Printable View
Does anyone use multiple setups in one program to run several parts in differents spots on the table?
We're more of a manufacturer than a job shop so I keep a list of what each G154 P** setup is used for, and when I install my fixtures to the table, I just modify the corresponding setup and never touch the code.
Am I making this harder than it should be?
No. Or at least that is my opinion.
We have dedicated vises or fixtures permanently mounted and also have dedicated tool sets permanently in the toolchanger or reserved for a particular program.
Setup involves installing the custom jaws on the vise, loading the correct tools if they are not already in the machine and running a program which just enters all the offsets for the setup; then running the part program.
It takes several minutes to set things up the first time and find the actual offset values but when the second and subsequent setups are done it is very quick.
Agreed
I worked in a shop that wanted a complete tear down after each job, all offsets cleared, stuff like that???? I think it is a total waste of time. I'm still not sure what their logic was behind it but that job didn't stay around for very long, I had to fire it.
If the question is, is their a more efficient way to jump from job to job I don't think so. JMO
Robert
Actually there is; use G52 and you can have a single constant primary work zero and then all the part work zeros are embedded in the program as G52 XYZ commands.Quote:
Originally Posted by littlerob
If you use vises or didacated fixtures, you can put a plate on the table with a series of pin and bolt holes. Your vises etc can be controlled from those locations and the work offsets can be written and just called up for that position. I have done that kind of programmig and machining for a long time. As far as only using one offset, that idea does not work good for a controlled manufacturing shop. If you use "G52" you mite as well go back to the dark ages and use a "G92" You can run as many operations on your table as you have room for vises or fixtures.
I guess I must be running an uncontrolled manufacturing shop in the dark ages then because we have recently completed a total retooling to use multiple part fixtures that locate all the part work zeros by G52 from a single primary work offset.Quote:
Originally Posted by cncwhiz
G52 is nothing like G92.
I'm always learning thanks Geof!!Quote:
Originally Posted by Geof
Robert
So tell me, if I put a "g10", "g54 etc" or "g92" in the program will do that same thin but with different codes? If you have a "primary" work offset, that is pretty much like everything starting from machine "O"? They all do pretty much the same thing? The way we have a hard time getting people in our shops that know what they are doing, I try to keep all my tooling and setups simple using common known formats? Do you do repeat jobs? How is your tooling mounted to the table and or tombstone. These all make a bigger difference than what code you use to position your program. I run Fanuc and like to use all the common work offsets as well as "G54.1". I then can set my "known" work offsets in my post processor and the setup people do not have to find the work offset? I have my system built so a Walmart reject with a little bit of training can do a setup.
That is a bit derogatory. :)Quote:
Originally Posted by cncwhiz
Having a single primary work zero is not quite equivalent to using machine zero. Here are links to a couple of threads I started showing some of my setups.
http://www.cnczone.com/forums/showthread.php?t=38283
http://www.cnczone.com/forums/showthread.php?t=51582
I don't have any more recent pictures and descriptions but we have now switched almost exclusively to the use of G52 working from the single offset. This works very well for us because periodicall we switch out the rotary fixtures for vises and then back to the rotary. When the rotary is replaced all we need to do is dialing in to a central reference hole which becomes the G54 work zero; all the programs use this for the G52 shifts. It does not matter if the rotary goes back into a slightly different position in machine coordinates because we refind its G54 location after reinstalling it; trying to use machine coordinates for the G52 would mean the rotary has to go back exactly correct otherwise all the program G52s would be out. This is why I say above the two are not quite equivalent.
Sometimes we do use more than one primary work zero but it is not really more than one because they all have the same X, Y coordinates. The reason for this is that we can then have a different Z value to shift our tool zero plane according to the position the fixture is rotated to.
To anser your G10, G54, G92 question:
G10 is used to enter offset values, etc so you can use it to enter a G54 value, or any work zero value.
G92 is an archaic way of doing work zeros that as I understand it comes from the time when machine memory was limited and it was not possible to store dozens of offset values. The G92 command without any coordinates included tells the machine to make its current position the primary work zero from then on. This means if you move to X-5., Y-5. in machine coordinates then command G92 your work zero from then on is at X-5., Y-5. If you move to the same spot and command G92 X3., Y2. the work zero is moved this distance from the current machine position so it becomes X-2., Y-3.
G92 is tricky to use because you need to know where you are in machine coordinates before giving the command.
G52 is not at all tricky because it uses the current primary work zero and shifts the G52 work zero relative to that.
