Still new to G Code

[Larry Myers]

Hi All,

I am trying a simple (I think) side mill cut along the x axis. No change in Y. I have entered the program below. What happens is that I get a change in Y, like cutting at an angel. Can’t seem to figure out what I am doing wrong. Any ideas would sure help this rank beginner, wet behind the ears, complete novice. This is my first trying to use cutter comp (a 5/8” end mill and I added the GEOM D in the offset page)

Machine- Sharp 2412 mini VMC Controller-Fanuc Oi

T1M6;
G0 G90 G54 X3.05 Y1.5 S4000 M3;
G43 H1 Z.1 M8 ;
G01 Z-1.6 F50;
G42 D01 F15
X-2.425
G28 G91 Z0
M30:

The end mill at the end point is 5/8” in the negative at the end point of the cut. Makes quite a nice angle should I ever need one! 

Thanks all
Larry

[Geof]

Originally Posted by Larry Myers ... T1M6; G0 G90 G54 X3.05 Y1.5 S4000 M3; G43 H1 Z.1 M8 ; G01 Z-1.6 F50; G42 D01 F15 X-2.425 G28 G91 Z0 M30: Thanks all Larry

What you have here is the controller applying the tool compensation as it does the move from X3.05 to X-2.425.

In the line with your tool compensation command G42 you have not given any motion comand so the motion needed to set the compensated position is applied to the next motion command.

Write a program where you come to a start point clear of the workpiece. Then give the tool compensation command with a move that is larger than you tool radius but still puts the tool clear of the start of the cut; this can still be a G00 move.

Now you have compensation set and can move into your cut with a G01 and make your straight cut. Then move clear, lift Z clear and give the G40 with a small move to cancel compensation

[Larry Myers]

Hi Geof
Thanks

>>Write a program where you come to a start point clear of the workpiece. Then give the tool compensation command with a move that is larger than you tool radius but still puts the tool clear of the start of the cut; this can still be a G00 move.<<

Actually the X position is indeed clear of the part by just over the diameter of the tool. So Maybe something like this?

T1M6;
G0 G90 G54 G42 D01 X3.05 Y1.5 S4000 M3;
G43 H1 Z.1 ;
G01 Z-1.6 F50;
X-2.425
G28 G91 Z0
M30:

Thanks again
Larry

[Geof]

You still have not separated things out as far as I can see. Where are you actually cutting from and to? For simplicity when learning the code I found it best to be a bit laborious, something like this when described in words:


Choose the tool
Set tool length compensation
Star the spindle
Move with a rapid somewhere close but not to close to the start of the cut keep Z still well above
Move a little bit closer and at the same time set Tool Compensation; this can still be a rapid
Now make a feed move to the start of the cut and the correct Z depth
Feed along the cut to the end
Now move a little bit away from the end still feeding and lift Z clear
Now cancel Tool Compensation with a short rapid move
End program, tool change, whatever

Does your machine have a graphics simulator so you can step through these moves on a screen. This often helps.

It is perfectly legitimate to combine some of the command lines I have written separately above. You start doing this once you are comfortable that you know what is going where.

[timlkallam]

Try this Larry
T1M6
N1 G0 G90 G40 S4000 M3 X3.5 Y2
N2 G43 H1 Z.1
N3 G1Z-1.6 F50
N4 G42 D1 X3.05 Y1.5
N5 X-2.425
N6 G40 Y2
N7 G28 G91 Z0
M30

Line 1 place cutter half the rad. or more ahead of the start point.
Line 3 z should be at depth before cutter comp. is activated
Line 4 activate cutter comp to start point
Line 6 Very improtant after cut is done cutter comp MUST be cut off with movement.
Tim

[Larry Myers]

Thanks again Tim and thank you Geof. I'll try this first thing in the morning and see how it works.

Tim, from what you have suggested, if I want to continue on around this work piece, can I contine with out restating the G42?

Thanks
Larry

[Geof]

Originally Posted by Larry Myers .. can I contine with out restating the G42? Thanks Larry

Yes, and it did not register that you had G42...this gives you conventional milling, climb milling is much better, this is G41.

You can continue all the way around the perimeter of a part without changing the tool compensation but you have to make sure you do not reverse direction. Tool compensation puts the center of the tool either to the right G42 or left G41 of the cut line. When you reverse direction that means the tool has to move to the other side of the cut line for the right or left to still be correct. Obviously this means the tool has to pass through the work to get there. Most machines will alarm if you try this.

[timlkallam]

http://www.shoptalkmag.com/index.cfm...rs=0&artid=155

[Larry Myers]

Tim,
I sent you a message off line.
larry