What's new
What's new

Concentricity Error With Fanuc 5x A + B Table On Doosan

Matt_W

Cast Iron
Joined
Dec 20, 2011
Location
UK
Hi,

Hoping someone can help me. I am helping a friend out with a project on his Doosan DNM 4500 (I think the model is) with a Fanuc bolt on 5 axis A + B table. We have machined a part which requires some 3+2 machining and a bit of simultaneous. Looking at the part though it looks like the centre lines of the 4th 5th axis haven't been set correct as the part isn't concentric to our datum, and is off centre in the Y axis to our datum. I know how to do a test cut and adjust this in Hurco Winamx and have done it Heidenhain in a previous life. I am guessing it would be something similar with a fanuc control, were there will be a G53 Z and Y figure in a parameter field somewhere for the A axis and X and Y figure for the B axis.

Don't suppose anyone could shed some light on this for me, and point me in the direction were to adjust the centre points of rotation.

Thanks in advance.
Matt
 

Denim

Aluminum
Joined
Oct 27, 2007
Location
Norway
Rotary axis centerline posistions are stored in parameters 19700-19705.

19700,19701,19702 = X,Y,Z position of first rotary axis.
19703,19704,19705 = X,Y,Z intersection offset between first and second rotary axis.

These parameters are used by TCP (G43.4), TWP (G68.2) and Workpiece setting error compensation (G54.4)
 

LockNut

Stainless
Joined
Jan 6, 2007
Location
Bergen County
The Oi-F control on the DNM400 does not support full 5 axis machining (g43.4) but it will support TWP (G68.2). I don't know what the OP means by "simultaneous". But only if G68.2 is used will there be any values in the #19700-#19705 parameters. Otherwise, the COR values would go into a normal work offset and the part prrogrammed from this point.
With B Axis at "0", the center of the A Axis needs alligning with the spindle C/L for X and Y and with B axis at 90, the Z C/L can be found.
 

Matt_W

Cast Iron
Joined
Dec 20, 2011
Location
UK
Rotary axis centerline posistions are stored in parameters 19700-19705.

19700,19701,19702 = X,Y,Z position of first rotary axis.
19703,19704,19705 = X,Y,Z intersection offset between first and second rotary axis.

These parameters are used by TCP (G43.4), TWP (G68.2) and Workpiece setting error compensation (G54.4)

Brillant, thanks, So the parameter 19703, 19704 and 19705 are offsets from the first rotary, guest that will be obvious when we look at the values.

The Oi-F control on the DNM400 does not support full 5 axis machining (g43.4) but it will support TWP (G68.2). I don't know what the OP means by "simultaneous". But only if G68.2 is used will there be any values in the #19700-#19705 parameters. Otherwise, the COR values would go into a normal work offset and the part prrogrammed from this point.
With B Axis at "0", the center of the A Axis needs alligning with the spindle C/L for X and Y and with B axis at 90, the Z C/L can be found.

Think its the DNM4500. Must have a different control as it is supporting g43.4 /m128
 

DouglasJRizzo

Titanium
Joined
Jun 7, 2011
Location
Ramsey, NJ.
Brillant, thanks, So the parameter 19703, 19704 and 19705 are offsets from the first rotary, guest that will be obvious when we look at the values.



Think its the DNM4500. Must have a different control as it is supporting g43.4 /m128

Is your Siemens or Heidenhain? Fanuc 0 will go up to 4 axis simultaneous, but to go more you'll need a minimum of a Fanuc 31 or another brand of controller.
 

Matt_W

Cast Iron
Joined
Dec 20, 2011
Location
UK
Is your Siemens or Heidenhain? Fanuc 0 will go up to 4 axis simultaneous, but to go more you'll need a minimum of a Fanuc 31 or another brand of controller.

Not sure of the version of Fanuc controller, I've programmed the job for my mate and its cut fine using full 5x simultaneous, its just of centre in the Y. My has had the table off but then just plonked it back on the machine. So I was guessing from working with other machines with the bolt on that the centres of rotation are out.

Would presume that if the controller didn't support simultaneous that it would just error out??
 

DouglasJRizzo

Titanium
Joined
Jun 7, 2011
Location
Ramsey, NJ.
Not sure of the version of Fanuc controller, I've programmed the job for my mate and its cut fine using full 5x simultaneous, its just of centre in the Y. My has had the table off but then just plonked it back on the machine. So I was guessing from working with other machines with the bolt on that the centres of rotation are out.

Would presume that if the controller didn't support simultaneous that it would just error out??

It would. Could be a Fanuc 31 then.
 








 
Top