Could use insight on some post modification for Hurco

[parkerbender]

Hello All!

 

I am trying to throw together a post for my older Ultimax 2 machine. I'm prety computer-fluent, but am having a hard time figuring out how to make a working post. I'm working with Mastercam x3, and can't figure out how to change the Z values after a canned cycle is called out. I have been told to use a standard Fanuc post, I'm assuming that means to start with the 'generic Fanuc 3X Mill.pst file. The tricky part is Hurco uses standard Fanuc until you go into a canned cycle. Once in canned, all z values become a positive value to reach a negative point after you have reached the R plane. Once R is reached the final Z depth will be incramental from the R plane.

 

Does anyone have a clue how to make that happen?

 

Thanks so much for any ideas/insight!

 

-Parker

[parkerbender]

Here is a post of the G81, G83, and G84 cycles. Also, is it hard to make the post only use feedrates with one decimal place?

 

Thanks for all the help!

 

-Parker

 

 

%

G0 Z0.1M8

G81 X3. Y1. Z0.6F5.0

G80

 

G0 Z0.1M8

G83 X1.Z0Z0Z.125F3.0

G80

 

G0Z0

S400M3

G0 Z0

G84 X3. Y2.Z0.5F25

G80

E

[Ron Branch @ Verisurf]

quote:

---

is it hard to make the post only use feedrates with one decimal place?

---

No look in the post for the fmt area to see what equals what and then just use the correct one and done. Also do a search things along this lane have been covered before.

 

HTH

[parkerbender]

That's how they're posting out of bobcad, with the correct post. So, that's how they are supposed to look, at least I think...

[Rstewart]

There's No way thats how the code is supposed to look.

 

All I know is Fanuc/HAAS G-code, but where is the Rapid plane or the inc. depth on the G83?

[[email protected]]

Another thing to remember: Hurco's G02/G03 are reversed on G18/G19 planes

I dont know why

 

HTH

 

edit: I have a good MPMASTER modified for Hurco's that I wouldn't mind sharing with you to get you started

[parkerbender]

okay, I think that I found a correct example. I'm sorry for the confusion, I'm an engineer, not a machinist...

 

"Here is the G83 for a Hurco BX:

 

N10G83X4.0Y3.0Z.8Z.5Z.2F10.0

 

after a rapid to X4Y3 Z will feed a distance of .5 rapid out, rapid in and feed a distance of .2, rapid out .7, rapid in and feed .1 for a total z feed of .8.

 

The Z moves in Hurco canned cycles are INCREMENTAL from the Z location commanded in the prevoius block. The 1st z in the G83 code is the total z travel, the 2nd z is the incremental move for the 1st peck only, the 3rd z is the peck increment for all remaining pecks until the z specified in the 1st z distance is reached. Z2 must be smaller than Z1. If no third Z is entered then the 2nd Z is the peck increment for all remaining pecks."

 

Thanks again for any help!

[[email protected]]

Did you read the post above your last one? Just wanna make sure you notice the part about G18/G19

 

HTH

[veedubnut115]

I will have to look at my post when I get back to work. I had to change our post so it worked with out hurcos...that is all we run. If I remember correctly, you need to reformat the drill depth to be a positive value, in your format statements, and you need to add the z start to your z depth to get the correct z output.

 

Its always confusing when I talk with other guys and they see that a drill cycle has all positive z values.

 

The one thing I found that sucks, is you can't use the clearance plane check box...screws everything up. If u backplot in mastercam it works, but when the hurco runs it....no such luck.

[veedubnut115]

If anyone has found a why to modify your post so that clearance planes do work...I would greatly appriciate the info...What I would want...If you have ever run the hurco conversational programs is.

 

Position above the hole, lets say at 1" then rapid down to lets say .02" then start the drilling cycle, once done drilling that hole, rapid back up to 1" and move to the next location, rapid back down to .02" and start all over again.

[[email protected]]

When I have to drill on different planes, I use a "Point" toolpath to make it rapid down to the plane I want to drill at then do the drill op.

 

It works, but more time consuming. Hurco drill cycles SUCK!!!

[Fred @ Slate Industries]

You have to have the Hurco ISNC option.

Then you can run all the Standard G code.

Your in Hurco Basic NC right now and that's why your getting all the Drilling hassles.

 

Hurco's are Work horses in any Mold Shop!

ISNC is a $500.00 option last time I checked.

You can peck tap with it too.

I'll send you my post if you need it.

But you have to have the ISNC option .

