[little bubba]

'97 4020 with a 88HS control, which I do believe means Horribly Slow. Lately we've been doing quite a few parts that require work on one end and work on the other. So finish one end and then wait for a tool change, (12-14 seconds or so, is everyones this slow???) and then wait for it to "rapid" 36 inches over. Seems to me that there has to be a way for the table to rapid over while the tool change is going on. It may only save a few seconds, but on some longer run jobs, those seconds can add up.

[nervis1]

I'm pretty sure the answer is no, when you call for a tool change it won't do anything until it is complete.

I guess you could put in an M6t* and an X Y rapid on the same line and see what happens.


Let us know.

[DareBee]

Yes my 94 is about the same and if you can figure out positioning during tool change please let us know.

[TR MFG]

I asked this question to Fadal some time ago and the answer was absolutely not. The "M6" command prevents the machine from making any movement till the command is finished.
10 sec. tool change is about right, the sad thing is the side mount, swing arm tool changer isn't much faster. Our 1981 Hitachi Sieki is faster at tool changes, about 6 sec.

[Neal]

TR--
If you do NOT need to move the X and Y axes to make clearence for any reason, Try G53 Z0 and leave the X & Y where they are. This will cause the Z axis to go straight up and the X & Y will stay where thay are. This will eliminate the long rapid move after the fact.

Neal

[TR MFG]

Neal,
The question is can X and Y move at the same time the M6 command is being executed.

'97 4020 with a 88HS control, which I do believe means Horribly Slow. Lately we've been doing quite a few parts that require work on one end and work on the other. So finish one end and then wait for a tool change, (12-14 seconds or so, is everyones this slow???) and then wait for it to "rapid" 36 inches over. Seems to me that there has to be a way for the table to rapid over while the tool change is going on. It may only save a few seconds, but on some longer run jobs, those seconds can add up.

[Scott_bob]

As much as I'd like to see this kind of flexibility, this might be one of those "be careful what you ask for" situations...
I know that normal M funtions must be single action because until the M function is "finished" you don't want the CNC to go onto anything else. It is a safegaurd.
Now if you want to speed up each of your tool start ups you CAN do this:

T3M6
M8
G0 G54 G90 X-26.1 Y5.5 M3 S8500 G43 Z1. H3
Z0.1
...
Rapid in X Y and Z simultaniously
Just be sure your clearance plane is high enough to clear everything...
It is best to turn on your coolant before this though as you may not want to cut dry...
It's a little hairy seeing rapid in X, Y and Z but it is faster...

[little bubba]

No problem with the XYZ moves, but its so frustrating seeing the table sit there during a tool change, especially when you need to move 36" after the tool change. Gear changes too.

It is an 'HS' designated controller afterall, lookahead and all that, it "should" know that a G0 can be accomplished during a toolchange, (at least the XandY components) a G1 can't, seems simple enough, but, I didn't design the controller. Exactly what does the 'HS' do for me anyways? Does it rapidly increase the amount of time it takes for me to make a part? Don't get me wrong, I like the machine, it makes money, the price was right, I just don't love it, now the Mazak FJV, 10 feet away, now thats Love.

[Neal]

I understand the original question. As stated in other posts, the answer is no. The X and Y can not move during a tool change. My response was a suggestion to help negate the need for the long 36 inch rapid move after the tool change thereby saving some time.

Neal

[little bubba]

Ok, so its impossible to move the table while doing a tool change, so is there anyway to possibly speed up the toolchange. Someone said a toolchange takes about 10 seconds, I've timed it a couple of times and it takes 14 seconds from the time the Z stops until the tool changer clunks back, that is on tools next to each other. I know 4 seconds sounds like nothing but a while back we ran a job about 200pcs with 21 tool changes, so thats 4 hours and 20 minutes I could have saved, without pushing the tools any harder.

Another question on picking things up. This machine ('97 4020) is susposed to be running 400ipm. I've never actually timed it, but is there a way, if I'm running slow to mess with the pots on the driver boards or one of the other cards to get there and maybe a little faster. An old Bandit control we have says your susposed to adjust to 50ipm and I've pretty much always adjusted it to 100ipm without any negative effects(totally different animal, I know). I'm not saying that it would be a good idea to squeek out 800ipm from a machine designed for 400, but a little bit more couldn't hurt, could it??

[dango]

yes you can do it by adjusting the pot second from the
bottom 1020 clock card
it will efect the 3 axis
but to speed up you can first check if your machine is with
metric ballscrew you can do this by ENTER NEXT COMMAND>SETP
then two time on P to chnge to page 3 there you can see
if you have metric ballscrew if yes you can change there the
parameter to 700 IPM
then you have to adjust the folowing eror to 735 by running 3 axis

[Neal]

Where in the world did you dig up the 735 following error? DC servo machine are set to 595. Ac servos with AC0015 or earlier eproms are set to 302 and AC0017 and later are set to 600.


