Siemens 840D Control

[Mick]

If anyone here has experience with these controls, could you please email me? I'm running through a post setup for a customer, and I need to check the drill cycle output, to ensure its correct. I have the MP_SIEMENS post from Inhouse, but I'd just like to double check the output

 

Thanks

[Rekd™]

Mick, you'd prolly be better off and more accurate to get a sample code from the customer that they use on the machine now, unless it's a new machine for them or somfin.

 

Just a thought

 

'Rekd

[Fig sign]

Mick !

 

Siemence controller is very configurable and varies from machine to machine and from one machine builder to another .

I run DMC63V with Sinumeric810m ,which differs from 840 only that it has no support for 4-5 axes stuff .

I am busy now and can not reply more .Use search option with my user name#498 and words Siemence ,810,840and you`ll got a lot of info .

HTH

 

 

PS Anyway I am with Rekd ,be more specific what machine and what drill format you expect (there are many in Sinumeric ,I hate them all ).

[Mick]

Yep, thats why I want an email contact. I need some sample drilling cycle programmes

 

Any help would be appreciated

 

Cheers

[Fig sign]

Like this :

quote:

---

%_N_sampledrill_MPF

;$PATH=/_N_MPF_DIR

;(============)

;( DRILL CD )

T1

M6

M01

;( T1 - CD DIA. - 6.25 )

G00 G64 G90 G54 X100. Y0. S900 CFTCP NORM M3

Z70. M8

F45.

R0=0 R1=.3 R2=3. R3=-1.5 R4=0.5 R5=.3 R10=70. R11=0.3

G83

X100. Y0.

X-100.

G80

M5

M9

T2

M6

M01

;( DRILL WDR 8.5 )

;( T2 -DRILL 8.5 DIA. - 8.5 )

G00 G64 G90 G54 X100. Y0. S680 CFTCP NORM M3

Z70. M8

F70.

R0=0 R1=1. R2=3. R3=-40. R4=0.5 R5=1. R10=70. R11=0.3

G83

X100. Y0.

X-100.

G80

M5

M9

T3

M6

M01

;( DRILL WDR 9.7 )

;( T3 -DRILL 9.7 DIA. - 9.7 )

G00 G64 G90 G54 X100. Y0. S595 CFTCP NORM M3

Z70. M8

F70.

R2=3. R3=-40. R10=70.

G81

X100. Y0.

X-100.

G80

M5

M9

T4

M6

M01

;( DRILL WREAM 10 )

;( T4 -REAMER 10 DIA. - 10. )

G00 G64 G90 G54 X100. Y0. S270 CFTCP NORM M3

Z70. M8

F50.

R2=3. R3=-10. R4=0.5 R6=0 R7=100 R8=150 R10=70.

G89

X100. Y0.

X-100.

G80

M5

M9

;( DRILL WTAP M10 )

T5

M6

M01

;( T5 -TAP M10*1.5 DIA. - 10. )

G00 G64 G90 G54 X100. Y0. S150 CFTCP NORM M3

Z70. M8

R2=3. R3=-30. R4=0.5 R7=100 R9=1.5 R10=70. R12=0

G84

X100. Y0.

X-100.

G80

M5

M9

END

M30

 

%_N_END_SPF

;$PATH=/_N_SPF_DIR

N10 G90

;N20 G0 Z100 M9

N30g0 G53 Z=(-50-$P_TOOLL[1])

N40 G53 X50 Y450

N50 M17

---

 

[ 01-26-2004, 02:05 AM: Message edited by: Iskander teh Owl ]

[Fig sign]

mICK !

 

Look on this this and this

 

HTH

[Mick]

Thanks Iskander. I need to know:

 

Does the code have to be output like this:

 

N1030 R0=0 R1=0.7 R2=2 R3=-20 R4=0.5 R5=0.7 R10=45 R11=0.3

N1040 G83

 

or is this ok: (The following is how the post is currently set to output)

 

CYCLE83(155,150,1,5,145,10,50,20,1,,0.5,1)

 

Cheers

[Fig sign]

Both OK !

The first is easy to understand ,that `s a difference ,that`s IMHO !

 

Just pay attention to this -All variables for cycle must be initialized ,otherwice the controller `ll take the variable anyway ,the THE ACTIVE (LAST USED )!

Just imagine what can happen!

 

You are welcome ,Mick .

I am at your service ,sir!

 

[Fig sign]

That`s what Siemence wrote in their manual :

quote:

---

Caution -danger of collision !

Parameters .... remain stored in the memory also after the cycle has been deactivated and the control unit has been switched off .

Be sure to program paremeters anew after each cycle call !!!!

---

HF

HTH

ITHH

[Jimmy Wakeford from Barefoot CNC]

Mick,

 

The 840d is a popular control type for some routers, it usually comes with macros that handle everything from tool setting to surfacing fixture.

 

The main problem with seimens controls is it is hard to find info on them.

If you can have customer go into the conversational programming screens and create the dif types of cycles it would be best. There was an 810 ost that supported all the cycles, back in V6, but dont know if it ever got updated.(Not real sure where it came from neither.)

 

[ 01-26-2004, 07:54 AM: Message edited by: Jimmy Wakeford, from Barefoot CNC ]

[Fig sign]

Yes I also have a bunch like engraving ,pocket milling and more ..

 

But what I have they are primitive rude crips ,never use them,with Mastercam I work faster and nice ,who now use in-built dialog programming .

But I wrote my own ...

[Jimmy Wakeford from Barefoot CNC]

Iskanedr,

 

That is the neat thing bout the r vars, you can set up like fanuc macro b. If you have time and patience.

[pip]

This is how our post outputs a drilling cycle.

The MCALL before the cycle, and after the cycle, are used when you must machine a group of holes.

 

N40 T01 ;DRILL 10MM:

N50 M6 ; T01 in Spindel

N60 G0 G40 G60 G90 D1 S1145 F137.4 M3 T0

N70 MCALL CYCLE82(10.,0.,10.,,25.,0.)

N80 X0. Y0.

N90 MCALL

 

Hope this helps

[Fig sign]

Pip !

This is a legit code for my machine too !

But ...

The first time I saw one like this I said i will NEVER run a machine with such a crap !

The way you start to count this (..,,,...,) can

drive crazy anyone .

Nevertheless it is a matter of taste .

I like something more looking like a mainstream code (fanuc -like ).

And I don`t use staging .

M6 in my machine can allow to run

T1

M6

with first tool in spindel it simply skips it

And I don`t call D they are called automatically with a toolchange in my machine

It makes my life easier cause I also run my machines ,I am the solo mill programmer/machinist in a shop ,and I care about myself

 

Iskander teh me and my buddy Eeyore are sometimes

nuts

[pip]

Iskander

 

Without the "D1" our machine (SW25) will try to plant the tool downstairs in the celler. I think it is a manufacturers thing. If the D1 is not read then the tool length compansation in not added, and so results in a very big bang. Our screen also shows a dialog when you pass over each parameter, so you know what you are adjusting. It id look a bit daunting when I first used this controll, but I have grown quite fond of it now. I downloaded all the manuals (siemens 840D) from the siemens hompage. All is very well explained.

[pip]

http://www3.ad.siemens.de/doconweb/content...102_E&scope=all

 

is the address mentioned above

[Fig sign]

Pip!

May be this feature is machine-builder add-on on my 810D.

And sure for 4-5 axes that`s the 840 for it is completly different story .

I do not like Siemence (after Fanuc and Okuma ),

but I run what I have .

And I read manuals before I pressed the button for the first time .

What I do like is the E axis and the tricks you can do with it !

[Mick]

Thanks everyone for your replies. It's clarified the format for the drilling cycles, and hopefully the customer will have everything sorted.

Again, thanks for your assistance.

[ak762]

Iskander

quote:

---

What I do like is the E axis and the tricks you can do with it

---

Could you explain us more precise what is E axis

[Fig sign]

E axis is spindel axis .

It has it`s own incoder and you can see it in positioning table.

You can set it in the homes settings different

for every home.

Due to it rigid tapping is enabled you can do it in pecking stile .

You can do more...

You can position boring cutter to any angle with SPOSA(...) command

You can stop your spindel and make vertical slotting

You can use spindel as C axis setting your spindel to position control

command SPCON()

and using SPOS command relying to your spindel like c axis

SPCON

SPOS=0

Z50 C180 (SPINDEL IS TRAVELED WITH LINEAR INTERPOLATION IN Z AXIS )

..

..

..

SPCOF (return spindel to speed control )

nATURALLY WHEN IT IS A MILL-TURN MACHINE IT IS NOT MATTERS ,BUT ON MY MILL i WOULD do it only on

soft material or setting special head (pneumatic ) enabling to me to turn my head to C axis

You can do more ...

 

Is it cool ?!?