[angelw]

You need to describe the layout of the machine more. If the machine is a 2 axes with a Front and Rear Tool Turret (one X axis slide) like a Mazak M5 for example, then the Circular Interpolation "G" code for the similar operation Front and Rear will be different. In this case the Rear Tools use minus coordinates with larger diameters being described with larger minus values.

If the machine simply has the one turret at the front of the machine with the minus direction away from the operator, then the Circular Interpolation "G" codes should be the same as the one turret at the rear machine with the minus direction towards the front of the machine. Imagine the upside down tool at the rear of the machine being rotated about the centre line of the spindle, so that it is now top side up and at the front of the machine, then the CCW at the rear is still CCW at the front because the tool is viewed from beneath when the tool is at the front. Accordingly, G03 with the Upside Down tool at the rear will be G03 at the front.

Regards,

Bill

[angelw]

Hi Bill

If i use this code ...
G03 X125.0 Z-1.8 I0.0 K-1.8
I get an alarm .

Unfortunately this 5t doesnt have a simple R otherwise im sure it would be easy to program using just an R value.....

Hi Shottie,
Post the Blocks preceding the G03 and G02 Blocks in your example code.

Irrespective of the layout of your machine, G03 X125.0 Z-1.8 I0.0 K-1.8, shouldn't raise an alarm if your Start Coordinates are correct. About the worst it should do is Circular Interpolate in the wrong direction. Also post the alarm number being raised. The Series 5T control can only Circular Interpolate to the end of a quadrant, ie. if you wanted to Circular Interpolate from 3 o'clock to 10 o'clock in a CCW direction, two Circular Interpolation blocks are required to get there. Accordingly, if the G03 is going the long way around to X125.0 Z-1.8 from your Start point, then you will get an error due to exceeding a quadrant in one Block. I assume that the decimal point included in your code was for clarity in the Post, because the 5T control doesn't tolerate decimal point Format.


Using "R" format is only a fudge if your Start/End points are incorrect. If the Radius being machines is only for deburring, or a blend Radius, then nothing too much lost. If the Radius is part of a profile that must be correct, then using "R" format can lead to an incorrect profile without you being aware (no alarm raised) until the part is finally inspected. If either the Start/End points are incorrect, and if its geometrically possible, the control simple calculates an arc centre so that the Radius fits.

Regards,

Bill

[Shottie_gp]

Thanks Bill .

You are right yes im just using the decimals for clarity ,and my 6t control takes decimals so im used to it .

Here is the code ...
G0X40.0 Z12.0
G71 P10 Q20 U-0.5 W0.05 D2500 F0.28
N10 G0 X145.0
G1 Z0.0
G1 X128.6
G3 X125.0 Z-1.8 I0.0 K-1.8
G1 Z-10.0
G1 X52.2
G3 X45.0 Z-13.6 I0.0 K-3.6
G1 Z-75.0
N20 G1 X40.0
G0 Z20.0..................

Like i say this is weird because it all seems fine to me ....but then again im no pro at programming yet , and this 5t is really something ill have to get used to .
Maybe im missing something silly ?

[angelw]

Thanks Bill .

You are right yes im just using the decimals for clarity ,and my 6t control takes decimals so im used to it .

Here is the code ...
G0X40.0 Z12.0
G71 P10 Q20 U-0.5 W0.05 D2500 F0.28
N10 G0 X145.0
G1 Z0.0
G1 X128.6
G3 X125.0 Z-1.8 I0.0 K-1.8
G1 Z-10.0
G1 X52.2
G3 X45.0 Z-13.6 I0.0 K-3.6
G1 Z-75.0
N20 G1 X40.0
G0 Z20.0..................

Like i say this is weird because it all seems fine to me ....but then again im no pro at programming yet , and this 5t is really something ill have to get used to .
Maybe im missing something silly ?

