| | |
Hey guys im tryin to get my lathe LB15 with 5020 controller to recognize ccs command. When I have g97 on it will recognize the speed I program and do the process at that speed. However today I was messin with it, and when I program g96 it recognizes my programmed speed for a second. Then it goes to maximum spindle speed does the process and never changes.Does this make any sense at all
Originally Posted by mbm
Yeah it makes sense, I think you are not understanding what CSS is. First you have to understand "Surface Feet per Minute". If you understand that then you have to understand that the machine has to keep up with the SFM by increasing the RPM while the diameter gets smaller. =Constant Surface Speed.
Experiment with your calculator, different G96 commands, the actual position page, and you will see.
Robert
The beaten path, is exclusively for beaten men.
You need G50 Sxxx to set the maximum spindle speed.
Super X3. 3600rpm. Sheridan 6"x24" Lathe + more. Three ways to fix things: The right way, the other way, and maybe your way, which is possibly a faster wrong way.
I think that part is figured out, you can't run that machine without G50, it will alarm.
The beaten path, is exclusively for beaten men.
This formulae is for calculating the spindle speed in a Metric world...
RPM=[CS*1000]/[Pi*D]
where RPM = spindle speed
CS = Cutting Speed in Metres/Minute
Pi = Mathematical term pi (or you can use 3.1416 and that will be accurate enough!)
D = Diameter you are working out your speed at.
Once you can work out your required starting RPM you will be better off!
Then you need to make sure of the Maximum RPM that you do not want to exceed... Like neilw20 states... use G50 Sxxxx where Sxxxx is the MAX spindle speed you want the machine to run at.
Note that once the max spindle speed is set, it will stay at the set speed until changed again, even if you power off the machine.
Once you activate G96 the machine will try to keep the spindle rotating at a speed equal to the designated surface speed. The closer you get to the centre line of the machine the faster the spindle will want to run. Obviously you can not go faster than the maximum spindle speed of the machine!
If you have a large part in the machine, and you need to face off down to the centreline, be aware of the mass you will have spinning! This is where the G50 command will come in handy for you.
Hope this helps.
Brian
Hmm... well ours would... it would just use the last setting programmed.
Are consistency... gotta love it eh?
Inconsistently, it is call persistence, not always what we want though.
Super X3. 3600rpm. Sheridan 6"x24" Lathe + more. Three ways to fix things: The right way, the other way, and maybe your way, which is possibly a faster wrong way.
Yeah thanks Brian, but the turning features will still not run unless there is a Max Speed designated, (OT) even though I am almost positive that ours will alarm if the G50 isn't assigned within each program.
The beaten path, is exclusively for beaten men.
They will alarm if G50 is not in the program on the initial power up of the control. If it had run a previous program with G50, that will stay modal. Hope that clears up any confusion. As far as CSS, your S number is either too large, or it's just a small part. Usually for alum for example, G96s1000 is in the ballpark. Just remember to cancel G96 on your return to home, otherwise you will exceed the duty cycle of the spindle drive, and can let the smoke out after a while.
Hey guys still trying to figure out this G96 thing, i understand the principal on how it works.My G50 is set at 2000 rpms and is in the line of program,Im doing a grooving process in stainless. When I program my speed at 600 rpm with a G96 the spindle will start at 600 then goes directly to 2000 before I even start to do the grooving procees.
Heres my lines of programming that are in question:
G96S600M08
G00X1.6 Z-1.875T030303
X1.1
G96S600
G73X0.89Z-1.875K0.093D0.08L0.375E0.107
G00X1.6
G96S600M09
X20Z20T0300
i program with the IGF function on my machine so I didnt insert that many S commands - the machine did. Didnt think that was my issue though.Just went and watched it again and the spindle starts at 600 and as the tool approaches work piece the spindle starts increasing to 2000 (my G50 setting) Im grooving a 1" dia piece
Makes sense. Small diameter. As the axis with the tool offset approaches the part, it will speed up. If you don't believe me, try S100 with the G96. Also for production runs, approach the part in G97, then go to G96. At 1" diameter, kind of a waste to use G96 anyway.
The reason why your machine is doing what you say is that the G96 command is a "Constant Surface Speed" Command.
This means that the machine will try and maintain whatever surface speed is commanded by the "S" value following the G96.
In your program example above, G96 S600 at an X diameter of 1.6" should give you a spindle speed of 1432RPM
Then the machine will accelerate to S2083 RPM when it gets to X1.1
Then speed up to S2575 RPM when it moves towards the X0.89 diameter.
It will then slow down to S1432 RPM when the machine returns to X1.6
When the machine moves at rapid to X20 (or to the limit of the machine) it will try to slow down to follow the 600SFM instruction.
Obviously, with G50 S2000 commanded, your spindle will not reach the speeds as calculated... but I do this to only show what the machine would be doing if the G50 command was higher, with it set at S2000 the spindle will be restricted to 2000 RPM no mater what.
What you really need to be doing is this:
G97S2083M08 <----------- Changed to G97 and S2083 (600 SFM at X1.1)
G00X1.6 Z-1.875T030303
X1.1
G96S600
G73X0.89Z-1.875K0.093D0.08L0.375E0.107
G00X1.6
G97S1432M09 <----------- Changed to G97 and S1432 (600 SFM at X1.6)
X20Z20T0300
This will reduce the load on your spindle drive unit also, as the machine will start up at the designated RPM and then move to position.
If you start up in G96 mode, the spindle drive unit is working very hard to keep the spindle moving at a speed equivalent to the diameter that the tool is at.
Your program will also run faster like this as well.
If IGF produced the program as stated, I would be very carefully checking out your parameters to see what you can do about the use of G97 and G96, as that output is not very nice at all.
Hope this helps.
Brian.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
