[Zak@CWS]

We're using a VF-5/50 built in 2004. Having read through a bunch of posts while searching my problem, I've seen that when using G28, the Z axis should move first, then X and Y. On this machine, this is not the case. Is there a parameter to change this? We would also like to have the machine remain where it is for a tool change as we have no clearance problems and are trying to maximize run-time. Any help would be greatly appreciated.

[mactec54]

Hi Zac@CWS

Post some of your G code program so we can see what is wrong the G28 is not always good or necessary to use

[pit202]

What is your problem ? Is your machine move in XY while going to tool change ?

If yes, show me your part of program before the M06 command.

[Zak@CWS]

What is your problem ? Is your machine move in XY while going to tool change ?

If yes, show me your part of program before the M06 command.

My concern with the G28 is not in a program but just even in hand jog mode. As I understand it, z is always supposed to "home" first. Our machine does not do this, all three axis will move at the same time. When calling out for a tool change, we do not use a G28 command, simply the M06. The machine rapids to far 2nd quadrant (machine head, not table) to change tools and then will move to the call out for the first cut. I'd like it to not move the table for a tool change just like our VF-3. This is why I believe it to be a parameter setting as we use the same programs between each, only the part offsets change as the tools are set up similarly.
X2.5205Y.7781I-.0625J0.
G1G40X2.491Y.7486
G0Z2.
M5
G91G28Z0.M9
M01
( 3/8 BALL ENDMILL CARB|TOOL - 5)
(MILL WATER OUTLETS)
T5M6 (on the VF-3, z is already at Machine zero as is the VF-5 but at this time, the VF-5 moves x and y)
G0G90G55X0.Y1.175S5000M3
G43H5Z2.
M8
Z.1

[Geof]

Zak

You should go to the Haas website and contact the Haas Answer Man. This link should get you to the page:

http://www.haascnc.com/custserv_tech....asp#technical

[Zak@CWS]

Thanks Geof, I'll give that a try.

[iamstink2k]

g28 g91 g00 z0

im pretty sure this will work try it, you have to put it all in one line

[Haas_Apps]

Please check parameter 266 bit 3 (Zero Axis TC) and parameter 267 bit 3 (Zero Axis TC) if they are a 1 then the machine will perform as you have described.

[mactec54]

Hi Zak@CWS

I hope haas Apps has the answer for your problem If not take the G91G28Z0. out of your programs as well this can be a problem sometimes

[Zak@CWS]

Please check parameter 266 bit 3 (Zero Axis TC) and parameter 267 bit 3 (Zero Axis TC) if they are a 1 then the machine will perform as you have described.

Just to verify, if I do find that they are "1" I should change them to "0" to get the VF-5 to behave the same way our VF-3 does as above? Thank you all for your replies.

[Haas_Apps]

Call us here at the factory and we can help you change them to 0 if they are a 1

805-278-8500

[Zak@CWS]

I was able to change those parameters. Works as advertised! Thanks again for all the help.