So this is a boring bar you're using on the front turret. Let me see more of the code for the X minus code example you had in your earlier post. If your machine is like a M5 Mazak, the program example in your last Post should use G02 not G03, and the alarm you're getting is because G03 is wanting to make the tool travel through 270degs to get to X125.0

Regards,

Bill

[Shottie_gp]

Bill
Ill get all my ducks in a row and post just now Thanks Again for the replies .
Im also going to try and save some screen shots in bobcad to explain a little easier .
Let me get all the info i can gather and re-post .

[Shottie_gp]

Right lets see if i can clear things up a bit......
Firstly here is a pic of the tool turrets that i found on the net .....
Attachment 241890

Ok so the rear turret would be the hex turret at the rear of the machine and the front turret would be the square one in the front .


Now forget the sizes ive mentioned above (they were just for reference ).
Here is some code for the rear turret with a small boring bar for the job i want to do .....
G0 X-40.0 Z12.0
G71 P10 Q20 U0.5 W0.05 D250 F0.28 (U POSITIVE )
N10 G0 X-145.0
G1 Z0.0
G1 X-129.6
G2 X-126.0 Z-1.8 I0.0 K-1.8
G1 Z-10.0
G1 X-52.2
G2 X-45.0 Z-13.6 I0.0 K-3.6
G1 Z-75.0
N20 G1 X-40.0
G0Z12.0

ok .
So that works with a small boring bar upside down in the rear turret .(like most normal cnc lathes )

Now the problem is with the front turret you mount tools facing upwards and not upside down . so u mounting them like u would in a manual lathe .
Also now you will be cutting the opposite side of the work piece aswell .
Here is a pic that will help describe what im saying ....
Attachment 241892

As you can see in the top half of the screen is what i would do normally .
The bottom half of the screen is what im trying to do now .

Here is what ive tied to program ....

G0 X40.0 Z12.0
G71 P10 Q20 U-0.5 W0.05 D250 F0.28 (U NEG )
N10 G0 X145.0
G1 Z0.0
G1 X129.6
G3 X126.0 Z-1.8 I0.0 K-1.8
G1 Z-10.0
G1 X52.2
G3 X45.0 Z-13.6 I0.0 K-3.6
G1 Z-75.0
N20 G1 X40.0
G0Z12.0

now as soon as it gets to the radius it gives an alarm 20 .
if i change the I to -1.8 and K to 0.0 i still get the alarm .
If i change the G3 to G2 then it cuts a radius but a concave radius and not convex if that makes any sense .....?
Anyway im hoping to get some clarity on this issue as it seems the 5T guys around here are very few and far between.
Oh and in-case you were wondering ........i cant use the back turret cos you cant mount a big enough bar in there.

Any other ideas ? Anyone ?

Thanks

[angelw]

Hi Shottie,
You're correct when the Front and Rear turret shares the one slide. G02 for a convex radius on the corner of a face and an ID using the Rear Turret will equate to a convex radius on the corner of a face and an OD using the Front Turret.

The fact that the radius can be cut but in the wrong direction with the Front Turret, confirms that G03 for the ID convex radius is correct. I have a client who's 5T controlled lathe will only perform a Circular Interpolation if the tool started at the Start/End of a quadrant; 3, 6, 9, and 12 o'clock. It could finish at any point around the arc of the quadrant, but if the arc started at, say, 2 o'clock, an alarm 20 would be raised. The problem was deemed by Fanuc to be a control problem and never fixed.

Alarm 20 is an out of tolerance error for Circular Interpolation, but as the calculations for your radii are "off the top of your head" calcs; your numbers are correct, including the "I" and "K" address, I believe your issue is with the control.

Regards,

Bill.

[Shottie_gp]

Hi Bill .
I reckon you might just be right , although im no pro at programming im pretty sure the code above should work .
Ill try find someone here that works on the control and see if i can get to the bottom of it .

Thanks for your replies though Bill ! Much appreciated