Problem- wedm programing problem

[steve hill]

I have a wire edm that is controlled by a Fanuc SP-150 controller. I am new to g codes as I have always had a post prosessor to write the programs for the Agie edm , which we have had for years. However, our new used machine ,Hitachi wire edm with Fanuc controller, has to have different programing then the Agie has. I have been working with Esprit and so far every program we have written wants to zero X and Y to the start of the program and losing my original reference point. I have a block which has to have eight .375 dowel pin at holes burned in it at exact locations. I want to zero the corner of the block and move to a location ,burn a hole ,move to the next , burn the hole and so on. I want the program to start wherever I put it ,start and stop at the same X and Y location. The machine is not an auto threader. The Agie works like this so I feel this is a matter of programing. Could someone give me an example of programing that would do this. Any help will be greatly appreciated. This is my first post. Thanks much Steve

[Kiwi]

Originally Posted by steve hill .... move to a location ,burn a hole ,move to the next , burn the hole and so on. I want the program to start wherever I put it ,start and stop at the same X and Y location.....

Sounds like you should program the code for the hole using G91 (Increment). I'm guessing you need some code like a mill would use. I've never used a EDM.

Start at centre of hole.

G91 G01 X0.1875
G03 X0 Y0 I-0.1875 J0
G01 X-0.1875
G90
CHECK BEFORE YOU CUT

[steve hill]

Thank you Kiwi for your response. I tried it but the machine wouldn't take it. I have a friend who has one of these machines and he programes it with Bridgeport mill software, like you mentioned, but he doesn't do multiple holes only one cut pieces. Guess I'll just keep hammering it out with Esprit untill we get something that works. Thanks again for your reply. Steve

[Kiwi]

Can you send some code. Two or three holes only so I can see what does work.

Just a thought, may require circle to be two arcs.

G91 G01 X0.1875
G03 X-0.375 Y0 I-0.1875 J0
G03 X0.375 Y0 I0.1875 J0
G01 X-0.1875
G90

[steve hill]

Hi kiwi - I finally got the programing I was after. The answer was to write it incrementally. This is the programing for a .500 hole with 2 skim cuts on a wire edm. The s code is the power setting and the d code is the offsets.
g91
s1 do
g52 g41 g01 y.25 t5.
g03 x.0299 y-.0018 i0 j-.25
m00
x-.0299 y.0018 i-.0299 j-.2482
g50 g40 g01 y-.03
s2 d01
g52 g42 g01 y-.03 t5.
g02 i0 j-.25
g50 g40 g01 y-.03
s2 d02
g52 g41 g01 y.03 t5.
g03 i0 j-.25
g50 g40 g01 y-.25
g00 x0 y0
m30
this progaming allows me to start anywhere and it will end where it was started, without losing my reference at the corner of the block.

thanks for your interest Steve

[Kiwi]

Your code appears to have more detail and moves than I offered.
Glad you have got what you required.
Cheers.