Neal

[little bubba]

I do have metric screws and I am definitely not getting 700IPM rapids, I would say I'm lucky if I'm getting to the 400 range. To set the following error I just need to call up one of those programs inbedded in the controller and follow the instructions in the manual, correct? As to the exact value I need to set it at, I'll let you two guys duke it out, and maybe learn something, I'll check the manual.
Thanx.

[dango]

to Neal I am sorry it have to be 0.735 volt that you measured across point 2 and 3 on the amplifier this will get you to the following error of 302
but you have one mistake also DC machine can set to 302 the difference is if you have metric ball screw
you need to set the rigid taping in page 3 to normal instead of high
the program to check and to set the axis following error is
N1 O12345 (number of program)
N2 L100 (for Subroutine)
N3 X-6.Y-6.Z-6.G1G91F150.
N4 X6.Y6.Z6.
N5 M17
N6 M30
N7 M49 (for 100% move)
N8 L101.1 (endless subroutine)
N9 M2 (end of program)

[carbidecraters]

If you are running a phase converter or a transformer to make 3 phase then your not getting your full power out of the machine. One way to cheat the system is like someone metioned. Assume that you want to make a triangular tool change and move x,y and z at the same time to bring up your tool in the middle of the rapid then use the same movement to ramp down to the part splitting the 36" move into 2 18" moves. Its more psycological.....LOL. Seriously though does your tool carraige stop at each tool bay or does it rotate to get to the next tool?

[HuFlungDung]

Actually, CarbideCraters, moving to the X midpoint as the tool moves to home for the toolchange should save a bit of time. It depends though, if the tool moves all the way up in Z first. To fool the control into making an interpolated XZ movement, with Z going home, the programmer may need to use a very high feedrate G01 movement just for that block.

[Scott_bob]

Carbide, nice idea...
HuFlung, G1 is good too...
Only problem is, the max programmable feed rate is 300 IPM. (slower than Rapid)

One of the Achilles heel issue with fadal is their acc/dec.
When a fadal needs to rapid in both X and Y, acc to rapid speed is initiated
Then when X or Y is close to target, deceleration is initiated FOR BOTH AXIS RAPID MOTION
Then the axis that has more distance to travel, is Accelerates back up to rapid speed,
then back down at deceleration point.

A bell curve representation of that axis that had to ramp up, back down, back up, back down FOR RAPID MOTION, is really, really bad!

This one of those Fadal intricacies that has always plagued this control on cycle time performance.

[Goat]

to Neal I am sorry it have to be 0.735 volt that you measured across point 2 and 3 on the amplifier this will get you to the following error of 302
but you have one mistake also DC machine can set to 302 the difference is if you have metric ball screw
you need to set the rigid taping in page 3 to normal instead of high
the program to check and to set the axis following error is
N1 O12345 (number of program)
N2 L100 (for Subroutine)
N3 X-6.Y-6.Z-6.G1G91F150.
N4 X6.Y6.Z6.
N5 M17
N6 M30
N7 M49 (for 100% move)
N8 L101.1 (endless subroutine)
N9 M2 (end of program)

So you mean to tell me that the 2 4020's I have w/ metric ballscrews are capable of 700ipm rapids? I take that increasing the rapids won't wear the machine faster or will it if so what is a guess-imate on wear?

This is some of the best news I've heard since I started working on these machines...is there a quick way to ID if the machine is AC or DC servo?

[dango]

So you mean to tell me that the 2 4020's I have w/ metric ballscrews are capable of 700ipm rapids? I take that increasing the rapids won't wear the machine faster or will it if so what is a guess-imate on wear?

This is some of the best news I've heard since I started working on these machines...is there a quick way to ID if the machine is AC or DC servo?

There 2 ways to find if it AC or DC
First look on the motor if the motor is round the machine are DC
If it is square then the machine are AC
Second open the electric door on the side where there is allot of red lamps
Blinking on the door there is place where Fadal hide the papers there is written some time it written also on the pendant door inside

But this does not effect what I was write metric ball screw machine capable
To run on 700 IPM if they are now on 400 IPM it mistake
You can ask on the factory at Fadal

[Goat]

T3M6
M8
G0 G54 G90 X-26.1 Y5.5 M3 S8500 G43 Z1. H3
Z0.1

Doesn't work on my machines...it won't use my work offset.