Macro tool offset or tool R adjustment Hwacheon Lathe Fanuc 0i-TD

bspear · Sep 24, 2019

Hwacheon Lathe Fanuc 0i-TD

Milling this profile on my C axis:

sorted the finished profile but can't take it in a single cut so need some ruffing cuts.
Could work out each ruf profiles but could I simply adjust the tool offset or tool R on the fly to offset the finish geometry for multiple ruffing passes?
Can I adjust the appropriate param for each call of the profile as a sub?
These are the only params I can find? any suggestions? Cheers, Sean

angelw · Sep 24, 2019

bspear said:
Hwacheon Lathe Fanuc 0i-TD

Milling this profile on my C axis:

View attachment 265712

sorted the finished profile but can't take it in a single cut so need some ruffing cuts.
Could work out each ruf profiles but could I simply adjust the tool offset or tool R on the fly to offset the finish geometry for multiple ruffing passes?
Can I adjust the appropriate param for each call of the profile as a sub?
These are the only params I can find? any suggestions? Cheers, Sean

View attachment 265713

Hello bspear,
Yes, you can run the finish profile program with larger Tool Radius Offset values to take roughing cuts.

Post as copy of your Finish Tool Path code.

Regards,

Bill

bspear · Sep 24, 2019

This is the profile code:

O0105
G28W0
T1010
G98
M28
G28H0
S1000M3
G0Z5
X100C0
G12.1
G1Z-20F100
G41G1X36C-11.75F400
X8C-25,R1
X-8,R1
X-36C-11.75,R1
C11.75,R1
X-8C25,R1
X8,R1
X36C11.75,R1
C-11.75,R1
X8C-25
G40X8C-40
G13.1
G28W0
M29
M30
%

bspear · Sep 24, 2019

'course I could set up a bunch of offsets and call a new tool/offset before each sub call?
(I have 12 tools, I'm using T10)
T1010
then
T1013
T1014
T1015
etc......

?

angelw · Sep 24, 2019

bspear said:
'course I could set up a bunch of offsets and call a new tool/offset before each sub call?
(I have 12 tools, I'm using T10)
T1010
then
T1013
T1014
T1015
etc......

?

Hello Sean,
Yes you could do that. However, as G65 is allowable within Polar Interpolation Mode, another way would be to enter the Profile Code in a program to be called as a Macro and pass as an argument to the Macro, a desired Depth Of Cut. In the Macro you would arrange the Profile Machining Commands in a Loop and increment the System Variable for the Tool Radius Offset being used by the DOC passed to the Macro. The advantage of this method, is that you can easily change the DOC by editing the value being passed to the Macro, rather than have to change the values of multiple Offsets.

Regards,

Bill

bspear · Sep 24, 2019

That looks like what I'm after Bill, but do you know what the variable/param no. is for the tool radius offset and whether it's writable? (I presume your referring to depth of cut in the X/C plane) cheers, Sean

angelw · Sep 24, 2019

bspear said:
That looks like what I'm after Bill, but do you know what the variable/param no. is for the tool radius offset and whether it's writable? (I presume your referring to depth of cut in the X/C plane) cheers, Sean

Hello Sean,
Yes, DOC for X/C and yes, its writable. Take a picture of the Offset Page where you have the Tool Radius Comp Offset set for the X/C and Post here.

Regards,

Bill

bspear · Sep 25, 2019

Are these useful?
View attachment offsets.zip

angelw · Sep 25, 2019

bspear said:
Are these useful?
View attachment 265804

Hello Sean,
Following is one method to determine the System Variable for the Tool Radius Comp Offset Value.

Lets say that the Tool Call command is T1011, then:
(GET OFFSET NUMBER)
#1 = #4120 (#1=1011)
#2 = FIX[#1 / 100] (#2=10)
#2 = #1 - #2 * 100 (#2=11)

(GET OFFSET SYSTEM VARIABLE)
#3=#[2200+#2] (#2211)

Having obtained the Offset System Variable, it can be manipulated to change the Tool Path Offset from the Finish Profile.

Regards,

Bill

Search

Largest Manufacturing Technology Community on the Web

Search

Macro tool offset or tool R adjustment Hwacheon Lathe Fanuc 0i-TD

bspear

Plastic

angelw

Diamond

bspear

Plastic

bspear

Plastic

angelw

Diamond

bspear

Plastic

angelw

Diamond

bspear

Plastic

angelw

Diamond

Similar threads