[bostontrader]

We have a Charmilles 310 machine and have used the old Esprit/W for years and years. Yes, we do have the new version, but I don't like the way it works. The ONLY issue I wish would work would be for the program post to make a G00 move to insure the start point matches the program. As it stands, we have to manually enter the coordinates and once in a while (at the worst moment) numbers get transposed or just entered incorrectly.
Is it so hard to edit the asc file or is that something that needs the pst file changed and recompiled?
Here is an example. The first hole is X 2.93 Y0.0
%
N5 G90
N10 G92 G70 X2.93 Y0.0
N15 G60
N25 M20
N30(E501 Rough Cut 1.25")
N35 E501 H1.5
N40 G01 X3.1175
N45 G42 D0
etc...

would work well if it would output as in (manually added) N11 so the first move is to the first hole.
%
N5 G90
N10 G92 G70
N11 G00 X2.93 Y0.0
N15 G60
N25 M20
N30(E501 Rough Cut 1.25")
N35 E501 H1.5
N40 G01 X3.1175
N45 G42 D0
etc...

I know we'll have to use the new version at some point but it hasn't wowed me yet. I uploaded the post file to http://www.compuspider.com/uploads/fil2ax.asc if anyone can take a look. Thanks in advance.

[Royster]

Dont be ashamed of using esprit/w it's a fantastic package and does what is says on the tin!

Before we go down the route of adjusting your post processor.
Can you confirm that you have the following in your operation list
Set Origin
MANUAL
Contour 2
for example?

[bostontrader]

Thank you for your response. Although I usually don't "set" an origin as much as "move" the origin, it doesn't have any effect on the code even when I do set the origin to the first move. When you say to use "EDM manual" I never have, but the help file says
"Manual allows you to create feed or rapid moves by simply selecting points. No structure is required. First create points at the destination of your moves.
First Open the Manual menu.
For Mill or Lathe Manual, you must use a tool, but not for EDM."

Are you saying that I could do it to make a first move to my start? I can't see how by looking at it.
As for contour2 or 4, I do use that to create my operations. Thanks again for your time, Al in MA

[Royster]

With esprit/w 3.1 you "have" to initiate the first move with edm manual and it helps to specify the origin. (Specifing the origin merely creates the G92 line)

So a simple program running from the middle of a round shape should have the origin added here (x0 y0 in esprit) so long as your machine starts at this same point.

Then select edm manual, click first on it's start point (ie 0,0) and then click where you'd like your machine to end up ie wire start point (eg x20,y0) When I make NC code on the attached esw I get this:

%
L1/Test
(Mitsubishi-W-EDM)
H01 = 0.205
G62 X0 Y0
G97 X0
G71
G90
G92 X0 Y0
N11 G01 X20.000 Y0 F635. M91
N12 M20
N13 E961 F1.5
N14 M78 M78
N15 M80
N16 M82
N17 M84
N18 G90
N19 G92 X20.000 Y0
N20 G42 G01 X10.000 H01 M90
N21 G03 X-9.988 Y.500 I-10.000 J0
N22 X9.950 Y-.998 I9.988 J-.500
N23 M00
N24 X10.000 Y0 I-9.950 J.998
N25 M00
N26 G40 G01 X20.000 A0. F228.6 M91
N27 M88
N28 G23
N29 M02
%

I hope this makes sense

[bostontrader]

I did as you said, entered the origin as the first op, then made the manual move to my start point and it did make the code to move as I wanted. I will do some further tests but it looks like just a quick couple of clicks and everything should go as expected.

%
N5 G90
N10 G92 G70 X0.0 Y0.0
N20 M20
N25 G00 X0.0471 Y0.0
N30 G60
N40 M20
N45 E501 H1.0
N50 G01 X0.04789
N55 G42 D0
N60 G02 X-0.04789 Y-0.00049 I0.0 J0.0
N65 X0.04788 Y0.00098 I0.0 J0.0
N70 M01
etc...

I will get back to you regarding my results. Thanks again!

[Royster]

I'm delighted that all seems well.

I look forward to your findings

Any other Esprit/W questions you know where to find me..

EDIT: Oh as you probably already know. You shouldn't do a manual move for each aperture as the omission of this initiates your wire threading cycle.

If, however, you want it to move to next cut point without any tank drains, AF cuts or threads. then a "MANUAL position" is your function

[diemaker89460]

Hello, I have run a mits fx-10 with mastercam about 8 years ago ande found it very powerfull and easy to learn and use. I just hired at a company with the same wire machine and am now using esprit/w version 1. Anybody else using this old software? It sure seems less user friendly. On the skims page you have the ability to add additional skims but how to you set these skims to different power and offset settings? Do I manually have to edit the code?

[bostontrader]

Hi,
You do add or append them manually, but right click and save them once you're done. I usually start with one and save it right click, save as), then change the height of the part and keep saving them. That way you can just call them up. For example, EDM2>Current Settings (right click, open) I have tec files for everything I use such as 125RRR for cutting a 1.25 inch part with a rough and two skims all wire to the right, etc. It isn't perfect but once you use it, it does get easier.

[bostontrader]

Still using Esprit, now Version 5 in Windows 7 x64. Someone had asked me about using the parallel dongle. I had to load new Sentinel drivers You can use it with Win7, just download the file Sentinel System Driver Installer 7.5.8 from the Sentinel Page. The EDM Technology pages are different but I made a few changes to my FIL2AX.ASC post and it seems to be just fine.
My only issue I have left is that I want to see an M06 (thread) after the first move. I tried this:
EX_FIRSTRAPID : N M12*
: N G00* X Y
: N M06*
but I still haven't got it right. It never cut or threaded, just cut the metal to the next start.
Now I wonder if I should be looking at the CL (Cutter Location) file instead. Back to the reading.