Hello,
My first thread on CNC Zone and was wondering if anyone has a simple warmup program.
Thanks,
Hello,
My first thread on CNC Zone and was wondering if anyone has a simple warmup program.
Thanks,
I don't know what you want to warm up. Is it a standard lathe? Or does it have a C or Y axis that you want warmed up? If it is a standard lathe, and all you want to do is warm up the spindle and move the turret around a bit, then there is nothing to it. I expect no one has answered you because it is so simple. Use incremental moves. Move the turret to a safe position where it will be further from the chuck or X over travel than the incremental moves in your program.
Don't call up a tool offset.
G97S500M3
G0W-3.
U-5.
W3.
U5.
M99
%
Or you could give it a feedrate instead of a rapid move if desired.
G97S500M3
G1G98W-3.F300.
U-5.
W3.
U5.
M99
%
Does it have a Fanuc control? I'm pretty sure there is a macro for the timer, but I've never needed it nor am I where I can look it up, but you could still make the RPM vary using Macro B (or Macro A, but I've never used Macro A) without knowing the timer macro number.
IF[#1LE100]THEN#2=500
IF[#1GT100]THEN#2=1000
IF[#1GT200]THEN#2=2000
G97S#2M3
G1G98W-3.F300.
U-5.
W3.
U5.
#1=[#1+1]
M99
%
What this will do is run the spindle at S500 for the first 101 'squares', S1000 for the next 100 'squares' and then at S2000 until you hit reset. Naturally you can set these numbers to any value you desire. You could change the RPMs you want to run. You can change the number of times the turret completes the square before ramping up. You can add more IF/THEN statements to make the RPMs go higher or to step them back down.
EDIT: Of course you can make the warm up program as complicated as you'd like. You can make angular moves, make it swing large arcs, or a full circle for that matter. Or any combination of moves. Whatever your head can dream up.
Thanks for the reply. We are currently setting up a manufacturing cell and working long every day. I just didn't want to take the time because of just not enough hours in the day. To many other problems to deal with.
Regards
My Doosan 300MC is less than a year old, but I find I don't have to do any kind of warm-up for the machine to cut accurately. I turn the machine on at the start of the day, origin the axis and cut away.
Just a quick note about "Warm-ups".
What they do. Why some would feel that they aren't needed while other claim that they can't get good parts unless a warm-up is done.
It comes down to three things: Clearance, Lubrication, and Thermal Expansion.
First things first: Your expensive machine will run happier/longer if you do warm-ups. Why? Because you will have it at working temperature (consistency) and well lubed BEFORE you put it under cutting load.
Clearance: Some machines of the "High speed" variety are going to heat up (basic physics) and their heat will cause expansion of complex internal parts. If those parts were not designed to have "clearance" they would "grow" into a binding state. They are designed to grow through the clearances into a perfect "running state" (hence needing the warm-up or parts might be "sloppy")
Lubrication: Warm components allow grease or lube to gravity displace. Moving through without load allows even redistribution.
Thermal Expansion: A properly built machine knows that Ballscrews expand when warmed. If a ballscrew is loose-fit trapped between pillow-blocks it will "bow" and the linear distance expected will not match the hypotenuse distance traveled. If the ballscrew is appropriately stretched during install, the bearings, when cold, have slightly too much pressure on them for "loaded run". Warm-up allows growth to alleviate that overage, yet the stretch is enough to let it grow to relaxed and not into "Bowing".
If cold run is accurate, but warm run is not: Thermal stretch of ballscrew was not done correctly (or heat is in excess of stretched amount)
If warm run is accurate, but cold run is not: Thermal stretch of ballscrew was not done correctly but someone over compensated it through parameters or other means, but did not correct the underlying issue.
Doosan Service Technician
[email protected] O:973-618-2461 M:973-803-9479
Nice post dhardt.
Don't know the age of our TW20s, but they aren't spring chickens anymore.
This is the cut-off operation from the main spindle (left side).
N1200M191 (CUT-OFF)
T1212S1500M3 We found on this particular TW20 that starting the spindle at too high an RPM caused problems with pickup
X1.18Z.5M8
Z-1.61
X.92
M75
M100
M101
G1X.89F.006
G50S3500
G96S700 BTW, this is an aluminum part
X.1F.0035
X-.03F.002
M102
M103
G0X1.4M9
G28W0M5
M30
%
This is the pickup operation on the subspindle (right side).
:4450 (511310 REV. NONE)
M100 Don't know why, but we can't use comments on the same block thus why it is on the next block
M191 (GET PART)
G28U0W0
T1100
M96
M11
M74
W-#530
G1G98W-#531F100.
G4U.5
M10
M101
M102
G28W0M97
M103
M1
Notes:
#530 SETS RAPID TO FRONT OF PART
#531 SETS FEED OVER PART
How to find #530.
Assure right side turret and spindle are in the home position. Doesn't hurt to have both turrets at X-home. Record Z-value for the Work Shift. (Always plus value on our lathes.) In MDI type in M95; (EOB) INSERT Cycle Start. M95 allows right spindle to move into the left spindle area. Move right spindle to the position where you want it to rapid in front of the part. This will be a negative number. Record this value. Add this number to the home position value. Insert this value as a positive value into #530.
How to find #531
Bring left spindle over the part to where you want it to clamp. Take this number and from it subtract the previously recorded position from in front of the part. This goes into #531 as a positive number.
I always set up my programs so the set-up guy does not need to remember the negative sign. I take care of that in the program. If you can't trust your people to always put a positive number in these two variables, you can always make it an absolute number before programing the W-#530 and W-#531. In case you don't know #530=ABS[#530] makes #530 a positive number no matter what sign the guy used when he put the value in #530.
In case your are wondering what subprogram M191 calls:
:9001(SAFE START PREP)
G0G18G20G40G80G97G99M7
M41
G28W0
M99
EDIT: Always use incremental values (Ws). This ignores the work shift so the spindle always goes to the same spot regardless of what the work shift is.
Darryl Hardt is correct.
Given your machine a warm up cycle before the day's cutting is a very good thing.