Kinda O/T kinda post issue?

[mold100]

As far as milling I know my way around Mcam and can edit a post for milling - but I have some wire issues.

 

We cut multiple features like say ejector pin holes and on the current job there are 70 .1253 + .0002 /-0. and our wire guy has to make a lot of manual changes as far as MOV points and things and I am not sure why.We have a .005 location error because he accidentally tranposed some numbers and I am confused as to why he cant program what he wants post it and send it to the machine without any manual editing? Machine is a 1994 charmille 4020.Is it a Machine/Post or operator issue?

 

I guess milling has me spoiled -

 

Also for personal info does any one run a wire and and have post for it they can post and cut most anything with, without manual editing? If so what machine type is it and how much post work have you done.

 

Thanks in advance.

[mayday]

quote:

---

operator issue?

---

Thats my guess, we have an FX10 and have no problems with moves between burns. its in your cut and thread positions in MC. been a while since I have used our wire seat. but I never had an issue with it when I was running the machine

[mold100]

He does not think that it can do (He has me confused on this) a CCF situation.

 

Iso is the geo, and the command file incorps the Iso and a tech file(Burn conditions?)and some how

he has to put something in between holes.

I am having him get me some code of what is posts and what it looks like after he edits it.

[mold100]

Ok what he gets:

 

N100 X-2.36221 Y1.08

N102 Y-1.08

N104 X2.36221

N106 Y1.08

N108 X4.54275 Y.625

% (TESTT )

N110 G92 G70 G60 X-4.54275 Y-.625 W0. H1. R1.

N112 M20

N114 G00 X-4.54275 Y-.625

N116 M02

 

What he has to do;

(304-A1C.MASTER CMD )

;SPA,X0,Y0

;SMA,X0,Y0

ROT,0

;MPA,Xe,Ye

;MPR,Xe,Ye

;CPA,Xe,Ye

;CPR,Xe,Ye

;CEN,X0,Y0

;ZCL

MOV,X-4.54275,Y-.625

CCF,HL1.CMD

MOV,X-2.36221,Y1.08

CCF,HL1.CMD

MOV,Y-1.08

CCF,HL1.CMD

MOV,X2.36221

CCF,HL1.CMD

MOV,Y1.08

CCF,HL1.CMD

MOV,X4.54275 Y.625

CCF,HL1.CMD

MOV,X0,Y0

MSG, END OF PROGRAM 304-A1B

[mayday]

Thanks for the lesson in greek

Im not gonna be any help after seeing that funky code. ours is a mits with the fanuc code

sorry

[mold100]

I dont like mills that arent at minimal somewhat fanuc, so i am really hating this thing.

[Roger Martin from CNC Software]

So he is creating the (main) Command file, which happens to be calling a (sub) Command file (HL1.CMD), which I must assume actually does the SPG calls of the ISO (path motion) file.

 

There are several (many?) ways to program these Charmilles.

I would not say "this way is better than that", but it is whatever method works for you doing your parts in your shop.

[mold100]

Roger whats the easiest, most effiecient way so we can eliminate manual errors?

[mold100]

Bump, any one else on the way they recomend?

[Roger Martin from CNC Software]

quote:

---

Roger whats the easiest, most effiecient way so we can eliminate manual errors?

---

No way to tell with the limited info I have.

Other than make sure the guy punching in values isn’t dyslexic

[mold100]

quote:

---

Other than make sure the guy punching in values isn’t dyslexic

---

C'mon man, we're an equal oppurtunity employer.

[d00d]

Program a Mits FX-10 here as well nothing has to be done manual EVER. But I have to believe that if the control on the machine can be loaded manually to make these moves then there has to be a post that will work. Our sister company has 22 wire machines and a few of them are the charmille's. If I can free up enough time to get down that way this week I'll talk to there wire "guru" and see if I can get some answers for you.

[mold100]

d00d , htat would be great, I would really appreciate it.

[Lars Christensen]

I am not going to be to much help.

But you can edit a post to read charmilles laungues, but man it is going to be alot of work.

Charmilles new machines (Millinium) understand both fanuc and Charmilles langues.

I have edited our FA (Mitsubitshi) post, so I can do everything from Mcam, from doing feedrate ajustments(special feature on Mits), power ajustments, wire speed and so on, have the Misc. values all used. How long? not sure, it took a while speciely because everything is in reverse order compared to Mpmaster for mill.

Now it seems to me that it would be well worth doing this post, even if it is going to take alot of work. I can not imagen having a guy doing all the geometry in mastercam, for there after editing everything after he has posted it, sounds like alot of wasted time, and a high risk of mistakes. Maybe you should try to give your local Charmille dealer a call, or Chamilles in Chicago, they might have something you can use.

 

Lars

[Roger Martin from CNC Software]

Corey,

 

Did you get my email (yesterday) ?

[Lucky]

Our older Agie Wire EDM uses a similar program structure. A .GEO file is the NC code to cut the shape. A .JOB file is the main program that takes care of positioning and calling of the .GEO file. Your command file is VERY similar to our .JOB file.

 

Our post for the older Agie does not support .JOB files and you may have a similar problem with command files for the Charmilles.

 

Several years ago we had a job requiring 300 precise holes in a plate. There was no way we could type all those locations without a mistake. I edited the drill cycles in a Fanuc mill post to create the .JOB file. Something like this:

 

pdrill

"MOV,", x, y, e

"CCF, HL1.CMD", e

 

pheader

";SPA,X0,Y0", e

";SMA,X0,Y0", e

"ROT,0", e

";MPA,Xe,Ye", e

";MPR,Xe,Ye", e

";CPA,Xe,Ye", e

";CPR,Xe,Ye", e

";CEN,X0,Y0", e

";ZCL", e

 

Once the post is ready, simply select drilling, window the points and you're done.

[mold100]

Roger, yep, I got him gatering the info, he takes his time I will try to get it to you some time today. Thanks alot.

[d00d]

Corey, spoke with our wire guru at the other plant, they have so many new mits machines that on the rare occasion that theyt do use the old machines they are doing it pretty much the way you guys are. Sorry couldnt be more help and good luck .