Wire post

[thtalim]

I need information about wire post.

I want to get value from wire parameter register 1 - 10.

I try with ~prmcode$, " = ", sparameter$, e$

other value appear but not this register 1 - 10 value.

Any help apreciated.

BTW I wat to make post for sodick what is the best base post?

[BERTRAM BOY]

What model Sodick are you running? Also, what control?

[thtalim]

I use AQ327 control LN1W

[Roger Martin from CNC Software]

The 'Aux Registers' in Wire are predefined variables.

Access them directly using prm1$, prm2$ - prm10$

 

For Sodick, have your Dealer get you the Sodick Mark_30 4X.pst (and the related Mach/Control Definitions).

 

Is is definitely the one to use!

[edmBosto]

quote:

---

For Sodick, have your Dealer get you the Sodick Mark_30 4X.pst (and the related Mach/Control Definitions).

 

Is is definitely the one to use!

---

Thanks Roger. I will keep this info since we are looking at getting a new Sodick.

[Guest]

quote:

---

I will keep this info since we are looking at getting a new Sodick.

---

get the fanuc

[edmBosto]

WHAT! Fanucs suck!!!!!

 

 

Just kiddin' Del as we have 2 and there very good.

[BERTRAM BOY]

Are you sure your controller is a LN and not an LQ? The LN is an older controller found on a lot of 1st generation linear machines.

 

Anyway, I have to respectfully disagree with Mr. Martin. I found that the MPWSD350 required far less post modifications for an LQ1 controller than the Mark 30 post.

 

[ 03-19-2007, 01:37 PM: Message edited by: BERTRAM BOY ]

[Storkman]

edmBosto, you got mail

[thtalim]

to Roger Martin from CNC Software

thanks for the info.

 

to BERTRAM BOY

I'll ask for that post.

My machine just came on nov last year.

Inside controler still using win nt 4.0

after dec 2006 they use win xp

sodick give choice, LQ more expensive with 3d cadcam. LN only 2d cadcam.

anybody use sodick?

 

to del

I prefer sodick than fanuc from result of tescut using 0.07mm wire.

[Roger Martin from CNC Software]

quote:

---

I found that the MPWSD350 required far less post modifications for an LQ1 controller than the Mark 30 post.

---

I'd also like to see this 'tuned' MPSSD350 post.

[Guest]

quote:

---

to del

I prefer sodick than fanuc from result of tescut using 0.07mm wire.

---

what were your results?

 

i have an old sodick 280. i use it to set things on.

[BERTRAM BOY]

quote:

------------------------------------------------

I'd also like to see this 'tuned' MPSSD350 post.

------------------------------------------------

 

 

After a lukewarm experience with our local reseller, You'll understand why I'm reluctant share our post with anyone

affiliated with a reseller or CNC software.

 

 

Our local reseller tried to charge us for "modifying" our post. They added a date comment and changed nothing else,

then told us the post had been modified. As can be predicted, the post didn't fuction any differently.

So, from that point on we modify all our own posts in house.

[thtalim]

to del

I satisfy enough with sodick, 0.07 mm wire work nicely, can make corner radius 0.05mm die, but standart thickness only 15 mm(not enough for punch), so must find myself the condition,

since 0.07 mm wire just an option.

 

to BERTRAM BOY

can you show me nc program result, just give me some idea.

[BERTRAM BOY]

This is a code for a 2" square with .250 corner radii and no taper.There is a glue stop -.025 from the lead in on the rough cut only. There are 4 cuts total.

I'm not sure how your LN control works, but the the LQ inserts a "header" above the G-code for settings such as power settings and offset values. That is why there are no offset values in the code. I hope this helps.

 

 

N5 G90

N10 TP1.000

N15 TN0.000

N20 G54

N25 G00 X0. Y0.

N30 T91

N35 T84

N40 C001 H001

N45 G01 G42 Y1.

N50 X.75

N55 G02 X1. Y.75 I0. J-.25

N60 G01 Y-.75

N65 G02 X.75 Y-1. I-.25 J0.

N70 G01 X-.75

N75 G02 X-1. Y-.75 I0. J.25

N80 G01 Y.75

N85 G02 X-.75 Y1. I.25 J0.

N90 G01 X-.025

N95 M01

N100 G50 X0.

N105 G40 Y0.

N110 C002 H002

N115 G01 G42 Y1.

N120 X.75

N125 G02 X1. Y.75 I0. J-.25

N130 G01 Y-.75

N135 G02 X.75 Y-1. I-.25 J0.

N140 G01 X-.75

N145 G02 X-1. Y-.75 I0. J.25

N150 G01 Y.75

N155 G02 X-.75 Y1. I.25 J0.

N160 G01 X-.025

N165 G50 X0.

N170 G40 Y0.

N175 C903 H003

N180 G01 G42 Y1.

N185 X.75

N190 G02 X1. Y.75 I0. J-.25

N195 G01 Y-.75

N200 G02 X.75 Y-1. I-.25 J0.

N205 G01 X-.75

N210 G02 X-1. Y-.75 I0. J.25

N215 G01 Y.75

N220 G02 X-.75 Y1. I.25 J0.

N225 G01 X-.025

N230 G50 X0.

N235 G40 Y0.

N240 C904 H004

N245 G01 G42 Y1.

