I need to engrave p/n on an OD .I have win-cnc but the sub program out puts doesn't seem to make any sense??
any help or advise on programing G12.1 possibly?
I have used Win-Cnc for engraving for years. Works well, but the sub program is only the cutting code. You must get the tool to the part and ready to cut before the sub program starts. You can also set the direction, size and axis' before you create the code. See the manual that comes with the software. (On the CD)
You can engrave on the OD if you have milling interpolation (G12.1) you will also need to change to "cylindrical plane" (G16) along with the G12.1. OR you can just use the C' axis commands.
Attached are snap shots of the settings in Win-Cnc on how to get the code right for OD etching.
On the Citizen machines you choose what plane you want to use during G12.1 "milling interpolation" when you choose the "G16" plane you are then using "cylindrical machining" .
G12.1- (option)Converts C axis degrees and X axis movement to work like
a milling machine. Program X-Y axis and the control converts all the
commands to degrees automatically. X and Y are programmed in radius
values and zero is at the center of the part, like a milling machine.
Tool nose rad comp is also needed to use G12.1 correctly.
There are some new options while calling G12.1. We used to have to
change parameters to use G12.1 #1125 Mill_AX and #1126 MillC , now
we can set these while calling G12.1 . See also G16 below.
G12.1 D0 E=C (the D and E= are new to the C/M series)
D0 -You can use "C" or "Y" as the virtual axis while in G12.1
The manual suggests using "D1" to use "C" but I don't agree.
If in G17 X-Y plane, then I suggest you use "D0" to use Y".
Your choice, it makes no difference which you use! If D is
not on the G12.1 line then "C" is default.
Always have "D" first on the G12.1 line!
E=C -This will set the axis number of the system to use as the
polar axis. This depends if you are using the gang plate in
$1 or the U121B option in $2 or $3. Setting E=C will set the
proper axis automatically. If you don't use E=C on the line then
$1 C axis is default. For safety, always use E=C
(MILL A .3 SQUARE WITH .02R CORNERS)
G12.1 D0 E=C
G13.1- cancels G12.1 by setting control of the C axis back to C and H
G16- Plane select cylindrical machining. To use this plane you need the
option of G12.1 milling interpolation. G16 is used to convert polar
C axis degrees to linear Y when machining "J" slots or cylindrical
cams. Most of these part prints are dimensioned with linear and radial
values, not degrees. Also the prints usually show the part cut and
spread flat. Radii are hard to program and adjust without G16 and tool
nose radius comp. G41-G42. Programming would be linear "Z Y".
The polar "C" axis is converted to a linear "Y" axis. Another use of G16
is to chamfer a cross hole equaly all the way around the hole.
C= Position of X axis to calculate from if the actual cutting
position is different. This is in radial value. C.15 = X.3
(MILL A J SLOT Sample program not tested yet but should work)
T600(.125" cutter / 1/2"bar/ to cut .156 slot)
X.3(to depth of J slot)
G12.1 D0 E=C
G1Z.1,R.02(or use G2/some controls ,R didn't work)
G17- Plane select- X-Y used when milling with "Y" on the Gang Tools
G18- Plane select- X-Z normally used. G18 is when power on.
G19- Plane select- Y-Z
Does it mean that the [code] output does not look right to you?
The WIN-CNC engraving software is very simple and straight forward.
If you've "answered" all the GUI questions correctly then the code will execute as you've planned.
If you employ G12.1 you would need to "answer" the WIN-CNC GUI as if you were using YZ and not CZ and would be more "confusing" the just interacting with the software under "normal" CZ mode.
Maybe post the output and/or screen shots of the WIN-CNC GUI for the engraving
Cogmac1, you are right G12.1 does on OD with G16 ...... now engrave on cylinder will so much easier compare to G107.
The best way to learn is trial error.