What am I missing here?

[Japazo]

Hey everyone,

I just took a job as an engineer with one of my responsibilities being the programming of a CNC Mill using CAMWorks and Solidworks. I have been trying to get the correct post processor for CAMWorks from our supplier, but so far I have no solution from them.

Controller: GE Fanuc 0i-MC
Machine: Mag-Fadal VMC 4020-FX

In the meantime, I have a simple part that needs to be machined but is on hold because I'm too new to this to be able to simply write the code myself. I have some code which is very close to what I need, but I still can't get it exactly right. Here is what I've got so far,

% 
O0007
G40 G90 G17 G80 G49 
G49 G40 
T11 M06 (3/8 4 FLUTE COA EM) 
G40 G90 G80 G49 
G0 G56
G0 X-.4 Y0 M3 S1000
G00 G43 H11 Z.50 M8
G0 G56
G01 Z-.75 F4.
G0 G41 D11 X-.4 
G02 I.3025 J0
G0 X-.4 
G01 Z-1.375 
G02 I.3025 J0
G0 X-.4 
G01 Z-1.9999
G02 I.3025 J0
G1 G40 D11 X-.5 Y0.0 
G0 Z0.25
M5 
M9 
G0 G91 G28 Z0 
G90 M2
%

What I am trying to accomplish is to simply interpolate around the outside of a square peg and mill it down into a round one (don't worry about the potential problems with that). The peg is 0.25" x 0.25" x 2.0" long. I am milling it in three steps from top to bottom.

The machine does everything correct except it doesn't seem to be centered on the part like it should be. I'm not totally sure if it starts out centered or not, but it definitely ends up off of center (by visual inspection). Am I accidentally offsetting the tool by using 'G0 X-.4' and the machine is not returning afterward? Any ideas on what is wrong here would be great. If you need more information I'll be happy to provide it.

Thanks,
Andy

Also: If anyone knows where I can find the correct CAMWorks post processor for my controller and machine, I would really appreciate it. I'm tired of receiving the wrong ones from my supplier!

[annoying]

Well, the X-.4 and then the I.3025 is stabbing me in the eye. Not sure what diameter you are trying to cut down to, but I was guessing that maybe the I.3025 included the tool radius and the radius you are cutting??.?.? Assuming you part is centered at 0,0, the obvious problem is that you are calling the X- quadrant of the circle to be -.4, then shooting at a radius of .3025, which is making that circle center -.0975 of 0

And then, if the I.3025 is a combination of arc radius and tool radius... don't. Or don't use tool comp (G41).

So, assuming you were trying to cut a .115" radius... You could try something like this


%
O0007
G40 G90 G17 G80 G49
T11 M06 (3/8 4 FLUTE COA EM)
G56
D11 G43 H11
G0 X-.315 Y0 M3 S1000
G0 Z.50 M8
G1 Z-.75 F4
G41 G1 X-.115 F4 (approach, comp on)
G2 I.115 (cut CW circle)
G40 G1 X-.315 (release, comp off)
G1 Z-1.375 F4
G41 G1 X-.115 F4
G2 I.115
G40 G1 X-.315
G1 Z-1.9999 F4
G41 G1 X-.115 F4
G2 I.115
G40 G1 X-.315
G0 Z0.25
M5
M9
G0 G91 G28 Z0
G90 M2
%



That could work, but will leave marks at approach, release. I prefer to roll in, roll out


%
O0007
G40 G90 G17 G80 G49
T11 M06 (3/8 4 FLUTE COA EM)
G56
D11 G43 H11
G0 X-.315 Y0 M3 S1000
G0 Z.50 M8
G1 Z-.75 F4
G41 G1 Y-.2 F4
G3 X-.115 Y0 J.2
G2 I.115
G3 X-.515 I-.2
G1 Z-1.375
G3X-.115 I.2
G2 I.115
G3 X-.515 I-.2
G1 Z-1.9999
G3X-.115 I.2
G2 I.115
G3 X-.315 Y.2 I-.2
G40 G1 Y0
G0 Z0.25
M5
M9
G0 G91 G28 Z0
G90 M2
%

No promises though. Can't say I've used that control. And, can't say that it wont be hell trying to cut that. Also, got rid of some of the extra fubar in there

[sinha_nsit]

There are several mistakes.
To start with, write programs without radius compensation. In many cases, it is possible to take into account the cutter radius without using G41 or G42. After gaining some experience, try G41/G42. Take care of lead-in/lead-out distances.

[angelw]

Hey everyone,

%
O0007
G40 G90 G17 G80 G49
G49 G40
T11 M06 (3/8 4 FLUTE COA EM)
G40 G90 G80 G49
G0 G56
G0 X-.4 Y0 M3 S1000
G00 G43 H11 Z.50 M8
G0 G56
G01 Z-.75 F4.
G0 G41 D11 X-.4
G02 I.3025 J0
G0 X-.4
G01 Z-1.375
G02 I.3025 J0
G0 X-.4
G01 Z-1.9999
G02 I.3025 J0
G1 G40 D11 X-.5 Y0.0
G0 Z0.25
M5
M9
G0 G91 G28 Z0
G90 M2
%

Thanks,
Andy

Hi Andy,

As Sinha has said, you have made several mistakes, but the question that begs to be answered is where X0 Y0 is set on the workpiece.

Irrespective of whether cutter radius comp is used or not, starting at X-0.4 Y0.0 followed by G02 I.3025 J0 will result in a circular path with a center coordinate of X-0.0975 Y0.0. If the X0 Y0 of the workpiece is supposed to be the centre of the square, then this is the reason for the out of center result.

The I and J in the G02 block describes where the center of the radius being cut is relative to the current cutter location. As the I and J are incremental values, the absolute value in X of the circle center is -0.4 + 0.3025 = X-0.0975

Regards,

Bill