Printable View
Hi everyone.
We have just purchased and set up a Chiron FZ12w with Fanuc 21i control. 1999. I have it up and running, however it doesnt have tool offset wear screen, or anywhere to enter the dia of a tool. When you select the offset page, all you can enter is the tool length on the Geom page, or the G54 etc, or the parameters page. Is there a parameter I need to change to show the tool wear offset page , or diameters?
Pete
That sounds strange. But i have one time before encountered a fanuc machine with only a offset page and no tool dia or wear page. The idea there was that you had 999 offsets these could be used for both radius and lenght offset so what i suggest to them was that you would use offset no 1 for tool 1 as a lenght and offset 101 for radius compensation and for tools 2 for length offset nr 2 and for dia offset no 102 and so on.
Hi, thanks for your reply. The only thing is on the offset page I have there are 31 available tool numbers, with 20 tools in the carousel . So all you can put in is the tool length. for each tool.
So I cant see where offset 101 would be entered for example. Totally stumped .
Could i see a picture of your offset page?
Hi, yes tomorrow I will take a photo and post it ,
Thanks
Pete
Hi Again,
well the first thing to say is its a Fanuc 21M not i
Anyway. here are the pictures of the offset screen
Attachment 224622
Attachment 224624
Okay. That is the same control as on the Emco machine i talked about yesterday. If you keep pressing page down. You only have 31? Try to make a small program where you use the tool and the height you assigned and use one off the other offset numbers as a Radius comp.
Thank you Riddersholm,
Now I will show my lack of knowledge! What would I program for the radius comp? G01 X Y is it an R?
he is rightQuote:
Originally Posted by Riddersholm
it is simple
T01 M06
G41 H1----TOOL LENGHT------IN THE TABLE AT POSITION 1 IS THE LENGHT
G41 D2----TOOL RADIUS------IN THE TABLE AT POSITION 2 IS THE RADIUS(same tool)
if you have a table with 31 position it means you can set up 15 tools with lenght and radius
Thank you zavateandu
I now feel stupid :) I will try it , Thank you everyone . I will update you when the job is running :banana:
Ok. Zavateandu is wrong.
O0001 (TEST)
G17 G21 G40 G80
G54 (zero offset G54)
G0 G91 G30 Z0 (machine goes to home postion in Z)
G0 G91 G30 X0 Y0 (Machine goes to home position in X and Y)
G90
G0 G43 H1 D2 Z100 (H 1 for offset nr 1 and G43 for height compensation and D 2 for radius comp offset nr 2)
It should then move to Z100 mm over your G54 zero point In Z not in X or Y
Do something simple a square.
G0 X-5 Y-5 Z2
G0 Z-10
G41 X0 Y-2 ( Now radius compensation is to the left G41)
G01 Y50 F500
G01 X50 F500
G01 Y0 F500
G01 X-5 F500
G00 Z2
G40 (Radius comp off)
G0 G91 G30 Z0
G0 G91 G30 X0 Y0
G90
M30
It should do a square that is 50x50 mm with the X0 and Y0 at the lower left corner.
Hi, yes I use G43 and H now for tool length, so just adding a D and the other number for Radius now seems simple. I should have known. Thank you again
Good.
i have send you a private message as well
Or, you can get tool comp "B". allows for diameter and wear on the same tool number.
i was not wrong
my idea was ok ,didn't explained well
i miised the G43 H1 D2\next time use other words Riddersholm
You replaced G43 with G41, thats way i said your wrong, He could have crashed to tool straight into the machine, but yes we all do typo mistakes but my words where correct
every operator i think ,first time keep the feedrate at low position and look at "distance to go" on the first piece so the crash issue is away from happen ,but yeah your point it has some truth.