N250 X.75

N255 G02 X1. Y.75 I0. J-.25

N260 G01 Y-.75

N265 G02 X.75 Y-1. I-.25 J0.

N270 G01 X-.75

N275 G02 X-1. Y-.75 I0. J.25

N280 G01 Y.75

N285 G02 X-.75 Y1. I.25 J0.

N290 G01 X-.025

N295 G50 X0.

N300 G40 Y0.

N305 T90

N310 M02

[thtalim]

I can make already post with "header" base on comment from power library also I do both compensation ( computer do wire & overburn offset, only small adjustment, maybe 0.003 mm by machine operator)

I prefer both compensation to afoid cutting interference in the corner since my things are very tiny.

I got another problem here.

I want to make comment like original sodick cadcam ( inside machine) like:

(Die / punch / open 1 - 1st cut)

(Die / punch / open 1 - 2nd cut)

(Die / punch / open 2 - 1st cut)

(Die / punch / open 2 - 2nd cut)

 

about 1 / 2 / 3 / 4 cut I can get from pass$ inside MPWSDMK30.pst.

also die / punch I can get from pdo_type$ it is predefined variables.

how about die / punch number information?

as example chain 1 / 2 / 3 where can I get?

I don't like to make counter, since I plan to do cut everything 1st pass (many figure, more than 5 drawing) after that do finishing .

I see from mastercam it make :

chain 1 - 1st cut

chain 2 - 1st cut

chain 3 - 1st cut

chain 3 - 2nd cut

chain 3 - 3rd cut

chain 2 - 2nd cut

chain 2 - 3 rd cut

chain 1 - 2nd cut

chain 1 - 3rd cut

 

also I need to do taper but this post cannot output g51/g52 ,

only g41/42 X...Y... A...

Thanks

[thtalim]

where can I get complete list of predefined variables.

[Roger Martin from CNC Software]

quote:

---

also I need to do taper but this post cannot output g51/g52 ,

only g41/42 X...Y... A...

---

"this post" - What PST would that be ?

 

 

quote:

---

where can I get complete list of predefined variables

---

Ask your Mastercam Dealer for the 'Post Processor Reference Guide'. (22 meg. of indexed PDFs)

[thtalim]

To Roger Martin from CNC Software

I use MPWSDMK30.pst

[Roger Martin from CNC Software]

Hmmm...

 

I took the MPWSDMK30.PST (a v9 post) and ran it thru UpdatePost for use with X2.

Then created a simple profile and contoured it using a 5deg taper.

 

Result ->

 

(T)

H001 = .006

 

G20

G90

G92 X0. Y0.

T91

C101 H001

G41 G01 G51 Y.38344 A5.

X-.49708

G03 X-.73208 Y.14844 J-.235

G01 Y-.44985

X.9147

Y.14844

G03 X.6797 Y.38344 I-.235

G01 X0.

G40 G50 Y0.

T90

M02

%

 

 

If you post your wirepath using the Sodick Mark_30 4X.pst, do you get different results?

[thtalim]

I Ask my Mastercam Dealer for the 'Post Processor Reference Guide' and he tell me to check on mcamdocumentation.

I can see MastercamX_Post_Parameter_Ref.pdf

Is this the one you mention?

but don't have predefined variables.

[Roger Martin from CNC Software]

The 'Post Processor Reference Guide' is not on the X (X2) install CD.

The 'MastercamX_Post_Parameter_Ref.pdf' is updated list of changes regarding the Post Parameters.

('parameters' <> 'predefined variables')

[thtalim]

I got from my distributor, but it is for version 9. is there any for newer version?

[Colin Gilchrist]

Tonny,

 

The V9 Post Reference Guide and the X Post Parameter Update are meant to be used together. Its kind of a pain because you have to figure out how it worked in V9, then figure out if they have changed anything for version X(2).

 

HTH,

[thtalim]

Finally, after 2 weeks sleep at 3 AM everyday, I become more crazy than before, because I found some "crazy thing" on wire.

 

1. we have option to reset pass number on tab cuts.

If I make it blank, pass number going up,

as example,

I Perform rough cut and 2 additional skim cuts,

continue with 2 tab cut ( see, crazy thing begin )

first tab cut become pass 4 mean condition code use is on 4th cut, ( but first tab cut must use first condition code, same as rough cut)

continue with second tab cut.

I prefer always reset pass number on tab cuts.

 

2. If I use make tab cutoff move with skim cut

I miss condition code if additional skim cuts [before tab] <> 0

as example,

I perform rough cut continue with 2 additional skim cuts [before tab] and do 2 tabcut with make tab cutoff move with skim cut.

on 2nd skim cuts [before tab] condition code is 3

but when do tab cutoff, condition doesn't change to condition code 1, but still on 3 (you must waste alot of wire because of wire break, also no high pressure on)

 

3. I do Rough, tab & finish separate,

I found, if number of tab cuts <> additional skim cuts [before tab] + 1 (first rough)

when I do skim cuts after tab together is ok, but separate is not ok. if use both together and separate is ok.

as example.

I perform rough cut continue with 2 additional skim cuts [before tab] and do 2 tabcut.

when I do skim cuts after tab separate,

condition code is 3.

It should be condition code 4, since we already cut 3 times.

 

Anybody can explain to me?