| | |
I started a new job 6 months ago at a shop that uses all mazak mills. The guys that have been running these machines for years have never looked into parameter issues that constantly cost them time and money.
In this time I've come up with a little list of things i'd like to know if anyone here can point me to the right parameter, if there is one. So here goes, broken down by machine. We have three machines but most of these issues need to be corrected on all of them.
20+ year-old AJV w/ M-32 control
1-I'd like the Position screen to always default to the command screen, like our other machine does, which is a newer VTC w/ M-PLUS control
2-we always use rigid taps and I always have to set the tap data to 1 for rigid and 100 for return feedrate, I'd like this to be the default when defining taps
VTC w/M-PLUS control
1-When changing any part of the tool data, for instance: .5A endmill to .5B endmill, the tool length is erased automatically. I wish it would quit that.
VCN w/Matrix control
1-When using a line or face unit, the tool always pauses for a moment before any change in direction. This is happening hundreds of times each cycle for a part being machined this week and its unnecessary. I need to know how to make it move continuously.
2-When a machining unit has an initial depth of say Z-1., the tool will only retract to .125" above that depth for repositioning to the next pass. So it'll crash into the side of the part at a depth of Z-.875 instead of retracting to the programs initial Z which may be Z4.0. We can change this in the TPC for each unit that needs it, but I'd like this to be the default for all machines and all type of machining units.
That's it for now but the list keeps growing.
I greatly appreciate any help you guys might be able to give me
See if you can get your hands on the manuals for these machines first off. They are sometimes a little confusing, but once you get a good idea of what parameter does what, you can go in and adjust to your liking.
Since you have several machines of varying ages, you will definetly need to study and tinker.
On the AJV with the M32:
There is no parameter to default to the command screen and there is no parameter to default set tap float to "1" these were issues that Mazak knew needed to be changed which they did in the M+. (I asked an application engineer years ago).
On the VTC with the M+:
I am unsure of the answer, I will look tomorrow when I can get to a parameter book.
On the VCN with the Matrix:
Look in the parameter book around E90-E95, these bit parameters set the tool path for line, pocket, and face units. A parameter for each type of unit. I suggest setting them so the tool always retracts to safety clearance, then rapids back to the next surface + E9 (i think) and also be sure that the tool always starts at the approach point.
As for the stop and wait after each move, this is because the machine is set to G61.1 (exact stop check) instead of G64 when in auto mode. You can look on th MODAL display on the COMMAND screen it will say one or the other. I will look up that parameter for you tomorrow also (I believe it is a "F" para though). I do know that when the machine is in G64 it may cutoff corners if the feed rate is very high (ie roughing aluminum and 3D work) one way around this problem is to leave more finish allowance.
thanks so much Bildoo
at least I can ease my mind about the AJV and get used to it
for the tool retract on the VCN, parameters E91- E95 are the same between the VCN and the VTC, and they're all set the same too, yet they act differently. I'm a little clearer on the situation after tinkering with it today in between cycles.
(VCN) On a face or line unit I start out with a total depth of 1", SRV-Z is .5", and depth per pass is .1"
the tool rapids to Z-.6, makes a cut, then rapids to Z-.4 to reposition to the next cut, which causes a crash.
The VTC however, rapids to Z2.0 (the initial Z) after making the first cut, and each cut after
Heres where it gets even weirder: I found E104 while studying the TPC on these machines and its set the same on both - all 0's. According to the manual, setting bit 1 and 2 to a value of 1 will send the tool back to initial Z each time. So I change them to 1's and voila, the tool retracts to Z2.0 each time. Funny thing is, the VTC was already retracting to initial Z even thought E104 bit 1 and 2 were set to 0's and still is.
So before I can feel confident about changing this parameter I need to understand the difference between whats going on here.
Also, I looked at the modal display on all the machines and every one says G64. We have two VCNs w/matrix controls, one of them does this stop-start motion and the other cuts continuously. Is there a way to print out all the parameter settings, or back them up into a version that I can compare? If not, I'm looking for related parameters and checking them one by one.
As for the E91-E98 parameters being set the same between the machine yet they act different puzzles me. Maybe the settings on the parameters are maybe opposite going between series of controls. I have never compared them side by side. I will look into this tomorrow. (I would really think they wouldn't change these between controls) One time I did find a typo in a parameter book I got from Mazak mill training and it was published opposite of what the actual para book said.
The pausing of the cutting: Parameter F72 sets the high accuracy mode on and off (G61.1/G64). Maybe check into the parameters for corner decel. maybe the min and max angles are set high/low. Although I thought these were only for inside corners. I will look into this a little further also.
You could also call a Mazak application engineer maybe they could some up with something.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