[[email protected]]

Tony,

I do have the ISNC option, just never used it. I would like to try your post.

khorton(AT)murraymold(DOT)com

 

Thanks Tony

[Josh T™]

Parker... you've got mail

[parkerbender]

Thanks Josh, I'll try that out later today!

[Bryan Johnson]

quote:

---

If anyone has found a why to modify your post so that clearance planes do work...I would greatly appriciate the info

---

I copied an example Hurco post to the FTP site.

 

"Mill_Hurco_PostX4"

it is in the Text_&_post_files folder.

 

It includes the support for clearance and the correct format for drill cycles (same as B'Port).

[parkerbender]

okay, now I have a post that is mostly working, but it inserts line numbers on both the front and back of the line following a G0, when there is only an X and Y coordinate on the line.

 

e.g.

N7310 G0 Z.25

N7320 X1.1675 Y-.4467 N7320 <------

N7330 Z.1

N7340 G1 Z0. F12.0

N7350 G3 X1.1751 Y-.4262 I0. J0. F43.2

N7360 G2 X1.2609 Y-.3479 I1.2926 J-0.4688

N7370 G3 X1.302 Y-.1254 I1.2292 J-0.227

N7380 G2 X1.2498 Y-.0216 I1.3748 J-0.0238

N7390 G3 X1.25 Y.0003 I0. J0.

N7400 G2 X1.1771 Y-.1134 I1.125 J0.0002

N7410 G3 X1.14 Y-.3145 I1.2292 J-0.227

N7420 G2 X1.1675 Y-.4467 I1.0507 J-0.402

N7430 G1 Z.1 F45.0

N7440 G0 Z.25

N7450 X1.2498 Y.0232 N7450 <--------

N7460 Z.1

N7470 G1 Z0. F12.0

 

Does anybody know what I did wrong?

 

thanks again!

 

-Parker

[parkerbender]

I'm still lost in here, I've been moving N$'s and E$'s around, and can't make it stop doing what it's doing...

 

Here's a copy of my motion control section:

 

# Axis Motion Definition section

# --------------------------------------------------------------------------

 

protaxis1 # Substitute Axis X/Y with Rotary axis (Custom Post Required)

pcan1, n$, sccomp, pccdia, sgcode, xangle, y$, z$, pfr, strcantext, e$

 

protaxis2 # Substitute Axis X/Y with Rotary axis (Custom Post Required)

pcan1, n$, sccomp, pccdia, sgcode, x$, yangle, z$, pfr, strcantext, e$

 

protaxis # Substitute Axis X/Y with Rotary axis (Custom Post Required)

xangle = x$ * 2 * rad2deg$ / rotdia$

yangle = y$ * 2 * rad2deg$ / rotdia$

if gcode$ > 1, "(ERROR - ARCS MUST BROKEN)", e$, ex$

pcan

if rotaxis$ = 1, protaxis1

if rotaxis$ = 2, protaxis2

pcan2

 

prapidm # Linear line movement - at rapid feedrate 0

pcan

pcan1, n$, sgplane, sccomp, pccdia, sgcode, x$, y$, z$, strcantext, !fr$,

pcan

 

prapid$ # Linear line movement - at rapid feedrate 0

if rotaxis$ <> 0, protaxis

if rotaxis$ = 0, prapidm

 

pzrapid$ # Linear movement in Z axis only - at rapid feedrate 0

n$, sccomp, pccdia, sgcode, pccdia, z$, e$

 

pedm # 5-Axis example (Custom Post Required) 11

"(5 AXIS EXAMPLE)", *xnci$, *ynci$, *znci$, *u$, *v$, *w$ #*i, *j, *k

 

plinm # Linear line movement - at feedrate 1

pcan

pcan1, n$, sccomp, sgcode, x$, y$, z$, pfr, strcantext, e$

pcan2

 

 

plin$ # Linear line movement - at feedrate 1

if rotaxis$ <> 0, protaxis

if rotaxis$ = 0, plinm

 

pz$ # Linear movement in Z axis only - at feedrate 1

n$, ptllncomp, sgcode, z$, pfr,e$

 

pcirm # Circular interpolation 2

pcan

pcan1, n$, sgplane, sccomp, pccdia, psgcode, x$, y$, z$, pijk, pfr, strcantext, e$

pcan2

 

pcir$ # Circular interpolation 2

if rotaxis$ <> 0, protaxis

if rotaxis$ = 0, pcirm

[Bryan Johnson]

you need a ", e$" at the end of

prapidm