[Dover]

I've recently acquired a Hitachi Seiki HiCell 23 turning centre with XYZC axis, unfortunately it never came with programming manuals and as such I am having trouble working out the Y axis. Problem I am having is that I am trying to interpolate "finger grips" around the perimeter of a plastic hose fitting that I am machining for a customer. After writing the program and dry running it, I noticed that it is only moving half of it's programmed distance in the x plane as obviously it is still in turning mode in other words it's machining an eliptical shape instead of a circular shape. My question is - does anyone know if there is a specific G or M code to make the x axis move it's true programmed distance.

Simplified example machining 40mm square with 10mm endmill using X & Y axis :

N8 T080800
G28 H0 M43 (Engage C axis)
M44 (Live tool engage)
G17 G98 ( x-y plane, feed per minute)
G97 S1000 M08
G00 Z3.0 M13 (Live tool start CW)
G00X25.0Y-25.0
G01Z3.0F200 (Feed mm/min)
Y25.0
X-25.0
Y-25.0
X25.0
G00Z3.0
Y0
G00X250.0Z150.0
M15 (Live tool stop and orient)
M45 (live tool disengage)
M41 (C axis disengage)
G99
M01

When I run the above program machines a rectangle 40 x 20 instead of 40 x 40.

Look forward to hearing your thoughts.

Thanks.

[cogsman1]

The "X" axis is in diameter so 25 gets you 12.5.

[Bluesman]

I've recently acquired a Hitachi Seiki HiCell 23 turning centre with XYZC axis, unfortunately it never came with programming manuals and as such I am having trouble working out the Y axis. Problem I am having is that I am trying to interpolate "finger grips" around the perimeter of a plastic hose fitting that I am machining for a customer. After writing the program and dry running it, I noticed that it is only moving half of it's programmed distance in the x plane as obviously it is still in turning mode in other words it's machining an eliptical shape instead of a circular shape. My question is - does anyone know if there is a specific G or M code to make the x axis move it's true programmed distance.

Simplified example machining 40mm square with 10mm endmill using X & Y axis :

N8 T080800
G28 H0 M43 (Engage C axis)
M44 (Live tool engage)
G17 G98 ( x-y plane, feed per minute)
G97 S1000 M08
G00 Z3.0 M13 (Live tool start CW)
G00X25.0Y-25.0
G01Z3.0F200 (Feed mm/min)
Y25.0
X-25.0
Y-25.0
X25.0
G00Z3.0
Y0
G00X250.0Z150.0
M15 (Live tool stop and orient)
M45 (live tool disengage)
M41 (C axis disengage)
G99
M01

When I run the above program machines a rectangle 40 x 20 instead of 40 x 40.

Look forward to hearing your thoughts.

Thanks.

On the High Cell ( iused to Program one years ago) when you go into Milling mode with the M13the X axis comes from the center of the chuck. So yes you have to work off the diameter. As far as I know you can change the paramerter to Rad instead but then everytime you go back and forth from mill to turn you would have to stop and change that parrameter. So just program for it . If you need 40mm thick you need to program 80.00mm
The control I believe is call a Sekie Secos as far as I can remember that is what we had. Dependong on how new you have. You may be able to go and use a L50 function and change the parameters back and forth. But I would just program around it as I always did

Bluesman

[ChattaMan]

cogsman1...

The "X" axis is in diameter so 25 gets you 12.5.

...

He's probably using a 10mm endmill without cutter comp

Dover...

Maybe try G12.1 (milling mode). Cancelled with G13.1

[imtdick]

I've recently acquired a Hitachi Seiki HiCell 23 turning centre with XYZC axis, unfortunately it never came with programming manuals and as such I am having trouble working out the Y axis. Problem I am having is that I am trying to interpolate "finger grips" around the perimeter of a plastic hose fitting that I am machining for a customer. After writing the program and dry running it, I noticed that it is only moving half of it's programmed distance in the x plane as obviously it is still in turning mode in other words it's machining an eliptical shape instead of a circular shape. My question is - does anyone know if there is a specific G or M code to make the x axis move it's true programmed distance.

Simplified example machining 40mm square with 10mm endmill using X & Y axis :

N8 T080800
G28 H0 M43 (Engage C axis)
M44 (Live tool engage)
G17 G98 ( x-y plane, feed per minute)
G97 S1000 M08
G00 Z3.0 M13 (Live tool start CW)
G00X25.0Y-25.0
G01Z3.0F200 (Feed mm/min)
Y25.0
X-25.0
Y-25.0
X25.0
G00Z3.0
Y0
G00X250.0Z150.0
M15 (Live tool stop and orient)
M45 (live tool disengage)
M41 (C axis disengage)
G99
M01

When I run the above program machines a rectangle 40 x 20 instead of 40 x 40.

Look forward to hearing your thoughts.

Thanks.

I program several of these machines which include the B (tilting along X). I have programming manuals but have not referred to them in a long time. I wrote a post processor for these machines for my CAM system. The X value of the moves when programming (milling) in Y and/or B is output in Radius rather than diameter

[CNCRim]

Dover,

You are doing fine the way you are doing. Don't change the paremter or buy any post. Just double in X of the milling portion after you post that's all or you can edit the post little bit it's give you the same result.

[Dover]

I realise the problem can be overcome by doubling the x value. However the problem I need to overcome is when x-y machining involves circular interpolation,G02 G03.

[CNCRim]

I think I know what you are thinking...... just think machine as a milling, except know the X is in diameter, and Y will still be Y and radius will still be radius and you don't have change anything. The Y,R(IJ) will be remain the same as milling no difference.

If you're still curious about what I am talking about..... give it a test. Post a simple program for milling with G2/G3 in it and test cut a piece on a milling machine, then use the same program and just double in X and chamge few code to match the machine format,then put in the lathe and test a piece. I quite sure you will get the same result as milling.

[CNCRim]

Qqqq