I normally only allow 1-1.5 thousands to cut, and possibly run it twice without coming out.

Yea safety is great until you cant do your job
Gary
 
You can no longer have the spindle on at all with the doors open.

Shuttle jog doent work if the door is open on the remote pendant. which kinda defeats the purpose of the remote jog.

you're looking for parameter 2083 "Setup Mode Safety Type", you want it set to Normal rather than Strict. The parameters aren't visible to users, so you'll have to let HFO know and they should be able to patch that for you
 
@ jm0502

My "guess" is that the tool path is a polygon when feed rates are too high. The controller is simply taking a few "short cuts" during its attempt to profile that small (centerline) tool path at that speed.

In a development lab I managed in a past life, we used a "Heidenhain KGM grid encoder" to evaluate tool paths under various conditions (programmed path, feed rate, mass on the table). The effects of those settings/conditions on *actual* tool path becomes very obvious with that tool.

If it was possible, I suspect that if you would use a 1/4" end mill instead of 3/8", you may be able to bump the feed rate back up before you see this same issue.

PM
 
There is a formula around for figuring out true interpolated size depending on feedrate, I don't know if it is accurate for next gen or not, but I think it's still valid in the older controls. It's basically a function of how often the control calculates the next section and has to do with the time constant setting. Coyinu?
 
I personally would find having to close the doors to run the auger super annoying but I have thought to myself that what If I lost my balance or something while shoveling the chips toward the auger and got my hand caught in it.

I don't get the rational with not being able to run coolant with doors open. How do you hose down the machine then?
 
We are running into the same issue on an O.D. of 1.5" being cut with a .500" endmill using G02 circular interpolation, not point to point. When we run our Haas VM2 at 27ipm it cuts the OD at 1.501. Without changing anything other than RPM and feedrate to 100ipm the OD gets cut to 1.499. If you increase to 200ipm the OD gets cut to 1.497.

We tested on another machine, Haas VF8, and got similar results except at 200ipm the OD was cut to 1.496. A little more lag.

On an OD the Haas is removing material.
On an ID the Haas is leaving material.

Is there a Lag between controller and servos?
Have tried different G187 settings with not much change. Used G187 P3 E.001 and the same result.
 
I think its a limitation of many controls, at least haas ones. My 2012 control does similar.

Think of it this way. Assume a servo loop of 1ms, or 1000 blocks per second. This means there is a period of time between each calculation where the position is relatively unknown, and the velocity is probably changing. If point to point is essentially a straight line, then this straight line is going to cut to the inner side.
 
We are running into the same issue on an O.D. of 1.5" being cut with a .500" endmill using G02 circular interpolation, not point to point. When we run our Haas VM2 at 27ipm it cuts the OD at 1.501. Without changing anything other than RPM and feedrate to 100ipm the OD gets cut to 1.499. If you increase to 200ipm the OD gets cut to 1.497.

We tested on another machine, Haas VF8, and got similar results except at 200ipm the OD was cut to 1.496. A little more lag.

On an OD the Haas is removing material.
On an ID the Haas is leaving material.

Is there a Lag between controller and servos?
Have tried different G187 settings with not much change. Used G187 P3 E.001 and the same result.


with the bore being ~1.5", there's no way the machine is ever reaching 200 IPM

there's always servo error between the commanded position vs. actual position; the larger the feed rate, the larger the error.

at lower feed rates, servo error is minimal.

if I try to circle interpolate at too high of a feed rate on my '95 VF2, I end up with diamond-shaped holes

in short, try to interpolate precision bores at 40 IPM or less.
 
in short, try to interpolate precision bores at 40 IPM or less.

It depends on size, ultimately you need to keep acceleration low, so if the interpolation is say, 0.100", its probably more like 15-20ipm I'd say.
 
Per my message of ~3 years ago, see if you can get a Heidenhain field rep to bring one of these by your shop and "demo" it for you.

KGM 200 grid encoders for machine tool inspection

The effects on *actual* tool path due to feed rates, programming methods, and total mass on the work table will be instantly apparent (displayed on a laptop screen as "programmed tool path vs. actual tool path").

PM
 








 
Back
Top