Offset change at turning a axis

[Mobbbl]

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

[cadcam]

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

[cadcam]

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.

[Mobbbl]

Hello cadcam
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

[Mobbbl]

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

[Superman]

Hello cadcam
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

[cadcam]

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.

[Mobbbl]

Hi
A screenshot from 3 + 2 indexing.
Thanks mobbbl

[Superman]

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 )

as for the last link,
- 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 )

[Mobbbl]

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

[Mobbbl]

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