# Thread: Offset change at turning a axis

1. ## Offset change at turning a axis

Hello there
First of all Sorry for my bad english.
I have a Haas VF 2 5 axis machine. 3 axis milling is working well. Now i wanted to use a and b axis. My Part is not in the middle of the a axis. So if i turn the a axis the x and y Zero Point is changing. What do i have to change that my Mill knows where my part is after turning a axis ?
LG mobbbl

2. is this a VF2 with a Trunnion 160 on the table?

3. If it is this setup you have to use the center of the two rotary's on this setup as you X,Y,Z home position and Top in your mastercam then define a plane to do 3+2 indexing.
On the Trunnion it should be in the park between .111 and .140 as they do not differ to much from the factory.

Yes it is VF2 with a trunnion table. So if i understand this wright i take the X, y, and z rotary center coordinates and top it in mastercam machine defintion at a, b axis rotary center. The plane i define must have the same x , y, and z coordinates like my rotary center? Please could you explain to me how to make a 3 + 2 indexing?
Tank you very much
Mobbbl

• It would be very nice if you have a screenshot for me.

• Originally Posted by Mobbbl
Yes it is VF2 with a trunnion table. So if i understand this wright i take the X, y, and z rotary center coordinates and top it in mastercam machine defintion at a, b axis rotary center. The plane i define must have the same x , y, and z coordinates like my rotary center? Please could you explain to me how to make a 3 + 2 indexing?
Tank you very much
Mobbbl
There are 2 methods

1/- place the part to be machined ( in mastercam ) in the same position in respect of the rotational XYZ origin of the machine
the G54 origin will always be the point of rotation of all machine axes
- cons - that you have to place the stock in the same place as the part cannot be moved to another position on the table

2/- use of RTCP control (tool point control) ( or a method of recalculating & resetting a new origin within the running program
- pros - you can program to a known point on the stock, set the G54 origin to that point, the stock could be placed anywhere in the machining zone
- cons - crashes can occur when a previously proven program is run & the stock placement is different ( on the table ) from the initial setup when it was run.t
ie stock is X centred at the rear of the table, - has easy access to the back of the part. But next time is placed at the front of the table.....your spindle may hit the table/column ( or tools be too short) when trying to machine those same features

A bit of reading for you
5-axis machining = terminology etc
COE : Forums : Fanuc 16m using RTCP G43.1 ( might be of assistance )
B Axis Turning – A recent and welcomed possibility | CAMZone

• I am sorry a picture of what sir?

Superman you think that op2 will work with this configuration and control.
And your last link is regards to say a Mazak intrgrex that is lathe and 5axis configuration I do not think you can do that on this setup. just a thought but is cool reading.

• Hi
A screenshot from 3 + 2 indexing.
Thanks mobbbl

Superman you think that op2 will work with this configuration and control.
And your last link is regards to say a Mazak intrgrex that is lathe and 5axis configuration I do not think you can do that on this setup. just a thought but is cool reading.
Op2 ?? - really depends on what features are left to be machined

typically, you would try to program it so the remaining ops are easier to setup & machine and not require a complex machine to do it with ( read this as only needing a 3-axis or a 3+1 operation to complete the part )

- it was for the RTCP references about 1/4 of the way down

- & I have worked on a Mill/Turn 5ax that was on a trunnion ( OKUMA MU-500 ) table was a Ø500mm plus we had a smaller one that was only a 5ax machine (MU-400). both a real b\$tch when programming using method 1, hard to get machining to blend in together.

Plus I programmed for a DMG (DMC-80FD) mill/turn that had a nutating head ( Milplus control ),,,now, this machine was complex & had it's own Tool point control built in

for the Okuma's,
we ended up having to run a program that maps & updates the "swing point" at regular intervals - or after "a knock"
&
having a library file for re-mapping the origin "shift amount" when machining using 3 + 2 positioning---automatically called up when our running program did any rotational re-positioning ( this involved a machine option called "Fixture Offset"

We were progamming our origins to the stock, so we were able to place the stock anywhere within the machining area ( NOTE--- the tool setters & operators were told in which area it was to be placed, so that tooling is used to it's best advantage-short as possible....we also used Vericut that guaranteed NO CRASHES - that system is veerry expensive to purchase and involves a lot of training. but when Vericut was used ...any crashes ended up being the result of operator or toolsetter errors )

• Hello Superman
First i will try method 1 and i think this will work. Thanks for your reply!
Mobbbl

• Hello Superman
thanks for these links . They are very interesting for me !!!
mobbbl