feeds on a Variaxis

[DIARMUID]

Hi all

Recently I have been asking some questions about a Mazak Variaxis with Fusion control and I have had god success from you guys!

I am now looking at a feed problem on the machine, I've turned off the inverse time feed and I am trying to run programmed feeds but the machine is very jumpy when profiling semi complex 2D components and not a smooth movement at the programmed feed, I am assuming that the G61.1 is affecting this and that there may a parameter tolerance on the machine that I need to adjust, or a code that I can input into the program. Would anybody have any info on this as the machine technicians here don't seem to have the knowledge!

cheers D

[DavidB]

I don't know that control or machine.But if its 2D work the inverse feed shouldn't make a differance?

I'd look at your toolpath see the code, is it point to point code? Are you using the Filter in MC to create arcs?

 

[DIARMUID]

I am using 2 types of software and I am having the same problem, so I'm thinking it's the machine!

[somename75]

G61.1 only looks ahead 5 blocks, if your block size is very small point to point this is probably not enough. you will have to either loosen the tolerance in G61.1 with a K value I believe, or use the higher end look ahead package which is g5.

 

hth

[DavidB]

Does that controller use G05 P1000 to turn on High speed option and G05 P0 to turn off.

 

I still don't think any option should be needed for 2D work!

[DIARMUID]

somename, can you give me an example of program line layout for the "K" ?

[somename75]

dang its really been a while, and I cant remember exactly how it goes. but i believe it is something like g61.1 K 0-100. What I would do is run the program off the part, put in a K of say 1, see what happens, and then try a 100, hopefully the differance will be very noticable. I will try to write more later on today as things are nuts right now.

 

HTH

[Guest CNC Apps Guy 1]

David,

 

That is HPCC which is a Fanuc option.

[DIARMUID]

I've checked the programming manual and there is a G05P2 option mentioned for high speed machining which may work but I'm worried about machine accuracy! I will have to do some tests! There is no mention of inputting any "K" values at any stage.

[Psychomill]

The easiest way to test the machine is to shut off the G61.1 and run the program in G64. Now switch back to G61.1. Do you see a considerable difference in the jumps? If so then some parameter adjustment is in order. The problem probably lies in the "gains" and the acceleration/deceleration rates for different angles/corners. David is right about the code. Is it point to point? Usually this machine (as well as other ones from Mazak) ends up with accuracy problems when running high feed rates in PTP, not "jumping" around. The jumping around problem at high feeds is usually associated with Fanuc controlled machines.

 

G61.1 is a must have option on these machines. I have it on 100% of the time and running extremely high feed rates with awesome results including alot of 3D.

 

The "K" value is discussed in the programming manual (although very briefly). It's in the section for 2D Shape option. I'll have to check the page number. Basically it controls the percentage rate of decelleration when approaching and cutting over intersects, angles, tight arcs, etc. (all of these are parameter controlled). The "K" is basically a "user" adjustable setting. Say your program feed is 300ipm. If you set "K" to "50", then the machine will slow to 150ipm when hitting the corners. In the program you type in as follows: "G61.1, K50". Yes, you need the comma.

 

The machine default should be at 70 (Also controlled by parameter). Setting a "K" in the program remains until you change it, hit the 'reset', or M30. In my experience, the jumping around has been a machine software related problem. You'll want to contact "Programming support" at one of the factory centers to double check software version and baseline parameter settings.

 

Sorry this is so long. First time posting. I'll try to keep these much shorter in the future.