Chmer Wire EDM Sample program.

Hi All,

We have just obtained a new Chmer GX650L wire EDM. Upon running a couple of jobs, I find it frustrating that we have to use "local Origin" points. Is there any easier way to do this?

I am used to running with different work offsets like G54,G55 etc. I am being told the CHMER supports this.

Please can you let me know how ? Would you also be able to a share a sample code how I can use the G54,G55 ? The present output I am getting from my post from Mastercam is as follows :

%
O0001
(DATE=DD-MM-YY - 29-10-18 TIME=HH:MM - 21:37)

N100 G0 G20 G90
N110 G92 X1. Y0. I1. J0.
N120 G0 X1. Y0.
N130 M60
N140 M35
N150 M81
N160 S101 D1
N170 G42 G1 X0. Y-.015
N180 X-1.23175
N190 G2 X-1.295 Y-.065 I-.06353 J.01535
N200 G1 X-1.46237 Y-.06395
N210 G2 X-1.51706 Y.00012 I.01018 J.06407
N220 X-1.45219 Y.06499 I.06487
N230 X-1.452 Y.065 J-.06487
N240 G1 X-1.28403 Y.06405
N250 G2 X-1.23175 Y.015 I-.01132 J-.06445
N260 G1 X0.
N270 G40 X.5 Y0.
N280 M50
N290 M30
%

Can any improvements be made to make my life easier?

Thanks in advance.

Hi Radiant:
Are you trying to make a pattern of the same part over and over?
If so, I can give you a quickie sample of a subroutine method I use on my Chmer G32S for this kind of problem.

On another note, does the sample code you posted even run on your machine?
I ask because there are bits in your code that my machine will definitely choke on.
Mine's vintage 2011, so maybe yours is different?

Cheers

Marcus

Hi Marcus,

It is not a repeatable job. It was just a one off.

The sample program ran on the machine. But I was not happy with the way the coordinate system it called for.

Thanks.

Hi again Radiant:
I don't quite understand what you're asking.
Your sample code does not explicitly state which co-ordinate system you're using so of course it will default to G54 like many controls do.
Also, when you state G92, it will reset the co-ordinate system to match the co-ordinates on the G92 line, so I normally leave the G92 line out unless I specifically want to reset my co-ordinate system like when I'm running a subroutine.
I'll pick up my main part origin, call it my origin by using G54 stated explicitly in my first line, but I'll use G55 in my subroutine and just move to my new position in G54, call it my origin in G55 using G92 to do it and then run the sub in G55, then go back to G54 for my next location, set it up as my origin again in G55 using G92 to do it and run the sub again.

That way I can keep the point I originally picked up unmodified and all my locations remain relative to that point which has never been altered during the whole program.
This is a good way to keep small errors from stacking.

But to go back to my main point; if I understand correctly, you're asking how to make the machine accept different work co-ordinate offsets, and the answer is simply to state which co-ordinate system you want to be in explicitly in the G code.
My machine has a page you can go to where you set up the co-ordinates in each ; it's accessed by hitting F7 when you're in the "MAN" menu; unless the controls have completely changed since 2011, yours should be the same.

You can select your coordinate system on that page by scrolling to it, and then simply type in your desired axis and the dimension you want it to be after you've positioned the wire with a touch off.
So if you want the center of a touched off bore to be X0 Y0 in G55, do your touch off, go to that page, scroll to G55 and when it's highlighted, type in X0Y0 and hit "ENTER".

So is that what you're asking about?
Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Hi again Radiant:
I'm wondering, do you know how to get the machine into G54 or any other work co-ordinate system in all the screens that are available?
Again, from my control; if you are in MDI mode for example, and you want to also be in G55 work co-ordinate system, you can scroll using the up/down/left/right arrow keys until the work co-ordinate field on the upper left of your screen is highlighted, and then type in the WCS you want and hit "ENTER"
There are also a set of choices in red lettering on the bottom bar of your screen so if you want to go to the local co-ordinate system or the machine co-ordinate system, you can pick from the menu and select one of these options.
So for Local Co-ordinate System on my machine, you'd select "3" and hit ENTER.
To go back to G54, you'd type in "G54" and hit ENTER.

Be aware you have to do that for each screen you go into; I'm not aware of a global setting where every screen will change automatically.
So go through all the screens, set them all up to G54 and then ignore them until you need to change one or more.

Radiant, I know the Chmer has a particularly crappy Chinglish manual, riddled with errors and incomprehensible gibberish, so don't get too frustrated...the machine is actually pretty good for a commodity grade machine and once you get the hang of it, they're pretty simple to run and are pretty bulletproof too.
Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Thanks Marcus. I shall try your suggestions in setting up the co-ordinates.

Regarding the G92, This is due to the output I am getting from the mastercam posts. The mastercam post spits out only G92 and not G55.

Thanks Marcus.

My Mastercam outputs only to G92. I have asked them for a new post.

Do you add wire compensation in the mastercam or on the machine. I tried adding the "Auto" for compensation in mastercam, but it didn't post any compensation and on my trial job, the cut was the wire diameter bigger than required.

Even though I asked for two cuts when I brought the program to the machine, there was only one cut. No skim cuts.

I have tried speaking to the machine distributor, but they are limited in programming knowledge and the capabilities on this machine. Would you know if there is a 1 800 number or support line for the Chmer machines.


I appreciate all your help and time.


Thanks a ton.

Hi Radiant:
I most commonly program with compensation in the control, such that if the compensation is zero, the centerline of the wire will follow the wire path.
I add my offset for wire radius plus overburn plus skim allowance in the program header and call it using an "H" word that references the offset I've put at the top of the program.
I can then run my roughing pass and my skim passes by just calling the code as a subroutine and telling it to run each pass with my desired power setting and offset.
This is how probably 99% of wire guys run their code because it's efficient to program and efficient to edit.
So for the CHMER machine a typical program looks like this:

(casket hinge bore)
;SC****= OV PW ON OFF AN AFF SV FR WF WT WL FM F
SC0100= 003 010 003 0012 002 0012 050 004 008 008 004 000 0.0000
SC0200= 003 010 001 0012 001 0012 050 009 008 011 000 000 0.0000
H021=0.0082 H022=0.0056
;SPARK DATA AND OFFSET [ 2018/03/11 03:36:12 ]


G90
G54 G0 X0. Y0.
S100 H021
G22 H1000
S200 H022
G22 H1000
M02


N1000 (0.103 BORE)
G01 G41 X.0515
G03 X-.0515 I-.0515 J0.
X.0515 I.0515 J0.
G01 G40 X0.
G23

This program makes a simple round bore whose center is at X0 Y0.
The program is called using H1000 to call subroutine N1000
G22 is the subroutine call word, and G23 signals that the sub is done

Sxxx is the power setting for the cut and Hxxx is the offset.

G54 is my work co-ordinate system.

The program cuts a bore diameter of 0.103", so as you can see, if the wire offset is zero, the center of the wire will be at 0.0515" radius.
I am using G41 as my offset direction so this bore is cut with the wire going counterclockwise around the inside of the bore.

It's that simple on my machine.
Hopefully yours is not too different!

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining