Programming a Mazak Variaxis 630

[DIARMUID]

Hi Guys

We have just installed a Mazak Variaxis 630 with Fusion controller, has anyone programmed jobs for these machines as it appears that I may have to set my WCS to exactly where the part is positioned on the machine table for 5 axis machining! So if the job comes back again and the job is set up in a different position, I may have to move my WCS and possibly edit my Z depths again, is this correct?? Or do I program my depths incrementally?

cheers D

[Harryman]

I think the litmus test for using WCS is:

 

If you use a machine axis to get to a feature, do not use WCS use Cplane and Tplane.

 

If you fixture a part to align it with a machine axis use WCS.

[somename75]

I was programming the same exact machine for quite a while. I would always move the part to where it was located on the machine, then regen the toolpaths. You are correct about using incremental, when doing multi-axis I always use incremental for everything. Let me know if you have any other questions, I miss working on that machine.

[Roger Peterson]

From what I remember the variaxis are trunion machines with a rotary, correct? If so, typically you would pick up your machine zero at the intersection of the two rotary axis. Place your part on your machine. Place your part in Mastercam in relation to the origin just as your part is in relation to the intersection of the two rotary axis. I am not extrememly farmiliar with the 640 fusion but that's how it would be done on a typical fanuc equipped machine.

 

 

HTH

[Tinny]

hmmmmmm,

are you using the dynamic compensation??

[Greg Williams]

Hi,

 

Roger is on the money, We have one of these beasts and that is how I do it, Let the post do all the kinematics

[DIARMUID]

Thanks guys

How do i set my initial wcs, do I set the datum of my job in mcam relative to the distance from the home position of the machine?

[Tinny]

hi,

you guys must do it differently to my company. We tend to use a lot of jigs and fixtures which wont go onto the machine in exactly the same place the next time the job is issued again. We use G54.2 ( dynamic compensation ) in the post and all the operator does is set the new datum ( in the dynamic comp page in the work offsets )as he would with a 3 axis and the machine works out where it is in the workspace in all 5 axis.

 

Rob

[Allan Brown]

Tinny - any documentation on G54.2? I can't find any references to it. We typically exploit any decent control features like that, but have left the Variaxis post boiled down to old-school Fanuc method that Roger mentions.

[Tinny]

Dave,

I will try to find something for you. I know Mazak themselves said we are about the only ones in the UK using it.

 

Rob

[DIARMUID]

Thanks Tinny

This makes a whole lot more sense than programming jobs incremently, if you can get more info on this I would appreciate it.

Cheers Diarmuid

[Tinny]

Dave/Diarmuid,

I had a quick look before going home, and the only thing I could find is in the back of the Mazak programming manual. I will look futher tomorrow. A word of warning though, the post processor required to do this was supplied by Cimco, and it wasn't cheap. It is more suited to a medium/large company maybe???

[Allan Brown]

Well if G54.2 offers dynamic datum tracking, you can just pick any datum on the part rather than intersection point of rotary axis lines, and use G54.2 in place of G54. Easy peasy. Not a huge change for anyone with an existing (and pimped-out) multi-axis post.

 

[ 09-17-2004, 08:49 AM: Message edited by: Dave Thomson ]