[johny0407]

Hey I'm a young guy who's been programming for a little over a year, and i want to know how to properly mirror an image of any part. Im using the machines manual to guide me through it, using the G51.1 code to tell it which axis to mirror and G50.1 to turn it off. My problem is that the machine, goes and totally ignores the Z coordinate I programmed it to do. Here is the code:

N18 T1 M6
N19 G0 G17 G20 G40 G49 G80 G90
N21 G0 G90 G54 X0 Y0
N22 G51.1 X0
N23 G0 G90 G54 X0.115 Y0 S2000M3
N24 G43 H1 Z3.
N25 G1 Z2. F15.

The manual told me to mirror off the program's zero, as I did on line 21 & 22 and it [I]does[I] in fact mirror the code about the X axis because the next line reads X -.115 on the machine. But, when it reads the next line (line 24) the spindle goes past Z3. and keeps going down then, it goes up and finally starts reading Z3 and goes down again to Z2. and performs well after that. (Everything is correct: offsets, tool lengths...etc.)
What is causing this problem? any help would be deeply appreciated Thanks in advance guys.

[gar]

070208-1910 EST USA

Do you have a lookahead problem?

.

[Geof]

Try setting the tool length, G43 H1, before the mirror command.

[dcoupar]

I agree with Geoff. Also, you are calling a G54 while Mirror Imaging is on. Try moving the stuff in N21 after N24.

From the Operators Manual:

In programmable mirror image mode, G codes related to reference
position return (G27, G28, G29, G30, etc.) and those for changing the
coordinate system (G52 to G59, G92, etc.) must not be specified. If any
of these G codes is necessary, specify it only after canceling the
programmable mirror image mode.

[johny0407]

Thanks guys I'll try these modifications and hopefully it'll work.

[Willbird]

From my own experience keep in mind that most endmills will cut a differant size when using mirror, due to the non mirror part being climb cut, and the mirror part being conventional cut(or the reverse if the non mirror program uses conventional milling). This differance can be quite significant in some cases.

Bill

[johny0407]

You're right Bill, the manual states that some of the G41 will have to be converted into G42 and vice versa. I'm still trying..

[Willbird]

I mean other than the cutter comp right/left issue (been so long since I ran the jobs I am rembering I do not recall if they HAD cutter comp even)

The effect I mention could be illustrated by running the same program once with a RH tool, and again with a LH endmill using the proper spindle rotation for each cutter, the pulling action of the cut changes due to climb cut or not...and changes the size quite a bit :-)



Bill

[sluggo]

The whole conventional climb cut thing is why i hardly ever mirror, but I do rotate 180 degrees quite often, but that might not suit your needs. Some of the conversatonal machines I have run will reverse your tool path when mirrored so to that you can climb cut both sides.

[Willbird]

Axis rotation (G68 on the machines I ran) is sure a neato thing isnt it ?? once you start to really use it it can be very powerful, I used it all the time for rotated features. For example an elongated slot at 37 degrees to all the other features on the part, far far faster to write it along either the X or Y axis, and use G68 to rotate it the 37 degrees.

Also 2 or more features can often be G68 with a subroutine as opposed to crunching all the numbers to write them.

CAM makes some things easier to WRITE but it is hell to debug it on the floor if it isnt working or if you need to alter it for a print revision and you don't have CAM on the shop floor at 3 am and your the night shift guy.


Bill

[notallhere]

I agree with Willbird G68 is a great way to do alot of time saving in writing code.
Most stuff I write subs and then rotate for my "mirror" parts.