Obviously we do repeat jobs, actually we make our own product, and we keep our setups as simple as possible (if you can call a rotating fixture holding 16 parts using 48 work zeros and 4 angular positions simple). The thing is my simple is maybe different to your simple; it all depends on what you are familiar with. I came to the conclusion that using G52 was the way to reduce the number of values the operator has to enter into the machine during a setup; can't get much fewer than 1.
"That is a bit derogatory" In this business anymore, it is the norm? I have a machine that is an older Fanuc 11m. It has FAPT that we have never used. This does not allow more than G54-G59. I use position macros for this machine. The machine is a 3 axis machine with an indexing table. I run six sided tombstones on the machine. I work off "X0" and the face of the parts for the operators. I use all the offsets in the normal operation of the parts. Now for the kicker, I also have angle holes that I need to drill. I use the center of rotation for this. I have a macro that will either call up my "Z" face and the center of rotation. Your fixturing and methods are like my processes except you spindle is all wrong it need to be laying down. I guess I would have to see more about program wise how you use "G52". I do my best to keep the thinking /setup out of the job. Not saying all people are dumb, I have a new CNC forman on the floor that knows what he is doing?
In one sense G52 is so simple that people try to make it complicated. Here is the complicated explanation:Quote:
Originally Posted by cncwhiz
On machines that recognize G52 as being a command for secondary work zeroes (most Fanuc I think, Yasnac does not) the G52 coordinates are added into the active work zero coordinates.
If your active work zero (G54 or any other) is at X-10. Y-10. and you give the command G54 X0. Y0. the machine goes to 0, 0 in G54 which in machine coordinates is X-10. Y-10..
If you command G52 X5. Y5. then command G54 X0. Y0. the machine goes to 0, 0 in G52 which is X-5. Y-5. in machine coordinates; the G52 coordinates have been added to the G54 coordinates like I mentioned above.
The G52 coordinates are always added to the active work zero coordinates but if they are zero the G52 work zero is in the same place as the G54 work zero.
In a program you can change the G52 coordinates as many times as you like so you can have as many work zeros as you need.
So, its like using the "common" offset and offsetting from that point on your "G54"? I have a machine that would have an issue with that. I shows thermal expansion in the "Z" axis. When you put a value in it like a value in "Z" to stay away from something, it resets when it does a tool change?
I can do that with a "G10". I can change it as many times as I want in the program?
This I cannot comment on because I am unfamiliar with "common" offsets and what is meant by this.Quote:
Originally Posted by cncwhiz
Depending on the machine and Settings/Parameters G52 may or may not be zeroed at M30 or on RESET. I use Haas and when they are running in 'Fanuc Mode' the G52 does not zero, you have to set it to zero with the command G52 X0. Y0. Z0.
Regarding G10 yes you can do the equivalent; create as many work zero locations as you like. I have convinced myself the G52 route needs less typing. :)
I have "G10" built into some of my old post processors so I only have to input it one time. Have you ever thought about doing some of this in a Macro?
Very briefly and I could not see any advantage.Quote:
Originally Posted by cncwhiz
To some extent I think the way many people use macros is an archaic hangover from the days of limited memory. (That comment will probably get some people exercised to respond.)
We do 'families of parts' that differ in a few key dimensions and we could have a single program containing macros and then the setup person would enter the variables for the part being made. When the machines had only a few kilobytes of memory that was probably sensible but when the machine has 1meg or 16megs it is possible to copy the programs and change the coordinates to have individual programs for each part. This way no variables need to be entered, each part has its own program and each program uses the same primary work zero via the G52s.
I use macro's on a daily bases to take either weaknesses of the machine and or control my processes to reduce mistakes. I run programs with A and B pallets. I the past operators would run the wrong program on the wrong fixture. I have fixed this issue with macro's. I use them for tool changes. All I need to do is call up T# M6 and the machine moves into the correct position and exacutes a tool change. I am going one step further. I use two reference models in my CAM programming. They are the same except for a few minor changes. I do one setup , then when I finish with one job I will run the other part an use either a blockskip on or off. This feature has jumps etc to run the other part with no setup.
Yes some of those things do need macros. Regarding tool change macros I am a bit spoilt: I use Haas and the only command needed is Tn M06, the machine stops the spindle and simultaneously raises Z to the tool change position, turns off the coolant and does the change. On the side mount changers the Haas controller sees the upcoming Tn M06 in look ahead and moves the correct pocket into position so it is ready when the change is executed.
Haas also has canned cycles for bolt hole circles, bolt holes on an arc, bolt holes along and angle, some free form pocketing routines which can include islands or bosses; these all remove the need for macro (thank goodness, I can write them slowly but have never needed to get fast and efficient.).