DOOSAN DNM5700 Probing

I have a round part held in a 3 jaw vise on a mill. I would like to probe and rest center at the start of each part cycle. Our cam software can easily handle the correct probe cycle but I am curious if there are parameters or some where I can look to see the difference between each part?

Either the new G54 offset or how much it changed G54 offset by?

Thank you

If you look at the Renishaw document that comes with Inspection Plus or Doosan's embedded version of it, there is a chart that shows every macro variable for every cycle and what it is used for. One or more of them will show the "error" or difference between the last time it was measured.

Paul

LockNut said:

If you look at the Renishaw document that comes with Inspection Plus or Doosan's embedded version of it, there is a chart that shows every macro variable for every cycle and what it is used for. One or more of them will show the "error" or difference between the last time it was measured.

Paul

Click to expand...

Looks like #135 #136 and #145. However I can't seem to find where they are displayed.

I can find the custom variables but they say "Data Empty"

csharp said:

Looks like #135 #136 and #145. However I can't seem to find where they are displayed.

I can find the custom variables but they say "Data Empty"

Click to expand...

Those variables get reset to NULL when the power is cycled and when "reset" is pressed. If you don't want to lose them when reset is pressed, change Parameter #6001 bit 6 to a "1".

Thank you I will give it a try.

csharp said:

I have a round part held in a 3 jaw vise on a mill. I would like to probe and rest center at the start of each part cycle. Our cam software can easily handle the correct probe cycle but I am curious if there are parameters or some where I can look to see the difference between each part?

Either the new G54 offset or how much it changed G54 offset by?

Thank you

Click to expand...

The way the WCS is set is not given.
Assuming that you are using Inspection + commands, and the “HOME” is set in the center of the bore, the position of each measured WCS can be stored in non volatile memory. In order to do so, add immediately after G65P9814D**.**S* line G65P7654 and load to the memory following program:
%
O7654(STORE WCS)
IF[#900NE0]GOTO10
#900=0
N10
#14=901(STARTING STORAGE VARIABLE NUMBER X)
#15=902(STARTING STORAGE VARIABLE NUMBER Y)
#16=10 (NUMBER OF STORED WCS)
#16=54 (WCS NUMBER, EDIT ACCORDINGLY)
#[#14+#900*2]=#[5201+20*[#16-53]]
#[#15+#900*2]=#[5202+20*[#16-53]]
#900=#900+1
IF[#900EQ10]THEN#900=0
M99
%
This will store in variables 901-920 the X and Y machine coordinates 10 consecutive positions of your WCS. After stated in #16 number of measurements it starts to load the result from the beginning.

csharp said:

I have a round part held in a 3 jaw vise on a mill. I would like to probe and rest center at the start of each part cycle. Our cam software can easily handle the correct probe cycle but I am curious if there are parameters or some where I can look to see the difference between each part?

Either the new G54 offset or how much it changed G54 offset by?

Thank you

Click to expand...

I have the classroom docs on this if you'd like.